PART 1: BASIC MACHINING
|
|
- Clementine Cunningham
- 5 years ago
- Views:
Transcription
1 PART 1: BASIC MACHINING CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 1 CREATING A MANUFACTURING MODEL In this Lesson you will create a Manufacturing Model by assembling the Design Model. The Design Model represents the finished part (after all of the machining takes place). You are actually going to start with a forging of this part and remove only a small amount of material in some areas. In this case, you are not going to assemble the forging (as a Workpiece). In later Lessons, you will learn how to utilize both the design part and the forging together. Before starting this tutorial: Ensure that you have downloaded all CAM files from the write-protected drive (P:\Courses\41617-CAM) and placed them on your own drive (M:\) Set the Working Directory to the directory on your own drive where you placed the CAM files. 1. Create a Manufacturing Model. Choose Home from the Menu bar Choose New Notice NC Assembly from the Subtype list is the default choice. Give it a name... Typically, let this be selected, (it controls whether you work in mm or in inches). When you initially open Creo on a new system, please make certain that it opens in mm. This should be checked for each file type. To verify which units the file is set up to, you can open top menu File / Prepare / Model Properties under the Materials paragraph. The Model Properties dialoque allows you to change units by choosing the change button to the right. Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 1
2 CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 1 Choose Manufacturing from the Type list Type your initials_basic1 and hit ENTER or choose OK If you are able to choose units in this dialogue choose mmns 2. Assemble the Design Model. (Open the design model when you reside in the Manufacturing module) Set the graphic display to Shaded Click the Reference Model icon (not the text below with the arrow) In the dialoque box choose Profile1.prt and hit ENTER The Profile1.prt will appear on the screen - probably in a temporary state indicated by the dark purple color. If the model displays in white color (= automatic placement), you should skip the actions in the red frame underneath. If you dont see anything on the screen, press CTRL+ D To constrain (place) the model press the Automatic button and choose default far down - This will position the model in the same 3D space as when constructed... The system may ask you to enter a Density value, just accept the suggested one, using Accept position by clicking Begin the NC Sequence by defining the minimum Operation data of a WorkCell Type. 1. Start the Sequence Click the Work Center icon on the top ribbon menu. The Milling Work Center dialogue will appear Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 2
3 CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 1 The Milling Work Center displays Define the Cell Type Choose Mill from the Machine Type option menu - Default choice... Choose 3 Axis from the Number of Axes option menu - Default choice... Choose OK - Yes, you didn t change anything in this box, but this entry can t be skipped.- You will notice that MILL 01 now appears on the model tree. OPERATION SETUP The Work Center has now been defined. Now it is time to create an Operation. You need to do this before you can start defining NC sequences. Think of 1 operation = 1 clamping in the vice. An operation can contain one or several NC sequences. Define An Operation On the top ribbon, choose the Operation icon A Machine Coordinate system (MCS) has to be defined. The system wants you to either create one or to point on an existing coordinate system. Here, one comes with the part: You are now going to define the Machine Coordinate System (MCS). Whether you Select or Create the Machine Zero coordinate system, you must always make sure that the Z Axis is pointing "up" towards the spindle on the NC Machine, and that the X Axis is pointing along the default tool motion. Remember, the tool axis is also going to be parallel to the Z Axis. Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 3
4 CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 1 Select CSO by clicking it in the display window (provided you have turned on Csys Display). Please click on the CSO label and not on the 3D cross itself.(arrow in bottom of page 3) Click on the accept icon. The system has now created a new csys (NC_CS0) to act as the MCS. (Machine Coordinate System) A new pane Mill has now appeared on the top Ribbon. By clicking it, a range of Milling options appears. With the Mill pane active, choose the grey Milling zone (Arrow) Choose Pocketing (meaning Digging holes ) Now the Operation has been partially defined. It appears on the Model tree, and the Menu Manager pops up, requiring you to define the remaining variables: The Menu Manager will appear on the right side of the sreen. Note that the Sequence Setup menu displays, showing you the required items: - Here you will have to fill out 4 dialogue boxes. Choose Done - The system will display the first of the four, Tools Setup window as shown next page: Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 4
5 CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 1 When you choose Done, the system will begin to offer you the menus to specify the required information...which in this case will be Tool, Parameters, Retract Surf, and Surfaces. These kinds of menus are known as "Walk Through" menus. You can manually add or remove entries, but stick to these four right now Define the Tool Choose End Mill ( Arrow)... Type 25 for diameter and 100 for height ( Arrows)... Verify that the units are Millimeters ( Arrow)... Choose Apply, followed by OK (more Arrows) For unknown reasons, the Tools setup may be defined in Inlbs even when the manufacturing file is set to mm... - A flat ended 25 mm/100 mm tool has now been defined Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 5
6 CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 1 SPECIFYING PARAMETERS Now to the second entry on the four-point list: Specify all of the required parameters, marked yellow: The system now displays the Edit Parameters of Sequence window containing the minimum set of the parameters that are appropriate for the type of NC Sequence you are using.(pale yellow) Click with the mouse cursor in the field to the right of the text CUT_FEED Type 75 and hit ENTER Click with the mouse cursor in the field to the right of the text STEP_DEPTH Type 6 and hit ENTER Click with the mouse cursor in the field to the right of the text STEP_OVER Type 6 and hit ENTER Click with the mouse cursor in the field to the right of the text CUT_ANGLE Type 90 and hit ENTER Click with the mouse cursor in the field to the right of the text SCAN_TYPE Click on TYPE_2 and hit ENTER Click with the mouse cursor in the field to the right of the text CLEAR_DIST Type 2.5 Click with the mouse cursor in the field to the right of the text SPINDLE_SPEED and type 500 Choose the All button located at the upper left in the window to display all parameters Find the POCKET_EXTEND option Change TOOL_ON to TOOL_TO Choose OK to exit the parameter setup window - The box closes, and a small third dialogue box, Retract Setup, comes next... Choose Done Alternatively, you can use the DOWN arrow key on the keyboard instead of clicking in the field... You should come back and explore more by changing the parameter values after playing the path and then notice the difference each parameter causes. Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 6
