VisualMILL Getting Started Guide

Transcription

1 VisualMILL Getting Started Guide Welcome to VisualMILL Getting Started Guide... 4 About this Guide... 4 Where to go for more help... 4 Tutorial 1: Machining a Gasket... 5 Introduction... 6 Preparing the part for Machining... 6 Create Tools...15 Create/Extract Regions...17 Create Machining Operations ½ Axis Profiling...19 Creating a 2 ½ Axis Profile for the Outer Region...30 Reports...33 Post Processing...35 Tutorial 2: Machining a Slotted Gear...37 Introduction...38 Preparing the part for Machining...39 Create Tools...46 Create Regions for Machining...48 Create Machining Operations ½ Axis Profiling...53 Creating an Engraving Operation...65 Post Processing...71 Tutorial 3: Machining a Shaft Base...73 Introduction...74 Preparing the part for Machining...75 Create Tools...84 Create Machining Operations ½ Axis Facing ½ Axis Pocketing...91 Hole Pocketing Operation ½ Axis Engraving Operation ½ Axis Profiling Post Processing Tutorial 4: Simple V-Carving Introduction Preparing the part for Machining Create Tools Create Machining Operations V-Carving Post Processing Tutorial 5: Embossing Introduction Preparing the part for Machining Copyright , MecSoft Corporation, 1

2 Create Tools Create Machining Operations V-Carving Roughing V-Carving Post Processing Tutorial 6: Chamfering Introduction Preparing the part for Machining Create Tools Create Machining Operations Chamfering Post Processing Tutorial 7: 3 Axis Milling Introduction Preparing the part for Machining Create Tools Create Machining Operations axis Horizontal Roughing axis Parallel Finishing axis Horizontal Finishing Post Processing Tutorial 8: Profiling with Bridges (Tabs) Introduction Preparing the part for Machining Create Tools Create Machining Operations ½ Axis Profiling Post Processing Tutorial 9: Hole Making Introduction Preparing the part for Machining Create Tools Create/Extract Regions Create Machining Operations Hole Machining Creating the Drill operation for the 0.25 Holes Post Processing Tutorial 10: Re-Machining a 3D Mold Introduction Preparing the part for Machining Create Machining Operations axis Pencil Tracing axis Valley Re-Machining Post Processing Tutorial 11: Machining a Ring Introduction Preparing the part for Machining Create Tools Create Machining Operations axis Roughing axis Finishing Post Processing Tutorial 12: Engraving on a Cylinder Copyright , MecSoft Corporation, 2

3 Introduction Preparing the part for Machining Create Tools Create Machining Operations Axis Engraving Post Processing Tutorial 13: Machining a Ring Introduction Preparing the part for Machining Create Tools Create Machining Operations th axis Roughing th Axis Roughing operation # th axis Finishing Post Processing Tutorial 14: Pocketing and Drilling on a Ring Introduction Preparing the part for Machining Create Tools Create Machining Operations Axis Drilling axis Pocketing Post Processing Copyright , MecSoft Corporation, 3

4 Welcome to VisualMILL Getting Started Guide Welcome to VisualMILL and thank you for choosing one of most powerful and easy to use complete CAD/CAM packages on the market today. VisualMILL is a unique CAM product plug-in that runs inside of VisualCAM. Plug-ins can be considered as independent applications that can be loaded and unloaded on demand from the host program, which in this case is VisualCAM. This fully integrated VisualMILL plug-in seamlessly integrates VisualCAM s CAD functionality with toolpath generation and cutting simulation/verification, in one package that is both easy and fun to use. You can work with the native VisualCAM design data as well as use any of the data types that can be imported into VisualCAM such as solids, surfaces and meshes. Then you can use VisualMILL with its wide selection of tools and toolpath strategies to create machining operations and associated toolpaths. These toolpaths can then be simulated and verified, and finally post-processed to the controller of your choice. About this Guide Welcome to the VisualMILL getting started guide. This file contains various tutorials to help you get started with learning VisualMILL. Each tutorial lesson has two associated VisualCAM files that you can find located in the Tutorials folder under the installation folder of VisualMILL. The first file is a completed file that contains all of the completed toolpaths and machining operations and represents the file that you should end up with after working through the tutorial. The other file is a starter file that contains only the geometry. Use the completed file as a reference. Copy the starter file and use this file to begin each tutorial. Good luck and have fun! Where to go for more help Apart from the on-line help system you can download tutorials and projects from MecSoft Corporation's web site at This will help you get started with using VisualMILL. If you need additional help, or if you have any questions regarding VisualMILL, you may contact us via at support@mecsoft.com MecSoft offers Online training as well as personalized full day training sessions. Please look up our website or us at sales@mecsoft.com for further details Please do continue to visit our home page to learn about the latest updates to VisualMILL and any other help material. Copyright , MecSoft Corporation, 4

5 Tutorial 1: Machining a Gasket Copyright , MecSoft Corporation, 5

6 Introduction This tutorial will illustrate machining of a simple prismatic part such as this gasket using 2-1/2 milling operations. Even though we have created a 3-D representation of the gasket, it will be seen later on that we can machine this using just 2-D curves. The reason we are able to do this is because of the prismatic nature of this model. The stepped instructions are accompanied by explanatory and introductory text. Reading this text will help you understand the tutorial methodology and provide information about additional options available. Don t forget to save your work periodically! You may want to save the file under a different name so that the original file will be preserved. Strategy to Machine the Gasket We will machine the Gasket by using a 2-½ axis machining operation called Profiling. The part will be machined out of a 8 ½ x 5 x ¼ inch poplar wood sheet using a ½ inch Flat End Mill. The wooden sheet will be held to the machine table or the spoil sheet on the table using double-sided tape. Main Programming Steps In creating programs for each setup, the following steps will be followed: Create the Stock geometry Set the Machine zero point or Locate geometry with respect to the machine coordinates Create / Select the tool used for machining Set the feeds and speeds Set the clearance plane for the non-cutting transfer moves of the cutter Select the machining regions for containing the cutter to specific areas to cut Select the machining operations and set the parameters Generate the toolpath Simulate the toolpath. You may have to repeat either all or part of these steps for subsequent operations. Preparing the part for Machining Loading the Part Model Part refers to the geometry that represents the final manufactured product. You can create parts within VisualMILL, but it is more typical to import geometry created in another CAD system. To load a part: Copyright , MecSoft Corporation, 6

7 1. Select File / Open from the Menu, or click the Open icon from the Standard bar. 2. From the Open dialog box, select the Gasket.vcp file from the Tutorials folder in the VisualMILL 6.0 installation folder. (C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMILL 6.0\Tutorials) The imported part appears as shown below Note: You can import solid models, Stereo-Lithography (both ASCII and binary) format files. Surfaces can be imported from IGES, STEP or Rhino 3DM. Faceted (triangulated) models can be imported from VRML, Raw Triangle, DXF / DWG facet data, or Rhino Mesh. Non-faceted geometry, once imported, is immediately converted and stored as triangulated data. Imported geometry is stored internally as a VisualCAM part file. This allows for much faster part loading time. Copyright , MecSoft Corporation, 7

8 Setup Tab 1. Go to the VisualMILL- MOps browser and click on the Setup tab 2. Select Machine Setup from the setup tab. 3. Set the Machine type to 3 axis Copyright , MecSoft Corporation, 8

9 4. Select Post from the setup tab to specify the post processor options 5. Set the current post processor that is on your controller. We will select Haas as the post processor for this exercise. Set the posted file extension type to.nc Note: By default post processor files are located under C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMill 6.0\Posts Copyright , MecSoft Corporation, 9

10 The program to send the posted output is set to notepad. This would output the G code to a notepad. Create Stock Geometry 1. Select Create/Load stock from the setup tab and create a Box Stock 2. This brings up the Box Stock parameters. Set the Length (L) = 8.50, Width W = 5.00 and Height (H) = Leave the other parameters as default and Click OK. Copyright , MecSoft Corporation, 10

11 3. The stock geometry is now created, and a semi-transparent stock box is displayed on top of the part geometry. 4. The setup tab now displays the following information: Machine Type, Post Processor, and Stock type as show below. Copyright , MecSoft Corporation, 11

12 Locate Machine Zero The steps below help you determine the machine home (also know as machine zero or tool touch off point) for the part/stock geometry. 1. Select Locate WCS from the Setup tab 2. Under Set WCS Origin, choose Set to Stock Box, the Zero Face to Highest Z, and Zero Position to South West corner. This sets the machine home to the top of the stock material and the southwest corner of the part geometry. Copyright , MecSoft Corporation, 12

13 Note: You can change the stock model transparency under standard mode by selecting Simulation Preferences that is located at the bottom of the MOps browser. Copyright , MecSoft Corporation, 13

14 Align Part and Stock In this process, we can align the part and the stock geometry. As we have set the Machine zero to the Stock Box, we will now move the part relative to the stock. 1. Select Align Part and Stock from the Setup tab 2. Set to Object to Move as Move Part, Z alignment to Top and XY alignment to Center Copyright , MecSoft Corporation, 14

15 The part geometry is aligned to the center of stock in XY and top in Z. Click Save to save the work and specify a file name as Gasket-Rev1. The file is now saved with extension vcp. (VisualCAM Part File) Create Tools To machine the above part we will now create a ½ inch (0.5 ) Flat End Mill. 1. Go to the VisualMILL-Tools browser that is located below the VisualMILL- MOps browser and select Create/Edit Tools. Select the Tool Type to Flat End Mill. 2. Set the tool name as FlatMill-0.5, Tool Diameter = 0.5, Under the Properties tab set Tool Number = 1. Copyright , MecSoft Corporation, 15

16 Setting Feeds and Speeds You can assign Feeds & Speeds to a tool or you can load from a table. In this exercise, we will assign feeds and speeds to the tool. 3. Switch to the Feeds & Speeds tab inside the create/select tool dialog. 4. Use the following settings for feeds and speeds. 5. Click Save as New Tool. The tool is now created and listed under Tools in Library. Click OK to close the dialog. Note: You can edit the tool properties and click Save Edits to Tool to save the changes. You can create additional tools by assigning a different name and specify the tool parameters. The created tools are now listed under the VisualMILL-Tools browser. Copyright , MecSoft Corporation, 16

17 Create/Extract Regions In order to machine the Gasket, we need to extract the curves from the 3d model to select them as machining regions. 1. Select the Layer Manager from the Standard bar. 2. The layer manager is now open. Set the Layer01 as the active layer. 3. Close the Layer Manager. 4. From the Curves tab on the Geometry Bar to your right, select Single Flat Area Regions. 5. The command bar will now prompt the user to select a flat area to extract the curves. Copyright , MecSoft Corporation, 17

18 6. Select the top face (surface) on the Gasket. A selection list will display the geometries that can be selected. Browsing through the selection tree will highlight the surface that corresponds to the selection. 7. The curves are now created and displayed in red on the part geometry. Copyright , MecSoft Corporation, 18

19 Note: You can toggle the stock model display by selecting Stock Visibility that is located at the bottom of the VisualMill-MOps Browser Create Machining Operations In this process we will create a 2.5 axis profiling operation. 1. Switch to the Create Operations tab in VisualMILL-Mops browser. 2 ½ Axis Profiling 1. Select 2.5 Axis Mill and choose Profiling This brings up the 2 ½ Axis Profiling Operations dialog. We will go over the steps for creating the profile operations for the inner features of the Gasket. Copyright , MecSoft Corporation, 19

20 Select Machining Features/Regions 2. Go to the Machining Features/ Regions tab and click Select Curves as Regions 3. Now select the 3 inner circles by using the left mouse click starting from left to right. Copyright , MecSoft Corporation, 20

21 4. Right mouse click or select enter from the keypad to complete the selection. 5. The selected regions are now displayed under Machining Regions Copyright , MecSoft Corporation, 21

22 Selecting the Tool 6. Switch to the Tools tab inside the 2 ½ Axis Profiling operation. 7. Select the FlatMill-0.5. The 0.5 Flat End mill is now selected as the active tool and the Tool parameters are displayed to the right of the Tools window. Copyright , MecSoft Corporation, 22

23 Set Feeds and Speeds 8. Click on the Feeds and Speeds tab. 9. Select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. Copyright , MecSoft Corporation, 23

24 Clearance Control 10. Switch to Clearance Tab. 11. Set the Clearance Plane Definition to Automatic and Cut Transfer Method to Clearance Plane. VisualMILL will determine a safe Z height for the Entry & Exit when set to automatic. Setting Cut Transfer to Clearance Plane would apply the automatic Z clearance between transfers when the tool moves from a machining region to another. Copyright , MecSoft Corporation, 24

25 Specifying Cut Parameters 12. Switch to Cut Parameters tab 13. Set the Stock = 0 and under cut start Side check Use Outside/Inside for Closed Curves and select Inside. Alternatively you can also use Determine using 3D model. 14. Select the Cut Levels Tab and specify the Total Cut Depth = The cut depth is always set as an absolute value. Copyright , MecSoft Corporation, 25

26 Copyright , MecSoft Corporation, 26

27 Entry/Exit 15. Switch to Entry/Exit Tab and Set the Entry and Exit Type to None. 16. Click Generate. The 2½ Axis Profile toolpath is now generated and the Operation is listed under the VisualMILL-MOps browser. Note: Toolpath display can be turned on/off by selecting Toolpath Visibility under the MOps browser. Copyright , MecSoft Corporation, 27

28 Copyright , MecSoft Corporation, 28

29 Simulate Toolpath The generated toolpath can now be simulated. 1. Switch to the Simulate tab in the VisualMILL-MOps browser. 2. Select the 2 ½ Axis Profiling Operation and click to Simulate. 3. The simulated part is as shown below. Note: You can adjust the simulation speed by selecting Simulation Preferences that is located to the bottom right corner of the VisualMILL-MOps browser. Copyright , MecSoft Corporation, 29

30 To exit the Simulation mode, pause the Simulation and click Exit Simulation. This switches back to the Create Operations tab. Creating a 2 ½ Axis Profile for the Outer Region 1. Switch to the Create Operation tab. 2. Select Profiling from the 2 ½ Axis operations menu. 3. Under Machining Features/ Regions, select Remove All. 4. Now click on Select Curves as Regions and select the Outer profile of the Gasket as the region. 5. Right mouse click to complete the selection. 6. Switch to Tools tab and select FlatMill-0.5 as the active tool. Copyright , MecSoft Corporation, 30

31 7. Under Feeds/Speeds select Load from Tool. 8. Set the Clearance control to Automatic. 9. Switch to Cut Parameters tab, check Use Outside/Inside for Closed Curves, and set the Cut Start Side to Outside 10. Go over to Cut Levels and set the Total Cut Depth = Click Generate to Create the 2 ½ Axis Profile Toolpath. 12. The 2 ½ Axis Profile Operation is now created and is listed in the MOps Browser. Copyright , MecSoft Corporation, 31

32 13. Switch to Simulate Tab, select 2 ½ Axis Profiling, and click to simulate toolpath. Copyright , MecSoft Corporation, 32

33 Reports 1. Switch to Create Operations Tab. 2. Select the MOp Set1 and right click and select Information. This provides the estimated machining time for the operations created under MOp Set1. Note: You can also go over to Machining Operations and right click and select information determine the estimated machining time for all the MOp Sets. Copyright , MecSoft Corporation, 33

34 Shop Docs Shop documentation can be generated selecting Machining Operations under the Create Operations tab. Right mouse click and Shop Documentation. User can select from one of the 2 templates and generate shop documentation. This is saved as an html file and can be printed and handed over to the operator in preparation for the part to be machined on the CNC. Copyright , MecSoft Corporation, 34

35 Post Processing 1. Select Machining Operations from the Create Operations tab and right click and select post process. 2. Specify the File Name as Gasket.nc and click Save. The post by default is set to Haas as specified under the Post processor setup. You can change the post processor by selecting a different one from the drop down menu Copyright , MecSoft Corporation, 35

36 in the list. The posted g code by default will be saved to the folder where the part file is located. End of Tutorial 1! Copyright , MecSoft Corporation, 36

37 Tutorial 2: Machining a Slotted Gear Copyright , MecSoft Corporation, 37

38 Introduction This tutorial will introduce the usage of 2 ½ axis profiling and Engraving Machining Operations of VisualMill. We will be using the Gear.vcp part file. It should be noted that, even though the part file contains a 3-D geometry representing the part, we could machine this entirely by using just 2-D curves due to the prismatic nature of this model. The stepped instructions are accompanied by explanatory and introductory text. Reading this text will help you understand the tutorial methodology and provide information about additional options available. However, if you prefer to work straight through the steps without any additional reading, look for the following symbol: Don t forget to save your work periodically! You may want to save the file under a different name so that the original file will be preserved. Strategy to Machine the Slotted Gear We will machine the gear completely using 2 ½ axis-machining operations. We will use the Profiling operation to cut the outer shape of the gear and the Engraving operation to cut the slots. The engraving option is preferred in situations where the cutter can be driven to create a slot that conforms to the shape of the tool trajectory. This is because of the computational efficiency as well as the accuracy of this method. The part itself will be machined out of a 3 inch x 3 inch x ½ inch poplar wood sheet. The wooden sheet will be held to the machine table or the spoil sheet on the table using double-sided tape. The part will be machined using a single ¼ inch flat end mill. Main Programming Steps In creating programs for each setup, the following steps will be followed: Create the Stock geometry Set the Machine zero point or Locate geometry with respect to the machine coordinates Create / Select the tool used for machining Set the feeds and speeds Set the clearance plane for the non-cutting transfer moves of the cutter Select the machining regions for containing the cutter to specific areas to cut Select the machining operations and set the parameters Generate the toolpath Simulate the toolpath. You may have to repeat either all or part of these steps for subsequent operations. Copyright , MecSoft Corporation, 38

39 Preparing the part for Machining Loading the Part Model Part refers to the geometry that represents the final manufactured product. You can create parts within VisualMILL, but it is more typical to import geometry created in another CAD system. To load a part: 1. Select File / Open from the Menu, or click the Open icon from the Standard bar. 2. From the Open dialog box, select the Gear.vcp file from the Tutorials folder in the VisualMILL 6.0 installation folder. (C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMILL 6.0\Tutorials) The imported part appears as shown below. Copyright , MecSoft Corporation, 39

40 Setup Tab 1. Go to the VisualMILL- MOps browser and click on the Setup tab. 2. Select Machine Setup from the setup tab. 3. Set the Machine type to 3 axis. Copyright , MecSoft Corporation, 40

41 4. Select Post from the setup tab to specify the post processor options. 5. Set the current post processor that is on your controller. We will select Haas as the post processor for this exercise. Note: By default post processor files are located under C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMill 6.0\Posts Copyright , MecSoft Corporation, 41

42 The program to send the posted output is set to notepad. This would output the G code to a notepad. Create Stock Geometry 1. Select Create/Load stock from the setup tab and create a Box Stock. 2. This brings up the Box Stock parameters. Set the Length (L) = 3.00, Width W = 3.00, and Height (H) = Leave the other parameters as default, and click OK. Copyright , MecSoft Corporation, 42

43 3. The stock geometry is now created, and a semi-transparent stock box is displayed on top of the part geometry. 4. The setup tab now displays the following information: Machine Type, Post Processor, and Stock type as show below. Copyright , MecSoft Corporation, 43

44 Locate Machine Zero The steps below help you determine the machine home (also know as machine zero or tool touch off point) for the part/stock geometry. 1. Select Locate WCS from the Setup tab. 2. Under Set WCS Origin, choose Set to Stock Box, the Zero Face to Highest Z, and Zero Position to South West corner. This sets the machine home to the top of the stock material and the southwest corner of the part geometry. Copyright , MecSoft Corporation, 44

