BobCAD-CAM FAQ #50: How do I use a rotary 4th axis on a mill?
|
|
- Christiana Oliver
- 6 years ago
- Views:
Transcription
1 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 setup file is covered in a cusory way in that FAQ. The proper checkboxes do need to be set in it, but that s only the first step. There are two basic methods to using a 4th axis in BobCAD-CAM - wrapping and indexing. Wrapping refers a continuously moving rotary axis where one axis is dropped in favor of the rotary. The most common axis conversion is Y to A, as A (rotary around the X axis) normally displaces the Y axis by a number of degrees on each move. By contrast, indexing is the practice of rotating a part to a certain angle and then machine it in 3 axes as normal using the X, Y, and Z axes. Both methods have their uses which will be apparent in Steps 3 and 4 of the tutorials to follow. Remember that these are essentially two examples in one: both machine two rectangles using a 4th axis milling method, with both tutorials sharing Steps 1, 2, and 5. The machine configuration and the post processor file must be both edited to enable BobCAD-CAM to produce the rotary axis codes in the final program. The changes here only need to be done once and then saved. When the rotary axis is not used, BobCAD-CAM will not attempt to output any rotary axis coordinates using it at all so the post processor will remain safe for 3 axis (XYZ) use. Step 1: Close BobCAD if it s open. Double click the MillingMachineSetup.exe program normally located in the BobCAD-CAM installation folder, usually C:\Program Files\ BobCAD-CAM\BobCAD-CAM V23\, and the program will start. In the Settings tab, at the bottom, there will be three options the user can choose to enable or disable 4 axis programming in this machine. Choose the option that matches the machine s capabilities best. Click Save at the bottom of the box and then close the program.
2 Step 2: Open the desired (.MillPst) post processor file in any text editor. The file must not have any formatting applied to it, so opening it in a word processor of any kind is not advised. It must contain ASCII text only. For that reason, text editors such as Notepad (in the Accessories category from the Windows Start menu) or Notepad++ (a free, enhanced version of Notepad) are recommended as they are not capable of producing any formatting tags in the saved file. Wordpad is not recommended because it can produce rich text output accidentally. Once the file is open, scroll though it and make the following changes: Place a rotary_xyr_angle and an output_rotary_angle variable into the Start of file Standard (line 2) for indexing: Example: Before: 2. Start of file Standard n,t, M06 n,spindle_on,s n,rapid_move,absolute_coord,work_coord,force_x,xr,force_y,yr n,rapid_move,length_offset,coolant_on After: 2. Start of file Standard n,t, M06 n,spindle_on,s n,rapid_move,absolute_coord,work_coord,force_x,xr,force_y,yr,rotary_xyr_angle n,rapid_move,length_offset,coolant_on output_rotary_angle Place a rotary_xyr_angle in the Tool change (line 3): Before: 3. Tool change n_forced,t, M06 n,s,spindle_on n,rapid_move,absolute_coord,work_coord,force_x,xr,force_y,yr
3 After: 3. Tool change n_forced,t, M06 n,s,spindle_on n,rapid_move,absolute_coord,work_coord,force_x,xr,force_y,yr,rotary_xyr_angle Also place it in the Null tool change (line 4) for indexing: Before: 4. Null tool change n,rapid_move,force_x,xr,force_y,yr After: 4. Null tool change n,rapid_move,force_x,xr,force_y,yr,rotary_xyr_angle For wrapping, place the same rotary_xyr_angle variable in Line move rapid XY (line 52). Before: 52. Line rapid move XY. n,rapid_move,xr,yr After: 52. Line rapid move XY. n,rapid_move,xr,yr,rotary_xyr_angle There is no need to add anything to the feed moves because the Y axis will be converted to A automatically. The axis register (or, letter ) needs to be set at line 690 as shown below: 690. Prefix for X Rotation Move? A That is all that should need to change in the post processor. There could be more added, of course, but these are the bare minimum requirements for 4 axis milling. Save the file and close the text editor. Steps 3 and 4 are the only steps that need to be repeated each time 4th axis is required. There are two versions - one for wrapping and one for indexing. Wrapping in the 4th Axis Step 3: Open BobCAD-CAM V23. The first thing to do is to define the stock to be cylindrical for a 4th axis wrap of the toolpath. The stock dialog will appear.
