Presentation is loading. Please wait.

Presentation is loading. Please wait.

Copyright DASSAULT SYSTEMES 20021 Prismatic Machining CATIA Training Foils Version 5 Release 9 June 2002 EDU-CAT-E-PMG-FF-V5R9.

Similar presentations


Presentation on theme: "Copyright DASSAULT SYSTEMES 20021 Prismatic Machining CATIA Training Foils Version 5 Release 9 June 2002 EDU-CAT-E-PMG-FF-V5R9."— Presentation transcript:

1 Copyright DASSAULT SYSTEMES Prismatic Machining CATIA Training Foils Version 5 Release 9 June 2002 EDU-CAT-E-PMG-FF-V5R9

2 Copyright DASSAULT SYSTEMES Course Presentation Objectives of the course In this course you will see how to define and manage NC programs to machine parts designed in 3D Wireframe or Solid geometry with 2.5 Axis machining operations. Targeted audience Manufacturing users knowing how to work with CATIA V5 Parts Prerequisites CATIA V5 Fundamentals 1 day

3 Copyright DASSAULT SYSTEMES Table of Contents 1.Differences between PG1 & PMG 2.Introduction to Prismatic Machining 3.Milling operations 4.Facing operations 5.NC Macro definition 6.Pocketing operations 7.Profile Contouring operations 8.Prismatic Rework Area 9.Curve following operations 10.Point to point operations

4 Copyright DASSAULT SYSTEMES « Prismatic Machining P1 » Product (PG1) « Prismatic Machining P1 »: the Entry product for Small and Medium Entreprise Product Content: Basically « Prismatic Machining P2 » Product (PMG) EXCEPT: ‘Between 2 Curves’, ‘ Between Curve & Surface’ in Contouring Machining Operation ‘Auto Draft Angle’ capability in Pocketing Machining Operation Support of Machining Processes for Axial Operations ‘Sectioning’ capability for Drive Curve Selection Connection to V4 Tool Database Material Removal Simulation (Photo & Video modes) Support of DELMIA VNC Machine-Tools 2D Rework area Let ’s see now all about PMG Product…

5 Copyright DASSAULT SYSTEMES In this lesson, you will learn basics of Prismatic Machining Skillet 1 Accessing the Workbench Skillet 2 Exploring the user interface Skillet 3 Create a milling operation Introduction to Prismatic Machining

6 Copyright DASSAULT SYSTEMES Anywhere from 1- Start menu or 2- File menu + New or 3- Workbench Icon See Tools + Customize + Start menu for the content of this Welcome Box Blank Manufacturing CATProcess to start Accessing the workbench Many different ways…

7 Copyright DASSAULT SYSTEMES Prismatic Machining Product Prismatic Machining Workbench Workbench user interface Pocketing Operation Creation Facing Operation Creation Profile Contouring Operation Creation Curve Following Operation Creation Point To Point Operation Creation Prismatic Rework Area

8 Copyright DASSAULT SYSTEMES Click on the milling operation icon to be created 2 The new Operation is created after the current one The Operation dialog box appears to edit it Define the Operation geometry and parameters in the dialog box Let ’s see now the User interface Replay the Tool Path Confirm Operation creation The Operation is created in the PPR tree with a default tool. This capability can be removed by customizing the NC Manufacturing options. At any time click on « ? » To have more information on the option Create a milling operation

9 Copyright DASSAULT SYSTEMES Facing operation You will learn how to create a Facing Operation A Facing Operation consists in cutting a constant offset of material on a planar area without inner domains The Planar area is delimited only with soft boundaries The tool axis is normal to the planar area The material will be removed in one or several cuts along the radial and axial directions The area is machined with Inward Helical, Back & Forth or One Way tool path style

10 Copyright DASSAULT SYSTEMES Define operation parameters using the 5 tab pages Strategy tab page Geometry tab page Tool tab page Feeds & Speeds tab page Macros tab page 11 Enter the Name of the Operation. (Optional because a default name is given by the system ‘Type_Of_Operation.X’) 1 2 Enter a line of comment (Optional) 3 Replay and / or Simulate the operation tool path 4 Facing operation : Presentation