45 Note: You can change the stock model transparency under standard mode by selecting Simulation Preferences that is located at the bottom of the MOps browser. Copyright , MecSoft Corporation, 45

46 Create Tools To machine the above part we will now create a ¼ inch (0.25 ) Flat End Mill. 1. Go to the VisualMILL-Tools browser that is located below the VisualMILL-MOps browser and select Create/Edit Tools. Select the Tool Type to Flat End Mill. 2. Set the tool name as FlatMill-0.25, Tool Diameter = Under the Properties tab, set Tool Number = 1. Copyright , MecSoft Corporation, 46

47 Setting Feeds and Speeds You can assign Feeds & Speeds to a tool or you can load from a table. In this exercise we will assign feeds and speeds to the tool. 3. Switch to the Feeds & Speeds tab inside the create/select tool dialog. 4. Use the following settings for feeds and speeds. 5. Click Save as New Tool. The tool is now created and listed under Tools in Library. Click OK to close the dialog. Note: You can edit the tool properties and click Save Edits to Tool to save the changes. You can create additional tools by assigning a different name and specify the tool parameters. The created tools are now listed under the VisualMILL-Tools browser. Copyright , MecSoft Corporation, 47

48 Create Regions for Machining In the steps below we will extract regions from the 3D model and create curves for engraving. 1. Turn off stock model visibility from the VisualMILL-MOps browser. 2. Select the Layer Manager from the Standard bar. 3. The layer manager is now open. Set Layer 01 as the active layer. 4. Close the Layer Manager. 5. From the Curves tab on the Geometry Bar to your right, select Single Flat Area Regions. 6. The command bar will now prompt the user to select a flat area to extract the curves. 7. Select the top face (surface) of the part geometry. A selection list will display the geometries that can be selected. Browsing through the selection tree will highlight the surface that corresponds to the selection. The flat area curves are created and displayed on top of the part geometry. Copyright , MecSoft Corporation, 48

49 8. Switch to the Top view and create a circle using Center and Radius. 9. Select Circles & Arcs from the Geometry Bar and pick Circle Center & Radius. 10. Specify 1.5,1.5 as the center coordinates and hit the enter key. 11. Specify 0.99 as the radius of the circle and hit the enter key We will now create lines, which can be selected for engraving the slots on the gear. 12. Turn on the Mid Point and Quad Point snap from the status bar and turn off the other snaps. Copyright , MecSoft Corporation, 49

50 13. Switch to the Top view and select Lines from the Geometry Bar and pick Create Line. 14. For the first coordinate, snap to the quad point on the circle as show below. 15. For the second coordinate, snap to the center of the arc as shown below. A line is now created at the center of the slot. We will now array the line across other slots on the gear. Copyright , MecSoft Corporation, 50

51 16. Select the Line, go to the menu at the top, and select Transform -> Polar Array. 17. Use the following settings. Rotate about X = 1.5, Y = 1.5, Z = 0, Angle to Fill = 360, and Number of Copies = The lines created and shown below. Copyright , MecSoft Corporation, 51

52 We have now created the regions for machining. Turn on the Stock Model Visibility and save the file. Copyright , MecSoft Corporation, 52

53 Create Machining Operations In this process we will create a 2.5 axis profiling operation. 1. Switch to the Create Operations tab in VisualMILL-Mops browser. 2 ½ Axis Profiling 2. Select 2.5 Axis Mill and choose Profiling. This brings up the 2 ½ Axis Profiling Operations dialog. We will go over the steps for creating the profile operations. Copyright , MecSoft Corporation, 53

54 Select Machining Features/Regions 3. Go to the Machining Features/ Regions tab and click Select Curves as Regions 4. Now select the inner circle first by using the left mouse click and then the outer circle. Copyright , MecSoft Corporation, 54

55 5. Right mouse click or select enter from the keypad to complete the selection. 6. The selected regions are now displayed under Machining Regions. Copyright , MecSoft Corporation, 55

56 Selecting the Tool 7. Switch to the Tools tab inside the 2 ½ Axis Profiling operation. 8. Select the FlatMill The 0.25 Flat End mill is now selected as the active tool, and the Tool parameters are displayed to the right of the Tools window. Copyright , MecSoft Corporation, 56

57 Set Feeds and Speeds 9. Click on the Feeds and Speeds tab. 10. Select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. Copyright , MecSoft Corporation, 57

58 Clearance Control 11. Switch to Clearance Tab. 12. Set the Clearance Plane Definition to Automatic and Cut Transfer Method to Clearance Plane. VisualMILL will determine a safe Z height for the Entry & Exit when set to automatic. Setting Cut Transfer to Clearance Plane would apply the automatic Z clearance between transfers when the tool moves from a machining region to another. Copyright , MecSoft Corporation, 58

59 Specifying Cut Parameters 13. Switch to Cut Parameters tab. 14. Set the Stock = 0, cut start Side as Right. Copyright , MecSoft Corporation, 59

60 15. Select the Cut Levels Tab and specify the Total Cut Depth = 0.25, Rough Depth/Cut = This would cut the profile in 2 cuts of each Make sure the cut level ordering is set to Depth First. This would profile the inner circle and then the outer profile. Copyright , MecSoft Corporation, 60

61 Entry/Exit 16. Switch to Entry/Exit Tab, and Set the Entry and Exit Type to None. Copyright , MecSoft Corporation, 61

62 17. Click Generate. The 2½ Axis Profile toolpath is now generated, and the Operation is listed under the VisualMILL-MOps browser. Toolpath display can be turned on/off by selecting Toolpath Visibility under the MOps browser. Copyright , MecSoft Corporation, 62

63 Simulate Toolpath The generated toolpath can now be simulated. 1. Switch to the Simulate tab in the VisualMILL-MOps browser. 2. Select the 2 ½ Axis Profiling Operation and click to Simulate. Copyright , MecSoft Corporation, 63

64 3. The simulated part is as shown below. Note: You can adjust the simulation speed by selecting Simulation Preferences that is located to the bottom right corner of the VisualMILL-MOps browser. Copyright , MecSoft Corporation, 64

65 To exit the Simulation mode, pause the Simulation, and click Exit Simulation. This switches back to the Create Operations tab. Creating an Engraving Operation Now we will use engraving operation to cut the slots of the gear by driving the 0.25 inch tool in the slot. As already mentioned, the most efficient way of machining slots is to use the Engraving option and drive the cutter along the center of the slot. 1. Switch to the Create Operation tab. 2. Select Engraving from the 2 ½ Axis operations menu. Copyright , MecSoft Corporation, 65

66 Select Machining Regions 3. Under Machining Features/ Regions click on Remove All to deselect any regions that could have been selected from the previous machining operation. 4. Now click on Select Curves as Regions and select the 6 lines on the slotted gear as shown below. Copyright , MecSoft Corporation, 66

67 5. Right mouse click to complete the selection. 6. The 6 selected regions are listed under the Machining Features/Regions Select Tool 7. Switch to Tools tab and select FlatMill-0.25 as the active tool. 8. Under Feeds/Speeds, select Load from Tool. 9. Set the Clearance control to Automatic. Specify Engraving Cut Parameters 10. Switch to Cut Parameters tab. Under Cut Depth Control, set the Total Cut Depth = 0.25, Rough Depth = 0.25, and Rough Depth/Cut = Copyright , MecSoft Corporation, 67

68 11. Click Generate to Create the Engraving Toolpath. 12. The Engraving Operation is now created and is listed in the MOps Browser. Copyright , MecSoft Corporation, 68

69 Copyright , MecSoft Corporation, 69

70 Simulate Toolpath 13. Switch to Simulate Tab, select Engraving, and click to simulate toolpath. Copyright , MecSoft Corporation, 70

71 Post Processing 5. Select Machining Operations from the Create Operations tab, right click, and select post process. 6. Specify the File Name as Gear.nc and click Save. Copyright , MecSoft Corporation, 71

72 The post by default is set to Haas as specified under the Post processor setup. You can change the post processor by selecting a different one from the drop down menu in the list. The posted g code by default will be saved to the folder where the part file is located. End of Tutorial 2! Copyright , MecSoft Corporation, 72

73 Tutorial 3: Machining a Shaft Base Copyright , MecSoft Corporation, 73

74 Introduction This tutorial will illustrate machining of a prismatic part such as this Shaft Base using 2-1/2 milling operations. Even though we have created a 3-D representation of the part, it will be seen later on that we can machine this using just 2-D curves. The reason we are able to do this is because of the prismatic nature of this model. This tutorial will introduce the usage of 2 ½ axis machining for a simple one sided part. We will use profiling, pocketing and hole pocketing operations. The stepped instructions are accompanied by explanatory and introductory text. Reading this text will help you understand the tutorial methodology and provide information about additional options available. Don t forget to save your work periodically! You may want to save the file under a different name so that the original file will be preserved. Strategy to Machine the Shaft Base We will machine the shaft base completely using 2 ½ axis-machining operations. The starting material for the Shaft Base is soft wood and the size is 5.5 x 3.25 x 0.75 inches. The wooden sheet will be held to the machine table or the spoil sheet on the table using double-sided tape. The part will be machined using a single ¼ inch flat end mill. Determining the sequence of machining operations o As the part thickness is thick and the available stock is 0.75 the first operation would involve reducing the thickness of the stock over the entire area from 0.75 to To carry out this operation we will use the 2 ½ axis Facing Operation as the toolpath extends past the region. o The next step would involve machining the areas around and inside the boss. As the thickness of material to be removed is not the same for both the areas we would have to use 2 separate operations to clear the material. We will use 2 ½ axis Pocketing Operation which is ideal removing material inside a specified region. o We are now down to the level where the step holes need to be machined. As the holes are circular we will use 2 ½ axis Hole Pocketing operation to machine the holes to its depth in 2 separate operations. o The 2 inner holes can be drilled using an engraving operation to its depth. o Finally we will cut out the shape of the part from the rectangular using a contour toolpath. This is accomplished using a 2 ½ axis Profiling Operation which separates the finished part from the stock material. Main Programming Steps In creating programs for each setup, the following steps will be followed: Create the Stock geometry Set the Machine zero point or Locate geometry with respect to the machine coordinates Create / Select the tool used for machining Copyright , MecSoft Corporation, 74

75 Set the feeds and speeds Set the clearance plane for the non-cutting transfer moves of the cutter Select the machining regions for containing the cutter to specific areas to cut Select the machining operations and set the parameters Generate the toolpath Simulate the toolpath. You may have to repeat either all or part of these steps for subsequent operations. Preparing the part for Machining Loading the Part Model Part refers to the geometry that represents the final manufactured product. You can create parts within VisualMILL, but it is more typical to import geometry created in another CAD system. To load a part: 1. Select File / Open from the Menu, or click the Open icon from the Standard bar. 2. From the Open dialog box, select the ShaftBase.vcp file from the Tutorials folder in the VisualMILL 6.0 installation folder. (C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMILL 6.0\Tutorials) The imported part appears as shown below Copyright , MecSoft Corporation, 75

76 Setup Tab 1. Go to the VisualMILL- MOps browser and click on the Setup tab. 2. Select Machine Setup from the setup tab. 3. Set the Machine type to 3 axis. Copyright , MecSoft Corporation, 76

77 4. Select Post from the setup tab to specify the post processor options. 5. Set the current post processor that is on your controller. We will select Haas as the post processor for this exercise. Note: By default post processor files are located under C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMill 6.0\Posts The program to send the posted output is set to notepad. This would output the G code to a notepad. Copyright , MecSoft Corporation, 77

78 Create Stock Geometry 1. Select Create/Load stock from the setup tab and create a Box Stock. 2. This brings up the Box Stock parameters. Set the Length (L) = 5.50, Width W = 3.25, and Height (H) = Leave the other parameters as default, and click OK. Copyright , MecSoft Corporation, 78

79 3. The stock geometry is now created, and a semi-transparent stock box is displayed on top of the part geometry. Copyright , MecSoft Corporation, 79

80 4. The setup tab now displays the following information: Machine Type, Post Processor, and Stock type as show below. Locate Machine Zero 1. The steps below help you determine the machine home (also know as machine zero or tool touch off point) for the part/stock geometry. 2. Select Locate WCS from the Setup tab. 3. Under Set WCS Origin, choose Set to Stock Box, the Zero Face to Highest Z, and Zero Position to South West corner. This sets the machine home to the top of the stock material and the southwest corner of the part geometry. Copyright , MecSoft Corporation, 80

81 Note: You can change the stock model transparency under standard mode by selecting Simulation Preferences that is located at the bottom of the MOps browser. Copyright , MecSoft Corporation, 81

82 Align Part and Stock During this step, we will align the part inside the stock geometry. 1. Select Align Part and Stock from the Setup tab. In this step, we will position the part to the bottom of the stock and center in XY. 2. Use the following settings - Object to Move: Move Part, Z alignment: Bottom and XY Alignment: Center. 3. The part is now aligned inside the stock as shown below. Copyright , MecSoft Corporation, 82

83 Front View Top View Copyright , MecSoft Corporation, 83

84 Create Tools To machine the above part we will now create a ¼ inch (0.25 ) Flat End Mill. 1. Go to the VisualMILL-Tools browser that is located below the VisualMILL- MOps browser and select Create/Edit Tools. Select the Tool Type to Flat End Mill. 2. Set the tool name as FlatMill-0.25 and Tool Diameter = Under the Properties tab, set Tool Number = 1. Copyright , MecSoft Corporation, 84

85 Setting Feeds and Speeds You can assign Feeds & Speeds to a tool or you can load from a table. In this exercise, we will assign feeds and speeds to the tool. 3. Switch to the Feeds & Speeds tab inside the create/select tool dialog. 4. Use the following settings for feeds and speeds. 5. Click Save as New Tool. The tool is now created and listed under Tools in Library. Click OK to close the dialog. Note: You can edit the tool properties and click Save Edits to Tool to save the changes. You can create additional tools by assigning a different name and specify the tool parameters. The created tools are now listed under the VisualMILL-Tools browser. Copyright , MecSoft Corporation, 85

86 Create Machining Operations We will machine the Shaft Base using 4 different machining operations Facing, Pocketing, Hole Pocketing and Engraving. The stock geometry has a thickness of 0.75 and the finished part is We will create a 2.5 axis facing operation to mill the thickness of material from the stock geometry. 1. Switch to the Create Operations tab in VisualMILL-Mops browser. 2 ½ Axis Facing 1. Select 2.5 Axis Milling and choose Facing. 2. This brings up the 2 ½ Axis Facing Operation Dialog. We will now go over the steps for creating the toolpath. Copyright , MecSoft Corporation, 86

87 Select Machining Features/Regions 1. Go to the Machining Features/ Regions tab and click Select Curves as Regions. 2. Select the Rectangle and right mouse click to complete the selection. Region1 is now listed under Machining Features/Regions. 3. Switch to the Tools tab inside the 2 ½ Axis Facing operation and select FlatMill Click on the Feeds and Speeds tab and select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. 5. Switch to the Clearance Tab and set the Clearance Plane Definition to Automatic and Cut Transfer Method to Clearance Plane. Copyright , MecSoft Corporation, 87

88 Specify Cut Parameters 1. Click on the Roughing tab. 2. Set the Tolerance to 0.01, Stock to leave to 0, Cut Pattern to Island Offset Cuts, and Step Distance to 50 (% Tool Diameter). 3. Switch to the Cut Levels Tab. Copyright , MecSoft Corporation, 88

89 4. Use the Following Settings. a. Pick Top = 0 (As the selected region at Z = , we would need to start the first cut from Z =0). b. Total Cut Depth = 0.125, Rough Depth = 0.125, and Rough Depth/Cut = Switch to the Entry/Exit tab and set the Entry and Exit parameters to none. 6. Click Generate. The 2½ Axis Facing toolpath is now generated, and the Operation is listed under the VisualMILL-MOps browser. Copyright , MecSoft Corporation, 89

90 7. Switch to Simulate tab, Select 2 ½ Axis Facing, and click Simulate to run the simulation. Copyright , MecSoft Corporation, 90

91 2 ½ Axis Pocketing We will now use 2½ axis Pocketing operation to machine the area inside the boss. Preparing the part for Pocketing In Preparation for the pocketing Operation, we will now create regions by extracting curves from the 3D model. 1. Turn off the Stock Model and Toolpath Visibility from the VisualMILL-MOps browser. 2. Open Layer Manager and Select Layer 01 as the Active Layer. 3. Click on the Geometry Bar and select the Curves Tab. Select Single Flat Area Region. Copyright , MecSoft Corporation, 91

92 4. The command bar would now prompt the user to select a flat area to extract the curves 5. Pick the flat area as shown below. 6. Flat area curves are created and are on Layer 01. We are now ready to create the pocketing operation for the inner region. 7. Switch to the Create Operations tab. Copyright , MecSoft Corporation, 92

93 Creating the Pocketing Operation #1 1. From the Create Operations tab, select 2½ axis Milling and Pocketing. This brings up the 2 ½ Axis Pocketing Operations dialog. We will go over the steps for creating the pocketing operation. 2. Go to the Machining Features/ Regions tab and click Select Curves as Regions. 3. Select the curve and right mouse click to complete the selection. Region1 is now listed under Machining Features/Regions. 4. Switch to the Tools tab inside the 2½ Axis Pocketing operation and select FlatMill Click on the Feeds and Speeds tab and select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. 6. Switch to the Clearance Tab and set the Clearance Plane Definition to Automatic and Cut Transfer Method to Clearance Plane. Copyright , MecSoft Corporation, 93

94 Specify Cut Parameters 1. Click on the Cut Parameters tab. 2. Set the Tolerance to 0.001, Stock to leave to 0, Cut Pattern to Offset Cuts, and Step over distance to 25 (% Tool Diameter). 3. Switch to the Cut Levels Tab. Copyright , MecSoft Corporation, 94

95 4. Use the Following Settings. a. Location of Cut Geometry at Bottom (As the selected region is at the bottom of the part, and we need to cut above it). We will determine the Total Cut Depth from the 3D model by snapping at 2 points. b. Select the Depth measuring tool located to the right of Total Cut Depth. This will minimize the Pocketing Operation parameters dialog. c. Turn on the End Point Snap from the Status bar. d. Pick the top of the boss as the start point and the bottom of the boss as the end point as shown below. e. The pocketing operation dialog shows up and determines Total Cut Depth = f. Set the Rough Depth = 0.25 and Rough Depth/Cut = Copyright , MecSoft Corporation, 95

96 This would machine the pocket in steps of 0.05 resulting in 5 cut levels. Note: You can also specify the Total Cut Depth by entering the depth values under Total Cut Depth. Copyright , MecSoft Corporation, 96

97 5. Switch to the Entry/Exit tab. 6. Use the following settings for Entry/Exit. Make sure to check Apply Entry/Exit at all cut levels. 7. Click Generate. The 2½ Axis Pocketing toolpath is now generated and the Operation is listed under the 2 ½ Axis Facing Operation in the VisualMILL- MOps browser. Note: You can rearrange the operations in the MOps browser by selecting the operation and dragging and dropping. Copyright , MecSoft Corporation, 97

98 8. Switch to Simulate tab, select 2 ½ Axis Pocketing, and click Simulate to run the simulation. Copyright , MecSoft Corporation, 98

99 Creating the Pocketing Operation #2 We will now create a 2 nd pocketing operation for machining the region around the boss. 1. Switch to the Create Operations tab. 2. Open Layer Manager and select Layer 01 as the active layer. 3. Click on the Geometry Bar and select the Curves Tab. Select Single Flat Area Region. 4. The command bar would now prompt the user to select a flat area to extract the curves. 5. Pick the flat area as shown below. Copyright , MecSoft Corporation, 99