4 In the Type field, click on the down arrow and choose Cylindrical Stock from the list. The fields in the rest of the dialog will change to those used for that stock type. Set the Stock Diameter to 4 and the Stock Width (X) to 6. The Lower Edge Rotation Angle sets where the rotation starts from the bottom of the stock. If this is set to something other that 0, the 4th axis wrap will begin from the number set here. For example, if the field is set to 45, BobCAD-CAM will assume Y0 on the stock to be the 45 degree mark and the Y value at the circumference to be , i.e., 405 degrees. For simplicity and so that the rotary angles in the code are easier to see, leave this field at 0. The Rotary Axis section permits the user to assign the axis that the rotary table is mounted to. Remember that this will be the cross-axis to the direction of the rotation. For an A axis, the most common setup, it will be the X axis that is rotated around. For B it will be the Y. Click OK on the box to have BobCAD-CAM accept the new stock setup. Once the stock is set up, geometry will need to be drawn in the workspace to machine. Click on Other in the main menu and choose Rectangle. The Rectangle dialog will appear in the Data-CAM Tree Manager. For Width, type in 2 to make the rectangle 2 inches wide. Click on Sharp Corner and choose Enter in the Origin section. From the dropdown box, choose Bottom Left. and set the X parameter to 2. The Height field and the Y field under Origin will need some figuring out. See below before clicking OK to finish drawing the first rectangle. The fields in the Rectangle dialog don t represent degrees around the stock. They represent real distances in Y that have to be found from distances around the circumference of the stock. Usually that will involved finding out how many degrees equal what distance in Y. Some basic algebra is all that s required to figure out how far in Y is how many degrees on the stock. The basic formula is S = Rθ, where θ is the angle in radians. Most prints don t give the angles in radians, so the degrees will have to be converted to radians in order to get a good Y number. y = the Y of the part on the screen R = the radius of the stock θ = the angle of the same measurement on the print in degrees.
5 The new formula that incorporates this is: That s all fine and dandy, but how does this get entered into BobCAD-CAM? It turns out that all of the data entry fields in BobCAD-CAM that take numbers will also accept simple mathematical formulae. This makes getting the correct answer easy. The above formula is the same as this: y=r*(θ*pi()/180) If the radius of the stock is 2 (4 diameter) and θ is 45 degrees, enter this in the Y field: 2*(45*pi()/180) When the text cursor is removed from the field, BobCAD-CAM will work the math problem and display the answer in the field instead of the formula itself. This one evaluates to That means that 45 degrees on the outside of a cylindrical stock with a 4 diameter is roughly inches. Why not just enter ? That answer is simple as well. BobCAD-CAM internally represents π out to 15 decimal places. The is a rounded figure because the field can t display more digits than the system decimal display is set to. However, even though only shows, the field actually contains a number accurate to 15 decimals out. If the rounded figure is just typed in, the angle will be wrong - in this case, This might not be off by a lot in this example, but it isn t 45.0, and if that kind of accuracy is neccesary (on extremely small and accurate machines it can be) then it will simply be wrong. Enter this in the Height field at the top of the box and also in the Y field under Origin: 2*(45*pi()/180) Click OK and BobCAD-CAM will draw a 45-degree-high rectangle 45 degrees from the bottom of the stock in Y. Enter 2*(225*pi()/180) in the Y field under Origin and click OK again to draw a second rectangle 180 degrees from the first. Click Cancel in the Rectangle dialog to end the function. The stock in the Workspace should appear as this illustration. That concludes drawing the geometry for a 4th-Axis wrap.