7 CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 1 MACHINING SURFACES The third point on the list: The system now wants you to define a Retract Plane and select the surfaces to be machined.the Retract Setup dialog has opened by it self and the brown grid shows its current distance from plane to model (=0) In the (Z Depth) Value text field type 25 and hit ENTER Choose the OK action button: The box closes. Now the tool will idle in a comfortable 25 mm Z distance from the Workpiece... The Retract Plane defines the height above the Workpiece where the tool safely can hover around when moving from one job to another without crashing into the Workpiece. The retract Plane distance is now 25 mm Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 7
8 CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 1 Finally the system prompts you to specify which surfaces to be machined. Choose Model from the SURF PICK menu: Here the system wants you to choose some surfaces on the model for the purpose of milling these. Choose Done Select the green colored face shown below It may appear red on your screen... In the Select box, Choose OK Choose Done/Return Play the tool path Choose Play Path Choose Screen Play Choose Play Forward Button First this... Followed by this... In the Play Path dialogue under View there are various display settings for the tool, shaded, wireframe etc. And then this... Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 8
9 CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 1 Here is the tool is shown shaded, the tool tip and the tool kerf is visible. Screen play with Play Path : This is how your first sequence will look. You may notice a few things about this tool path. The cutter moved in straight lines, parallel to the Y-Axis because the CUT_ANGLE is 90 degrees. The tool followed along the sides of the pocket to avoid cutting through the part. The tool cut around the protrusion or "island". This type of movement is a result of using the TYPE_2 - SCAN_TYPE. The path also retracts to the Retract Plane each time it must move to a new area. Retracts are automatically created in Creo/NC. Choose Close 4. Save this tool path in memory. Choose Done Sec: - This step is important - it saves the whole operation Choose Done / Return Now you will create a second NC Sequence to finish machine the pocket in the other side of the part. 1. Begin a new sequence. Choose Pocketing - like you did at the upper middle of page 4 Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 9
10 CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 1 The Menu Manager appears, and it only promts you for information on Parameters and Surfaces. Please notice that it in this new sequence the system reuses data from your previous sequense.(same Tool, MCS, and Retract plane) Choose Done - The Parameter dialogue box appears - Here too you can reuse data: Choose Edit / Copy from Step: A small dialogue box, Select Step, opens Choose the top line: 1: Pocket Milling, Operation: OP010, and close with an OK Now all the tool parameter data from the previous sequense will be reused. Close the Parameters box with the OK in the bottom of the box Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 10
11 CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 1 Now the Menu Manager will appear and promt you for which surfaces you want milled: In the Menu Manager, under SURF PICK / MODEL, click Done Select the green colored face below Choose OK Choose Done/Return 4. Play the tool path. Choose Play Path Choose Screen Play Choose Close 5. Save this tool path in memory. Choose Done Seq 6. Take one more step. Play the entire Operation to see both pockets machined: Please remember: It takes one or more Sequences to define an Operation. One Clamping in the vice equals one operation Choose - in the top ribbon - the Manufacturing pane Click on the Rapid Fedrat icon: The Menu Manager opens Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 11
12 CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 1 In the Menu Manager choose Operation / OP010 / Done: The Play Path interface appears. Choose Play, let it run and notice that both sequences run in one continous movement ATTENTION The final step of the above exercise (The play of the whole operation) must be REVIEWED and APPROVED by your INSTRUCTOR to make you eligible for a signature on your approval sheet confirming your successful completion of this tutorial. Leave this file open and continue to the next exercise. Before asking for review and approval please have both the completed exercises opened. Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 12
13 PART 2: VOLUME MILLING DEFINING A VOLUME CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 2 Create a mill volume to rough remove material from a block of graphite which is used to form the EDM electrode shown below. 1. Create a manufacturing model using the NC Assembly manufacturing type and assemble the Ref Model called volume1.prt into it, similarly to the previous lesson - Remember to check that you work in mm. Accept the (Default) positioning of the Ref Model. 2. Create a workpiece. This simulates a raw piece of material being milled. It is color coded green by default. Click on the arrow under the Workpiece icon Choose Create Workpiece Type stock_vol1 as the workpiece part name and hit ENTER In the Menu Manager choose Protrusion / Done Select NC_ASM_TOP as the Sketch Plane. You can select it on the screen or in the model tree. As son as the Sketch plane is chosen, the Sketcher ribbon appears. You can ignore the References dialogue. Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 13
14 CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 2 Sketch Plane can be chosen here or here Choose the Project tool... In the Missing References dialogue chose Yes Project tool Use Chain Click on the edge, approximately here, and then approximately here, In the Menu Manager click Accept - If the four edges do not want to chain, click Next to make it happen. click yes to the Loop question click the OK accept-sign Enter 85 for the protrusion Depth value and accept The Workpiece (stock) has been created and, as you can see, contains the entire part. Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 14
15 CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 2 Workpiece has been created 3. Create the mill volume. Choose the Create Mill Volume tool Choose the Extrude tool Choose Placement, followed by Define- The Sketch Dialog box appears Right-click here repeatedly to highlight this face and left-click it to choose it as the sketch plane From this surface is where the Mill Volume will rise.(it is the deepest Z level the tool reaches) The Mill Volume will extend upward to the surface which you will specify. Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 15
16 CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 2 Choose Sketch to begin sketching You don t need references for this sketch Choose the Use Project tool, like before Choose Chain type Repeat the edge selection procedure you used before, when you drew the sketch for the Workpiece. The chain may be easyer to create if you select the bottom edges of the part (Arrow) In the Menu Manager click Accept click yes to the Loop question click the OK accept-sign Choose the Extrude to tool, and select the top surface of the Workpiece click the OK accept-sign. The system has now created a volume that is a large block...in the next Segment, you will see how to exclude the volume containing your part from this block. You will have to trim the Milling volume with the Ref Model. This is preferably done right after the creation of the Milling Volume... TRIMMING A VOLUME Trim the volume to the part. 1. Perform the trim operation. Choose the Trim tool Select VOLUME1.PRT in the viewport or in the model tree Click OK... Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 16