100 Copying a MOp 1. Switch to the Create operations tab. 2. Select the 2 ½ axis Pocketing Operation created from the previous step, right mouse click, and select Copy. 3. Right click and select Paste. 4. This would create a copy of the 2 ½ axis Pocketing Operation listed below the first pocketing operation as show below. Copyright , MecSoft Corporation, 100

101 5. Expand the 2 ½ Axis Pocketing (1) folder and double click on Machining Features. Copyright , MecSoft Corporation, 101

102 6. Click Remove All under Machining Features and click Select Curves as Regions. 7. Select the rectangle and curve and right mouse click to complete the selection. 8. Region1 & Region2 are now listed under Machining Features/Regions. Click Save to Close the Machining Regions Dialog. 9. Double click under Parameters and switch to the Cut Levels Tab. 10. Use the Following Settings. a. Location of Cut Geometry Select Pick at Top = b. Total Cut Depth Set this to c. Set the Rough Depth = and Rough Depth /Cut = 0.05 d. Switch to the Entry/Exit tab and set the Retract Motion to Linear, Length = 0.1 and Angle = 0 e. Click Generate. Copyright , MecSoft Corporation, 102

103 11. The pocketing toolpath is now created and displayed in the MOps browser. Copyright , MecSoft Corporation, 103

104 12. Switch to Simulate tab, select 2 ½ Axis Pocketing (1), and click Simulate to run the simulation. Note: To turn on/off the toolpath and stock model visibilities use the controls located at the bottom of the MOps Browser. Copyright , MecSoft Corporation, 104

105 Hole Pocketing Operation In order to machine the 6 holes, we will now use 2 ½ axis hole pocketing operation. Preparing the part for Machining 1. Open the Layer manager and Make Layer 03 as the active layer. 2. Click on the Geometry Bar and select the Curves Tab. Select Single Flat Area Region. 3. The command bar would now prompt the user to select a flat area to extract the curves 4. Pick the flat area as shown below. 5. Flat area curves are created and are on Layer 03. We are now ready to create the pocketing operation for the inner region. 6. Switch to the Create Operations tab. Creating the Hole Pocketing Operation #1 1. Select 2 ½ Axis Milling and Hole Pocketing. Copyright , MecSoft Corporation, 105

106 2. Go to the Machining Features/ Regions tab and click Select Curves as Regions. 3. Select the 6 circles and right mouse click to complete the selection. Regions 1 to 6 are now listed under Machining Features/Regions. 4. Switch to the Tools tab inside the Hole Pocketing operation and select FlatMill Click on the Feeds and Speeds tab and select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. 6. Switch to the Clearance Tab and set the Clearance Plane Definition to Automatic and Cut Transfer Method to Clearance Plane. Specify Cut Parameters 7. Click on the Cut Parameters tab. 8. Use the following Settings a. Tolerance to 0.001, b. Hole Depth (H) =0.0625, Uncheck Use 3D model to Detect Depth, c. Hole Diameter (D) = 0.5, d. Step over distance = 25 (% Tool Diameter), e. Step Down Control (dz) = 50 (% Tool Diameter), f. Cut Direction = Climb (Down Cutting). Copyright , MecSoft Corporation, 106

107 9. Switch to the Entry Exit Tab and set the Helix Diameter = Copyright , MecSoft Corporation, 107

108 10. Click Generate. The Hole Pocketing operation is now created and is listed under the MOps browser. 11. Switch to the Simulate tab, select Hole Pocketing, and click Simulate to run the simulation. 12. The simulated part is shown below. Copyright , MecSoft Corporation, 108

109 Copyright , MecSoft Corporation, 109

110 Creating the Hole Pocketing Operation #2 6. Switch to the Create Operations tab. 7. Open Layer Manager and select Layer 04 as the active layer. 8. Click on the Geometry Bar and select the Curves Tab. Select Single Flat Area Region. 9. The command bar would now prompt the user to select a flat area to extract the curves. 10. Pick the flat area as shown below. 11. Repeat the flat area region for the other 5 holes. The extracted curves are as shown below. Creating the Hole Pocketing Operation 12. Select the Hole Pocketing Operation created from the previous step, right mouse click, and select Copy. 13. Right click and select Paste. 14. This would create a copy of the Hole Pocketing Operation listed below the first Hole Pocketing operation as show below. Copyright , MecSoft Corporation, 110

111 15. Expand the Hole Pocketing (1) folder and double click on Machining Features. 16. Click Remove All under Machining Features and click Select Curves as Regions. 17. Select the 6 inner circles and right mouse click to complete the selection. 18. Regions 1 to 6 are now listed under Machining Features/Regions. Click Save to Close the Machining Regions Dialog. 19. Double Click under Parameters and set the Hole Depth = , Hole Diameter = Copyright , MecSoft Corporation, 111

112 20. Switch to the Entry/Exit tab and set the Helix Diameter to Click Generate. The Hole Pocketing Operation for the inner holes is now created. Copyright , MecSoft Corporation, 112

113 22. Switch to the Simulate tab, select Hole Pocketing(1), and click Simulate to run the simulation. Copyright , MecSoft Corporation, 113

114 Copyright , MecSoft Corporation, 114

115 2 ½ Axis Engraving Operation Now we will use engraving operation to drill the 2 holes. This can also be accomplished by using a drilling operation that is available under Hole Machining. Preparing the part for machining Turn on the Center Point Snap from the status bar and turn off the other snaps. 1. Click on the Geometry Bar and select the Points Tab. Select Create Point. 2. The command input bar will now prompt the user to pick or enter the coordinates for the point. We will now use the pick option by creating a point that snaps to the center of the circle as show below. 3. Repeat the above steps for the other circle. Copyright , MecSoft Corporation, 115

116 Creating the Engraving Toolpath 1. From the Create Operations tab, select 2 ½ Axis Milling and Engraving. 2. Go to the Machining Features/ Regions tab, click Remove All under Machining Features, and click Select Curves as Regions. 3. Select the 2 points as regions for engraving. Right click to complete the selection. 4. Switch to the Tools tab inside the Engraving operation and select FlatMill Click on the Feeds and Speeds tab and select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. 6. Switch to the Clearance Tab and set the Clearance Plane Definition to Automatic and Cut Transfer Method to Clearance Plane. 7. Switch to the Cut Parameters tab and use the following parameters - Tolerance = 0.001, Location of Cut Geometry At Top, Total Cut Depth = 0.375, Rough Depth = and Rough Depth/Cut = Set the Entry and Exit to None under the Entry/Exit tab. 9. Click Generate. The Engraving operation is now created. 10. Switch to Simulate tab, select Engraving, and click Simulate to run the simulation. Copyright , MecSoft Corporation, 116

117 Copyright , MecSoft Corporation, 117

118 2 ½ Axis Profiling 1. Switch to the Create Operations tab and select 2.5 Axis Milling and choose Profiling. 2. Go to the Machining Features/ Regions tab, click Remove All under Machining Features, and click Select Curves as Regions. 3. Select the outer curve. Right mouse click or select enter from the keypad to complete the selection. 4. The selected region is now displayed under Machining Features/Regions. 5. Switch to the Tools tab inside 2 ½ Axis Profiling operation and Select the FlatMill Click on the Feeds and Speeds tab. And select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. 7. Switch to Clearance Tab. Set the Clearance Plane Definition to Automatic and Cut Transfer Method to Clearance Plane. Copyright , MecSoft Corporation, 118

119 Specifying Cut Parameters 8. Switch to Cut Parameters tab and use the following Settings a. Tolerance = 0.001, b. Stock = 0, c. Cut Start Side- Check Use Outside/Inside for closed curves and pick Outside. Copyright , MecSoft Corporation, 119

120 9. Select the Cut Levels Tab and specify the Total Cut Depth = 0.25, Rough Depth/Cut = Switch to Entry/Exit Tab and Set the Entry and Exit Type to None. 11. Click Generate. The 2½ Axis Profile toolpath is now generated and the Operation is listed under the VisualMILL-MOps browser. Toolpath display can be turned on/off by selecting Toolpath Visibility under the MOps browser. Copyright , MecSoft Corporation, 120

121 12. Switch to the Simulate tab in the VisualMILL-MOps browser. Select the 2 ½ Axis Profiling Operation and click to Simulate. 13. The simulated part is as shown below. Copyright , MecSoft Corporation, 121

122 Note: You can adjust the simulation speed by selecting Simulation Preferences that is located to the bottom right corner of the VisualMILL-MOps browser. To exit the Simulation mode, pause the Simulation, and click Exit Simulation. Copyright , MecSoft Corporation, 122

123 Post Processing 1. Select Machining Operations from the Create Operations tab and right click and select post process. 2. Specify the File Name as Shaftbase.nc and click save. The post by default is set to Haas as specified under the Post processor setup. You can change the post processor by selecting a different one from the drop down menu in the list. The posted g code by default will be saved to the folder where the part file is located. End of Tutorial 3! Copyright , MecSoft Corporation, 123

124 Tutorial 4: Simple V-Carving Copyright , MecSoft Corporation, 124

125 Introduction This tutorial will illustrate machining a Sign using 2-1/2 axis-engraving operations. We can engrave the sign using 2-D curves. This tutorial will introduce the usage of 2- ½ axis simple V Carving using V bit. V carving refers to a cutting strategy employed by sign makers to create sharp corners. V carving is performed using a tapered bit or conical tool (as shown below) usually known in the industry as a V Bit. The V-bit is made to rise from the cutting depth to the top of the surface at the corners in such a way that the tapered sides of the cutter are always in contact with the corners. When the cutter finally reaches the top surface, only the bottom tip of the tool will be in contact with the corners, thereby creating clean and crisp cuts at the corners. The stepped instructions are accompanied by explanatory and introductory text. Reading this text will help you understand the tutorial methodology and provide information about additional options available. Don t forget to save your work periodically! You may want to save the file under a different name so that the original file will be preserved. Strategy to Machine the part V carving is performed using the 2 ½ axis Machining Operation. The part itself will be machined out of a inch x 4 inch x ½ inch poplar wood sheet The part would be machined using a single V-Groove bit. The wooden sheet will be held to the machine table or the spoil sheet on the table using double-sided tape. Main Programming Steps In creating programs for each setup, the following steps will be followed: Create the Stock geometry Set the Machine zero point or Locate geometry with respect to the machine coordinates Create / Select the tool used for machining Set the feeds and speeds Copyright , MecSoft Corporation, 125

126 Set the clearance plane for the non-cutting transfer moves of the cutter Select the machining regions for containing the cutter to specific areas to cut Select the machining operations and set the parameters Generate the toolpath Simulate the toolpath. You may have to repeat either all or part of these steps for subsequent operations. Preparing the part for Machining Loading the Part Model Part refers to the geometry that represents the final manufactured product. You can create parts within VisualMILL, but it is more typical to import geometry created in another CAD system. To load a part: 1. Select File / Open from the Menu, or click the Open icon from the Standard bar. 2. From the Open dialog box, select the V-Carve1.vcp file from the Tutorials folder in the VisualMILL 6.0 installation folder. (C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMILL 6.0\Tutorials) The imported part appears as shown below. Copyright , MecSoft Corporation, 126

127 Setup Tab 1. Go to the VisualMILL- MOps browser and click on the Setup tab. 2. Select Machine Setup from the setup tab. 3. Set the Machine type to 3 axis. Copyright , MecSoft Corporation, 127

128 4. Select Post from the setup tab to specify the post processor options. 5. Set the current post processor that is on your controller. We will select Haas as the post processor for this exercise. Note: By default post processor files are located under C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMill 6.0\Posts The program to send the posted output is set to notepad. This would output the G code to a notepad. Copyright , MecSoft Corporation, 128

129 Create Stock Geometry 1. Select Create/Load stock from the setup tab and create a Box Stock. 2. This brings up the Box Stock parameters. Set the Length (L) = 10.75, Width W = 4.00 and Height (H) = 0.5. Make sure to set the corner position to Southwest corner Top of Stock as shown below. Copyright , MecSoft Corporation, 129

130 3. The stock geometry is now created, and a semi-transparent stock box is displayed on top of the part geometry. 4. The setup tab now displays the following information: Machine Type, Post Processor, and Stock type as show below. Copyright , MecSoft Corporation, 130

131 Locate Machine Zero 1. The steps below help you determine the machine home (also know as machine zero or tool touch off point) for the part/stock geometry. 2. Select Locate WCS from the Setup tab. 3. Under Set WCS Origin, choose Set to Stock Box, the Zero Face to Highest Z, and Zero Position to South West corner. This sets the machine home to the top of the stock material and the southwest corner of the part geometry. Copyright , MecSoft Corporation, 131

132 Note: You can change the stock model transparency under standard mode by selecting Simulation Preferences that is located at the bottom of the MOps browser. Copyright , MecSoft Corporation, 132

133 Align Part and Stock In this process, we can align the part and the stock geometry. As we have set the Machine zero to the Stock Box, we will now move the part relative to the stock. 1. Select Align Part and Stock from the Setup tab. 2. Set to Object to Move as Move Part, Z alignment to Top, and XY alignment to Center. Copyright , MecSoft Corporation, 133

134 The part geometry is aligned to the center of stock in XY and top in Z. Click Save to save the work and specify a file name as VCarve-Rev1. The file is now saved with extension vcp. (VisualCAM Part File) Note: You can toggle the stock model display by selecting Stock Visibility that is located at the bottom of the VisualMill-MOps Browser Create Tools To machine the above part, we will now create a 60-degree Taper Tool. 1. Go to the VisualMILL-Tools browser that is located below the VisualMILL-MOps browser and select Create/Edit Tools. Select the Tool Type to VeeMill. 2. Set the tool name as VeeMill1, Taper Angle = 30, Flute Length = 0.4, Tool Length = 2. Under the Properties tab set Tool Number = 1. Copyright , MecSoft Corporation, 134

135 Note: Taper Angle represents the included angle for a taper tool. For example a 60- degree taper tool would have a included angle of 30 degrees. If you have a taper tool with a diameter select Chamfer Mill or Taper Mill under Create/Select Tool. Copyright , MecSoft Corporation, 135

136 Setting Feeds and Speeds You can assign Feeds & Speeds to a tool or you can load from a table. In this exercise we will assign feeds and speeds to the tool. 3. Switch to the Feeds & Speeds tab inside the create/select tool dialog. 4. Use the following settings for feeds and speeds. 5. Click Save as New Tool. The tool is now created and listed under Tools in Library. Click OK to close the dialog. Note: You can edit the tool properties and click Save Edits to Tool to save the changes. You can create additional tools by assigning a different name and specify the tool parameters. The created tools are now listed under the VisualMILL-Tools browser. Copyright , MecSoft Corporation, 136

137 Create Machining Operations In this process we will create a 2.5 axis operation. 1. Switch to the Create Operations tab in VisualMILL-Mops browser. V-Carving 2. Select 2.5 Axis Mill and choose V-Carving. This brings up the V-Carving Operations dialog. We will go over the steps for creating the toolpath. Copyright , MecSoft Corporation, 137

138 Select Machining Features/Regions 3. Go to the Machining Features/ Regions tab and click Select Curves as Regions. 4. Now, select the text by using the left mouse click, starting from left to right. Make sure to get the inner curves on the letters e and o. Each curve is separate (by curves, not by letters) and must be selected separately. Copyright , MecSoft Corporation, 138

139 5. Right mouse click or select enter from the keypad to complete the selection. 6. The selected regions are now displayed under Machining Regions. Copyright , MecSoft Corporation, 139

140 Selecting the Tool 7. Switch to the Tools tab inside the V-Carving operation. 8. Select VeeMill1. VeeMill1 is now selected as the active tool and the Tool parameters are displayed to the right of the Tools window. Copyright , MecSoft Corporation, 140

141 Set Feeds and Speeds 9. Click on the Feeds and Speeds tab. 10. Select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. Copyright , MecSoft Corporation, 141

142 Clearance Control 11. Switch to Clearance Tab. 12. Set the Clearance Plane Definition to Absolute Z Value = 0.25 and Cut Transfer Method to Clearance Plane. Setting Cut Transfer to Clearance Plane would apply the Absolute Z value clearance between transfers when the tool moves from a machining region to another. Copyright , MecSoft Corporation, 142

143 Specifying Cut Parameters 13. Switch to Cut Parameters tab. 14. Set the Tolerance = 0.001, Cut Side = Inside, Location of Cut Geometry = At Top, Total Cut Depth = 0.2, Rough Depth = 0.2 and Rough Depth/Cut = Click Generate. The V-Carving toolpath is now generated and the Operation is listed under the VisualMILL-MOps browser. Note: Toolpath display can be turned on/off by selecting Toolpath Visibility under the MOps browser. Copyright , MecSoft Corporation, 143

144 Copyright , MecSoft Corporation, 144

145 Simulate Toolpath The generated toolpath can now be simulated. 1. Switch to the Simulate tab in the VisualMILL-MOps browser. 2. Select the V-Carving Operation and click to Simulate. 3. The simulated part is as shown below. Note: You can adjust the simulation speed by selecting Simulation Preferences that is located to the bottom right corner of the VisualMILL-MOps browser. Copyright , MecSoft Corporation, 145

146 To exit the Simulation mode, pause the Simulation, and click Exit Simulation. This switches back to the Create Operations tab. Post Processing 1. Select Machining Operations from the Create Operations tab and right click and select post process. Copyright , MecSoft Corporation, 146

147 2. Specify the File Name as V-Carve.nc and click Save. The post by default is set to Haas as specified under the Post processor setup. You can change the post processor by selecting a different one from the drop down menu in the list. The posted g code by default will be saved to the folder where the part file is located. End of Tutorial 4! Copyright , MecSoft Corporation, 147

148 Tutorial 5: Embossing Copyright , MecSoft Corporation, 148

149 Introduction This tutorial will illustrate machining a Sign using 2-1/2 axis-engraving operations. We can engrave the sign using 2-D curves. This tutorial will introduce the usage of 2- ½ axis V Carve Roughing with a Flat End Mill and V Carving using V bit. V carving refers to a cutting strategy employed by sign makers to create sharp corners. V carving is performed using a tapered bit or conical tool (as shown below) usually known in the industry as a V Bit. The V-bit is made to rise from the cutting depth to the top of the surface at the corners in such a way that the tapered sides of the cutter are always in contact with the corners. When the cutter finally reaches the top surface, only the bottom tip of the tool will be in contact with the corners, thereby creating clean and crisp cuts at the corners. The stepped instructions are accompanied by explanatory and introductory text. Reading this text will help you understand the tutorial methodology and provide information about additional options available. Don t forget to save your work periodically! You may want to save the file under a different name so that the original file will be preserved. Strategy to Machine the part Embossing is performed using the 2 ½ axis Machining Operations. The part itself will be machined out of a 20 inch x 4 inch x 1 inch poplar wood sheet The part would be machined using a Flat End Mill and a V-Groove bit. The wooden sheet will be held to the machine table or the spoil sheet on the table using double-sided tape. Main Programming Steps In creating programs for each setup, the following steps will be followed: Create the Part Create the Stock geometry Set the Machine zero point or Locate geometry with respect to the machine coordinates Create / Select the tool used for machining Copyright , MecSoft Corporation, 149