6 Step 4: Right click on Milling Stock and hover the cursor over Mill 2 Axis. When the fly-out men u appears, choose Pocketing. A new Feature Pocket feature will be inserted into the tree. Under it, right click on Geometry and choose Re/Select. The software will automatically be placed into selection mode. Highlight both rectangles by dragging a box around both of them Click and hold the mouse button and drag the cursor as shown here. When both rectangles are covered, release the mouse button and both will highlight. Right click anywhere in the Workspace and click OK in the menu that will appear. Right click on Pocket under the feature and choose Edit. The Pocket dialog will appear where it is possible to set the parameters for the feature.
7 For the purpose of this example, the parameters for the pocket can all be left at the defaults. Of interest however is the Posting page. When a cylindrical stock is used, the only parameter that will be shown is the Work Offset field. This is because a 4th-Axis wrap and index cannot be combined. In the next part of the example, more parameters will appear in the box. Since the example uses the defaults for the feature, simply click OK. Right click on Pocket once more and choose Compute Toolpath. The result will appear like a simple milled pocket in 3 axes and the difference will not show until the NC code is post processed. To see the result, skip over the 4th axis indexing steps and go straight to Step 5. The computed toolpath will look like this illustration.
8 Indexing on the 4th Axis Step 3: Open BobCAD-CAM V23. The first thing to do is to define the stock. Right click on Milling Stock and choose Edit. The stock dialog will appear. In the Type field, click on the down arrow and make sure that Rectangular Stock from the list. The fields in the rest of the dialog will change to those used for that stock type. The Rotary Axis section permits the user to assign the axis that the rotary table is mounted to. Remember that this will be the cross-axis to the direction of the rotation. For an A axis, the most common setup, it will be the X axis that is rotated around. For B it will be the Y. Click OK on the box to have BobCAD-CAM accept the new stock setup. Setting up the stock for a 4th-Axis index does not necessarily have to be the same as setting it up for a wrapping operation. The stock when indexing can also be rectangular because the machine will cut one feature, then index for the other one. For the sake of the example here it s perfectly acceptable. The geometry can be quite different between the two types. Once the stock is set up, geometry will need to be drawn in the workspace to machine. Click on Other in the main menu and choose Rectangle. The Rectangle dialog will appear in the Data-CAM Tree Manager. This example will also cut two rectangles in the stock 180 degrees apart. The differences are that the Y height of the rectangles will be a real Y size and not converted from degrees, and if the rectangles are the same, only one needs to be drawn. This is true for any shape, not just a rectangle! In the Rectangle dialog, set both the Width and Height fields to 2. Click the Sharp Corner button. In the Origin section, set the drop-down list to Center and place 3 in the X field and 0 in the Y field. Click OK. This will draw a 2x2 rectangle centered directly on the X axis line as shown here.
9 The geometry for both indexed pockets will be shared between them because the indexing angles are handled in the feature parameters and not in the Workspace like the wrapping does. Step 4: Right click on Milling Stock and hover the cursor over Mill 2 Axis. When the fly-out menu appears, choose Pocketing from the list. A new Feature Pocket will be inserted into the tree. Since the rectangle will be cut twice at different indexed angles, two features will be required. Right click on Milling Stock once more and repeat this step to add a second, identical feature to the tree. Right click on Geometry in the first feature and choose Re/Select. The software will automatically be placed into selection mode. Highlight the rectangle by dragging a box around it. Click and hold the mouse button and drag the cursor as shown here. The rectangle should highlight. Right click anywhere in the Workspace and click OK in the menu that will appear. Right click on Geometry in the second feature and repeat the same steps to highlight the rectangle. The geometry will be associated with both features.
10 Right click on Pocket under the first feature and choose Edit. The Pocket dialog will be displayed to allow the user to change the parameters that will be used to machine the feature. For the purpose of this example, the parameters for the pocket can all be left at the defaults. Of interest however is the Posting page. When a rectangle stock is set up, the Output Rotary Angle button and the Rotary Angle field will be available. To index this feature a certain number of degrees, click the bottom and enter in the angle in the box. The first feature in this example will be indexed 45 degrees. Since the example uses the defaults for the feature with the exception of the index angle, simply click OK at the bottom of the dialog. Repeat this step for the second feature. Right click on Pocket under it and choose Edit.