17 CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 2 The Trim feature now appears in the Model tree The Mill Volume in purple (Defining the material that has to be milled away) displayed in wireframe and shaded, (seen from below, design model and workpiece hidden) 3. Define a Work center Click the Work Center icon on the top ribbon menu. The Milling Work Center dialogue will appear 4. Define the cell type. Choose Mill from the Machine Type list - Default setting Choose 3 Axis from the Number of Axes list - Default setting Choose OK from the Machine Tool Setup window - Yes, nothing was actually changed Define an Operation Setup and define Milling type. On the top ribbon, choose the operation icon Select the Coordinate System called CS0 Choose OK Choose the Mill Pane on the top ribbon Click on the Roughing icon, and below that, Click on the Volume Rough icon - The Volume Milling ribbon appears: The dialogue above is a replacement of the Menu Manager walk-through menus. It contains several variables, which all must be defined in order to run an NC sequence. The yellow color signals which entries are still missing. 6. Define the Tool : Choose the Tool icon.the familiar Tools setup appears: For Type, choose End Mill (preselected...) For tool length, type 100 For tool diameter, type 25 Verify that Tool specifications are in mm, and not in inches To exit, choose Apply, followed by OK - The profile Milling top dialog replaces the No Tool with 01: T0001 for Tool name Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 17
18 7. Define the References : - The system needs to know what to mill away... Choose the Reference tab and, to the right of Machining Reference choose Select Items: Select the Milling volume on the screen: 8. Define the Parameters : Choose the Parameters tab, and a small - scale version of the Parameter list appears: You can enter the full - scale version by clicking the icon in the bottom, but this is not necessary now... Focus on the yellow fields at this moment: To the right of CUT_FEED type 75 To the right of STEP_OVER type 6 To the right of ROUGH_STOCK_ALLOW type 1...This is not a yellow entry To the right of MAX_STEP_DEPTH type 25 To the right of ROUGH_OPTION Click on ROUGH_&_CLEAN_UP...This is not a yellow entry To the right of CLEAR_DIST type 2.5 To the right of SPINDLE_SPEED type Define the Clearance : - For defining the retract plane Choose the Parameters tab: The system now asks for a reference level in order to define a Z level where the tool can hover freely around without hitting anything: choose the top surface of the work piece as shown: To the right of the Value field type 15. = The Z distance between the tool tip and the work piece... Click the green Accept icon to save the Volume Milling sequence. 10. Play the Tool Path : Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 18
19 CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 2 Set Display style to Wireframe. In the Model Tree, find the Volume Milling listing, right-click it and choose Path (Arrow) Play Choose the Play Forward button Choose Close 11. Play the NC/CHECK display. Play Path View Before proceding, make sure that you can view the NC/CHECK simulation: Choose - in the upper left corner of the screen: File / Options. The Creo Parametric Options dialogue opens. Choose Configuration Editor (bottom left). On the long Config.pro list, being alphabetical, find nccheck_type. If the nccheck_type entry does not show, enter the Show field in the top of the dialogue: Click here Choose the All options. Now the list gets very long, and nccheck_type will show. in the Value column verify that the nccheck (not Vericut ) option is selected. Leave with OK. Choose NC Check as shown: In the Model Tree, find the Volume Milling listing, right-click it, and choose this time Material Removal Simulation (Arrow) In the Menu Manager, at the bottom,choose Run. NC CHECK display view. Colors may be different on your screen. You might be able to see that this is not a desirable path. Material was left around the outside of the volume and the outside of the part was not machined because the tool could not fit between the side walls of the part and the volume...to get an acceptable path, the Milling volume needs to be larger. Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 19
20 CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 2 OFFSETTING SURFACES Modify the volume to allow the tool to travel beyond the part. 1. Return to the PLAY PATH menu. Choose Done / Return from the NC CHECK menu 2. Modify the Mill volume by offsetting the walls. In the Model tree, right click the Trimmed Mill Volume from the feature list and choose Redefine Mill Volume Redefine Mill Volume You are now editing the trimmed Mill Volume Choose the Offset tool The system probably automatically pre - selects all the surfaces. Now you must manually choose which surfaces to offset Choose The four vertical walls, one by one, using the mouse and the CTRL button
21 The app CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 2 One wall has been chosen Choose Value Check that Expand Feature is the chosen option Type 25 as the Distance Four walls have been chosen The four walls have now been offset 25 mm outwards Click the green accept icon below the Offset tab Click the following green accept icon below the Mill Volume tab 3. Replay the tool path In the Model Tree, right-click the 1. Volume Milling [OP010] and Choose Play Path Choose Screen Play Choose Play Forward icon Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 21
22 CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 2 Choose Close 4. Play the NC/CHECK display. In the Model Tree, right-click the 1. Volume Milling [OP010] post and choose Material Removal Simulation - The Menu Manager appears In the Menu Manager choose Run Both views show that the tool now has access to the Workpiece on all four sides 5. Change the STEP_DEPTH value to allow for a more contoured rough tooling path. On the Model Tree, Single - click on 1. Volume Milling [OP010] post, to turn it active: verify that the Manufacturing pane is the active one, and open the Step Parameters dialogue Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 22
23 CAM Tutorial CREO PARAMETRIC 1.0 week 1 Part 2 Click with the mouse cursor in the field to the right of the text MAX_STEP_DEPTH Type 3 Exit the Parameter Setup window by choosing OK 6. Replay the tool path using the NC/CHECK display, like you did on the previous page. ATTENTION The final step of the above exercise must be REVIEWED and APPROVED by your INSTRUCTOR to make you eligible for a signature on your approval sheet confirming your successful completion of this tutorial. Please have your previous completed exercise (basic_ machining_xxx) opened, so both can be reviewed at the same time. Revised by Tomas Benzon DTU MEK March 2012 on basis of original COACH material Page 23
CAM Tutorial CREO PARAMETRIC 1.0 week 2 Part 3. Profile the outside of the bracket which you used in the Basic Machining Lesson.