11 Copyright DASSAULT SYSTEMES The 3 Tool path styles for a Facing Operation are : Inward HelicalBack & ForthOne Way Inward Helical : The tool starts from a point outside the area and follows inward paths parallel to the boundary Back & Forth : The tool alternatively machines in one direction then in the opposite direction One Way : The tool always machines in the same direction To change the machining direction select the arrow Facing operation : Strategy Tab Page 1/5

12 Copyright DASSAULT SYSTEMES Facing operation : Strategy Tab Page 2/5 Machining Strategy parameters Direction of Cut Climb : The front of the advancing tool cuts into the material first Conventional : The back of the advancing tool cuts into material first Machining Tolerance Value of the maximum allowable distance between the theoretical toolpath and the toolpath computed Fixture Accuracy Local machining tolerance for fixtures Type of Contour Circular : The tool pivots around the corner point, following a contour whose radius is equal to the tool radius Angular : The tool does not remain in contact with the corner point, following a contour comprised of 2 line segments Optimized : The tool follows a contour derived from the corner that is continuous in tangency Forced Circular : The tool follows a near-circular contour comprised of line segment Compensation : Number of the tool compensation used if this one is already defined on the tool Climb MillingConventional Milling Optimized Angular Circular

13 Copyright DASSAULT SYSTEMES Facing operation : Strategy Tab Page 3/5 Radial Strategy parameters End of Path INOUT Tool Side Approach Clearance Tool Diameter Ratio The distance between two paths will respect a tool diameter ratio recovery Overhang = 100% Overhang = 50% Overhang = 0% Overhang : Extension of the tool path in percentage of the tool diameter End of Path = IN Maximum Distance A maximum distance will be used to compute the distance between two paths Stepover Ratio The distance between two paths will respect a stepover ratio (10% stepover = 90% tool diameter)

14 Copyright DASSAULT SYSTEMES Bottom Finish Pass parameters Finish Pass Mode : No Finish Pass : No special finish pass At Bottom : Indicates that a finish pass is to be generated on the bottom plane of the Facing Operation. A thickness value must be given for that pass The Finishing Feed rate will be used to cut the material on the finish pass Axial Strategy parameters Axial Strategy Mode : Maximum Depth of Cut : Maximum depth of cut in axial direction between 2 levels Number of Levels : Number of levels to machine Number of Levels Without Top : To define the amount of material to cut in the axial direction without Top Plane definition Facing operation : Strategy Tab Page 4/5

15 Copyright DASSAULT SYSTEMES Facing Operation : Strategy Tab Page 5/5 High Speed milling parameters Limit Angle : Lowest angle between two segments that needs cornering Corner parameters This button activates high speed milling Corner radius Extra segment overlap Corner on Finish Pass parameters Corner radius Limit Angle : Lowest angle between two segments that needs cornerisation Transition radius Transition angle Transition length Transition parameters (only Inward or Outward)

16 Copyright DASSAULT SYSTEMES This Tab Page includes a Sensitive Icon dialog box that allows the selection of : Bottom Plane Top Plane (only for Multi-Level operations) Drive Elements Check Elements (Optional) Start Point (Optional) Offsets can be applied on the Top Plane, Bottom Plane, Contour and Check Elements (Double click on the value) Facing operation : Geometry Tab Page The system automatically computes the bounding rectangle of the part along Machining Direction in B&F

17 Copyright DASSAULT SYSTEMES Enter the Name of the Tool. Enter a line of comment (Optional) 5 Use the 2D Viewer to modify the parameters of the tool. The 2D Viewer is updated with the new values 1 Select the tool type available for the current operation 4 Specify a tool number that does not already exist Click More to expand the dialog box to access all tool ’s parameters such as Geometry, Technology, Feeds & Speeds and Compensation Facing operation : Tool Tab Page to search for a tool in the current document, a Catalog or external database