11 The Pocket dialog will again be displayed. In the Posting page is where the features will differ. The first feature was indexed to an angle of 45 degrees. To index this one 180 degrees from that, click on Posting on the left of the box. Click Output Rotary Angle on this feature as well and enter 225 degrees into the Rotary Angle field. Click OK and the setup for both features will be complete. Right click on Pocket under both features and choose Compute Toolpath. Note that when the toolpath is finished from the second feature that the displayed toolpath will be identical. This is because it is identical, and the rotary axis will not be indexed until the NC code is post processed in Step 5.
12 Step 5: The last step to see the NC results for both types of 4th axis code is to post process it. The method for generating the NC code is the same across all feature types and requires only one step. Click on the plus icon next to CAM Part to display the items underneath it. Right click on Milling Tools and choose Post from the menu that will appear. When the NC code is finished, it will be displayed in the Layer-UCS- Post Manager. If wrapping on the 4th axis, see the below code: Note that program has no Y axis except to center the tool over the rotation axis, normally located at Y0. The rest of the program has had the Y axis values replaced with angular A axis instead. When the machine cuts this NC code, it will use simultaneous X and A axis moves but will not use the Y axis. If indexing the 4th axis, see these examples: The example on the left is the first feature with only an index on the rotary axis of 45 degrees. The Y axis is not replaced when indexing. Further in the same program, note that the second feature has an index of 225 degrees around A, matching what was set in the Pocket dialog for each of them.
13 As is shown, the two methods vary greatly in how they deal with the 4th axis, both in how the geometry and features are set up and in the resultant NC code. Both have their uses that are dependent on the part to be cut in the real world. The next step is completely optional requires that the user have Level 2 of the Predator CNC Editor for BobCAD-CAM. Step 6: Right click in the NC code and choose Edit CNC. The Predator CNC Editor will open and automatically load the NC code. Change the stock line in the header from: (SBOX X-.25 Y-.25 Z0. L6.5 W H2.) to: (SCYL S1 X-.25 Y0. Z0. D4.0 L6.5).. as shown here. When the editor is open, change the Template to 4AXVMILL to enable the 4th axis backplotter. Note that the stock type was changed from a box to a cylinder and its orientation set to S1. The width and height (W and H) parameters in the stock setup were removed and replaced with D for diameter. The Y was changed to 0 to center the stock for the backplot on the Y axis. For help with the header and what all of its parameters are, see the Help system in the Predator Editor. When that is done, click on the Backplot icon on the toolbar. Predator will switch to backplot mode.
14 When it is available, click on the Start button on the Backplot toolbar. The backplot will run. When it is finished, the backplot will look like the below. This image has been rotated away from the default view in order to show one of the pockets generated with the 4th axis wrap better. The other is 180 degrees away on the other side of the stock!