CAM Tutorial CREO PARAMETRIC 1.0 week 2 Part 3 PART 3: PROFILING CREATING A BASIC PATH Profile the outside of the bracket which you used in the Basic Machining Lesson. Before starting this tutorial: Ensure
More informationCreo 3.0 G-code Tutorial
Creo 3.0 G-code Tutorial Irobotics µtan(clan) Table of Contents 1. Preface... 2 2. CAD... 3 A. Prepare the CAD... 3 B. Define the Coordinate System... 3 C. Save the CAD... 6 3. Create NC assembly... 6
More informationSETTING UP PRO/NC IN PREPARATION FOR CREATING TOOL PATHS
SETTING UP PRO/NC IN PREPARATION FOR CREATING TOOL PATHS PTC Technical Support - Advanced Manufacturing Technique 140 Kendrick St Needham, MA, USA 800-477-6435 Introduction This document introduces the
More informationTRAINING GUIDE MILL-LESSON-FBM-1 FBM MILL AND FBM DRILL
TRAINING GUIDE MILL-LESSON-FBM-1 FBM MILL AND FBM DRILL Mastercam Training Guide Objectives Previously in Mill-Lesson-6 and Mill-Lesson-7 geometry was created and machined using standard Mastercam methods.
More informationTRAINING GUIDE MILL-LESSON-FBM-2 FBM MILL AND FBM DRILL
TRAINING GUIDE MILL-LESSON-FBM-2 FBM MILL AND FBM DRILL Mastercam Training Guide Objectives This lesson will use the same Feature Based Machining (FBM) methods used in Mill-Lesson- FBM-1, how ever this
More informationECE415: NX TURNING CAM TUTORIAL
ECE415: NX TURNING CAM TUTORIAL Liangliang Chen, and Miao Yu Based on the turning tutorial in NX, this tutorial steps you through the process of creating NC codes for a shaft that can run on the machines
More informationMill Level 1 Training Tutorial
To order more books: Call 1-800-529-5517 or Visit www.inhousesolutions.com or Contact your Mastercam dealer Mastercam X 5 Copyright: 1998-2010 In-House Solutions Inc. All rights reserved Software: Mastercam
More informationTOOLPATHS TRAINING GUIDE. Sample. Distribution. not for MILL-LESSON-4-TOOLPATHS DRILL AND CONTOUR
TOOLPATHS TRAINING GUIDE MILL-LESSON-4-TOOLPATHS DRILL AND CONTOUR Mill-Lesson-4 Objectives You will generate a toolpath to machine the part on a CNC vertical milling machine. This lesson covers the following
More informationI bought Pro/NC Now What?!?
I bought Pro/NC Now What?!? Todd Liebenow Coldfire Enterprises www.coldfire-e.com Copyright 2007 Coldfire Enterprises Agenda 3 steps Foundation Workflow Documentation Supplemental information Q & A (time
More informationMASTERCAM DYNAMIC MILLING TUTORIAL. June 2018
MASTERCAM DYNAMIC MILLING TUTORIAL June 2018 MASTERCAM DYNAMIC MILLING TUTORIAL June 2018 2018 CNC Software, Inc. All rights reserved. Software: Mastercam 2019 Terms of Use Use of this document is subject
More informationLab Assignment #1: Introduction to Creo ME 170
Lab Assignment #1: Introduction to Creo ME 170 Instructor: Mike Philpott (email: mphilpot@illinois.edu) Date Due: One week from Start Day of Lab (turn in deadline 11pm night before next lab) Make sure
More informationBelt Buckle A. Create Rectangle. Step 1. If necessary start a new Mastercam file, click New
Mastercam 2017 Chapter 35 Belt Buckle A. Create Rectangle. Step 1. If necessary start a new Mastercam file, click New (Ctrl-N) on the Quick Access Toolbar QAT. Step 2. On the Wireframe tab click Rectangle.
More informationExercise Guide. Published: August MecSoft Corpotation
VisualCAD Exercise Guide Published: August 2018 MecSoft Corpotation Copyright 1998-2018 VisualCAD 2018 Exercise Guide by Mecsoft Corporation User Notes: Contents 2 Table of Contents About this Guide 4
More informationUsing Delcam Powermill
Written by: John Eberhart & Trevor Williams DM Lab Tutorial Using Delcam Powermill Powermill is a sophistical tool path generating software. This tutorial will walk you through the steps of creating a
More informationTRAINING GUIDE. Sample Only. not to be used. for training MILL-LESSON-15 CORE ROUGHING, WATERLINE, AND SURFACE FINISH LEFTOVER
TRAINING GUIDE MILL-LESSON-15 CORE ROUGHING, WATERLINE, AND SURFACE FINISH LEFTOVER Mastercam Training Guide Objectives You will use a provided model for Mill-Lesson-15, then generate the toolpaths to
More informationTRAINING GUIDE. Sample not. for Distribution LATHE-LESSON-1 FACE, ROUGH, FINISH AND CUTOFF
TRAINING GUIDE LATHE-LESSON-1 FACE, ROUGH, FINISH AND CUTOFF Mastercam Training Guide Objectives You will create the geometry for Lathe-Lesson-1, and then generate a toolpath to machine the part on a CNC
More informationComputer Essentials Session 1 Lesson Plan
Note: Completing the Mouse Tutorial and Mousercise exercise which are available on the Class Resources webpage constitutes the first part of this lesson. ABOUT PROGRAMS AND OPERATING SYSTEMS Any time a
More informationFeature-based CAM software for mills, multi-tasking lathes and wire EDM. Getting Started
Feature-based CAM software for mills, multi-tasking lathes and wire EDM www.featurecam.com Getting Started FeatureCAM 2015 R3 Getting Started FeatureCAM Copyright 1995-2015 Delcam Ltd. All rights reserved.
More informationCNC Programming Simplified. EZ-Turn Tutorial.