18 Copyright DASSAULT SYSTEMES Define the Feedrate values for Approach Feedrate : This feedrate is used by default during approach motion Machining Feedrate : This feedrate is used during Machining motion Retract Feedrate : This feedrate is used by default during retract motion Finishing Feedrate : This feedrate is used as Machining Feedrate for the Bottom Finish Pass According the unit Linear (mm/mn) or Angular (mm/turn) Define the Spindle Speed value according the unit Linear (m/mn) or Angular (turn/mn) You can exclude Spindle speed information from the NC data output by deactivating the checkbox Spindle Output 2 Facing operation : Feeds & Speeds Tab Page 3 Select Quality (Rough, Finish, Either) and compute it, according to value defined on the tool You can select « automatic compute » then feedrate and spindle speed will be automatically compute from tooling Feeds and Speeds

19 Copyright DASSAULT SYSTEMES Exercise Presentation And now practice on the step 2 of the Master Exercise, to learn how to: Create a Facing Operation.

20 Copyright DASSAULT SYSTEMES NC Macro Definition You will learn how to create NC Macros For all operations, macro parameters are accessible via this tab page

21 Copyright DASSAULT SYSTEMES different types of macros are available : Approach, Retract, Return between levels, Return in a level, Linking, Return to finish pass, Clearance Return in a level Linking Retract Return between level Approach Return to finish pass Clearance (next slide) 7 different types of macro…

22 Copyright DASSAULT SYSTEMES The Clearance Macro Each of the following macros : - Return between level - Return in a level - Return to finish pass - Linking is divided in two motions : Approach and Retract Between those two motions, the system computes a default tool path. If you want this transition tool path to be customized, activate Clearance Macro You can cornerize clearance via option beside Clearance Macro Clearance Corner radius Retract motionApproach motion Corner radius Default toolpath

23 Copyright DASSAULT SYSTEMES Depending on the type of macro you have selected, different type of pre-defined macros are available : Tangent, normal, axial Circular, axial Axial Ramping For ApproachFor Retract Not available Pre-defined macros

24 Copyright DASSAULT SYSTEMES Tool box to create your own macro Tangent Circular Ramping Axial motion up to a plane Erase You can create an great number of different macros combining these basic paths in any order. Copy Approach or Retract macro on all approach or retract motions of the other macros Macros Tool Box Normal Axial Insert PP word Distance along a line (to select) Tool axis motion (to select) Motion to a point (to select) 13 7 Motion perpendicular to a plane

25 Copyright DASSAULT SYSTEMES Insert a PP word on a point of the macro. Cross symbols localize the possible points to insert the PP word To insert a PP word, you can also press right mouse button on the cross and select « PP word list » Apply this Approach or Retract motion to all Return and Linking macros in the operation (only available on Approach macro and Retract macro) PP Table access capability: Possibility to select Major/Minor words and pre-defined syntaxes Create your own macro

26 Copyright DASSAULT SYSTEMES To locally modify a feedrate or spindle speed in the macro, press right mouse button on a element and select « feedrate » -To modify geometrical parameters of a macro, double- click on it. Depending on the feedrate selected, the element takes a different color : Yellow : Approach White : Local Green: Machining Blue : Retract Red : Rapid Modify parameters on your macro

27 Copyright DASSAULT SYSTEMES NC Manufacturing Courses Organization When you give a course, you need to respect the following order for each Product Now Insert here Replay and Video Simulation Fonctionnalities (NC Infrastructure Lesson 4) and come back to explain the other Machining Operations Switch to Replay Lesson Click here

28 Copyright DASSAULT SYSTEMES Pocketing Operation You will learn how to create a Pocketing Operation A Pocketing Operation is used to machine a pocket with or without inner domains. The external boundary is made of Hard/Soft elements The islands are limited only with Hard boundaries. The material will be removed in one or several levels of cut. The tool starts and finishes machining at the top of the pocket. The pocket is machined with Outward and Inward helical or Back & Forth tool path style.