3 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 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 / 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 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 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 informationGetting Started Manual Version 24 Mill Standard/Pro January 2011
Getting Started Manual Version 24 Mill Standard/Pro January 2011 Copyright 2011 by BobCAD-CAM Inc., All rights reserved. No part of this work may be reproduced or transmitted in any form or by any means,
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 informationCIMCO Machine Simulation Setup and configuration guide
CIMCO Machine Simulation Setup and configuration guide Contents Introduction to Machine Simulation... 3 1. Geometry Manager... 4 2. Simulation interface... 5 3. Simulation Report... 6 Setting up Machine
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 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 informationDentMILL. Basic Quick Guide. Copyright 2011.Roland DG Corporation R
DentMILL Basic Quick Guide R1-111221 Copyright 2011.Roland DG Corporation Table of Contents User Interface... 2 Workflow from the preparation to exporting data... 3 Basic operation procedures... 4 Step
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 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 informationGetting Started with Alibre CAM. Tutorial 12: Engraving on a Cylinder
Getting Started with Alibre CAM Tutorial 12: Engraving on a Cylinder 344 Introduction This tutorial will illustrate engraving text on a cylinder using a 4 Axis Engraving operation. The stepped instructions
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 informationAutodesk Inventor - Basics Tutorial Exercise 1
Autodesk Inventor - Basics Tutorial Exercise 1 Launch Inventor Professional 2015 1. Start a New part. Depending on how Inventor was installed, using this icon may get you an Inch or Metric file. To be
More informationContents. Toolbar Buttons. Overview of Toolbar Buttons
Contents Help topics are divided into categories represented by the icons below. To select a category with the mouse, point to its icon then click. With the keyboard, press Tab to highlight the category
More informationStep 1: Create A New Photoshop Document
Snowflakes Photo Border In this Photoshop tutorial, we ll learn how to create a simple snowflakes photo border, which can be a fun finishing touch for photos of family and friends during the holidays,
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 informationTutorial 1 Engraved Brass Plate R
Getting Started With Tutorial 1 Engraved Brass Plate R4-090123 Table of Contents What is V-Carving?... 2 What the software allows you to do... 3 What file formats can be used?... 3 Getting Help... 3 Overview
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 informationBobCAD-CAM Version 28 Training Workbook Posting
POSTING After creating all the toolpath to machine your part, the final step of using BobCAD-CAM is to output the NC program and get it to the machine. This topic provides an overview of how to generate
More informationWorking with PhotoVCarve files
Getting Started with Tutorial 4 Intermediate Level Working with PhotoVCarve files VCarve Pro Disclaimer All CNC machines (routing, engraving, and milling) are potentially dangerous and because Vectric
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 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 informationThis document shows you how to set the parameters for the ModuleWorks Material Removal Simulation.
Table of Contents Introduction:... 3 Select Profile:... 4 Tool Table - Create Tool(s)... 5 Tool properties:... 5 Tool Color R/G/B:... 6 Simulation Configurations - create stock... 7 What if plugin is greyed
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 informationTRAINING GUIDE SOLIDS-LESSON-3
TRAINING GUIDE SOLIDS-LESSON-3 Mastercam Training Guide Objectives You will generate the solid model from the existing 2-dimensional geometry. This Lesson covers the following topics: Open an existing
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 informationCNC 8055 MC EXAMPLES MANUAL REF Ref. 0601
EXAMPLES MANUAL Ref. 0601 All rights reserved. No part of this documentation may be copied, transcribed, stored in a data backup system or translated into any language without Fagor Automation's explicit
More informationWorking Model Tutorial for Slider Crank
Notes_02_01 1 of 15 1) Start Working Model 2D Working Model Tutorial for Slider Crank 2) Set display and units Select View then Workspace Check the X,Y Axes and Coordinates boxes and then select Close
More informationSciGraphica. Tutorial Manual - Tutorials 1and 2 Version 0.8.0
SciGraphica Tutorial Manual - Tutorials 1and 2 Version 0.8.0 Copyright (c) 2001 the SciGraphica documentation group Permission is granted to copy, distribute and/or modify this document under the terms
More information2D & 3D CAD SOFTWARE USER MANUAL. AutoQ3D CAD for ipad & iphone
Type to enter text 2D & 3D CAD SOFTWARE USER MANUAL AutoQ3D CAD for ipad & iphone AUTOQ3D TEAM FIRST EDITION AutoQ3D CAD for ipad & iphone 2D / 3D cad software user manual 2015 by AutoQ3D Team. All rights
More informationRelease notes for: NCG CAM v Date: 12/01/2017
NCG CAM Solutions Ltd are pleased to release There are some new features, enhancements to existing features, and some problems fixed. Please note that NCG CAM v15.0 will not install on Window XP, or on
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 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 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 information2D Tutorial. Project Description: Running VisualAnalysis: Setting Up the Project:
2D Tutorial Project Description: This project has been set-up to demonstrate the basic features of VisualAnalysis. You will model and analyze the following two-dimensional frame with a curved glue-laminated
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 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 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 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 informationIntroduction Make a plan with tool Rectangle Measurements Toolbar Enter Return Measurements Toolbar Measure Protractor
Introduction Open SketchUp, and an empty file appears. You are looking at the red-green plane, and the blue axis (vertical) is pointing toward you. By default, you are in the Line tool, as indicated by
More informationEdgecam Getting Started Guide
Edgecam Getting Started Guide Getting Started October 2016 1 Contents Contents... 2 Introduction... 4 About this Guide... 4 Other Resources... 5 What is Edgecam?... 6 Supporting Applications... 7 Installing
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 informationSNOWFLAKES PHOTO BORDER - PHOTOSHOP CS6 / CC
Photo Effects: Snowflakes Photo Border (Photoshop CS6 / CC) SNOWFLAKES PHOTO BORDER - PHOTOSHOP CS6 / CC In this Photoshop tutorial, we ll learn how to create a simple and fun snowflakes photo border,
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 informationUser Interface Guide
User Interface Guide 1 Contents Overview... 3 Tabmenu... 4 Design modes... 4 Tool groups... 5 Design function groups... 5 Main menu... 6 Toolbars... 7 Drawing area... 9 Status bar... 11 Coordinate box...