150 Set the feeds and speeds Set the clearance plane for the non-cutting transfer moves of the cutter Select the machining regions for containing the cutter to specific areas to cut Select the machining operations and set the parameters Generate the toolpath Simulate the toolpath. You may have to repeat either all or part of these steps for subsequent operations. Preparing the part for Machining Creating the Part Model Part refers to the geometry that represents the final manufactured product. To create a part: 1. Select File / New from the Menu, or click the New icon from the Standard bar. This creates a new session of VisualCAM. 2. Switch to the Top View by double clicking on the Top View under the Viewport. 3. Create a rectangle by selecting the Create Rectangle tool that is located on the Geometry Bar under Lines. 4. Under the Command bar, specify the First Corner as 0,0. 5. Specify the Second Corner as 20,4. 6. Create a 2 nd rectangle with the First Corner as 0.25,0.25 and Second Corner as 19.75,3.75. Copyright , MecSoft Corporation, 150

151 Create Text geometry 7. From the Curves Tab under the Geometry Bar, select Create Text tool. 8. This brings up Text to Create Dialog. Use the Following Settings. 9. Text Size = 2.5, Uncheck Auto Kern, and use the slide bar to specify the kerning for the text as shown in the picture below. Use Text to Create = VisualCAM. Copyright , MecSoft Corporation, 151

152 10. Click Done once you have the above settings. 11. The text would now appear on the screen and would expect the user to specify the Start point of text. 12. Specify 0.75,0.75 as the start point under the command bar. The text is now created and displayed as shown below. 13. From the File Menu, select Save and save the file under the Tutorials Folder as Embossing1.vcp. 14. The part geometry is now created. We are now ready to generate toolpath to machine the part. We will now switch to the VisualMILL-MOps browser. Note: You can skip the above steps for creating the part geometry by loading Embossing.vcp file into VisualCAM. This is available under the Tutorials folder in VisualMILL 6.0 Copyright , MecSoft Corporation, 152

153 Setup Tab 1. Go to the VisualMILL- MOps browser and click on the Setup tab. 2. Select Machine Setup from the setup tab. 3. Set the Machine type to 3 axis. Copyright , MecSoft Corporation, 153

154 4. Select Post from the setup tab to specify the post processor options. 5. Set the current post processor that is on your controller. We will select Haas as the post processor for this exercise. Note: By default post processor files are located under C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMill 6.0\Posts The program to send the posted output is set to notepad. This would output the G code to a notepad. Copyright , MecSoft Corporation, 154

155 Create Stock Geometry 1. Select Create/Load stock from the setup tab and create a Box Stock. 2. This brings up the Box Stock parameters and set the Length (L) = 20.00, Width W = 4.00 and Height (H) = 1.0. Make sure to set the corner position to Southwest corner Top of Stock as shown below. Copyright , MecSoft Corporation, 155

156 3. The stock geometry is now created, and a semi-transparent stock box is displayed on top of the part geometry. 4. The setup tab now displays the following information: Machine Type, Post Processor and Stock type as show below. Copyright , MecSoft Corporation, 156

157 Locate Machine Zero 1. The steps below help you determine the machine home (also know as machine zero or tool touch off point) for the part/stock geometry. 2. Select Locate WCS from the Setup tab. 3. Under Set WCS Origin, choose Set to Stock Box, the Zero Face to Highest Z and Zero Position to South West corner. This sets the machine home to the top of the stock material and the southwest corner of the part geometry. Copyright , MecSoft Corporation, 157

158 Note: You can change the stock model transparency under standard mode by selecting Simulation Preferences that is located at the bottom of the MOps browser. Copyright , MecSoft Corporation, 158

159 Align Part and Stock In this process, we can align the part and the stock geometry. As we have set the Machine zero to the Stock Box, we will now move the part relative to the stock. 1. Select Align Part and Stock from the Setup tab. 2. Set to Object to Move as Move Part, Z alignment to Top, and XY alignment to Center. Copyright , MecSoft Corporation, 159

160 The part geometry is aligned to the center of stock in XY and top in Z. Click Save to save the work and specify a file name as Embossing-Rev1. The file is now saved with extension vcp. (VisualCAM Part File) Note: You can toggle the stock model display by selecting Stock Visibility that is located at the bottom of the VisualMill-MOps Browser Copyright , MecSoft Corporation, 160

161 Create Tools To machine the above part, we will now create a 1/8 th inch (0.125 ) Flat End Mill for the V Carve Roughing operation and a VeeMill for the V Carve (finishing) operation. 1. Go to the VisualMILL-Tools browser that is located below the VisualMILL-MOps browser and select Create/Edit Tools. Select the Tool Type to Flat End Mill. 2. Set the tool name as FlatMill and the Tool Diameter = Under the Properties tab, set Tool Number = 1. Copyright , MecSoft Corporation, 161

162 Setting Feeds and Speeds You can assign Feeds & Speeds to a tool or you can load from a table. In this exercise, we will assign feeds and speeds to the tool. 3. Switch to the Feeds & Speeds tab inside the create/select tool dialog. 4. Use the following settings for feeds and speeds. 5. Click Save as New Tool. The tool is now created and listed under Tools in Library. Click OK to close the dialog. Note: You can edit the tool properties and click Save Edits to Tool to save the changes. You can create additional tools by assigning a different name and specify the tool parameters. The created tools are now listed under the VisualMILL-Tools browser. Copyright , MecSoft Corporation, 162

163 6. Create a 2 nd tool of type VeeMill. 7. Set the tool name as VeeMill1, Taper Angle = 30, Flute Length = 0.4, and Tool Length = 2. Under the Properties tab, set Tool Number = 2. Note: Taper Angle represents the included angle for a taper tool. For example a 60- degree taper tool would have a included angle of 30 degrees. If you have a taper tool with a diameter select Chamfer Mill or Taper Mill under Create/Select Tool. Copyright , MecSoft Corporation, 163

164 8. Switch to the Feeds & Speeds tab inside the create/select tool dialog and use the following settings for Feeds/Speeds for the VeeMill1. 9. Click Save as New Tool. The tool is now created and listed under Tools in Library. Click OK to close the dialog. Copyright , MecSoft Corporation, 164

165 Create Machining Operations In this process, we will create two 2 ½ axis-machining operations. 1. Switch to the Create Operations tab in VisualMILL-Mops browser. V-Carving Roughing 2. Select 2.5 Axis Mill and choose V-Carve Roughing. This brings up the V-Carve Roughing dialog. We will go over the steps for creating the toolpath. Copyright , MecSoft Corporation, 165

166 Select Machining Features/Regions 3. Go to the Machining Features/ Regions tab and click Select Curves as Regions. 4. Now, select the inner rectangle and text by using the left mouse click, starting from left to right. Be sure to include the inner curves for the letters a and A as well as the dot of the i. Each curve is separate (by curves, not by letters) and must be selected separately. Copyright , MecSoft Corporation, 166

167 5. Right mouse click or select enter from the keypad to complete the selection. 6. The selected regions are now displayed under Machining Regions. Selecting the Tool 7. Switch to the Tools tab inside the V-Carve Roughing operation. 8. Select FlatMill FlatMill is now selected as the active tool and the Tool parameters are displayed to the right of the Tools window. Copyright , MecSoft Corporation, 167

168 Set Feeds and Speeds 9. Click on the Feeds and Speeds tab. 10. Select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. Copyright , MecSoft Corporation, 168

169 Clearance Control 11. Switch to Clearance Tab. 12. Set the Clearance Plane Definition to Absolute Z Value = 0.25 and Cut Transfer Method to Clearance Plane. Setting Cut Transfer to Clearance Plane would apply the Absolute Z value clearance between transfers when the tool moves from a machining region to another. Copyright , MecSoft Corporation, 169

170 Specifying Cut Parameters 13. Switch to Cut Parameters tab. 14. Set the Tolerance = 0.001, Stock = 0, V-Carving Finish Tool Taper Angle = 30, Cut Type = Offset, and Cut Direction = Mixed. Check the Corner Cleanup option. Note: V-Carve Finishing Tool Taper Angle represents the included angle of the Vbit that would be used after the V-Carve Roughing Operation. If you have a 60 degree V-Bit, the Taper Angle would be 30 degrees. Copyright , MecSoft Corporation, 170

171 15. Switch to the Cut Levels tab and use the following settings. 16. Specify Location of Cut Geometry = At Top, Total Cut Depth = 0.25, Rough Depth = 0.25, and Rough Depth/Cut = Click Generate. The V-Carving toolpath is now generated and the Operation is listed under the VisualMILL- MOps browser. Note: Toolpath display can be turned on/off by selecting Toolpath Visibility under the MOps browser. Copyright , MecSoft Corporation, 171

172 Copyright , MecSoft Corporation, 172

173 Simulate Toolpath The generated toolpath can now be simulated. 1. Switch to the Simulate tab in the VisualMILL-MOps browser. 2. Select the V-Carving Operation and click to Simulate. 3. The simulated part is as shown below. Note: You can adjust the simulation speed by selecting Simulation Preferences that is located to the bottom right corner of the VisualMILL-MOps browser. Copyright , MecSoft Corporation, 173

174 To exit the Simulation mode, pause the Simulation and click Exit Simulation. This switches back to the Create Operations tab. We will now generate V Carve Finishing to finish the sign with a Taper Tool. V-Carving 1. Select 2.5 Axis Mill and choose V-Carving. This brings up the V-Carving Operations dialog. We will go over the steps for creating the toolpath. Select Machining Features/Regions 2. Go to the Machining Features/ Regions tab. The regions from the previous operations stay selected and the Machining Features would list the 13 regions. 3. If the regions are not listed under Selected Machining regions use single select and select the inner rectangle and the Text as shown below. Right mouse click to complete the selection. 4. The selected regions are now displayed under Machining Regions Selecting the Tool 5. Switch to the Tools tab inside the V-Carve Roughing operation. 6. Select VeeMill1. VeeMill1 is now selected as the active tool and the Tool parameters are displayed to the right of the Tools window. Copyright , MecSoft Corporation, 174

175 Set Feeds and Speeds 7. Click on the Feeds and Speeds tab. 8. Select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. Copyright , MecSoft Corporation, 175

176 Clearance Control 9. Switch to Clearance Tab. 10. Set the Clearance Plane Definition to Absolute Z Value = 0.25 and Cut Transfer Method to Clearance Plane. Setting Cut Transfer to Clearance Plane would apply the Absolute Z value clearance between transfers when the tool moves from a machining region to another. Copyright , MecSoft Corporation, 176

177 Specifying Cut Parameters 11. Switch to Cut Parameters tab. 12. Set the Tolerance = 0.001, Cut Side = Inside, Location of Cut Geometry = At Top, Total Cut Depth = 0.25, Rough Depth = 0.25, and Rough Depth/Cut = Click Generate. The V-Carving toolpath is now generated and the Operation is listed under the VisualMILL-MOps browser. Note: Toolpath display can be turned on/off by selecting Toolpath Visibility under the MOps browser. Copyright , MecSoft Corporation, 177

178 Copyright , MecSoft Corporation, 178

179 Simulate Toolpath The generated toolpath can now be simulated. 1. Switch to the Simulate tab in the VisualMILL-MOps browser and Select the V-Carving Operation and click to Simulate. 2. The Simulated part is as shown below. Copyright , MecSoft Corporation, 179

180 Post Processing 1. Select Machining Operations from the Create Operations tab and right click and select post process. 2. Specify the File Name as Embossing.nc and click Save. The post by default is set to Haas as specified under the Post processor setup. You can change the post processor by selecting a different one from the drop down menu in the list. The posted g code by default will be saved to the folder where the part file is located. End of Tutorial 5! Copyright , MecSoft Corporation, 180

181 Tutorial 6: Chamfering Copyright , MecSoft Corporation, 181

182 Introduction This tutorial is intended to show an easy way to chamfer and smooth sharp corners by using 2 ½ axis Chamfering operation. A tapered tool is suitable for this purpose. In this example, the chamfer is not modeled in the part. We plan to chamfer the edges of the part using a 30 degree taper tool that has 0 radius at the tip. The stepped instructions are accompanied by explanatory and introductory text. Reading this text will help you understand the tutorial methodology and provide information about additional options available. Don t forget to save your work periodically! You may want to save the file under a different name so that the original file will be preserved. Strategy to Machine the part Chamfering is performed using the 2 ½ axis Chamfer Machining Operation. The part would be machined using a single V-Groove bit. The wooden sheet will be held to the machine table or the spoil sheet on the table using double-sided tape. Main Programming Steps In creating programs for each setup, the following steps will be followed: Create the Stock geometry Set the Machine zero point or Locate geometry with respect to the machine coordinates Create / Select the tool used for machining Set the feeds and speeds Set the clearance plane for the non-cutting transfer moves of the cutter Select the machining regions for containing the cutter to specific areas to cut Select the machining operations and set the parameters Generate the toolpath Simulate the toolpath. You may have to repeat either all or part of these steps for subsequent operations. Preparing the part for Machining Loading the Part Model Part refers to the geometry that represents the final manufactured product. You can create parts within VisualMILL, but it is more typical to import geometry created in another CAD system. To load a part: 1. Select File / Open from the Menu, or click the Open icon from the Standard bar. Copyright , MecSoft Corporation, 182

183 2. From the Open dialog box, select the Chamfer.vcp file from the Tutorials folder in the VisualMILL 6.0 installation folder. (C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMILL 6.0\Tutorials) The imported part appears as shown below Copyright , MecSoft Corporation, 183

184 Setup Tab 1. Go to the VisualMILL- MOps browser and click on the Setup tab. The loaded part has the stock model defined and includes a 2 ½ axis Facing Operation with a 0.5 Flat End Mill. The Machining Operation information is listed in the MOps browser as shown below. Copyright , MecSoft Corporation, 184

185 Create Tools To machine the chamfer, we will now create a 60-degree Taper Tool. 1. Go to the VisualMILL-Tools browser that is located below the VisualMILL- MOps browser and select Create/Edit Tools. Select the Tool Type to Chamfer. 2. Set the tool name as ChamferMill1, Taper Angle = 30, Flute Length = 1, and Tool Length = 2. Under the Properties tab, set Tool Number = 2. Note: Taper Angle represents the included angle for a taper tool. For example a 60- degree taper tool would have a included angle of 30 degrees. If you have a taper tool with a diameter select Chamfer Mill or Taper Mill under Create/Select Tool. Copyright , MecSoft Corporation, 185

186 Setting Feeds and Speeds You can assign Feeds & Speeds to a tool or you can load from a table. In this exercise, we will assign feeds and speeds to the tool. 3. Switch to the Feeds & Speeds tab inside the create/select tool dialog. 4. Use the following settings for feeds and speeds. 5. Click Save as New Tool. The tool is now created and listed under Tools in Library. Click OK to close the dialog. Note: You can edit the tool properties and click Save Edits to Tool to save the changes. You can create additional tools by assigning a different name and specify the tool parameters. The created tools are now listed under the VisualMILL-Tools browser. Copyright , MecSoft Corporation, 186

187 Create Machining Operations Switch to the Create Operations tab in VisualMILL-Mops browser. Chamfering 1. Select 2.5 Axis Mill and choose Chamfering. This brings up the Chamfering Operations dialog. We will go over the steps for creating the toolpath. Copyright , MecSoft Corporation, 187

188 Select Machining Features/Regions 2. Go to the Machining Features/ Regions tab and click remove all if any Machining regions are listed. 3. Click Select Curves as Regions. 4. Now, select the curve that follows the profile of the spanner as shown below. Copyright , MecSoft Corporation, 188

189 5. Right mouse click or select enter from the keypad to complete the selection. 6. The selected region is now displayed under Machining Regions. Copyright , MecSoft Corporation, 189

190 Selecting the Tool 7. Switch to the Tools tab inside the Chamfering operation. 8. Select ChamferMill1. ChamferMill1 is now selected as the active tool, and the Tool parameters are displayed to the right of the Tools window. Copyright , MecSoft Corporation, 190

191 Set Feeds and Speeds 9. Click on the Feeds and Speeds tab. 10. Select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. Copyright , MecSoft Corporation, 191

192 Clearance Control 11. Switch to Clearance Tab. 12. Set the Clearance Plane Definition to Absolute Z Value = 0.25 and Cut Transfer Method to Clearance Plane. Setting Cut Transfer to Clearance Plane would apply the Absolute Z value clearance between transfers when the tool moves from a machining region to another. Copyright , MecSoft Corporation, 192

193 Specifying Cut Parameters 13. Switch to Cut Parameters tab. 14. Set the Tolerance = 0.001, Stock = 0, Chamfer Parameters use Chamfer Width = 0.05, Cut Side = Outside. Click Generate. The Chamfering toolpath is now generated and the Operation is listed under the VisualMILL- MOps browser. Note: Toolpath display can be turned on/off by selecting Toolpath Visibility under the MOps browser. Copyright , MecSoft Corporation, 193

194 Reorder a Machining Operation If the chamfer operation is created above the 2 ½ axis Facing operation, you can reorder the MOp using the steps below. 1. Minimize all MOps inside the Mop Set1. 2. Select the Chamfering MOp and drag it over the 2 ½ axis Facing MOp. This would move the Chamfer MOp below the Facing MOp. Copyright , MecSoft Corporation, 194

195 Simulate Toolpath The generated toolpath can now be simulated. 1. Switch to the Simulate tab in the VisualMILL-MOps browser. 2. Select the 2 ½ Axis Facing Operation and click to Simulate. 3. Once the Facing operation is simulated, select the Chamfering Operation and click Simulate to run the simulation. 4. The simulated part is as shown below. Note: You can adjust the simulation speed by selecting Simulation Preferences that is located to the bottom right corner of the VisualMILL-MOps browser. Copyright , MecSoft Corporation, 195

196 To exit the Simulation mode, pause the Simulation and click Exit Simulation. This switches back to the Create Operations tab. Post Processing 1. Select Machining Operations from the Create Operations tab and right click and select post process. 2. Specify the File Name as Chamfering.nc and click Save. Copyright , MecSoft Corporation, 196

197 The post by default is set to Haas as specified under the Post processor setup. You can change the post processor by selecting a different one from the drop down menu in the list. The posted g code by default will be saved to the folder where the part file is located. End of Tutorial 6! Copyright , MecSoft Corporation, 197

198 Tutorial 7: 3 Axis Milling Copyright , MecSoft Corporation, 198

199 Introduction This tutorial will illustrate machining this Mold using 3 axis-milling operations. This tutorial will introduce the usage of several 3-axis operations such as horizontal roughing, parallel finishing, and horizontal finishing. The stepped instructions are accompanied by explanatory and introductory text. Reading this text will help you understand the tutorial methodology and provide information about additional options available. Don t forget to save your work periodically! You may want to save the file under a different name so that the original file will be preserved. Strategy to Machine the mold We will machine the mold completely using 3 axis-machining operations. The part itself will be machined out of a 5.5 x 6.5 inch x 1.25-inch wood block. The stock may be held to the machine table or the spoil sheet on the table using double-sided tape or by clamps. The part will be machined using 0.5 flat end mill, 0.25 & ball end mills. Main Programming Steps In creating programs for each setup, the following steps will be followed: Create the Stock geometry Set the Machine zero point or Locate geometry with respect to the machine coordinates Create / Select the tool used for machining Set the feeds and speeds Set the clearance plane for the non-cutting transfer moves of the cutter Select the machining regions for containing the cutter to specific areas to cut Select the machining operations and set the parameters Generate the toolpath Simulate the toolpath. You may have to repeat either all or part of these steps for subsequent operations. Preparing the part for Machining Loading the Part Model Part refers to the geometry that represents the final manufactured product. You can create parts within VisualMILL, but it is more typical to import geometry created in another CAD system. To load a part: 1. Select File / Open from the Menu, or click the Open icon from the Standard bar. Copyright , MecSoft Corporation, 199

200 2. From the Open dialog box, select the 3Axis_Example1.vcp file from the Tutorials folder in the VisualMILL 6.0 installation folder. (C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMILL 6.0\Tutorials) The imported part appears as shown below Copyright , MecSoft Corporation, 200