29 Copyright DASSAULT SYSTEMES Enter the Name of the Operation. (Optional because a default name is given by the system ‘Type_Of_Operation.X’) 1 2 Enter a line of comment (Optional) Replay and / or Simulate the operation tool path 4 Before replaying or creating the operation, “Preview” checks that all parameters are coherent 5 Define operation parameters using the 5 tab pages Strategy tab page Geometry tab page Tool tab page Feeds & Speeds tab page Macros tab page 3 Pocketing Operation : Presentation

30 Copyright DASSAULT SYSTEMES Tool path styles for a Pocketing Operation are : Outward Helical Outward Helical : The tool starts from the center and follows outward paths parallel to the boundary avoiding islands Inward Helical Inward Helical : The tool starts from the contour and follows inward paths parallel to the boundary avoiding islands Pocketing Operation : Strategy Tab Page 1/8 Back & Forth Back & Forth : The tool alternatively machines in one direction then in opposite direction and follows the machining direction To change the machining or progression direction select either arrow Tool Axis must be normal to bottom plane

31 Copyright DASSAULT SYSTEMES Pocketing Operation : Strategy Tab Page 2/8 Machining Strategy parameters Climb Milling Conventional Milling Direction of Cut Climb : The front of the advancing tool cuts into the material first Conventional : The back of the advancing tool cuts into material first Machining Tolerance Value of the maximum allowable distance between the theoretical tool path and the computed tool path Fixture Accuracy Local machining tolerance for fixtures Compensation Number of the tool compensation used if this one is already defined on the tool

32 Copyright DASSAULT SYSTEMES Pocketing Operation : Strategy Tab Page 3/8 Radial Strategy Maximum Distance A maximum distance will be used to compute the distance between two paths Overhang : Extension of the tool path in percentage of the tool diameter. Only available for open pockets. Overhang of 100% is useful to machine properly this kind of geometry : Overhang = 100% Overhang = 50% Overhang = 0% Tool Diameter Ratio The distance between two paths will respect a Tool diameter overlap ratio Stepover Ratio The distance between two paths will respect a stepover ratio (10% stepover = 90% tool diameter)

33 Copyright DASSAULT SYSTEMES Pocketing Operation : Strategy Tab Page 4/8 Center path overlap Tool diameter ratio used for the overlapping of the first center path in Inward Helical only Truncated transition path Used with Back & Forth strategy Allows to modify progression direction Scallop pass Used with Back & Forth strategy Allow to remove scallop on contour Driven by a ratio of tool diameter Radial Strategy

34 Copyright DASSAULT SYSTEMES Pocketing Operation : Strategy Tab Page 5/8 Pocket Navigation option Always stay on bottom : the tool will never jump from one area to another Inward / outward mixture : The direction of cut is allowed to change at every new area machined. the Climb / Conventional direction of cut setting is given in the first strategy tab page. Inward / outward mixture option is available only if Always stay on bottom option is selected. If you select none of the Pocket Navigation options, the tool may jump over walls. Multi Domain Capability : If the tool diameter is too large to stay on the bottom, the tool will machine one by one the different areas.

35 Copyright DASSAULT SYSTEMES Pocketing Operation : Strategy Tab Page 6/8 Axial Strategy Max depth of cut You specify the distance between two levels Number of levels You specify the number of levels from the bottom to the top Nb of levels without top You specify the bottom, the number of levels and the depth of cut. Finish Pass mode At last level : activate a radial finish pass only at last level At each level : Activate a radial finish pass at each level At bottom : Activate a last level pass to machine the bottom Complete : Activate a radial finish pass at each level and a last level pass to machine the bottom. Automatic draft angle Incremental increase of thickness on flank Breakthrough Only in soft bottom pocket You give an offset in order to specify a virtual bottom

36 Copyright DASSAULT SYSTEMES Pocketing Operation : Strategy Tab Page 7/8 Special Finish Pass : Spring Pass : Duplicate last finish pass to compensate the spring of the tool Avoid scallop on bottom : Modify distance between pass on last level to avoid scallop on bottom. Finish Pass parameters Side finish thickness Side finish thickness on bottom Bottom finish thickness The Finishing Feedrate will be used to cut the material on the finish pass