CNC Programming Simplified EZ-Turn Tutorial www.ezcam.com Copyright Notice This manual describes software that contains published and unpublished works of authorship proprietary to EZCAM Solutions, Inc.
More informationTRAINING GUIDE WCS - VIEW MANAGER - PART-2
TRAINING GUIDE WCS - VIEW MANAGER - PART-2 Mastercam Training Guide Objectives The learner will create the geometry and toolpaths for WCS-Part-2. This Lesson will cover the following topics: Create a 3-dimensional
More information4 & 5 Axis Mill Training Tutorials. To order more books: Call or Visit or Contact your Mastercam Dealer
4 & 5 Axis Mill Training Tutorials To order more books: Call 1-800-529-5517 or Visit www.inhousesolutions.com or Contact your Mastercam Dealer Mastercam X Training Tutorials 4 & 5 Axis Mill Applications
More informationJewelry Box Lid. A. Sketch Lid Circle. Step 1. If necessary start a new Mastercam file, click FILE Menu > New. Fig. 3
Mastercam X9 Chapter 39 Jewelry Box Lid A. Sketch Lid Circle. Step 1. If necessary start a new Mastercam file, click FILE Menu > New. Step 2. Click CREATE Menu > Arc > Circle Center Point. Step 3. Key-in
More informationTRAINING GUIDE LATHE-LESSON-1 FACE, ROUGH, FINISH AND CUTOFF
TRAINING GUIDE LATHE-LESSON-1 FACE, ROUGH, FINISH AND CUTOFF Mastercam Training Guide Objectives You will create the geometry for Lathe-Lesson-1, and then generate a toolpath to machine the part on a CNC
More informationTRAINING GUIDE. Sample. Distribution. not for LATHE-LESSON-1 FACE, ROUGH, FINISH AND CUTOFF
TRAINING GUIDE LATHE-LESSON-1 FACE, ROUGH, FINISH AND CUTOFF Mastercam Training Guide Objectives You will create the geometry for Lathe-Lesson-1, and then generate a toolpath to machine the part on a CNC
More informationMASTERCAM WIRE TUTORIAL. June 2018
MASTERCAM WIRE TUTORIAL June 2018 MASTERCAM WIRE TUTORIAL June 2018 2018 CNC Software, Inc. All rights reserved. Software: Mastercam 2019 Terms of Use Use of this document is subject to the Mastercam End
More information3 AXIS STANDARD CAD. BobCAD-CAM Version 28 Training Workbook 3 Axis Standard CAD
3 AXIS STANDARD CAD This tutorial explains how to create the CAD model for the Mill 3 Axis Standard demonstration file. The design process includes using the Shape Library and other wireframe functions
More informationBrief Introduction to MasterCAM X4
Brief Introduction to MasterCAM X4 Fall 2013 Meung J Kim, Ph.D., Professor Department of Mechanical Engineering College of Engineering and Engineering Technology Northern Illinois University DeKalb, IL
More informationVERO UK TRAINING MATERIAL. 2D CAM Training
VERO UK TRAINING MATERIAL 2D CAM Training Vcamtech Co., Ltd 1 INTRODUCTION During this exercise, it is assumed that the user has a basic knowledge of the VISI-Series software. OBJECTIVE This tutorial has
More informationDrawing Tips ME170. Instructor: Mike Philpott (
Drawing Tips Instructor: Mike Philpott (email: mphilpot@illinois.edu) Configuration of Creo Prepare Creo for drawing creation. - Open Creo Parametric 3.0 from the Start Menu. - Set your working directory.
More informationVisualCAM 2018 for SOLIDWORKS-TURN Quick Start MecSoft Corporation
2 Table of Contents Useful Tips 4 What's New 5 Videos & Guides 6 About this Guide 8 About... the TURN Module 8 Using this... Guide 8 Getting Ready 10 Running... VisualCAM for SOLIDWORKS 10 Machining...
More informationWorking with the Dope Sheet Editor to speed up animation and reverse time.
Bouncing a Ball Page 1 of 2 Tutorial Bouncing a Ball A bouncing ball is a common first project for new animators. This classic example is an excellent tool for explaining basic animation processes in 3ds
More informationRhinoCAM 2018 MILL Quick Start Guide. MecSoft Corporation
2 Table of Contents About this Guide 4 1 Useful... Tips 4 2 About... the MILL Module 4 3 Using this... Guide 5 Getting Ready 6 1 Running... RhinoCAM 2018 6 2 About... the RhinoCAM Display 6 3 Launch...
More informationCNC Programming Simplified. EZ-Turn / TurnMill Tutorial.
CNC Programming Simplified EZ-Turn / TurnMill Tutorial www.ezcam.com Copyright Notice This manual describes software that contains published and unpublished works of authorship proprietary to EZCAM Solutions,
More informationAutodesk Inventor Design Exercise 2: F1 Team Challenge Car Developed by Tim Varner Synergis Technologies
Autodesk Inventor Design Exercise 2: F1 Team Challenge Car Developed by Tim Varner Synergis Technologies Tim Varner - 2004 The Inventor User Interface Command Panel Lists the commands that are currently
More informationLesson 14 Blends. For Resources go to > click on the Creo Parametric Book cover
Lesson 14 Blends Figure 14.1 Cap OBJECTIVES Create a Parallel Blend feature Use the Shell Tool Create a Swept Blend REFERENCES AND RESOURCES For Resources go to www.cad-resources.com > click on the Creo
More informationProfile Modeler Profile Modeler ( A SuperControl Product )
Profile Modeler ( A SuperControl Product ) - 1 - Index Overview... 3 Terminology... 3 Launching the Application... 4 File Menu... 4 Loading a File:... 4 To Load Multiple Files:... 4 Clearing Loaded Files:...
