Đây là hướng dẫn sử dụng phần mềm Mastercam-X4. hướng dẫn có các hình ảnh và ví dụ cụ thể
4 & 5 Axis Mill Training TutorialsTo order more books:Call 1-800-529-5517 orVisit www.inhousesolutions.com orContact your Mastercam Dealer Mastercam X Training Tutorials – 4 & 5 Axis Mill ApplicationsRevised Date: July 8, 2009Copyright © 1984 - 2009 In-House Solutions Inc. - All rights reserved.Software: Mastercam X MillAuthors: Mariana LendelISBN: 978-1-926566-41-2NoticeIn-House Solutions Inc. reserves the right to make improvements to this manual at any time and withoutnotice.Disclaimer Of All Warranties And LiabilityIn-House Solutions Inc. makes no warranties, either express or implied, with respect to this manual orwith respect to the software described in this manual, its quality, performance, merchantability, or fitnessfor any particular purpose. In-House Solutions Inc. manual is sold or licensed "as is." The entire risk as toits quality and performance is with the buyer. Should the manual prove defective following its purchase,the buyer (and not In-House Solutions Inc., its distributor, or its retailer) assumes the entire cost of allnecessary servicing, repair, of correction and any incidental or consequential damages. In no event will In-House Solutions Inc. be liable for direct, indirect, or consequential damages resulting from any defect inthe manual, even if In-House Solutions Inc. has been advised of the possibility of such damages. Somejurisdictions do not allow the exclusion or limitation of implied warranties or liability for incidental orconsequential damages, so the above limitation or exclusion may not apply to you.CopyrightsThis manual is protected under the copyright laws of Canada and the United States. All rights arereserved. This document may not, in whole or part, be copied, photocopied, reproduced, translated orreduced to any electronic medium or machine readable form without prior consent, in writing, from In-House Solutions Inc.TrademarksMastercam is a registered trademark of CNC Software, Inc.Microsoft, the Microsoft logo, MS, and MS-DOS are registered trademarks of Microsoft Corporation;Mastercam Verify is created in conjunction with Sirius Systems Corporation; Windows 95, and WindowsNT; Windows XP are registered trademarks of Microsoft Corporation. TABLE OF CONTENTSGetting Started .A-1Axis Substitution, Rotary Axis Positioning and Transform-Rotate Tutorial . 1-1Axis Substitution To Create A Cylindrical and A Conical Helix Tutorial .2-1Axis Substitution, Rolldie C-Hook Tutorial .3-1Chuck Indexing Tutorial 4-1Rotary4-Axis Toolpath and Axial 4ax Tutorial 5-1Curve 5-Axis Tutorial .6-1Drill 5-Axis and Circle Mill 5-Axis Tutorial 7-1Swarf 5-Axis With Wall Defined By Using 2 Contours Tutorial 8-1Flow 5-Axis Tutorial 9-1Multisurface 5-Axis Tutorial 10-1Port 5-Axis Tutorial . 11-1General Notes . B-1 TUTORIAL SERIES FORTUTORIAL 4CHUCK INDEXING TUTORIAL 4/5-Axis TUTORIAL 4Objectives:The Student will design a 3-dimensional drawing by:Creating the 2D geometry in the Right Side view.Creating the 3D geometry using translate command.Creating circles knowing the diameter and the center location.Changing the view of the part for better visualisation.The Student will create a 2-dimensional milling toolpath in different Tplanes consisting of:Using View Manager to select the Tplane for each face.Create an operation for each face using the same work offset (G54).Facing one flat surfaces.Facing the other two flat surfaces using Transform-Rotate toolpath.Drilling the two holes.Removing the material inside of one groove using contour toolpath.Machine the second groove using Transform-Rotate toolpath.The Student will check the toolpath using Mastercam’s Verify verification module by:Defining a 3-dimensional block, the size of the workpiece.Running