37 Copyright DASSAULT SYSTEMES Pocketing Operation : Strategy Tab Page 8/8 High Speed milling parameters Limit Angle : Lowest angle between two segments that needs cornering Corner parameters This button activates high speed milling strategy Corner radius Extra segment overlap Corner on Finish Pass parameters Corner radius Limit Angle : Lowest angle between two segments that needs cornerisation Transition radius Transition angle Transition length Transition parameters (only Inward or Outward)

38 Copyright DASSAULT SYSTEMES This Tab Page includes a Sensitive Icon dialog box that allows the selection of : 1. Bottom Plane 2. Top Plane (only in Multi-Levels strategy case) 3. Drive Elements 4. Check Elements 5. Islands 6. Start point 7. End point Via contextual menu, offsets can be applied on the Top Plane, Bottom Plane, Contour, Islands, Check Elements Soft and Hard Boundary Pocketing Operation : Geometry Tab Page 1/ To remove the bottom click on : Island Hard Boundary Soft Boundary Offset=contour+island Offset=contour+hard boundary Offset=soft boundary

39 Copyright DASSAULT SYSTEMES Pocketing Operation : Geometry Tab Page 2/3 To machine an open pocket click on : Soft boundaries will be automatically detected when selecting bottom (dotted lines) If you need to add more soft boundaries, select them after bottom selection To allow Start point definition outside the machining domain click on : In this case you can specify : A clearance Or select an edge and give a clearance Or select a point

40 Copyright DASSAULT SYSTEMES You can select a Start Point (1) and an End Point (2) as preferential start and end positions Pocketing Operation : Geometry Tab Page 3/3 Note that you can select a point or an edge as Start/End Point in Outward/Inward strategy. In case of selecting an edge, the point will be choosen near the middle of this edge (according to selected geometry, overhang, offset …) Start point will always be respected except if a ramping motion is defined in the macro (the start point will be near the selection) Note that End point is only available in Outward Strategy and it might be modified (according to selected geometry and computed toolpath) Note that you can specify a Start Point outside the machining domain for open pocket (see previous slide) 1 2

41 Copyright DASSAULT SYSTEMES Exercise Presentation And now practice on the step 3 of the Master Exercise, to learn how to: Create a Pocketing Operation. Create a pocketing operation with respect to the island Create a pocketing operation with a spring pass for finishing Machine Pocket with a High speed milling operation Machine Pocket 5 as an open pocket Pocket 1 Pocket 2 Pocket 3 Pocket 4 Pocket 5

42 Copyright DASSAULT SYSTEMES Contouring operation You will learn how to create a Contouring Operation A profile contouring Operation consists in cutting material along a hard boundary. The hard boundary may be open, closed or discontinuous. Along axial direction, the material will be removed from the top to the bottom in one or several cuts. Along radial direction, the material will be removed by approaching the hard boundary in one or several parallel paths The area is machined in One-way or in Zig-zag style.

43 Copyright DASSAULT SYSTEMES Enter the Name of the Operation. (Optional because a default name is given by the system ‘Type_Of_Operation.X’) 1 2 Enter a line of comment (Optional) Replay and / or Simulate the operation tool path 4 Define operation parameters using the 5 tab pages Strategy tab page Geometry tab page Tool tab page Feeds & Speeds tab page Macros tab page 3 Profile Contouring Operation : Presentation

44 Copyright DASSAULT SYSTEMES The two Tool path styles for a Profile Contouring Operation are : Zig - zag : The tool alternatively machines in one direction then in opposite direction One Way : The tool machines always in the same direction Profile Contouring Operation : Strategy Tab Page 1/5

45 Copyright DASSAULT SYSTEMES Profile Contouring Operation : Strategy Tab Page 2/5 Type of Contour Circular : The tool pivots around the corner point, following a contour whose radius is equal to the tool radius Angular : The tool does not remain in contact with the corner point, following a contour comprised of line segments Optimized : The tool follows a contour derived from the corner that is continuous in tangent Forced Circular : The tool follows a near-circular contour comprised of line segment Machining Strategy parameters 1/2 Climb Milling Conventional Milling Direction of Cut Climb : The front of the advancing tool cuts into the material first Conventional : The back of the advancing tool cuts into material first Machining Tolerance Value of the maximum allowable distance between the theoretical tool path and computed tool path Fixture Accuracy Local machining tolerance for fixtures Optimized Angular Circular