More informationChapter 39. Mastercam Jewelry Box Tray. A. Sketch Tray Circle. B. Twin Edge Point Circles. Mastercam 2017 Tray Jewelry Box Page 39-1
Mastercam 2017 Chapter 39 A. Sketch Tray Circle. Jewelry Box Tray Step 1. If necessary start a new Mastercam file, click New (Ctrl-N) on the Quick Access Toolbar QAT. Step 2. On the Wireframe tab click
More informationPrismatic Machining Overview What's New Getting Started User Tasks
Prismatic Machining Overview Conventions What's New Getting Started Enter the Workbench Create a Pocketing Operation Replay the Toolpath Create a Profile Contouring Operation Create a Drilling Operation
More informationEZ-Mill EXPRESS TUTORIAL 2. Release 13.0
E-Mill EPRESS TUTORIAL 2 Release 13.0 Copyright Notice This manual describes software that contains published and unpublished works of authorship proprietary to ECAM Solutions, Inc. It is made available
More informationIntroduction to SolidWorks Basics Materials Tech. Wood
Introduction to SolidWorks Basics Materials Tech. Wood Table of Contents Table of Contents... 1 Book End... 2 Introduction... 2 Learning Intentions... 2 Modelling the Base... 3 Modelling the Front... 10
More informationModule 4A: Creating the 3D Model of Right and Oblique Pyramids
Inventor (5) Module 4A: 4A- 1 Module 4A: Creating the 3D Model of Right and Oblique Pyramids In Module 4A, we will learn how to create 3D solid models of right-axis and oblique-axis pyramid (regular or
More informationLadybird Project - Vacuum Mould
- Vacuum Mould Prerequisite Mould drawn and saved as STL file from Solidworks Focus of the Lesson On completion of this exercise you will have completed: Opening STL file Setting Machining Constraints
More informationMastercam X9 for SOLIDWORKS
Chapter 21 CO2 Shell Car Mastercam X9 for SOLIDWORKS A. Enable Mastercam for SOLIDWORKS. Step 1. If necessary, turn on Mastercam for SOLIDWORKS, click the flyout of Options on the Standard toolbar and
More informationPowerMILL. Getting Started
PowerMILL R2 Getting Started PowerMILL 2012 R2 Getting Started Release issue 1 PowerMILL Copyright 1996-2012 Delcam plc. All rights reserved. Delcam plc has no control over the use made of the software
More informationDynamic Milling. March 2015
Dynamic Milling March 2015 Mastercam X9 Dynamic Milling TERMS OF USE Date: March 2015 Copyright 2015 CNC Software, Inc. All rights reserved. Software: Mastercam X9 Use of this document is subject to the
More informationPowerMILL 2016 Getting Started
PowerMILL 2016 Getting Started Release issue 1 PowerMILL Copyright 1996-2015 Delcam Ltd. All rights reserved. Delcam Ltd has no control over the use made of the software described in this manual and cannot
More information5 Axis Cutting Using Delcam Powermill Written by: John Eberhart DM Lab Tutorial
5 Axis Cutting Using Delcam Powermill Written by: John Eberhart DM Lab Tutorial This tutorial covers how to setup a job for a Multi-Axis Toolpath specifi cally using the Robot. Note: You need to follow
More informationSOLIDWORKS: Lesson III Patterns & Mirrors. UCF Engineering
SOLIDWORKS: Lesson III Patterns & Mirrors UCF Engineering Solidworks Review Last lesson we discussed several more features that can be added to models in order to increase their complexity. We are now
More informationMulti-Axis Surface Machining
CATIA V5 Training Foils Multi-Axis Surface Machining Version 5 Release 19 January 2009 EDU_CAT_EN_MMG_FI_V5R19 1 About this course Objectives of the course Upon completion of this course you will be able
More informationWhat's New in VCarve Pro 8.5
What's New in VCarve Pro 8.5 A quick start guide for VCarve Pro upgraders Copyright Vectric Ltd. Document V.1.0 Contents CONTENTS... 2 OVERVIEW... 3 ENHANCED & EXTENDED DRAWING TOOLS... 4 NEW TOOLPATH
More informationChapter 36. Mastercam Jewelry Box Fixture. A. Sketch Fixture Rectangle. Step 1. If necessary start a new Mastercam file, click New
Mastercam 2017 Chapter 36 Jewelry Box Fixture A. Sketch Fixture Rectangle. Step 1. If necessary start a new Mastercam file, click New (Ctrl-N) on the Quick Access Toolbar QAT. Step 2. On the Wireframe
More informationSOLIDWORKS: Lesson 1 - Basics and Modeling. Introduction to Robotics
SOLIDWORKS: Lesson 1 - Basics and Modeling Fundamentals Introduction to Robotics SolidWorks SolidWorks is a 3D solid modeling package which allows users to develop full solid models in a simulated environment
More informationVisualMILL Getting Started Guide
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
More informationModule 1B: Parallel-Line Flat Pattern Development of Sheet- Metal Folded Model Wrapping the 3D Space of A Truncated Right Prism
Inventor (5) Module 1B: 1B- 1 Module 1B: Parallel-Line Flat Pattern Development of Sheet- Metal Folded Model Wrapping the 3D Space of A Truncated Right Prism In this Module, we will learn how to create
More informationTraining Guide CAM Basic 1 Getting Started with WorkNC
Training Guide CAM Basic 1 Getting Started with WorkNC Table of Contents Table of Contents 1 Training Guide Objectives 1-1 2 Introduction 2-1 2.1 Part Geometry Preparation 2-1 2.2 Starting WorkNC 2-2
More informationVisualCAM 2018 MILL Quick Start Guide. MecSoft Corporation
2 Table of Contents About this Guide 4 1 Useful... Tips 4 2 About... the MILL Module 4 3 Using this... Guide 5 Getting Ready 6 1 Running... VisualCAM 2018 6 2 About... the VisualCAM Display 6 3 Launch...