the Verify function to machine the part on the screen.Page 4-2 4/5-AxisPage 4-3TUTORIAL 4 4/5-Axis TUTORIAL 4GEOMETRY CREATIONSTEP 1: CREATE THE 2D GEOMETRY IN THE RIGHT SIDE VIEWOption 1 The geometry file, Tutorial4_geometry.zip, can be downloaded fromwww.emastercam.com/filesThe finish part, Tutorial4_finish.zip including the toolpaths, is also provided on the same locationwww.emastercam.com/filesOption 2-Create the geometry using the following instructions:Create the 2D profile in the Right side view:Create/Arc/ Create Circle Center Point and set parameters to:Diameter = 5.0;Center OriginCreate/Line/ Create Line Endpoint and set parameters to:Specify an endpoint = OriginLine length = 2.45Angle = 165 deg.;Create/Line/ Create Line Perpendicular and set parameters to:Select line, arc or spline; Select the existing lineSketch a point; Select the Endpoint of the existing line opposite the origin.Select which line to keep; Select the line above the existing one.Repeat the steps to select the other perpendicular line below the first line that we created.Delete the first lineEdit/Join entitiesSelect the two colinear lines; Press enter to finish the commandEdit/ Trim/Break/ Trim/Break/ExtendEnable divide and select the arc left to the line and the two ends of the line.Select these lines andthe arc hereXform/ Xform RotateSelect the line; Enable Copy and set # to 1; Rotation angle 90 degXform/ Xform RotateSelect the rotated line; Enable Copy and set # to 1; Rotation angle 105 degPage 4-4 4/5-AxisEdit/ Trim/Break/ Trim/Break/ExtendEnable divide and select the two arcs one below andthe other one to the right of the rotated lines.Select Entity A hereTUTORIAL 4Create/Line/ Create Line Endpoint and setparameters to:Specify an endpoint = OriginLine length = 2.5Angle = 120 deg.;Create/Line/ Create Line Parallel and set parameters to:Select a line; Select the 120 deg lineSelect the point to place a parallel line through; Pick a point above the line; enter the distance 0.25Select the flip buton several times until you make both parallel lines (above and below the 120 deg. line)Edit/ Trim/Break/ Trim/Break/ExtendEnable Break in the ribbon bar.Select an entity to break; Select the first parallel line end that is further away from the origin.Enable the length button in the Ribbon bar and enter -0.25Repeat the command to break at 0.25 distance the other parallel line that we created in the previousstepDelete the center line and the parallel lines closest to the origin.Select these entitiesCreate/Line/ Create Line Endpoint and set parameters to:Select the endpoints of the parallel lines left to close the slot.Edit/ Trim/Break/ Trim/Break/ExtendEnable Divide in the ribbon bar.Select the arc between the two parallel lines.Edit/ Trim/Break/ Trim/Break/ExtendEnable Trim 2 entities in the ribbon bar.Select the entities at the top corners of the slot.Xform/ Xform RotateSelect the three lines of the slot; Enable Copy and set # to 1; Rotation angle 180 degEdit/ Trim/Break/ Trim/Break/ExtendEnable Divide in the ribbon bar.Page 4-5 [...]... Tut4_Rotary axis indexing.mcx Page 4-6 4/5-Axis TUTORIAL 4 TOOLPATH CREATION STEP 2: DEFINE THE STOCK To display the Toolpaths Manager press Alt + O Set the construction plane to Top Plane If a machine definition is already selected see Tutorial # 2 page 2-4 to learn how to change it Otherwise follow the next step Machine Type Mill Select Mill 4-AXIS VMC.MMD Page 4-7 4/5-Axis TUTORIAL 4 Select the plus... set to Drill/Counterbore Page 4-2 6 4/5-Axis TUTORIAL 4 Select the Linking Parameters and change the parameters as shown in the following screenshot Enable Tip comp Make the Breakthrough amount 0 Select the OK button to exit Page 4-2 7 4/5-Axis TUTORIAL 4 The part should appear as shown STEP 7: MACHINE THE GROOVE AT THE 120 DEGREES ANGLE