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 informationLet s Make a Front Panel using FrontCAD
Let s Make a Front Panel using FrontCAD By Jim Patchell FrontCad is meant to be a simple, easy to use CAD program for creating front panel designs and artwork. It is a free, open source program, with the
More informationAUTODESK FUSION 360 Designing a RC Car Body
AUTODESK FUSION 360 Designing a RC Car Body Abstract This project explores how to use the sculpting tools available in Autodesk Fusion 360 Ultimate to design the body of a RC car. John Helfen john.helfen@autodesk.com
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 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 informationPLAY VIDEO. Fences can be any shape from a simple rectangle to a multisided polygon, even a circle.
Chapter Eight Groups PLAY VIDEO INTRODUCTION There will be times when you need to perform the same operation on several elements. Although this can be done by repeating the operation for each individual
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 informationTutorial Tracing and Machining Images
Getting Started With Tutorial Tracing and Machining Images VCarve Pro Disclaimer All CNC machines (routing, engraving, and milling) are potentially dangerous and because Vectric Ltd has no control over
More informationMill - DXF and IPS Programming
Haas Technical Documentation Mill - DXF and IPS Programming Scan code to get the latest version of this document Translation Available INTRODUCTION AutoCAD DXF (Drawing Interchange Format, or Drawing Exchange
More informationStickFont v2.12 User Manual. Copyright 2012 NCPlot Software LLC
StickFont v2.12 User Manual Copyright 2012 NCPlot Software LLC StickFont Manual Table of Contents Welcome... 1 Registering StickFont... 3 Getting Started... 5 Getting Started... 5 Adding text to your
More information2. Open VCarve Pro. Click the Open an existing file button and select your file.
VCarve Pro This software is used for 2D design and calculation of 2D and 2.5D toolpaths for cutting parts on a CNC Router. The software can import 2D designs from other programs such as FormZ, Rhino and
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 informationBasic Electrodes. CimatronE 8.5 Tutorial
Basic Electrodes CimatronE 8.5 Tutorial Table of Contents Electrodes... 1 Attachment... 1 Electrodes Introduction... 1 Attachment... 1 Blank & Electrode UCS... 7 Blank & Electrode UCS... 7 Extension...