201 Setup Tab 1. Go to the VisualMILL- MOps browser and click on the Setup tab. 2. Select Machine Setup from the setup tab. 3. Set the Machine type to 3 axis. Copyright , MecSoft Corporation, 201

202 4. Select Post from the setup tab to specify the post processor options. 5. Set the current post processor that is on your controller. We will select Haas as the post processor for this exercise. Note: By default post processor files are located under C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMill 6.0\Posts The program to send the posted output is set to notepad. This would output the G code to a notepad. Copyright , MecSoft Corporation, 202

203 Create Stock Geometry 1. Select Create/Load stock from the setup tab and create a Box Stock. 2. This brings up the Box Stock parameters. Set the Length (L) = 5.50, Width W = 6.50, and Height (H) = Leave the other parameters as default and click OK. Copyright , MecSoft Corporation, 203

204 3. The stock geometry is now created, and a semi-transparent stock box is displayed on top of the part geometry. Copyright , MecSoft Corporation, 204

205 4. The setup tab now displays the following information: Machine Type, Post Processor, and Stock type as show below. Locate Machine Zero 1. The steps below help you determine the machine home (also know as machine zero or tool touch off point) for the part/stock geometry. 2. Select Locate WCS from the Setup tab. 3. Under Set WCS Origin, choose Set to Stock Box, the Zero Face to Highest Z, and Zero Position to South West corner. This sets the machine home to the top of the stock material and the southwest corner of the part geometry. Copyright , MecSoft Corporation, 205

206 Note: You can change the stock model transparency under standard mode by selecting Simulation Preferences that is located at the bottom of the MOps browser. Copyright , MecSoft Corporation, 206

207 Align Part and Stock During this step, we will align the part inside the stock geometry. 1. Select Align Part and Stock from the Setup tab In this step, we will position the part to the bottom of the stock and center in XY. 2. Use the following settings, Object to Move: Move Part, Z alignment: Bottom and XY Alignment: Center. 3. The part is now aligned inside the stock as shown below. Copyright , MecSoft Corporation, 207

208 Front View Top View Copyright , MecSoft Corporation, 208

209 Create Tools To machine the above part, we will now create a ¼ inch (0.25 ) Flat End Mill. 1. Go to the VisualMILL-Tools browser that is located below the VisualMILL- MOps browser and select Create/Edit Tools. Select the Tool Type to Flat End Mill. 2. Set the tool name as FlatMill-0.5 and Tool Diameter = 0.5. Under the Properties tab, set Tool Number = 1. Copyright , MecSoft Corporation, 209

210 Setting Feeds and Speeds You can assign Feeds & Speeds to a tool or you can load from a table. In this exercise, we will assign feeds and speeds to the tool. 3. Switch to the Feeds & Speeds tab inside the create/select tool dialog. 4. Use the following settings for feeds and speeds. 5. Click Save as New Tool. The tool is now created and listed under Tools in Library. Note: You can edit the tool properties and click Save Edits to Tool to save the changes. You can create additional tools by assigning a different name and specify the tool parameters. 6. Create a Ball End Mill with the following parameters. a. Tool Name: BallMill-0.25, Tool Number = 2. b. Switch to Feeds & Speeds tab set Spindle Speed = 5000 rpm, plunge & approach feed = 35 ipm, approach feed = 40 ipm, cut feed = 45 ipm, retract and departure feeds = 50 ipm. Set the Transfer Feedrate to Use Rapid. c. Click Save as New Tool. Copyright , MecSoft Corporation, 210

211 7. Create another Ball End Mill with the following parameters. d. Tool Name: BallMill-0.125, Tool Number = 3. e. Switch to Feeds & Speeds tab set Spindle Speed = 5000 rpm, plunge & approach feed = 35 ipm, approach feed = 40 ipm, cut feed = 45 ipm, retract and departure feeds = 50 ipm. Set the Transfer Feedrate to Use Rapid. f. Click Save as New Tool. The created tools are now listed under the VisualMILL-Tools browser. Copyright , MecSoft Corporation, 211

212 Create Machining Operations We will machine the mold using 3 different machining operations Horizontal Roughing, Parallel Finishing, and Horizontal Finishing. The first step in machining the mold will be a roughing operation. This type of machining is very efficient for removing large volumes of material and is typically performed with a large tool. Roughing is typically followed by semi-finishing or finishing toolpaths. Switch to the Create Operations tab in VisualMILL-Mops browser. 3 axis Horizontal Roughing 1. Select 3 Axis Milling and choose Horizontal Roughing. 2. This brings up the 3 Axis Horizontal Roughing Operation Dialog. We will now go over the steps for creating the toolpath. 3. Switch to the Tools tab inside the 3 axis Horizontal Roughing operation and select FlatMill-0.5. Copyright , MecSoft Corporation, 212

213 Copyright , MecSoft Corporation, 213

214 4. Click on the Feeds and Speeds tab and select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. Copyright , MecSoft Corporation, 214

215 5. Switch to the Clearance Tab and set the Clearance Plane Definition to Automatic and Cut Transfer Method to Clearance Plane. Copyright , MecSoft Corporation, 215

216 Specify Cut Parameters 8. Click on the Cut Parameters tab. 9. Set the Intol and Outol = 0.001, Stock to leave =0.025, Cut Pattern to Stock Offset, Cut Direction = Mixed, Step over distance = 40 (% Tool Diameter). 10. Switch to the Cut Levels Tab. Copyright , MecSoft Corporation, 216

217 11. Use the Following Settings. a. Step Down Control (dz) = 25 (% Tool Diameter). b. Check Clear Flats under Cut Levels. 12. Switch to the Engage/Retract tab and leave the entry/exit parameters as default. 13. Click Generate. The 3 axis Roughing toolpath is now generated, and the Operation is listed under the VisualMILL-MOps browser. Copyright , MecSoft Corporation, 217

218 14. Switch to Simulate tab, select Horizontal Roughing, and click Simulate to run the simulation. Copyright , MecSoft Corporation, 218

219 Copyright , MecSoft Corporation, 219

220 3 axis Parallel Finishing We will now use 3 axis Parallel Finishing operation to pre-finish the part using a 0.25 Ball End Mill. This is an efficient method of finishing or pre-finishing, typically used when part surfaces are relatively flat. A 2D linear zigzag pattern is generated on the XY plane above the part geometry. The tool moves along this cut pattern, following the contours of the part geometry below. 1. From the Create Operations tab, select 3 axis Milling and Parallel Finishing. This brings up the Parallel Finishing Operations dialog. We will go over the steps for creating the pocketing operation. 2. Switch to the Tools tab inside the Parallel Finishing operation and select BallMill Click on the Feeds and Speeds tab and select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. 4. Switch to the Clearance Tab and set the Clearance Plane Definition to Automatic and Cut Transfer Method to Clearance Plane. Copyright , MecSoft Corporation, 220

221 Specify Cut Parameters 5. Click on the Cut Parameters tab. 6. Set the Tolerance to 0.001, Stock to leave =0, Cut Direction = Mixed, Step over distance = 15 (% Tool Diameter). 7. Click Generate. The Parallel Finishing toolpath is now generated, and the Operation is listed under the 3 Axis Horizontal Roughing Operation in the VisualMILL-MOps browser. Copyright , MecSoft Corporation, 221

222 8. Switch to Simulate tab, select Parallel Finishing, and click Simulate to run the simulation. Copyright , MecSoft Corporation, 222

223 3 axis Horizontal Finishing We will now create a Horizontal Finishing operation for machining steep area regions. This method is used for pre-finishing or finishing in constant Z levels, typically used when the part has large vertical surfaces and when Parallel Finishing will not yield satisfactory results. Preparing the part for Horizontal Finishing In preparation for the Horizontal Finishing operation, we will now create regions by extracting curves from the 3D model. 1. Turn off the Stock Model and Toolpath Visibility from the VisualMILL-MOps browser. 2. Open the Layer Manager and select Layer 01 as the Active Layer. 3. Switch to the Top View by double clicking on the Top View under the Viewport. 4. Create a rectangle by selecting the Create Rectangle tool that is located on the Geometry Bar under Lines. Copyright , MecSoft Corporation, 223

224 5. Turn on the grid snap from the status bar and pick the first corner and second corner by snapping to 2 points on the grid as shown below. 6. The created rectangle is displayed in red and is on Layer 01. We are now ready to create the horizontal finishing operation. 1. Switch to the Create Operations tab. 2. Select 3 axis Milling and Horizontal Finishing. Copyright , MecSoft Corporation, 224

225 Select Machining Features/Regions 3. Go to the Machining Features/ Regions tab and click Select Curves as Regions. 4. Select the rectangle as machining region and right click to complete the selection. Copyright , MecSoft Corporation, 225

226 5. Switch to the Tools tab inside Horizontal Finishing operation and select BallMill Click on the Feeds and Speeds tab and select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. 7. Switch to the Clearance Tab and set the Clearance Plane Definition to Automatic and Cut Transfer Method to Clearance Plane. Specify Cut Parameters 8. Click on the Cut Parameters tab. 9. Set Intol, Outol = 0.001, Cut Direction = Cilmb/Conventional. Copyright , MecSoft Corporation, 226

227 10. Switch to the Cut Levels tab. 11. Set the Step Down Control (dz) = 15 (% Tool Diameter). 12. Leave the entry/exit parameters at default. 13. Click Generate. The Horizontal Finishing operation is now created and is listed under the MOps browser. Copyright , MecSoft Corporation, 227

228 14. Switch to the Simulate tab, select Horizontal Finishing, and click Simulate to run the simulation. 15. The simulated part is shown below. Copyright , MecSoft Corporation, 228

229 Post Processing 1. Select Machining Operations from the Create Operations tab and right click and select post process. 2. Specify the File Name as 3axisMold.nc and click save. The post by default is set to Haas as specified under the Post processor setup. You can change the post processor by selecting a different one from the drop down menu in the list. The posted g code by default will be saved to the folder where the part file is located. End of Tutorial 7! Copyright , MecSoft Corporation, 229

230 Tutorial 8: Profiling with Bridges (Tabs) Copyright , MecSoft Corporation, 230

231 Introduction This tutorial will illustrate machining of multiple parts on a single sheet of stock using 2-1/2 milling operations. The stepped instructions are accompanied by explanatory and introductory text. Reading this text will help you understand the tutorial methodology and provide information about additional options available. Don t forget to save your work periodically! You may want to save the file under a different name so that the original file will be preserved. Strategy to Machine the part We will machine the part using a 2-½ axis profiling operation. We will define bridges so that the parts do not fall off the sheet once its cut to its full depth. The part will be machined out of a 36 x 24 x ½ inch poplar wood sheet using a 0.25 inch Flat End Mill. The wooden sheet will be held to the machine table or the spoil sheet on the table using fixtures/clamps. Main Programming Steps In creating programs for each setup, the following steps will be followed: Create part geometry Create the Stock geometry Set the Machine zero point or Locate geometry with respect to the machine coordinates Create / Select the tool used for machining Set the feeds and speeds Set the clearance plane for the non-cutting transfer moves of the cutter Select the machining regions for containing the cutter to specific areas to cut Select the machining operations and set the parameters Generate the toolpath Simulate the toolpath. You may have to repeat either all or part of these steps for subsequent operations. Preparing the part for Machining Creating the Part Model Part refers to the geometry that represents the final manufactured product. To create a part: 1. Select File / New from the Menu, or click the New icon from the Standard bar. This creates a new session of VisualCAM. Copyright , MecSoft Corporation, 231

232 2. Switch to the Top View by double-clicking on the Top View under the Viewport. 3. The part will be modeled in Inches. VisualCAM status bar displays the model units. To switch units select Preferences->Part Units 4. Select Preferences from VisualCAM menu and Grid Preferences. Use the following grid settings. 5. Create a rectangle by selecting the Create Rectangle tool that is located on the Geometry Bar under Lines. 6. Under the Command bar, specify the first corner as 0,0. 7. Specify the second corner as 36,24. Copyright , MecSoft Corporation, 232

233 8. A rectangle of 36 X 24 is now created and displayed on the screen. This represents the extents of our stock model in XY plane. Create Rounded Rectangle We will now create the part geometry to be cut out inside the sheet. 1. Create a rounded rectangle by selecting Create Rounded Rectangle tool that is located on the Geometry Bar under Lines. 2. Under the command bar, specify the following parameters. 3. First corner as 0.5, Specify second corner (or you could specify in absolute dimensions as 3.5,4.5). 5. Set the radius to This creates a rounded rectangle of size 3 x 4 and a radius of Copyright , MecSoft Corporation, 233

234 Create Rectangular Array We will now create multiple copies of the rounded rectangle to fit it to a sheet of 36 x From the Transform Menu, select Array. 2. Select Pick Objects under Array Objects Dialog and pick the rounded rectangle. Right click to complete the selection. Copyright , MecSoft Corporation, 234

235 Step 1. Step 2 Step3. 3. Set the X Spacing = 3.75, Y Spacing = 4.75, and Z Spacing = 0. Copyright , MecSoft Corporation, 235

236 4. Set # of X Copies = 8, # of Y Copies = 4, and # of Z copies = Click OK. 7. We now have 5 rows and 9 columns of the rounded rectangle. A total of 45 parts on a sheet of 36 x From the File Menu, select Save and save the file under the Tutorials folder. 8. The part geometry is now created. We are now ready to generate a toolpath to machine the part. We will now switch to the VisualMILL-MOps browser. Note: You can skip the above steps for creating the part geometry by loading Profile_Tabs.vcp file into VisualCAM. This is available under the Tutorials folder in VisualMILL 6.0 Copyright , MecSoft Corporation, 236

237 Setup Tab 1. Go to the VisualMILL- MOps browser and click on the Setup tab. 2. Select Machine Setup from the setup tab. 3. Set the Machine type to 3 axis. Copyright , MecSoft Corporation, 237

238 4. Select Post from the setup tab to specify the post processor options. 5. Set the current post processor that is on your controller. We will select Haas as the post processor for this exercise. Note: By default post processor files are located under C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMill 6.0\Posts The program to send the posted output is set to notepad. This would output the G code to a notepad. Copyright , MecSoft Corporation, 238

239 Create Stock Geometry 1. Select Create/Load stock from the setup tab and create a Box Stock. 2. This brings up the Box Stock parameters. Set the Length (L) = 36, Width W = 24, and Height (H) = Make sure to set the corner position to Southwest corner Top of Stock as shown below. Copyright , MecSoft Corporation, 239

240 3. The stock geometry is now created, and a semi-transparent stock box is displayed on top of the part geometry. 4. The setup tab now displays the following information: Machine Type, Post Processor, and Stock type as show below. Copyright , MecSoft Corporation, 240

241 Locate Machine Zero 1. The steps below help you determine the machine home (also know as machine zero or tool touch off point) for the part/stock geometry. 2. Select Locate WCS from the Setup tab. 3. Under Set WCS Origin, choose Set to Stock Box, the Zero Face to Highest Z, and Zero Position to South West corner. This sets the machine home to the top of the stock material and the southwest corner of the part geometry. Copyright , MecSoft Corporation, 241

242 Note: You can change the stock model transparency under standard mode by selecting Simulation Preferences that is located at the bottom of the MOps browser. Copyright , MecSoft Corporation, 242

243 Align Part and Stock In this process, we can align the part and the stock geometry. As we have set the Machine zero to the Stock Box, we will now move the part relative to the stock. 1. Select Align Part and Stock from the Setup tab. 2. Set Object to Move as Move Part, Z alignment as Top, and XY alignment as Center. Copyright , MecSoft Corporation, 243

244 The part geometry is aligned to the center of stock in XY and top in Z. Click Save to save the work and specify a file name. The file is now saved with extension vcp. (VisualCAM Part File) Create Tools To machine the above part, we will now create a ¼ inch (0.25 ) Flat End Mill. 1. Go to the VisualMILL-Tools browser that is located below the VisualMILL-MOps browser and select Create/Edit Tools. Select the Tool Type to Flat End Mill. 2. Set the tool name as FlatMill-0.25 and Tool Diameter = Under the Properties tab, set Tool Number = 1. Copyright , MecSoft Corporation, 244

245 Setting Feeds and Speeds You can assign Feeds & Speeds to a tool or you can load from a table. In this exercise, we will assign feeds and speeds to the tool. 3. Switch to the Feeds & Speeds tab inside the create/select tool dialog. 4. Use the following settings for feeds and speeds. 5. Click Save as New Tool. The tool is now created and listed under Tools in Library. Click OK to close the dialog. Note: You can edit the tool properties and click Save Edits to Tool to save the changes. You can create additional tools by assigning a different name and specify the tool parameters. The created tools are now listed under the VisualMILL-Tools browser. Copyright , MecSoft Corporation, 245

246 Create Machining Operations In this process, we will create a 2.5 axis profiling operation. 1. Switch to the Create Operations tab in VisualMILL-Mops browser. 2 ½ Axis Profiling 2. Select 2.5 Axis Mill and choose Profiling. This brings up the 2 ½ Axis Profiling Operations dialog. We will go over the steps for creating the profile operation. Copyright , MecSoft Corporation, 246

247 Select Machining Features/Regions 3. Go to the Machining Features/ Regions tab, click Remove All, and click Select Curves as Regions. 4. Now, select the all the rounded rectangles. Use Select From the Menu and choose polycurves. Right mouse click or select enter from the keypad to complete the selection. Copyright , MecSoft Corporation, 247

248 5. The selected regions are now displayed under Machining Regions. Copyright , MecSoft Corporation, 248

249 Selecting the Tool 6. Switch to the Tools tab inside the 2 ½ Axis Profiling operation. 7. Select the FlatMill The 0.25 Flat End mill is now selected as the active tool and the Tool parameters are displayed to the right of the Tools window. Copyright , MecSoft Corporation, 249

250 Set Feeds and Speeds 8. Click on the Feeds and Speeds tab. 9. Select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. Copyright , MecSoft Corporation, 250

251 Clearance Control 10. Switch to Clearance Tab. 11. Set the Clearance Plane Definition to Automatic and Cut Transfer Method to Clearance Plane. VisualMILL will determine a safe Z height for the Entry & Exit when set to automatic. Setting Cut Transfer to Clearance Plane would apply the automatic Z clearance between transfers when the tool moves from a machining region to another. Copyright , MecSoft Corporation, 251

252 Specifying Cut Parameters 12. Switch to Cut Parameters tab. 13. Set the Stock = 0. Under Cut Start Side, check Use Outside/Inside for Closed Curves and select Outside. Copyright , MecSoft Corporation, 252

253 14. Select the Cut Levels Tab and specify the Total Cut Depth = 0.51, Rough Depth = 0.5, Rough Depth/Cut = The cut depth is always set as an absolute value. Note: The stock material is 0.5 in thickness. We will generate the toolpath to cut to a depth of 0.51to ensure that the part is cut to its full depth. Copyright , MecSoft Corporation, 253

254 Entry/Exit 15. Switch to Entry/Exit Tab and set the entry and exit type to None. Copyright , MecSoft Corporation, 254

255 Advanced Cut Parameters 16. Switch to Advanced Cut parameters tab and check Use Bridges/Tabs. 17. Specify bridge height = 0.1, bridge length = 0.6, and # of Bridges on each part = 4. In the next step, we will sort the order of machining the parts. Copyright , MecSoft Corporation, 255

256 Sorting 18. Switch to the Sorting tab and use Directional Sort. 19. Set Start Angle = 0 and traverse pattern to ZigZag. This would sort the toolpaths along X and then along Y. 20. Click Generate. The 2½ Axis Profile toolpath is now generated and the Operation is listed under the VisualMILL-MOps browser. Copyright , MecSoft Corporation, 256