Toolpath Preview: Page 4-2 8 4/5-Axis TUTORIAL 4 7.1 Set both Cplane... location of the chained geometry Select the OK button from the Facing parameter screen Page 4-1 6 4/5-Axis TUTORIAL 4 Your part should appear as shown Press Alt+T to remove the toolpath display STEP 4: FACE THE FLAT AT 255 DEGREES ANGLE USING ROTATE-TRANSFORM TOOLPATH Toolpath Preview: Toolpaths Transform Page 4-1 7 4/5-Axis TUTORIAL 4 Enable Rotate and the Method should be set to Tool plane to be able to... Rotation view and select the arrow button Page 4-1 8 4/5-Axis TUTORIAL 4 Select the Right Side View Select the OK button to exit View Selection Select the OK button to exit Transform Operation Parameters Your part should appear as shown Press Alt + T to remove the toolpath display Page 4-1 9 4/5-Axis TUTORIAL 4 STEP 5: FACE THE FLAT AT 0 DEGREES USING ROTATE-TRANSFORM TOOLPATH Toolpath Preview: Toolpaths... 4-1 3 4/5-Axis TUTORIAL 4 3.3 Face the plane Toolpaths Face Select the OK button to accept the NC name Enable C-plane in the Chaining dialog box [Select OK to use the defined stock or select chain 1]:Select the chain as shown Select the chain here Select the OK button to exit Chaining From Tool page, click on the Select library tool button Select the Filter button in the Tool Selection Page 4-1 4 4/5-Axis... the Transform operation as shown below Page 4-2 0 4/5-Axis TUTORIAL 4 Select the Rotate tab and change the parameters as shown Make sure that Rotation view is enabled and set to Right Side Otherwise follow the previous step to select the Rotation view Select the OK button to exit Transform Operation Parameters Your part should appear as shown Page 4-2 1 4/5-Axis TUTORIAL 4 STEP 6: DRILL THE 0.375 DIAMETER... to define a new plane by rotating the Top plane -9 0 degrees Press simultaneous Alt &T to disable the toolpath display if needed Note that pressing Alt + T again will display the toolpath of selected operations Select Planes in the Status Bar Select Top plane Select Planes in the Status Bar Select Rotate planes Page 4-2 2 4/5-Axis TUTORIAL 4 Enter About X -9 0 degrees The axis orientation of the plane should... axis (horizontal machining centers) Page 4-1 0 4/5-Axis TUTORIAL 4 Toolpath Preview: 3.1 Create the new view at 165 degrees Select WCS in the Status Bar Select View Manager Select Geometry button Select the second line here [Select a flat entity, 2 lines, or, 3 points]: Select the two lines as shown in the following picture Select the first line here Page 4-1 1 4/5-Axis TUTORIAL 4 The axis should be orientated... Properties Page 4-9 4/5-Axis TUTORIAL 4 STEP 3: FACE THE FLAT SURFACE AT 165 DEGREES Tool Planes and Axis Orientation The tool plane (Tplane) is the plane in which the tool approaches and machines the part The Tplane represents the CNC machine’s coordinate system (XY axis and origin) This is the cutting plane for a toolpath, typically normal to the tool axis The Rotary axis for our part is A-axis The axis... select the None button to disable all tools Select the Drill tool type as shown (upper right corner) In the Tool Diameter field click the pull-down arrow and select Equal Enter the Tool Diameter value to 0.375 Select the OK button to exit Tool List Filter Page 4-2 5 4/5-Axis TUTORIAL 4 Make sure that the tool is selected (highlighted) in the Tool Selection screen Select the OK button to exit the Tool Selection . 2009Copyright © 1984 - 2009 In-House Solutions Inc. - All rights reserved.Software: Mastercam X MillAuthors: Mariana LendelISBN: 97 8-1 -9 2656 6-4 1-2 NoticeIn-House Solutions. Tutorial..................................................................................................... 6-1 Drill 5-Axis and Circle Mill 5-Axis Tutorial ...................................................................... 7-1 Swarf 5-Axis With Wall