More informationHow to Make a Sign. Eagle Plasma LLC. Accessing the included step by step.dxf files
Eagle Plasma LLC How to Make a Sign Accessing the included step by step.dxf files The following tutorial is designed to teach beginners, screen by screen, to create a simple sign project. In this lesson
More informationAutodesk Inventor 2019 and Engineering Graphics
Autodesk Inventor 2019 and Engineering Graphics An Integrated Approach Randy H. Shih SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit the
More informationLesson 14 Blends. For Resources go to > click on the Creo Parametric 2.0 Book cover
Lesson 14 Blends Figure 14.1 Cap OBJECTIVES Create a Parallel Blend feature Use the Shell Tool Create a Hole Pattern REFERENCES AND RESOURCES For Resources go to www.cad-resources.com > click on the Creo
More informationLesson 17 Shell, Reorder, and Insert Mode
Lesson 17 Shell, Reorder, and Insert Mode Figure 17.1 Oil Sink OBJECTIVES Master the use of the Shell Tool Reorder features Insert a feature at a specific point in the design order Create a Hole Pattern
More informationMastercam X6 for SolidWorks Toolpaths
Chapter 14 Spinning Top Mastercam X6 for SolidWorks Toolpaths A. Insert Handle in New Assembly. Step 1. Click File Menu > New, click Assembly and OK. Step 2. Click Browse in the Property Manager, Fig.
More informationIntroduction to the Work Coordinate System (WCS) April 2015
Introduction to the Work Coordinate System (WCS) April 2015 Mastercam X9 Introduction to WCS TERMS OF USE Date: April 2015 Copyright 2015 CNC Software, Inc. All rights reserved. Software: Mastercam X9
More informationVectric Cut 3D (Frogmill)
II. Subtractive Rapid Prototyping / VECTRIC CUT 3D (Frogmill) SUBTRACTIVE RAPID PROTOTYPING Vectric Cut 3D (Frogmill) INTERFACE: VECTRIC CUT 3D Model: Frogmill Size: W3050 x D1828 X H419 Material: EPS
More informationCATIA Electrical Space Reservation TABLE OF CONTENTS
TABLE OF CONTENTS Introduction...1 Manual Format...2 Electrical Reservations...3 Equipment Reservations...5 Pathway Reservations...31 Advanced Reservations...49 Reservation Analysis...67 Clash...69 Sectioning...73
More informationBobCAD-CAM FAQ #50: How do I use a rotary 4th axis on a mill?
BobCAD-CAM FAQ #50: How do I use a rotary 4th axis on a mill? Q: I ve read FAQ #46 on how to set up my milling machine. How do I enable 4th axis to actually use it? A: Enabling 4th axis in the machine
More informationSolidCAM Training Course: Turning & Mill-Turn
SolidCAM Training Course: Turning & Mill-Turn imachining 2D & 3D 2.5D Milling HSS HSM Indexial Multi-Sided Simultaneous 5-Axis Turning & Mill-Turn Solid Probe SolidCAM + SolidWorks The Complete Integrated
More informationMulti-Pockets Machining
CATIA V5 Training Foils Multi-Pockets Machining Version 5 Release 19 January 2009 EDU_CAT_EN_MPG_FF_V5R19 1 About this course Objectives of the course Upon completion of this course you will be able to
More informationRevit Architecture 2015 Basics
Revit Architecture 2015 Basics From the Ground Up Elise Moss Authorized Author SDC P U B L I C AT I O N S Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit
More informationExcel 2013 Intermediate
Instructor s Excel 2013 Tutorial 2 - Charts Excel 2013 Intermediate 103-124 Unit 2 - Charts Quick Links Chart Concepts Page EX197 EX199 EX200 Selecting Source Data Pages EX198 EX234 EX237 Creating a Chart
More informationTutorial Second Level
AutoCAD 2018 Tutorial Second Level 3D Modeling Randy H. Shih SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit the following websites to learn
More informationGetting Started with ShowcaseChapter1:
Chapter 1 Getting Started with ShowcaseChapter1: In this chapter, you learn the purpose of Autodesk Showcase, about its interface, and how to import geometry and adjust imported geometry. Objectives After
More informationWhat's New in CAMWorks For Solid Edge-2015
Contents (Click a link below or use the bookmarks on the left) What s New in CAMWorks For Solid Edge 2015-SP0 2 Supported Platforms 2 Resolved CPR s document 2 General... 3 CAMWorks Virtual Machine for
More informationLearning the Pro/ENGINEER Interface
2 Learning the Pro/ENGINEER Interface This chapter introduces the Pro/ENGINEER interface tools: the menus, the dashboards, the selection tools and the viewing controls. As you go through this chapter,
More informationLesson 1 Parametric Modeling Fundamentals
1-1 Lesson 1 Parametric Modeling Fundamentals Create Simple Parametric Models. Understand the Basic Parametric Modeling Process. Create and Profile Rough Sketches. Understand the "Shape before size" approach.
More informationInventor 201. Work Planes, Features & Constraints: Advanced part features and constraints
Work Planes, Features & Constraints: 1. Select the Work Plane feature tool, move the cursor to the rim of the base so that inside and outside edges are highlighted and click once on the bottom rim of the
More informationTRAINING SESSION Q2 2016
There are 8 main topics in this training session which focus on the Sketch tools in IRONCAD. Content Sketch... 2 3D Scene Background Settings... 3 Creating a new empty Sketch... 4 Foam with cut out for
More informationMFG12197 FeatureCAM Hands On Milling, turning and mill turn with Feature Based Machining
MFG12197 FeatureCAM Hands On Milling, turning and mill turn with Feature Based Machining Jeremy Malan Delcam Learning Objectives Learn how to instantly machine parts once their features are defined Learn
More informationIntroduction And Overview ANSYS, Inc. All rights reserved. 1 ANSYS, Inc. Proprietary
Introduction And Overview 2006 ANSYS, Inc. All rights reserved. 1 ANSYS, Inc. Proprietary The ANSYS Workbench represents more than a general purpose engineering tool. It provides a highly integrated engineering
More informationTutorial: Connecting Rod
Tutorial: Connecting Rod Cut2D Disclaimer All CNC machines (routing, engraving, and milling) are potentially dangerous and because Vectric Ltd. has no control over how the software described in this manual
More informationTo familiarize of 3ds Max user interface and adapt a workflow based on preferences of navigating Autodesk 3D Max.