257 Note: Toolpath display can be turned on/off by selecting Toolpath Visibility under the MOps browser. Copyright , MecSoft Corporation, 257

258 Simulate Toolpath The generated toolpath can now be simulated. 1. Switch to the Simulate tab in the VisualMILL-MOps browser. 2. Select the 2 ½ Axis Profiling Operation and click to Simulate. 3. The simulated part is as shown below. Note: You can adjust the simulation speed by selecting Simulation Preferences that is located to the bottom right corner of the VisualMILL-MOps browser. Copyright , MecSoft Corporation, 258

259 To exit the Simulation mode, pause the Simulation, and click Exit Simulation. This switches back to the Create Operations tab. Copyright , MecSoft Corporation, 259

260 Post Processing 1. Select Machining Operations from the Create Operations tab and right click and select post process. 2. Specify the File Name as Profile_Tabs.nc and click Save. The post by default is set to Haas as specified under the Post processor setup. You can change the post processor by selecting a different one from the drop down menu in the list. The posted g code by default will be saved to the folder where the part file is located. End of Tutorial 8! Copyright , MecSoft Corporation, 260

261 Tutorial 9: Hole Making Copyright , MecSoft Corporation, 261

262 Introduction This tutorial will illustrate machining holes using Drilling operations. Even though we have created a 3-D representation of the part, it will be seen later on that we can machine this using just 2-D curves. The reason we are able to do this is because of the prismatic nature of this model. The stepped instructions are accompanied by explanatory and introductory text. Reading this text will help you understand the tutorial methodology and provide information about additional options available. Don t forget to save your work periodically! You may want to save the file under a different name so that the original file will be preserved. Strategy to Machine the part We will machine part by using a Hole machining operation called Drilling. The part will be machined out of a 7.25 x 8.5 x 0.75 inch poplar wood sheet using a 0.5 and 0.25 Standard Drill bit. The wooden sheet will be held to the machine table or the spoil sheet on the table using clamps. Main Programming Steps In creating programs for each setup, the following steps will be followed: Create the Stock geometry Set the Machine zero point or Locate geometry with respect to the machine coordinates Create / Select the tool used for machining Set the feeds and speeds Set the clearance plane for the non-cutting transfer moves of the cutter Select the machining regions for containing the cutter to specific areas to cut Select the machining operations and set the parameters Generate the toolpath Simulate the toolpath. You may have to repeat either all or part of these steps for subsequent operations. Preparing the part for Machining Loading the Part Model Part refers to the geometry that represents the final manufactured product. You can create parts within VisualMILL, but it is more typical to import geometry created in another CAD system. To load a part: 1. Select File / Open from the Menu, or click the Open icon from the Standard bar. Copyright , MecSoft Corporation, 262

263 2. From the Open dialog box, select the Bitholder.vcp file from the Tutorials folder in the VisualMILL 6.0 installation folder. (C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMILL 6.0\Tutorials) The imported part appears as shown below Copyright , MecSoft Corporation, 263

264 Setup Tab 1. Go to the VisualMILL- MOps browser and click on the Setup tab. 2. Select Machine Setup from the setup tab. 3. Set the Machine type to 3 axis. Copyright , MecSoft Corporation, 264

265 4. Select Post from the setup tab to specify the post processor options. 5. Set the current post processor that is on your controller. We will select Haas as the post processor for this exercise. Set the posted file extension type to.nc Note: By default post processor files are located under C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMill 6.0\Posts The program to send the posted output is set to notepad. This would output the G code to a notepad. Copyright , MecSoft Corporation, 265

266 Create Stock Geometry 1. Select Create/Load stock from the setup tab and create a Box Stock. 2. This brings up the Box Stock parameters. Set the Length (L) = 7.00, Width W = 8.50, and Height (H) = Leave the other parameters as default and Click OK. Copyright , MecSoft Corporation, 266

267 3. The stock geometry is now created, and a semi-transparent stock box is displayed on top of the part geometry. 4. The setup tab now displays the following information: Machine Type, Post Processor, and Stock type as show below. Copyright , MecSoft Corporation, 267

268 Locate Machine Zero 1. The steps below help you determine the machine home (also know as machine zero or tool touch off point) for the part/stock geometry. 2. Select Locate WCS from the Setup tab. 3. Under Set WCS Origin, choose Set to Stock Box, the Zero Face to Highest Z and Zero Position to South West corner. This sets the machine home to the top of the stock material and the southwest corner of the part geometry. Copyright , MecSoft Corporation, 268

269 Note: You can change the stock model transparency under standard mode by selecting Simulation Preferences that is located at the bottom of the MOps browser. Copyright , MecSoft Corporation, 269

270 Align Part and Stock In this process, we can align the part and the stock geometry. As we have set the Machine zero to the Stock Box, we will now move the part relative to the stock. 1. Select Align Part and Stock from the Setup tab 2. Set to Object to Move as Move Part, Z alignment as Top, and XY alignment as Center Copyright , MecSoft Corporation, 270

271 The part geometry is aligned to the center of stock in XY and top in Z. Click Save to save the work and specify a file name. The file is now saved with extension vcp. (VisualCAM Part File) Create Tools To machine the above part, we will now create 2 tools. 1. Go to the VisualMILL-Tools browser that is located below the VisualMILL-MOps browser and select Create/Edit Tools. Select the Tool Type to Drill Tool. 2. Set the tool name as Drill-0.5 and Tool Diameter = 0.5. Under the Properties tab, set Tool Number = 1. Copyright , MecSoft Corporation, 271

272 Setting Feeds and Speeds You can assign Feeds & Speeds to a tool or you can load from a table. In this exercise, we will assign feeds and speeds to the tool. 3. Switch to the Feeds & Speeds tab inside the create/select tool dialog. 4. Use the following settings for feeds and speeds. 5. Click Save as New Tool. The tool is now created and listed under Tools in Library. Note: You can edit the tool properties and click Save Edits to Tool to save the changes. You can create additional tools by assigning a different name and specify the tool parameters. 6. Create a second tool of type Drill. Set the Tool Name as Drill-0.25, Tool Number = 2. Use the same settings for the other parameters and click Save as New Tool. Click OK to close the dialog. The created tools are now listed under the VisualMILL-Tools browser. Copyright , MecSoft Corporation, 272

273 Create/Extract Regions In order to machine the holes, we need to extract the curves from the 3d model to select them as machining regions. 1. Select the Layer Manager from the Standard bar 2. The layer manager is now open. Set the Layer01 as the active layer. 3. Close the Layer Manager. 4. From the Curves tab on the Geometry Bar to your right, select Single Flat Area Regions. 5. The command bar would now prompt the user to select a flat area to extract the curves. Copyright , MecSoft Corporation, 273

274 6. Select the top face (surface) on the part. 7. The curves are now created and displayed in red on the part geometry. Note: You can toggle the stock model display by selecting Stock Visibility that is located at the bottom of the VisualMill-MOps Browser Copyright , MecSoft Corporation, 274

275 Create Machining Operations In this process, we will create a 2.5 axis profiling operation. 1. Switch to the Create Operations tab in VisualMILL-Mops browser. Hole Machining 2. Select Hole Machining and choose Drilling. This brings up the Drilling Operations dialog. We will go over the steps for creating the toolpath. Copyright , MecSoft Corporation, 275

276 Select Hole Features 3. Go to the Hole Features tab and click Select Drill Points/Circles. 4. Switch to the Top view and select the larger radius circles by using the rectangular selection as indicated below. Copyright , MecSoft Corporation, 276

277 5. Right mouse click or select enter from the keypad to complete the selection. 6. The selected regions are now displayed under Hole Features. Copyright , MecSoft Corporation, 277

278 Selecting the Tool 7. Switch to the Tools tab inside the Drilling operation. 8. Select the Drill-0.5. The 0.5 Drill is now selected as the active tool and the Tool parameters are displayed to the right of the Tools window. Copyright , MecSoft Corporation, 278

279 Set Feeds and Speeds 9. Click on the Feeds and Speeds tab. 10. Select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. Copyright , MecSoft Corporation, 279

280 Clearance Control 11. Switch to Clearance Tab. 12. Set the Clearance Plane Definition to Automatic and Cut Transfer Method to Clearance Plane. VisualMILL will determine a safe Z height for the Entry & Exit when set to automatic. Setting Cut Transfer to Clearance Plane would apply the automatic Z clearance between transfers when the tool moves from a machining region to another. Copyright , MecSoft Corporation, 280

281 Specifying Cut Parameters 13. Switch to Cut Parameters tab. 14. Set the Drill Type to Standard Drill, Drill Depth = 0.75, Check Add Tool Tip to Drill Depth, Location of Cut Geometry At Top, and Approach Distance = 0.1. Note: Adding Tool Tip to Drill Depth adds the taper height of the drill tool to the drill depth to make it a through hole. Copyright , MecSoft Corporation, 281

282 15. Select the Sorting Tab. Use Directional Sort, leave the primary sort direction Start Angle = 0, Secondary Sort direction (s) Low to High and Traverse Pattern to ZigZag. The holes will now be sorted row first starting from the lowest point moving up in Y in a ZigZag pattern. 16. Click Generate. The Drilling toolpath is now generated, and the Operation is listed under the VisualMILL-MOps browser. Note: Toolpath display can be turned on/off by selecting Toolpath Visibility under the MOps browser. Copyright , MecSoft Corporation, 282

283 Copyright , MecSoft Corporation, 283

284 Simulate Toolpath The generated toolpath can now be simulated. 1. Switch to the Simulate tab in the VisualMILL-MOps browser. 2. Select the 2 ½ Axis Profiling Operation and click to Simulate. 3. The simulated part is as shown below. Note: You can adjust the simulation speed by selecting Simulation Preferences that is located to the bottom right corner of the VisualMILL-MOps browser. Copyright , MecSoft Corporation, 284

285 To exit the Simulation mode, pause the Simulation and click Exit Simulation. This switches back to the Create Operations tab. Copyright , MecSoft Corporation, 285

286 Creating the Drill operation for the 0.25 Holes 1. Switch to the Create operations tab 2. Select the Standard Drill Operation created from the previous step, right mouse click, and select Copy. 3. Right click and select Paste. 4. This would create a copy of the Drilling Operation and lists below the first pocketing operation as show below. 5. Double click on the Standard Drill (1) to edit the Hole Features. 6. Click Remove All from the Hole Features Dialog to remove all the regions from the list. 7. Now use Select Drill Points/Circles and select the smaller radius circles using the rectangular select as shown below. 8. Right mouse click or select enter from the keypad to complete the selection. 9. The selected regions are now displayed under Hole Features. 10. Switch to the Tools tab under the Drilling Operations dialog and select Drill Copyright , MecSoft Corporation, 286

287 11. Click Generate. The toolpath for Drill Operation (1) is now generated. 12. Switch to Simulate tab and select Drill Operation (1) and click to simulate toolpath. Copyright , MecSoft Corporation, 287

288 Post Processing 1. Select Machining Operations from the Create Operations tab and right click and select post process. 2. Specify the File Name as Drilling.nc and click Save. The post by default is set to Haas as specified under the Post processor setup. You can change the post processor by selecting a different one from the drop down menu in the list. The posted g code by default will be saved to the folder where the part file is located. End of Tutorial 9! Copyright , MecSoft Corporation, 288

289 Tutorial 10: Re-Machining a 3D Mold Copyright , MecSoft Corporation, 289

290 Introduction This tutorial will illustrate machining this Mold using advanced 3 axis-milling operations. This tutorial will introduce the usage of advanced 3-axis operations such as pencil tracing & valley remachining. The stepped instructions are accompanied by explanatory and introductory text. Reading this text will help you understand the tutorial methodology and provide information about additional options available. However, if you prefer to work straight through the steps without any additional reading, look for the following symbol: Don t forget to save your work periodically! You may want to save the file under a different name so that the original file will be preserved. Strategy to Machine the mold We will machine the mold completely using 3 axis-machining operations. The part itself will be machined out of a 5.5 x 4.45 inch x 1.25-inch wood block. The stock may be held to the machine table or the spoil sheet on the table using double-sided tape or by clamps. The part will be machined using 0.5 flat end mill, 0.25 & ball end mills. Main Programming Steps In creating programs for each setup, the following steps will be followed: Create the Stock geometry Set the Machine zero point or Locate geometry with respect to the machine coordinates Create / Select the tool used for machining Set the feeds and speeds Set the clearance plane for the non-cutting transfer moves of the cutter Select the machining regions for containing the cutter to specific areas to cut Select the machining operations and set the parameters Generate the toolpath Simulate the toolpath. You may have to repeat either all or part of these steps for subsequent operations. Preparing the part for Machining Part refers to the geometry that represents the final manufactured product. You can create parts within VisualMILL, but it is more typical to import geometry created in another CAD system. 1. Select File / Open from the Menu, or click the Open icon from the Standard bar. Copyright , MecSoft Corporation, 290

291 2. From the Open dialog box, select the 3Axis_Example2.vcp file from the Tutorials folder in the VisualMILL 6.0 installation folder. (C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMILL 6.0\Tutorials) 3. The imported part appears as shown below Create Machining Operations Note: The part is pre-programmed with 2 machining operations. Horizontal Roughing and Parallel Finishing. We will now use remachining to finish the mold using 2 different machining operations Pencil Tracing and Valley Re-Machining. Switch to the Create Operations tab in VisualMILL-Mops browser. 3 axis Pencil Tracing Copyright , MecSoft Corporation, 291

292 1. Highlight the Parallel Finishing operation in the Create operations tab. This would ensure the next machining operation created would below the Parallel Finishing toolpath. 2. Select 3 Axis Milling and choose Pencil Tracing. 3. This brings up the 3 Axis Pencil Tracing Operation Dialog. We will now go over the steps for creating the toolpath. 4. Switch to the Tools tab inside the Pencil Tracing operation and select BallMill Copyright , MecSoft Corporation, 292

293 5. Click on the Feeds and Speeds tab and select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. Copyright , MecSoft Corporation, 293

294 6. Switch to the Clearance Tab and set the Clearance Plane Definition to Automatic and Cut Transfer Method to Clearance Plane. Copyright , MecSoft Corporation, 294

295 Specify Cut Parameters 1. Click on the Cut Parameters tab. 2. Set the Intol and Outol = 0.001, Stock to leave =0.0, Cut Direction to Climb, Select Do multiple cuts and set Number of Cuts = 2 and Step over control = 20 (% Tool Diameter). Copyright , MecSoft Corporation, 295

296 Advanced Cut parameters 3. Switch to the advanced cut parameters Tab. 4. Use the Following Settings. a. Limiting Steep Angle = 90 and Maximum included angle =180. Copyright , MecSoft Corporation, 296

297 Entry/Exit 5. Switch to the Entry/Exit tab and use the following settings. Copyright , MecSoft Corporation, 297

298 6. Switch to the Exit Tab and set the Retract motion length = and Angle = Click Generate. The 3-axis Pencil Tracing toolpath is now generated, and the Operation is listed under the VisualMILL-MOps browser. Copyright , MecSoft Corporation, 298

299 8. Switch to Simulate tab, select Pencil Trace, and click Simulate to run the simulation. Copyright , MecSoft Corporation, 299

300 3 axis Valley Re-Machining We will now use 3 axis Valley Re-Machining operation to finish the part using a Ball End Mill. 1. From the Create Operations tab, select 3 axis Milling and Valley Re-Machining. 2. This brings up the Valley Re-Machining Operations dialog. We will go over the steps for creating the pocketing operation. 3. Switch to the Tools tab inside the Parallel Finishing operation and select BallMill Click on the Feeds and Speeds tab and select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. 5. Switch to the Clearance Tab and set the Clearance Plane Definition to Automatic and Cut Transfer Method to Clearance Plane. 6. Click on the Cut control tab. Specify Cut Control 1. Click on the cut control tab. 2. Set the Tolerance to 0.001, Stock to leave =0, Under Reference Tool Parameters set Tool Diameter (D) = 0.25 (This is the diameter of the tool that was used for parallel finishing). Copyright , MecSoft Corporation, 300

301 Specify Cutting Parameters 1. Click on the Cutting Parameters tab. 2. Use Split Cuts under slope Control. Specify the Cuts Split Angle (A) = Select Output Flat and Steep Cuts. Copyright , MecSoft Corporation, 301

302 4. Select Flat Cut Parameters. 5. Select Cut Pattern as Along, Cut Direction as Along, Cut Direction as Mixed and specify Step Over control = 20 (% tool diameter). 6. Select Steep Cut Parameters. 7. Select Cut Pattern as Across, Cut Direction as Along, Cut Direction as Mixed and specify Step Over control = 20 (% tool diameter). Copyright , MecSoft Corporation, 302

303 8. Click Generate. The Valley Remachining toolpath is now generated, and the Operation is listed in the VisualMILL-MOps browser. 9. Switch to Simulate tab, select Valley Remachining, and click Simulate to run the simulation. Post Processing 1. Select Machining Operations from the Create Operations tab and right click and select post process. Copyright , MecSoft Corporation, 303

304 2. Specify the File Name as 3axisMold2.nc and click save. The post by default is set to Haas as specified under the Post processor setup. You can change the post processor by selecting a different one from the drop down menu in the list. The posted g code by default will be saved to the folder where the part file is located. End of Tutorial 10! Copyright , MecSoft Corporation, 304

305 Tutorial 11: Machining a Ring Copyright , MecSoft Corporation, 305

306 Introduction This tutorial will illustrate machining this Ring using 4 axis-milling operations. This tutorial will introduce the usage of several 4-axis operations such as 4 axis roughing and finishing. The stepped instructions are accompanied by explanatory and introductory text. Reading this text will help you understand the tutorial methodology and provide information about additional options available. Don t forget to save your work periodically! You may want to save the file under a different name so that the original file will be preserved. Strategy to Machine the ring We will machine the ring completely using 4 axis-machining operations. The part itself will be machined out of a cylindrical blank. The stock will be held to the machine table using a rotary chuck. The part will be machined using and ball end mills. Main Programming Steps In creating programs for each setup, the following steps will be followed: Create the Stock geometry Set the Machine zero point or Locate geometry with respect to the machine coordinates. Set the rotary axis and rotary center. Create / Select the tool used for machining Set the feeds and speeds Set the clearance plane for the non-cutting transfer moves of the cutter Select the machining operations and set the parameters Generate the toolpath Simulate the toolpath. You may have to repeat either all or part of these steps for subsequent operations. Preparing the part for Machining Loading the Part Model Part refers to the geometry that represents the final manufactured product. You can create parts within VisualMILL, but it is more typical to import geometry created in another CAD system. To load a part: 1. Select File / Open from the Menu, or click the Open icon from the Standard bar. 2. From the Open dialog box, select the RingExample_1.vcp file from the Tutorials folder in the VisualMILL 6.0 installation folder. (C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMILL 6.0\Tutorials) The imported part appears as shown below Copyright , MecSoft Corporation, 306

307 Copyright , MecSoft Corporation, 307

308 Setup Tab 1. Go to the VisualMILL- MOps browser and click on the Setup tab. 2. Select Machine Setup from the setup tab. 3. Set the Machine type to 4 axis and Rotary Axis to X axis. For most controllers rotation along X represents A axis and rotation along Y represents B axis. We will set the Rotary Center once we determine the Machine Zero. Copyright , MecSoft Corporation, 308

309 4. Select Post from the setup tab to specify the post processor options. 5. Set the current post processor that is on your controller. We will select Haas as the post processor for this exercise. Note: By default post processor files are located under C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMill 6.0\Posts The program to send the posted output is set to notepad. This would output the G code to a notepad. Copyright , MecSoft Corporation, 309