46 Copyright DASSAULT SYSTEMES Profile Contouring Operation : Strategy Tab Page 3/5 Close tool path Option to machine the complete contour of a closed area. Percentage overlap when « close tool path » is active, this is the overlap at the end of the tool path expressed as a percentage of the tool diameter Machining Strategy parameters 2/2 Output type : standard In the generated code, the toolpath is defined by the tool tip trajectory Output type : cutter profile In the generated code, the toolpath is defined by the contact point trajectory Compensation Number of the tool compensation. It must be a number available on the tool used for the operation Compensation application mode You have to choose if compensation is applied on the tool output or guiding point Tool position ON guide This option is equivalent to put an offset of tool radius on contour.

47 Copyright DASSAULT SYSTEMES Profile Contouring Operation : Strategy Tab Page 4/5 Stepover Max depth of cut You specify the distance between two levels Number of levels You specify the number of levels from the bottom to the top Number of levels without top you specify the bottom, the number of levels and the depth of cut. Radial Strategy Distance between paths : You enter directly the distance between two radial paths Number of paths : You enter directly the number of radial paths Radial firstAxial first Sequencing Axial Strategy Breakthrough Only in soft bottom You give an offset in order to specify a virtual bottom Automatic draft angle Incremental increase of thickness on flank Overhang for rework areas See next chapter on Prismatic Rework area

48 Copyright DASSAULT SYSTEMES Profile Contouring Operation : Strategy Tab Page 5/5 Side Finish Pass mode Spring Pass Duplicate last finish pass to compensate the spring of the tool The Finishing Feedrate will be used to cut the material on the Side and Bottom finish passes At last level : activate a radial finish pass only at last level At each level : Activate a radial finish pass at each level Bottom Finish Pass mode At bottom : Specify the thickness used for the bottom finishing

49 Copyright DASSAULT SYSTEMES This Tab Page includes a Sensitive Icon dialog box that allows the selection of : Bottom Plane Top Plane (for Multi-Levels operations only) Drive Elements Discontinuous contours is possible, allowing to machine several contours in one single Operation thus providing better support of thin wall finishing Check Elements (Optional) Limiting Element (Optional) Offsets can be applied on the Top Plane, Bottom Plane, Contour Check and Limiting Elements To remove the bottom, click on To start (or end) out of the part, click on with MB right Profile Contouring Operation : Geometry Tab Page 1/

50 Copyright DASSAULT SYSTEMES To reach 3 other contouring operations right click : - contouring between two curves : - contouring between curve and surfaces-By flank contouring between two curves & between curve and surfaces: Relimitation and offset options Profile Contouring Operation : Geometry Tab Page 2/2

51 Copyright DASSAULT SYSTEMES Exercise Presentation And now practice on the step 4 of the Master Exercise, to learn how to: Create a Contouring Operations. - contouring on open pocket - contouring a flank of the part while avoiding a fixture - contouring the inside of a pocket

52 Copyright DASSAULT SYSTEMES Prismatic Rework Area You will learn how to use 2D Rework area This functionnality allow you to find non machined area from a previous operation or manual parameters. Thus you can use this area with a pocketing or a profile contouring operation.