More informationLathe - DXF Import and IPS Programming
Haas Technical Documentation Lathe - DXF Import and IPS Programming Scan code to get the latest version of this document Translation Available INTRODUCTION AutoCAD DXF (Drawing Interchange Format, or Drawing
More informationCreating a Title Block & Border Using Chief Architect. Architectural Design & Residential Construction Penncrest High School
Creating a Title Block & Border Using Chief Architect Architectural Design & Residential Construction Penncrest High School 2017-2018 Select New Layout to begin designing your Title Block. Note: Once the
More informationThis tutorial will take you all the steps required to import files into ABAQUS from SolidWorks
ENGN 1750: Advanced Mechanics of Solids ABAQUS CAD INTERFACE TUTORIAL School of Engineering Brown University This tutorial will take you all the steps required to import files into ABAQUS from SolidWorks
More informationTutorial 3 Kitchen Cabinet Door
Getting Started With Tutorial 3 Kitchen Cabinet Door VCarve Pro Disclaimer All CNC machines (routing, engraving, and milling) are potentially dangerous and because Vectric Ltd has no control over how
More informationRoof Wizard. Advanced Software for Roof Modeling and Estimating. Tutorial for Modifying Reports
Roof Wizard Advanced Software for Roof Modeling and Estimating Tutorial for Modifying Reports Document Issue 1.0.0-25th October 1999 Table of Contents TABLE OF CONTENTS... 2 INTRODUCTION... 2 Using this
More informationAdobe Flash CS3 Reference Flash CS3 Application Window
Adobe Flash CS3 Reference Flash CS3 Application Window When you load up Flash CS3 and choose to create a new Flash document, the application window should look something like the screenshot below. Layers
More informationProgramming of Complex machine tools (Mill-Turn) in NX CAM Dr. Tom van t Erve, Director Development - NX CAM
Programming of Complex machine tools (Mill-Turn) in NX CAM Dr. Tom van t Erve, Director Development - NX CAM Restricted Siemens AG 2017 Realize innovation. Mill-Turn / Multi-Function programming with NX
More informationG47 Text Engraving (Group 00) - Mill. Troubleshooting. How it Works. Haas Technical Documentation. Setting 85 is Too High for Shallow Text Engraving
Haas Technical Documentation G47 Text Engraving (Group 00) - Mill Scan code to get the latest version of this document Translation Available Troubleshooting Setting 85 is Too High for Shallow Text Engraving
More informationWhat s new in EZ-CAM 2016 (version 23)
What s new in EZ-CAM 2016 (version 23) MILL Pro 64-bit Edition is Ready: EZ-MILL Pro 2016 comes with a 64-bit edition which now makes it possible to import and create 3D toolpaths for very large and complicated
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 informationHow to Make Graphs with Excel 2007
Appendix A How to Make Graphs with Excel 2007 A.1 Introduction This is a quick-and-dirty tutorial to teach you the basics of graph creation and formatting in Microsoft Excel. Many of the tasks that you
More informationHow To Capture Screen Shots
What Is FastStone Capture? FastStone Capture is a program that can be used to capture screen images that you want to place in a document, a brochure, an e-mail message, a slide show and for lots of other
More informationKEYCREATOR 3D Direct Modeling Software
KeyCreator Lesson KC5107 Graft The Graft Function is a powerful partner to the Prune Function that we used earlier. You will typically use the Graft Function immediately after performing a pruning operation
More informationActivLearning. Training Series. addendum
ActivLearning Training Series addendum ActivInspire 1.6 Update Promethean continues to evolve the ActivInspire software to maximize functionality, simplify lesson preparation, and enable you to deliver
More informationEXCEL BASICS: MICROSOFT OFFICE 2007
EXCEL BASICS: MICROSOFT OFFICE 2007 GETTING STARTED PAGE 02 Prerequisites What You Will Learn USING MICROSOFT EXCEL PAGE 03 Opening Microsoft Excel Microsoft Excel Features Keyboard Review Pointer Shapes
More informationL E S S O N 2 Background
Flight, Naperville Central High School, Naperville, Ill. No hard hat needed in the InDesign work area Once you learn the concepts of good page design, and you learn how to use InDesign, you are limited
More informationExcel 2003 Tutorial II
This tutorial was adapted from a tutorial by see its complete version at http://www.fgcu.edu/support/office2000/excel/index.html Excel 2003 Tutorial II Charts Chart Wizard Chart toolbar Resizing a chart
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 informationFAGOR AUTOMATION MC TRAINING MANUAL
FAGOR AUTOMATION MC TRAINING MANUAL ACER MC TRAINING MANUAL 8 holes 1/2" depth grid pattern R0.125 1.5 6 unit: inch R0.25 4 1.25 2 2.675 1/2" depth rectangular pocket 1/2" depth circular pocket R0.75 8
More informationQuickTutor. An Introductory SilverScreen Modeling Tutorial. Solid Modeler
QuickTutor An Introductory SilverScreen Modeling Tutorial Solid Modeler TM Copyright Copyright 2005 by Schroff Development Corporation, Shawnee-Mission, Kansas, United States of America. All rights reserved.