310 Create Stock Geometry 1. Select Create/Load stock from the setup tab and create a Cylinder Stock. 2. This brings up the Cylinder Stock parameters. Set the Axis (rotary) = X, Radius = 0.56 and Length (L) = Leave the other parameters as default and click OK. Copyright , MecSoft Corporation, 310

311 3. The stock geometry is now created, and a semi-transparent stock is displayed on top of the part geometry. Isometric View Front View Copyright , MecSoft Corporation, 311

312 4. You must switch the simulation model to Polygonal model to run 4 axis simulations. Select Preferences->Simulation Preferences from the Setup Tab and switch the simulation model to Polygonal if set to Voxel. Copyright , MecSoft Corporation, 312

313 5. The setup tab now displays the following information: Machine Type, Post Processor, and Stock type as show below. Locate Machine Zero 1. The steps below help you determine the machine home (also know as machine zero or tool touch off point) for the part/stock geometry. 2. Select Locate WCS from the Setup tab. 3. Under Set WCS Origin, choose Set to Stock Box, the Zero Face to Highest Z, and Zero Position to East. This sets the machine home to the top of the stock material and the right most edge of the part geometry. Copyright , MecSoft Corporation, 313

314 Copyright , MecSoft Corporation, 314

315 Isometric View Front View Note: You can change the stock model transparency under standard mode by selecting Simulation Preferences that is located at the bottom of the MOps browser. Copyright , MecSoft Corporation, 315

316 Align Part and Stock During this step, we will align the part inside the stock geometry. 1. Select Align Part and Stock from the Setup tab In this step, we will position the part to the center of the stock in XY & Z. 2. Use the following settings, Object to Move: Move Part, Z alignment: Center and XY Alignment: Center. 3. The part is now aligned inside the stock as shown below. Copyright , MecSoft Corporation, 316

317 Isometric View Front View Specify Rotary Center In this step we will determine the rotary center for the part geometry. The rotary center must pass thro the entire part geometry. VisualMILL will not compute a toolpath if the part/feature is below the rotary center as this is considered as an undercuts in the part. 1. Select Machine Setup from the setup tab. In the above example, the stock diameter is Set the rotary center in X and Y = 0 and Z = which is the center of the stock geometry. The rotary center is represented by an arrow and displayed on the part geometry when the Machine Setup Dialog is invoked. Copyright , MecSoft Corporation, 317

318 Copyright , MecSoft Corporation, 318

319 Create Tools To machine the above part, we will now create a Ball End Mill and a Ball End Mill. 1. Go to the VisualMILL-Tools browser that is located below the VisualMILL-MOps browser and select Create/Edit Tools. Select the Tool Type to Ball End Mill. 2. Set the tool name as BallMill and Tool Diameter = Under the Properties tab, set Tool Number = 1. Copyright , MecSoft Corporation, 319

320 Setting Feeds and Speeds You can assign Feeds & Speeds to a tool or you can load from a table. In this exercise, we will assign feeds and speeds to the tool. 3. Switch to the Feeds & Speeds tab inside the create/select tool dialog. 4. Use the following settings for feeds and speeds. 5. Click Save as New Tool. The tool is now created and listed under Tools in Library. Note: You can edit the tool properties and click Save Edits to Tool to save the changes. You can create additional tools by assigning a different name and specify the tool parameters. 6. Create a 2 nd Ball End Mill with the following parameters. a. Tool Name: BallMill , Tool Number = 2. b. Switch to Feeds & Speeds tab set Spindle Speed = 5000 rpm, plunge, approach & engage feed = 20 ipm, cut feed = 30 ipm, retract and departure feeds = 20 ipm. Set the Transfer Feedrate to Use Rapid. c. Click Save as New Tool. The created tools are now listed under the VisualMILL-Tools browser. Copyright , MecSoft Corporation, 320

321 Create Machining Operations We will machine the ring using 2 different machining operations 4 axis Roughing and Finishing. The first step in machining the ring will be a roughing operation. In this cut method, the tool cuts the stock in successive levels. The spacing between these levels are specified by the user. This type of machining is very efficient for removing large volumes of material and is typically performed with a large tool. Roughing is typically followed by semi-finishing or finishing toolpaths. Switch to the Create Operations tab in VisualMILL-Mops browser. Copyright , MecSoft Corporation, 321

322 4 axis Roughing 1. Select 4 Axis Milling and choose Roughing. If the rotary center is not set to the same location as the Machine Zero, a warning message dialog would be displayed at all times when a 4 axis machining operation is selected. Users can override this message by clicking OK in the dialog. Copyright , MecSoft Corporation, 322

323 Note: You can check Do no show this dialog again to stop the warning message appearing again when you create/edit a 4 axis machining operation. 2. This brings up the 4 Axis Roughing Operation Dialog. We will now go over the steps for creating the toolpath. 3. Switch to the Tools tab inside the 4th axis Roughing operation and select BallMill Copyright , MecSoft Corporation, 323

324 4. Click on the Feeds and Speeds tab and select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. Copyright , MecSoft Corporation, 324

325 5. Switch to the Clearance Tab and set the Clearance Plane Definition to Automatic and Cut Transfer Method to Clearance Plane. Copyright , MecSoft Corporation, 325

326 Specify Cut Parameters 6. Click on the Cut Parameters tab. 7. Set the Intol and Outol = 0.001, Stock to leave =0.005, Cut Pattern to Across Axis, Zig Zag and Low to High, Cut Containment Low Value = , High Value = 0 (as the machine zero is set to the right edge of the stock/ part), Step over distance = 25 (% Tool Diameter). 8. Switch to the Step Down Control Tab. Copyright , MecSoft Corporation, 326

327 Step Down Control 9. Use the Following Settings. a. Cut Levels, Check Top (T) and specify Top (T) = 0.56 (radius of stock material) b. Step Down Control (dr) = 75 (% Tool Diameter). 10. Click Generate. The 4th axis Roughing toolpath is now generated, and the Operation is listed under the VisualMILL-MOps browser. Copyright , MecSoft Corporation, 327

328 11. Switch to Simulate tab, select 4 Axis Roughing, and click Simulate to run the simulation. Copyright , MecSoft Corporation, 328

329 4 axis Finishing We will now use 4th Axis Finishing operation to finish the part using a Ball End Mill. In this method, the tool is always normal to the axis of table rotation (continuous mode). The tool motions can be parallel to or normal to the rotation axis. From the Create Operations tab, select 4 axis Milling and 4 Axis Finishing. This brings up the Finishing Operations dialog. We will go over the steps for creating the pocketing operation. 1. Switch to the Tools tab inside the 4 Axis Finishing operation dialog and select BallMill Copyright , MecSoft Corporation, 329

330 2. Click on the Feeds and Speeds tab and select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. 3. Switch to the Clearance Tab and set the Clearance Plane Definition to Automatic and Cut Transfer Method to Clearance Plane. Copyright , MecSoft Corporation, 330

331 Specify Cut Parameters 4. Click on the Cut Parameters tab. 5. Set the Tolerance to 0.001, Stock to leave =0, Cut Pattern = Along Axis, Zig Zag, Low to High, Set Cut Containment Low Value = -0.7, High Value = -0.1, Step over distance = 10 (% Tool Diameter). 6. Click Generate. The Finishing toolpath is now generated, and the Operation is listed under the 4th Axis Roughing Operation in the VisualMILL-MOps browser. Copyright , MecSoft Corporation, 331

332 7. Switch to Simulate tab, select 4 Axis Finishing, and click Simulate to run the simulation. Copyright , MecSoft Corporation, 332

333 Post Processing 1. Select Machining Operations from the Create Operations tab and right click and select post process. 2. Specify the File Name as Ring.nc and click save. The post by default is set to Haas as specified under the Post processor setup. You can change the post processor by selecting a different one from the drop down menu in the list. The posted g code by default will be saved to the folder where the part file is located. End of Tutorial 11! Copyright , MecSoft Corporation, 333

334 Tutorial 12: Engraving on a Cylinder Copyright , MecSoft Corporation, 334

335 Introduction This tutorial will illustrate engraving text on a cylinder using a 4 Axis Engraving operation. The stepped instructions are accompanied by explanatory and introductory text. Reading this text will help you understand the tutorial methodology and provide information about additional options available. Don t forget to save your work periodically! You may want to save the file under a different name so that the original file will be preserved. Strategy to engrave text on a cylinder We will machine the ring completely using 4 axis-machining operations. The part itself will be machined out of a cylindrical blank. The stock will be held to the machine table using a rotary chuck. The part will be machined using 15deg V-Bit. Main Programming Steps In creating programs for each setup, the following steps will be followed: Create the Stock geometry Set the Machine zero point or Locate geometry with respect to the machine coordinates. Set the rotary axis and rotary center. Create / Select the tool used for machining Set the feeds and speeds Set the clearance plane for the non-cutting transfer moves of the cutter Select the machining operations and set the parameters Generate the toolpath Simulate the toolpath. You may have to repeat either all or part of these steps for subsequent operations. Preparing the part for Machining Loading the Part Model Part refers to the geometry that represents the final manufactured product. You can create parts within VisualMILL, but it is more typical to import geometry created in another CAD system. To load a part: 1. Select File / Open from the Menu, or click the Open icon from the Standard bar. 2. From the Open dialog box, select the 4Axis_Engrave.vcp file from the Tutorials folder in the VisualMILL 6.0 installation folder. (C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMILL 6.0\Tutorials) The imported part appears as shown below Copyright , MecSoft Corporation, 335

336 Copyright , MecSoft Corporation, 336

337 Setup Tab 1. Go to the VisualMILL- MOps browser and click on the Setup tab. 2. Select Machine Setup from the setup tab. 3. Set the Machine type to 4 axis and Rotary Axis to X axis. For most controllers rotation along X represents A axis and rotation along Y represents B axis. We will set the Rotary Center once we determine the Machine Zero. Copyright , MecSoft Corporation, 337

338 4. Select Post from the setup tab to specify the post processor options. 5. Set the current post processor that is on your controller. We will select Haas as the post processor for this exercise. Note: By default post processor files are located under C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMill 6.0\Posts The program to send the posted output is set to notepad. This would output the G code to a notepad. Copyright , MecSoft Corporation, 338

339 Create Stock Geometry 1. Select Create/Load stock from the setup tab and create a Cylinder Stock. 2. This brings up the Cylinder Stock parameters. Set the Axis (rotary) = X, Radius = 1 and Length (L) = 8. Leave the other parameters as default and click OK. Copyright , MecSoft Corporation, 339

340 3. The stock geometry is now created, and a semi-transparent stock is displayed on top of the part geometry. 4. You must switch the simulation model to Polygonal model to run 4 axis simulations. Select Preferences->Simulation Preferences from the Setup Tab and switch the simulation model to Polygonal if set to Voxel. Copyright , MecSoft Corporation, 340

341 5. The setup tab now displays the following information: Machine Type, Post Processor, and Stock type as show below. Copyright , MecSoft Corporation, 341

342 Locate Machine Zero 1. The steps below help you determine the machine home (also know as machine zero or tool touch off point) for the part/stock geometry. 2. Select Locate WCS from the Setup tab. 3. Under Set WCS Origin, choose Set to Stock Box, the Zero Face to Mid Z, and Zero Position to West. This sets the machine home to the center of the stock material and the left most edge of the part geometry. Copyright , MecSoft Corporation, 342

343 Note: You can change the stock model transparency under standard mode by selecting Simulation Preferences that is located at the bottom of the MOps browser. Copyright , MecSoft Corporation, 343

344 Align Part and Stock During this step, we will align the part inside the stock geometry. 1. Select Align Part and Stock from the Setup tab In this step, we will position the part to the center of the stock in XY and Z. 2. Use the following settings, Object to Move: Move Part, Z alignment: Center and XY Alignment: Center. Copyright , MecSoft Corporation, 344

345 Specify Rotary Center In this step we will determine the rotary center for the part geometry. The rotary center must pass thro the entire part geometry. VisualMILL will not compute a toolpath if the part/feature is below the rotary center as this is considered as an undercuts in the part. 1. Select Machine Setup from the setup tab. 2. Set the rotary center in X, Y and Z = 0 which is the center of the stock geometry. In this tutorial both the Machine Zero and the Rotary center are at the same location. The rotary center is represented by an arrow and displayed on the part geometry when the Machine Setup Dialog is invoked. Copyright , MecSoft Corporation, 345

346 Create Tools To machine the above part, we will now create a 15 deg V-Bit. 1. Go to the VisualMILL-Tools browser that is located below the VisualMILL-MOps browser and select Create/Edit Tools. Select the Tool Type to VeeMill. 2. Set the tool name as VeeMill1, Taper Angle = 7.5, Flute Length = 0.5, Tool Length = 1. Under the Properties tab set Tool Number = 1. Copyright , MecSoft Corporation, 346

347 Copyright , MecSoft Corporation, 347

348 Setting Feeds and Speeds You can assign Feeds & Speeds to a tool or you can load from a table. In this exercise, we will assign feeds and speeds to the tool. 3. Switch to the Feeds & Speeds tab inside the create/select tool dialog. 4. Use the following settings for feeds and speeds. 5. Click Save as New Tool. The tool is now created and listed under Tools in Library. Note: You can edit the tool properties and click Save Edits to Tool to save the changes. You can create additional tools by assigning a different name and specify the tool parameters. The created tools are now listed under the VisualMILL-Tools browser. Copyright , MecSoft Corporation, 348

349 Create Machining Operations We will engrave the text on the cylinder using 4 Axis Engraving. This method machines text or logos by following the contours of the selected regions by projecting the text onto the cylinder. Switch to the Create Operations tab in VisualMILL-Mops browser. 4 Axis Engraving 1. Select 4 Axis Milling and choose Engraving. Copyright , MecSoft Corporation, 349

350 If the rotary center is not set to the same location as the Machine Zero, a warning message dialog would be displayed at all times when a 4 axis machining operation is selected. Users can override this message by clicking OK in the dialog. Note: You can check Do no show this dialog again to stop the warning message appearing again when you create/edit a 4 axis machining operation. 2. This brings up the 4 Axis Engraving Operation Dialog. We will now go over the steps for creating the toolpath. Copyright , MecSoft Corporation, 350

351 Select Machining Features/Regions 3. Go to the Machining Features/ Regions tab and click Select Curves as Regions. 4. Now, select the text by using the left mouse click, starting from left to right. Make sure to get the inner curves on the letters a, 0. Each curve is separate (by curves, not by letters) and must be selected separately. Copyright , MecSoft Corporation, 351

352 5. Right mouse click or select enter from the keypad to complete the selection. 6. The selected regions are now displayed under Machining Regions. 7. Switch to the Tools tab inside the 4th Axis Engraving operation and select VeeMill1. Copyright , MecSoft Corporation, 352

353 Copyright , MecSoft Corporation, 353

354 8. Click on the Feeds and Speeds tab and select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. Copyright , MecSoft Corporation, 354

355 9. Switch to the Clearance Tab and set the Clearance Plane Definition to Automatic and Cut Transfer Method to Clearance Plane. Copyright , MecSoft Corporation, 355

356 Specify Cut Parameters 10. Click on the Cut Parameters tab. 11. Set the Tolerance = 0.001, Check Project Curve(s) to Model, Check Finishing Passes and set # of finishing passes = 2, and R Depth (Rf) = 0.05 (this is the depth/pass. Total depth = 0.1 ). 12. Click Generate. The 4 axis Engraving toolpath is now generated, and the Operation is listed under the VisualMILL-MOps browser. Copyright , MecSoft Corporation, 356

357 13. Switch to Simulate tab, select 4 Axis Engraving, and click Simulate to run the simulation. Copyright , MecSoft Corporation, 357

358 Post Processing 1. Select Machining Operations from the Create Operations tab and right click and select post process. 2. Specify the File Name as 4AxisEngrave.nc and click save. Copyright , MecSoft Corporation, 358

359 The post by default is set to Haas as specified under the Post processor setup. You can change the post processor by selecting a different one from the drop down menu in the list. The posted g code by default will be saved to the folder where the part file is located. End of Tutorial 12! Copyright , MecSoft Corporation, 359

360 Tutorial 13: Machining a Ring Copyright , MecSoft Corporation, 360

361 Introduction This tutorial will illustrate machining this Ring using 4 axis-milling operations. This tutorial will introduce the usage of several 4-axis operations such as 4 axis roughing and finishing. The stepped instructions are accompanied by explanatory and introductory text. Reading this text will help you understand the tutorial methodology and provide information about additional options available. Don t forget to save your work periodically! You may want to save the file under a different name so that the original file will be preserved. Strategy to Machine the ring We will machine the ring completely using 4 axis-machining operations. The part itself will be machined out of a cylindrical blank. The stock will be held to the machine table using a rotary chuck. The part will be machined using and ball end mills. Main Programming Steps In creating programs for each setup, the following steps will be followed: Create the Stock geometry Set the Machine zero point or Locate geometry with respect to the machine coordinates. Set the rotary axis and rotary center. Create / Select the tool used for machining Set the feeds and speeds Set the clearance plane for the non-cutting transfer moves of the cutter Select the machining operations and set the parameters Generate the toolpath Simulate the toolpath. You may have to repeat either all or part of these steps for subsequent operations. Preparing the part for Machining Loading the Part Model Part refers to the geometry that represents the final manufactured product. You can create parts within VisualMILL, but it is more typical to import geometry created in another CAD system. To load a part: 1. Select File / Open from the Menu, or click the Open icon from the Standard bar. 2. From the Open dialog box, select the RingExample_2.vcp file from the Tutorials folder in the VisualMILL 6.0 installation folder. (C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMILL 6.0\Tutorials) The imported part appears as shown below Copyright , MecSoft Corporation, 361

362 Copyright , MecSoft Corporation, 362

363 Setup Tab 1. Go to the VisualMILL- MOps browser and click on the Setup tab. 2. Select Machine Setup from the setup tab. 3. Set the Machine type to 4 axis and Rotary Axis to X axis. For most controllers rotation along X represents A axis and rotation along Y represents B axis. We will set the Rotary Center once we determine the Machine Zero. Copyright , MecSoft Corporation, 363

364 4. Select Post from the setup tab to specify the post processor options. 5. Set the current post processor that is on your controller. We will select Haas as the post processor for this exercise. Note: By default post processor files are located under C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMill 6.0\Posts The program to send the posted output is set to notepad. This would output the G code to a notepad. Copyright , MecSoft Corporation, 364

365 Create Stock Geometry 1. Select Create/Load stock from the setup tab and create a Cylinder Stock. 2. This brings up the Cylinder Stock parameters. Set the Axis (rotary) = X, Radius = 0.48 and Length (L) = 0.4. Leave the other parameters as default and click OK. Copyright , MecSoft Corporation, 365

366 3. The stock geometry is now created, and a semi-transparent stock is displayed on top of the part geometry. Isometric View Front View Copyright , MecSoft Corporation, 366

367 4. You must switch the simulation model to Polygonal model to run 4 axis simulations. Select Preferences->Simulation Preferences from the Setup Tab and switch the simulation model to Polygonal if set to Voxel. Copyright , MecSoft Corporation, 367

368 5. The setup tab now displays the following information: Machine Type, Post Processor, and Stock type as show below. Locate Machine Zero 1. The steps below help you determine the machine home (also know as machine zero or tool touch off point) for the part/stock geometry. 2. Select Locate WCS from the Setup tab. 3. Under Set WCS Origin, choose Set to Stock Box, the Zero Face to Highest Z, and Zero Position to East. This sets the machine home to the top of the stock material and the right most edge of the part geometry. Copyright , MecSoft Corporation, 368