53 Copyright DASSAULT SYSTEMES Enter the Name of the Operation. (Optional because a default name is given by the system ‘Type_Of_Operation.X’) 1 2 Select the operation which will be used as input to compute the non machined area or Enter manually geometry and tool parameters then compute the non machined area 3 Prismatic Rework : Presentation 1 2 3

54 Copyright DASSAULT SYSTEMES Insert a Pocketing Operation 1 2 Select the area previously computed Prismatic Rework with Pocketing All geometry and associated parameters are selected You can choose corner and/or channel rework 3 Rework area is also available in « Mfg View » Sort by machinable features 4 4

55 Copyright DASSAULT SYSTEMES Insert a Profile Contouring Operation 1 2 Select the area previously computed Prismatic Rework with Profile Contouring 3 Rework area is also available in « Mfg View » Sort by machinable features All geometry and associated parameters are selected Only corner rework is available with Profile Contouring

56 Copyright DASSAULT SYSTEMES Point to point operation You will learn how to create a Point To Point Operation A Point To Point Operation consists in moving the tool from a selected point to another selected point at a given Machining Feedrate. This operation allow you to define sequential motions of points.

57 Copyright DASSAULT SYSTEMES Enter the Name of the Operation. (Optional because a default name is given by the system ‘Type_Of_Operation.X’) 1 2 Enter a line of comment (Optional) Replay and / or Simulate the operation tool path (See dedicated Job Aid ‘Replay a Tool Path’) 4 Define operation parameters using the 4 tab pages Strategy tab page Tool tab page Feeds & Speeds tab page Macros tab page 3 Point To Point Operation : Presentation

58 Copyright DASSAULT SYSTEMES Point To Point Operation : Strategy Tab Page Select tool compensation number from among those defined on the tool used by the Operation The Tool Axis can be specified by selecting the tool Axis. An Offset along Tool Axis can be applied on all the selected points Strategy is divided into Motions and Strategy Select “Goto point” or “Goto position” icon to enter points. Thus you can move/delete/edit properties of selected points

59 Copyright DASSAULT SYSTEMES Exercise Presentation And now practice on step 5 of the Master Exercise, to learn how to : Create a Point to Point Operation.

60 Copyright DASSAULT SYSTEMES Curve Following Operation You will learn how to create a Curve Following Operation A Curve Following Operation consists in machining a part by following a curve with the tool tip. The material will be removed in one or several level of cuts. The tool starts and finishes machining at the extremities of the curve. The area is machined in One-way or in Zig-zag style.

61 Copyright DASSAULT SYSTEMES Curve Following Operation : Presentation 11 Enter the Name of the Operation. (Optional because a default name is given by the system ‘Type_Of_Operation.X’) 1 2 Enter a line of comment (Optional) Replay and / or Simulate the operation tool path 4 Define operation parameters using the 5 tab pages Strategy tab page Geometry tab page Tool tab page Feeds & Speeds tab page Macros tab page

62 Copyright DASSAULT SYSTEMES Curve Following Operation : Strategy Tab Page 1/2 The available Tool path styles for a Curve Following Operation are: Zig - zag : The tool alternatively machines in one direction then in opposite direction One Way : The tool machines always in the same direction To change the tool axis orientation select the Axis representation

63 Copyright DASSAULT SYSTEMES Curve Following Operation : Strategy Tab Page 2/2 Machining Tolerance Value of the maximum allowable distance between the theoretical tool path and computed tool path Fixture Accuracy Local machining tolerance for fixtures Max depth of cut You specify the distance between two levels Number of levels You specify the number of levels from the bottom to the top Axial StrategyMachining Strategy parameters

64 Copyright DASSAULT SYSTEMES Curve Following Operation : Geometry Tab Page 2 1 This Tab Page includes a Sensitive Icon dialog box that allows the selection of : Guiding Element Check Elements (Optional) Offsets (axial) can be applied on Check Elements and Driving Curve

65 Copyright DASSAULT SYSTEMES Exercise Presentation And now practice on step 6 of the Master Exercise, to learn how to: Create a Curve Following Operation.

66 Copyright DASSAULT SYSTEMES NC Manufacturing Courses Organization When you give a course, you need to respect the following order for each Product Now Continue With NC Infrastructure Course (Lesson 5) up to the end Switch to NC infrastructure Lesson 5 Click here


Download ppt "Copyright DASSAULT SYSTEMES 20021 Prismatic Machining CATIA Training Foils Version 5 Release 9 June 2002 EDU-CAT-E-PMG-FF-V5R9."

Similar presentations


Ads by Google