More informationADOBE TRAINING CS6 PHOTOSHOP BASICS: EDITING PHOTOS & WORKING WITH TEXT - 1
ADOBE TRAINING CS6 PHOTOSHOP BASICS: EDITING PHOTOS & WORKING WITH TEXT Photoshop is the leading professional software for editing and adjusting photos, images and other graphic projects. It is a very
More informationAutodesk Fusion 360: Model. Overview. Modeling techniques in Fusion 360
Overview Modeling techniques in Fusion 360 Modeling in Fusion 360 is quite a different experience from how you would model in conventional history-based CAD software. Some users have expressed that it
More informationSummer Packet 7 th into 8 th grade. Name. Integer Operations = 2. (-7)(6)(-4) = = = = 6.
Integer Operations Name Adding Integers If the signs are the same, add the numbers and keep the sign. 7 + 9 = 16 - + -6 = -8 If the signs are different, find the difference between the numbers and keep
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 informationAn Approach to Content Creation for Trainz
An Approach to Content Creation for Trainz Paul Hobbs Part 6 GMax Basics (Updates and sample files available from http://www.44090digitalmodels.de) Page 1 of 18 Version 3 Index Foreward... 3 The Interface...
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 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 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 informationContents. Foreword. Examples of GeoGebra Applet Construction 1 A Straight Line Graph... 1 A Quadratic Graph... 6 The Scalar Product...
Contents Foreword ii Examples of GeoGebra Applet Construction 1 A Straight Line Graph............................... 1 A Quadratic Graph................................. 6 The Scalar Product.................................
More informationMach4 CNC Controller Screen Editing Guide Version 1.0
Mach4 CNC Controller Screen Editing Guide Version 1.0 1 Copyright 2014 Newfangled Solutions, Artsoft USA, All Rights Reserved The following are registered trademarks of Microsoft Corporation: Microsoft,
More informationDigital City: Introduction to 3D modeling
Digital City: Introduction to 3D modeling Weixuan Li, 2017 PART I: Install SketchUp and Introduction 1. Download SketchUp Download SketchUp from their official website: https://www.sketchup.com Go to the
More informationEXPERIENCE THE POWER. THE NEW BobCAD-CAM V31. We have upgraded the entire customer experience to be more intuitive, modern and efficient.
01 EXPERIENCE THE POWER V31 Whether you re a leading manufacturer or just starting out, BobCAD-CAM has the features, training & support you need to machine better parts FASTER and EASIER, for LESS. THE
More informationFigure 1: NC > 2 Axis menu > Options
Click To See: How to Use Online Documents SURFCAM Online Documents J 685)&$0Ã5HIHUHQFHÃ0DQXDO 7 &21),*85$7,21722/6 7.1 INTRODUCTION SURFCAM s default configuration parameters are contained in the SURFCAM.INI
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 informationDeskCNC setup and operation manual
DeskCNC setup and operation manual This document explains how to install, setup and cut foam shapes using DeskCNC 4 axis foam cutting software. The document will go through a step by step process of how
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 informationWhat's New in BobCAD-CAM V29
Introduction Release Date: August 31, 2016 The release of BobCAD-CAM V29 brings with it, the most powerful, versatile Lathe module in the history of the BobCAD-CAM software family. The Development team
More informationPolar coordinate interpolation function G12.1
Polar coordinate interpolation function G12.1 On a Turning Center that is equipped with a rotary axis (C-axis), interpolation between the linear axis X and the rotary axis C is possible by use of the G12.1-function.
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 information