369 Isometric View Front View Copyright , MecSoft Corporation, 369

370 Note: You can change the stock model transparency under standard mode by selecting Simulation Preferences that is located at the bottom of the MOps browser. Align Part and Stock During this step, we will align the part inside the stock geometry. 1. Select Align Part and Stock from the Setup tab In this step, we will position the part to the center of the stock in XY & Z. 2. Use the following settings, Object to Move: Move Part, Z alignment: Center and XY Alignment: Mid-East. Copyright , MecSoft Corporation, 370

371 3. The part is now aligned inside the stock as shown below. Copyright , MecSoft Corporation, 371

372 Isometric View Front View Specify Rotary Center In this step we will determine the rotary center for the part geometry. The rotary center must pass thro the entire part geometry. VisualMILL will not compute a toolpath if the part/feature is below the rotary center as this is considered as an undercuts in the part. 1. Select Machine Setup from the setup tab. In the above example, the stock diameter is Set the rotary center in X and Y = 0 and Z = which is the center of the stock geometry. The rotary center is represented by an arrow and displayed on the part geometry when the Machine Setup Dialog is invoked. Copyright , MecSoft Corporation, 372

373 Create Tools To machine the above part, we will now create and Ball End Mills. 1. Go to the VisualMILL-Tools browser that is located below the VisualMILL-MOps browser and select Create/Edit Tools. Select the Tool Type to Ball End Mill. 2. Set the tool name as BallMill , Tool Diameter = Flute Length = 1 and Tool Length = 1.5. Under the Properties tab, set Tool Number = 1. Copyright , MecSoft Corporation, 373

374 Copyright , MecSoft Corporation, 374

375 Setting Feeds and Speeds You can assign Feeds & Speeds to a tool or you can load from a table. In this exercise, we will assign feeds and speeds to the tool. 3. Switch to the Feeds & Speeds tab inside the create/select tool dialog. 4. Use the following settings for feeds and speeds. 5. Click Save as New Tool. The tool is now created and listed under Tools in Library. Note: You can edit the tool properties and click Save Edits to Tool to save the changes. You can create additional tools by assigning a different name and specify the tool parameters. 6. Create a 2 nd Ball End Mill with the following parameters. a. Tool Name: BallMill , Tool Number = 2. b. Switch to Feeds & Speeds tab set Spindle Speed = 5000 rpm, plunge, approach & engage feed = 20 ipm, cut feed = 30 ipm, retract and departure feeds = 20 ipm. Set the Transfer Feedrate to Use Rapid. c. Click Save as New Tool. The created tools are now listed under the VisualMILL-Tools browser. Copyright , MecSoft Corporation, 375

376 Create Machining Operations We will machine the ring using 2 different machining operations 4 axis Roughing and Finishing. The first step in machining the ring will be a roughing operation. In this cut method, the tool cuts the stock in successive levels. The spacing between these levels are specified by the user. This type of machining is very efficient for removing large volumes of material and is typically performed with a large tool. Roughing is typically followed by semi-finishing or finishing toolpaths. Switch to the Create Operations tab in VisualMILL-Mops browser. Copyright , MecSoft Corporation, 376

377 4 th axis Roughing 1. Select 4 Axis Milling and choose Roughing. If the rotary center is not set to the same location as the Machine Zero, a warning message dialog would be displayed at all times when a 4 axis machining operation is selected. Users can override this message by clicking OK in the dialog. Copyright , MecSoft Corporation, 377

378 Note: You can check Do no show this dialog again to stop the warning message appearing again when you create/edit a 4 axis machining operation. 2. This brings up the 4 Axis Roughing Operation Dialog. We will now go over the steps for creating the toolpath. 3. Switch to the Tools tab inside the 4 Axis Roughing operation and select BallMill Copyright , MecSoft Corporation, 378

379 4. Click on the Feeds and Speeds tab and select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. Copyright , MecSoft Corporation, 379

380 5. Switch to the Clearance Tab and set the Clearance Plane Definition to Automatic and Cut Transfer Method to Clearance Plane. Copyright , MecSoft Corporation, 380

381 Specify Cut Parameters 6. Click on the Cut Parameters tab. 7. Set the Intol and Outol = 0.001, Stock to leave =0.005, Cut Pattern to Along Axis, Zig Zag and Low to High, Cut Containment Low Value = -0.4, High Value = 0.03, Step over distance = 25 (% Tool Diameter). 8. Switch to the Step Down Control Tab. Copyright , MecSoft Corporation, 381

382 Step Down Control 9. Use the Following Settings. c. Cut Levels, Check Top (T) and specify Top (T) = 0.48 (radius of stock material), Bottom (B) = 0.4, Step Down Control (dr) = 75 (% Tool Diameter). 10. Click Generate. The 4 axis Roughing toolpath is now generated, and the Operation is listed under the VisualMILL-MOps browser. Copyright , MecSoft Corporation, 382

383 11. Switch to Simulate tab, select 4 Axis Roughing, and click Simulate to run the simulation. Copyright , MecSoft Corporation, 383

384 4 th Axis Roughing operation #2 We will now create a second 4 Axis Rough operation to machine the pocket areas around the ring by limiting the toolpath using start, end angle cut containments. Copying a MOp 1. Switch to the Create Operations tab in the Mops Browser. 2. Select the 4 Axis Roughing operation, right click copy. 3. Now right click and select paste. 4. A copy of the rough operation is created below the 4th Axis Roughing operation. The operation name is labeled 4th Axis Roughing(1) and is as shown below. Copyright , MecSoft Corporation, 384

385 Copyright , MecSoft Corporation, 385

386 Specify Cut Parameters 5. Double click on 4th Axis Roughing(1) to edit the operation. 6. Switch to the Cut parameters tab and use the following parameters. a. Leave the global parameters and cut pattern unchanged b. Under Cut Containment change the Start Angle (S) = -90, End Angle (E) = 90, Uncheck Do not cut past. 7. Switch to the Step Down Control tab Copyright , MecSoft Corporation, 386

387 Specify Step Down Control 8. Use the Following Settings. a. Cut Levels, Check Top (T) and specify Top (T) = 0.4 (as we had limited the toolpath to a radius = 0.4 on the 1 st Rough operation), Step Down Control (dr) = 75 (% Tool Diameter). 9. Click Generate. The 4 axis Roughing toolpath is now generated, and the Operation is listed under the VisualMILL-MOps browser. Copyright , MecSoft Corporation, 387

388 10. Switch to Simulate tab, select 4 Axis Roughing, and click Simulate to run the simulation. Copyright , MecSoft Corporation, 388

389 4 th axis Finishing We will now use 4th Axis Finishing operation to finish the part using a Ball End Mill. In this method, the tool is always normal to the axis of table rotation (continuous mode). The tool motions can be parallel to or normal to the rotation axis. From the Create Operations tab, select 4 axis Milling and 4 Axis Finishing. This brings up the Finishing Operations dialog. We will go over the steps for creating the pocketing operation. 1. Switch to the Tools tab inside the 4 Axis Finishing operation dialog and select BallMill Copyright , MecSoft Corporation, 389

390 2. Click on the Feeds and Speeds tab and select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. 3. Switch to the Clearance Tab and set the Clearance Plane Definition to Automatic and Cut Transfer Method to Clearance Plane. Copyright , MecSoft Corporation, 390

391 Specify Cut Parameters 4. Click on the Cut Parameters tab. 5. Set the Tolerance to 0.001, Stock to leave =0, Cut Pattern = Along Axis, Zig Zag, Low to High, Set Cut Containment Low Value = -0.4, High Value = -0.03, Step over distance = 10 (% Tool Diameter). 6. Click Generate. The Finishing toolpath is now generated, and the Operation is listed under the 4 Axis Roughing Operation in the VisualMILL-MOps browser. Copyright , MecSoft Corporation, 391

392 7. Switch to Simulate tab, select 4 Axis Finishing, and click Simulate to run the simulation. Copyright , MecSoft Corporation, 392

393 Post Processing 1. Select Machining Operations from the Create Operations tab and right click and select post process. 2. Specify the File Name as Ring2.nc and click save. The post by default is set to Haas as specified under the Post processor setup. You can change the post processor by selecting a different one from the drop down menu in the list. The posted g code by default will be saved to the folder where the part file is located. End of Tutorial 13! Copyright , MecSoft Corporation, 393

394 Tutorial 14: Pocketing and Drilling on a Ring Copyright , MecSoft Corporation, 394

395 Introduction This tutorial is intended to describe the 4 axis pocketing and hole making operations. Pocketing machines closed regions as if they were pockets - completely enclosed by inner and outer regions. The tool cannot go beyond the outer region, and cannot go within inner regions. This is unlike Facing, in which the outermost region is considered to enclose material to be removed. Hole making operations are used to create holes in a part; the hole types varying from simple drill holes, counter sunk holes, through holes to tapped and bored holes. Here you will learn to drill simple holes. The stepped instructions are accompanied by explanatory and introductory text. Reading this text will help you understand the tutorial methodology and provide information about additional options available. Don t forget to save your work periodically! You may want to save the file under a different name so that the original file will be preserved. Strategy to machine the part We will machine the ring completely using 4 axis-machining operations. The part itself will be machined out of a cylindrical blank. The stock will be held to the machine table using a rotary chuck. The part will be machined using a Flat End Mill and Standard Drill Main Programming Steps In creating programs for each setup, the following steps will be followed: Create the Stock geometry Set the Machine zero point or Locate geometry with respect to the machine coordinates. Set the rotary axis and rotary center. Create / Select the tool used for machining Set the feeds and speeds Set the clearance plane for the non-cutting transfer moves of the cutter Select the machining operations and set the parameters Generate the toolpath Simulate the toolpath. You may have to repeat either all or part of these steps for subsequent operations. Preparing the part for Machining Loading the Part Model Part refers to the geometry that represents the final manufactured product. You can create parts within VisualMILL, but it is more typical to import geometry created in another CAD system. To load a part: 1. Select File / Open from the Menu, or click the Open icon from the Standard bar. Copyright , MecSoft Corporation, 395

396 2. From the Open dialog box, select the 4AxisPocketing_1.vcp file from the Tutorials folder in the VisualMILL 6.0 installation folder. (C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMILL 6.0\Tutorials) The imported part appears as shown below Copyright , MecSoft Corporation, 396

397 Setup Tab 1. Go to the VisualMILL- MOps browser and click on the Setup tab. 2. Select Machine Setup from the setup tab. 3. Set the Machine type to 4 axis and Rotary Axis to X axis. For most controllers rotation along X represents A axis and rotation along Y represents B axis. We will set the Rotary Center once we determine the Machine Zero. Copyright , MecSoft Corporation, 397

398 4. Select Post from the setup tab to specify the post processor options. 5. Set the current post processor that is on your controller. We will select Haas as the post processor for this exercise. Note: By default post processor files are located under C:\Program Files\MecSoft Corporation\VisualCAM 1.0\Plug-ins\VisualMill 6.0\Posts The program to send the posted output is set to notepad. This would output the G code to a notepad. Copyright , MecSoft Corporation, 398

399 Create Stock Geometry 1. Select Create/Load stock from the setup tab and create a Cylinder Stock. 2. This brings up the Cylinder Stock parameters. Set the Axis (rotary) = X, Radius = 2 and Length (L) = 1. Leave the other parameters as default and click OK. Copyright , MecSoft Corporation, 399

400 3. The stock geometry is now created, and a semi-transparent stock is displayed on top of the part geometry. Copyright , MecSoft Corporation, 400

401 4. You must switch the simulation model to Polygonal model to run 4 axis simulations. Select Preferences->Simulation Preferences from the Setup Tab and switch the simulation model to Polygonal if set to Voxel. Copyright , MecSoft Corporation, 401

402 5. The setup tab now displays the following information: Machine Type, Post Processor, and Stock type as show below. Locate Machine Zero 1. The steps below help you determine the machine home (also know as machine zero or tool touch off point) for the part/stock geometry. 2. Select Locate WCS from the Setup tab. 3. Under Set WCS Origin, choose Set to Stock Box, the Zero Face to Highest Z, and Zero Position to East. This sets the machine home to the center of the stock material and the right most edge of the part geometry. Copyright , MecSoft Corporation, 402

403 Copyright , MecSoft Corporation, 403

404 Note: You can change the stock model transparency under standard mode by selecting Simulation Preferences that is located at the bottom of the MOps browser. Align Part and Stock During this step, we will align the part inside the stock geometry. 1. Select Align Part and Stock from the Setup tab In this step, we will position the part to the center of the stock in XY and Z. 2. Use the following settings, Object to Move: Move Part, Z alignment: Center and XY Alignment: Center. Copyright , MecSoft Corporation, 404

405 Specify Rotary Center In this step we will determine the rotary center for the part geometry. The rotary center must pass thro the entire part geometry. VisualMILL will not compute a toolpath if the part/feature is below the rotary center as this is considered as an undercuts in the part. 1. Select Machine Setup from the setup tab. 2. Set the rotary center in X, Y and Z = -2 (which is the center of the stock geometry Diameter of stock = 4 ). The rotary center is represented by an arrow and displayed on the part geometry when the Machine Setup Dialog is invoked. Copyright , MecSoft Corporation, 405

406 Create Tools To machine the above part, we will now create a Drill (Standard Drill) and a Flat End Mill. 1. Go to the VisualMILL-Tools browser that is located below the VisualMILL- MOps browser and select Create/Edit Tools. Select the Tool Type to Drill. 2. Set the tool name as Drill-0.125, Tool Diameter = 0.125, Tip Angle = 120. Under the Properties tab set Tool Number = 1. Copyright , MecSoft Corporation, 406

407 Copyright , MecSoft Corporation, 407

408 Setting Feeds and Speeds You can assign Feeds & Speeds to a tool or you can load from a table. In this exercise, we will assign feeds and speeds to the tool. 3. Switch to the Feeds & Speeds tab inside the create/select tool dialog. 4. Use the following settings for feeds and speeds. 5. Click Save as New Tool. The tool is now created and listed under Tools in Library. Note: You can edit the tool properties and click Save Edits to Tool to save the changes. You can create additional tools by assigning a different name and specify the tool parameters. 6. Create a 2 nd tool, a Flat End Mill with the following parameters. a. Tool Name: FlatMill , Tool Diameter = , Flute Length = 1,Tool Length = 1.5, Tool Number = 2. b. Switch to Feeds & Speeds tab set Spindle Speed = 5000 rpm, plunge, approach & engage feed = 20 ipm, cut feed = 30 ipm, retract and departure feeds = 20 ipm. Set the Transfer Feedrate to Use Rapid. c. Click Save as New Tool. The created tools are now listed under the VisualMILL-Tools browser. Copyright , MecSoft Corporation, 408

409 Create Machining Operations First we will drill the holes on the cylinder using 4 Axis Drilling. As in any other 4 axis operations, the tool is positioned normal (perpendicular) to the rotary axis. Once the holes (regions) are selected, the dialog boxes are similar to the 3 axis hole making operations. Sorting of holes is also possible to optimize the tool motion. Switch to the Create Operations tab in VisualMILL-Mops browser. Copyright , MecSoft Corporation, 409

410 4 Axis Drilling 1. Select Hole and choose 4 Axis Drilling. If the rotary center is not set to the same location as the Machine Zero, a warning message dialog would be displayed at all times when a 4 axis machining operation is selected. Users can override this message by clicking OK in the dialog. Copyright , MecSoft Corporation, 410

411 Note: You can check Do no show this dialog again to stop the warning message appearing again when you create/edit a 4 axis machining operation. 2. This brings up the 4 Axis Drilling Operation Dialog. We will now go over the steps for creating the toolpath. Select Hole Features 3. Go to the Machining Features/ Regions tab and click Hole Features. 4. Now, select the 12 circles around the part (represented in green color). You can also use the Select tool from the menu bar and use Select->By Layer and choose Layer 04. Copyright , MecSoft Corporation, 411

412 5. Right mouse click or select enter from the keypad to complete the selection. 6. The selected regions are now displayed under Hole Features. Copyright , MecSoft Corporation, 412

413 7. Switch to the Tools tab inside the 4 Axis Drilling operation and select Drill Copyright , MecSoft Corporation, 413

414 8. Click on the Feeds and Speeds tab and select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. 9. Switch to Clearance tab and set the Clearance Plane Definition to Stock Max R + Dist = Set the cut transfer method to Clearance Plane. Copyright , MecSoft Corporation, 414

415 Copyright , MecSoft Corporation, 415

416 Specify Cut Parameters 10. Click on the Cut Parameters tab. 11. Set the Drill Type = Standard Drill, Drill Depth = 0.1, Check Add Tool tip to Drill Depth and Approach Distance = Switch to Sorting tab in the 4 Axis Drilling dialog. Copyright , MecSoft Corporation, 416

417 Sorting 13. Use Minimum Distance Sort and specify the Start Point as Lower Left 14. Click Generate. The 4 Axis Drilling toolpath is now generated, and the Operation is listed under the VisualMILL-MOps browser. Copyright , MecSoft Corporation, 417

418 15. Switch to Simulate tab, select 4 Axis Drilling, and click Simulate to run the simulation. Copyright , MecSoft Corporation, 418

419 4 axis Pocketing 1. Select 4 Axis from the Create operations tab and choose 4 Axis Pocketing If the rotary center is not set to the same location as the Machine Zero, a warning message dialog would be displayed at all times when a 4 axis machining operation is selected. Users can override this message by clicking OK in the dialog. Copyright , MecSoft Corporation, 419

420 Note: You can check Do no show this dialog again to stop the warning message appearing again when you create/edit a 4 axis machining operation. 2. This brings up the 4 Axis Pocketing Operation Dialog. We will now go over the steps for creating the toolpath. Copyright , MecSoft Corporation, 420

421 Select Machining Features/Regions 3. Go to the Machining Features/ Regions tab and click Select Curves as Regions. 4. Select all the curves on Layer 02 using the Select from the menu, Select- >By Layer and choose Layer 02. Copyright , MecSoft Corporation, 421

422 5. Right mouse click or select enter from the keypad to complete the selection. 6. The selected regions are now displayed under Machining Regions. 7. Switch to the Tools tab inside the 4 axis pocketing operation and select FlatMill Copyright , MecSoft Corporation, 422

423 8. Click on the Feeds and Speeds tab and select Load From Tool. VisualMILL will now get the feeds and speeds information that was set when the tool was defined. 9. Switch to the Clearance Tab and set the Clearance Plane Definition to Automatic and Cut Transfer Method to Clearance Plane. Copyright , MecSoft Corporation, 423

424 Specify Cut Parameters 10. Click on the Cut Parameters tab. 11. Set Tolerance = 0.001, Stock = 0, Cut Pattern = Offset Cuts, Cut Direction = Mixed, Start Point = Inside, Step Distance = 25% (Tool Diameter), Check Corner Cleanup. 12. Switch to Cut Levels Tab. 13. Use the following Settings a. Location of Cut Geometry At Top. b. Total Cut Depth = 0.1, Rough Depth = 0.1 Copyright , MecSoft Corporation, 424

425 c. Rough Depth/Cut = d. Cut Level Ordering = Depth First. 14. Click Generate. The 4 Axis Pocketing toolpath is now generated, and the Operation is listed under the VisualMILL-MOps browser. Copyright , MecSoft Corporation, 425

426 15. Switch to Simulate tab, select 4 Axis Engraving, and click Simulate to run the simulation. Copyright , MecSoft Corporation, 426

427 Post Processing 1. Select Machining Operations from the Create Operations tab and right click and select post process. 2. Specify the File Name as 4AxisPocketing.nc and click save. The post by default is set to Haas as specified under the Post processor setup. You can change the post processor by selecting a different one from the drop down menu Copyright , MecSoft Corporation, 427