Job No: 01 Duration: 8H Job Title: User interface overview Objective: To familiarize of 3ds Max user interface and adapt a workflow based on preferences of navigating Autodesk 3D Max. Students should be
More informationCATIA V5 Training Foils
CATIA V5 Training Foils Prismatic Machining Version 5 Release 19 January 2009 EDU_CAT_EN_PMG_FF_V5R19 1 About this course Objectives of the course Upon completion of this course you will be able to: -
More informationParametric Modeling Design and Modeling 2011 Project Lead The Way, Inc.
Parametric Modeling Design and Modeling 2011 Project Lead The Way, Inc. 3D Modeling Steps - Sketch Step 1 Sketch Geometry Sketch Geometry Line Sketch Tool 3D Modeling Steps - Constrain Step 1 Sketch Geometry
More informationLesson 5: Board Design Files
5 Lesson 5: Board Design Files Learning Objectives In this lesson you will: Use the Mechanical Symbol Editor to create a mechanical board symbol Use the PCB Design Editor to create a master board design
More informationWhat's New in CAMWorks 2016
Contents (Click a link below or use the bookmarks on the left) About this Version (CAMWorks 2016 SP3)... 2 Supported Platforms 2 Resolved CPR s document 2 About this Version (CAMWorks 2016 SP2.2) 3 Supported
More informationWhat s new in EZCAM Version 18
CAD/CAM w w w. e z c a m. com What s new in EZCAM Version 18 MILL: New Curve Machining Wizard A new Curve Machining Wizard accessible from the Machining menu automates the machining of common part features
More informationSolidWorks Intro Part 1b
SolidWorks Intro Part 1b Dave Touretzky and Susan Finger 1. Create a new part We ll create a CAD model of the 2 ½ D key fob below to make on the laser cutter. Select File New Templates IPSpart If the SolidWorks
More informationIntroduction To Finite Element Analysis
Creating a Part In this part of the tutorial we will introduce you to some basic modelling concepts. If you are already familiar with modelling in Pro Engineer you will find this section very easy. Before
More informationAppendix B: Creating and Analyzing a Simple Model in Abaqus/CAE
Getting Started with Abaqus: Interactive Edition Appendix B: Creating and Analyzing a Simple Model in Abaqus/CAE The following section is a basic tutorial for the experienced Abaqus user. It leads you
More informationME009 Engineering Graphics and Design CAD 1. 1 Create a new part. Click. New Bar. 2 Click the Tutorial tab. 3 Select the Part icon. 4 Click OK.
PART A Reference: SolidWorks CAD Student Guide 2014 2 Lesson 2: Basic Functionality Active Learning Exercises Creating a Basic Part Use SolidWorks to create the box shown at the right. The step-by-step
More informationSOLIDWORKS: Lesson 1 - Basics and Modeling. UCF Engineering
SOLIDWORKS: Lesson 1 - Basics and Modeling Fundamentals UCF Engineering SolidWorks SolidWorks is a 3D solid modeling package which allows users to develop full solid models in a simulated environment for
More informationA cell is highlighted when a thick black border appears around it. Use TAB to move to the next cell to the LEFT. Use SHIFT-TAB to move to the RIGHT.
Instructional Center for Educational Technologies EXCEL 2010 BASICS Things to Know Before You Start The cursor in Excel looks like a plus sign. When you click in a cell, the column and row headings will
More informationAdding Fillet, Shell, and Draft Features
Learn how to: Adding Fillet, Shell, and Draft Features I-DEAS Tutorials: Fundamental Skills add draft features add fillet features use the Ball Corner Fillet option add shell features Before you begin...
More informationINTRODUCTION TO MULTIAXIS TOOLPATHS
INTRODUCTION TO MULTIAXIS TOOLPATHS June 2017 INTRODUCTION TO MULTIAXIS TOOLPATHS June 2017 2017 CNC Software, Inc. All rights reserved. Software: Mastercam 2018 Terms of Use Use of this document is subject
More informationMETBD 110 Hands-On 13 Exploded Assembly
METBD 110 Hands-On 13 Exploded Assembly 1. Open the assembly file created in Hands-On 12. IMPORTANT: For consistent success, use ONLY the method shown in this handout!! 2. Select the View Manager Icon
More informationCADCAM using Powermill
CADCAM using Powermill In this exercise you will create the toolpaths necessary to machine the Cowling model. Create a folder on your h: called Powermill. Inside this create a folder called cowling2009.
More informationSolidWorks 2½D Parts
SolidWorks 2½D Parts IDeATe Laser Micro Part 1b Dave Touretzky and Susan Finger 1. Create a new part In this lab, you ll create a CAD model of the 2 ½ D key fob below to make on the laser cutter. Select
More informationTechnique or Feature Where Introduced
Part 6: Keypad 4 Mirrored features Patterned features First extrusion Rounded corners In the earpiece part, you defined a radial pattern, one that created new instances of a feature at intervals around
More informationPenny Hockey SOLIDWORKS 17 to Mastercam 2017 A. Open File in Mastercam Step 1. If necessary, save your BASE file in SOLIDWORKS.
Mastercam 2017 Chapter 22 Chapter 7 Penny Hockey SOLIDWORKS 17 to Mastercam 2017 A. Open File in Mastercam 2017. Step 1. If necessary, save your BASE file in SOLIDWORKS. Step 2. In Mastercam 2017, click
More informationParametric Modeling. With. Autodesk Inventor. Randy H. Shih. Oregon Institute of Technology SDC PUBLICATIONS
Parametric Modeling With Autodesk Inventor R10 Randy H. Shih Oregon Institute of Technology SDC PUBLICATIONS Schroff Development Corporation www.schroff.com www.schroff-europe.com 2-1 Chapter 2 Parametric
More informationChapter 2 Parametric Modeling Fundamentals
2-1 Chapter 2 Parametric Modeling Fundamentals Create Simple Extruded Solid Models Understand the Basic Parametric Modeling Procedure Create 2-D Sketches Understand the Shape before Size Approach Use the
More information