外文翻译--刀具配置文件和默认工具（设计刀具及刀柄）

科技外文翻译 翻译 名称 VERICUT 翻译原文 系 别 机 电工程 系 专 业 机械设计制造及其自动化 班 级 姓 名 指导教师 外语文献： Session 10- Mill Tool Profiles and a Default Tool（设计刀具及刀柄） This session shows how to use VERICUTs Tool Manager to define a tool assembly (cutter and holder) via profile descriptions. The tool is specified as the default tool via the Override feature. Supplying a tool description in this manner is useful when the tool path file does not contain tool descriptions, or to test alternate tools. This session demonstrates defining a corner rounding mill tool assembly similar to that shown below. The Tool Manager allows tools having almost any shape to be easily defined, as well as provides collision detection between non-cutting portions of the tool and the workpiece. Session Steps: 1. In VERICUT, open the sample mcdblock.usr User file File Open Shortcut=CGTECH_SAMPLES File Name=mcdblock.usr, Open （ 3 坐标立铣） If prompted, respond as follows: Reset cut model? Reset / Save changes? No 2. To improve visibility of tool profiles, rotate the view another 50 degrees X- View Layout Standard 1 View View Orient Increment=50, X- Fit Close 3. Change the position of the program zero (Work Offset G54) View Axes Driven Point Zero Close Setup G-Code Settings； Tables Highlight the table record below Work Offsets Add/Modify Select From/To Location In the From row, Name = Tool In the To row, Name = Stock Offset= -2 0 4.6 Modify Close OK 4. Access the Tool Manager and create a new Tool Library file Setup Tool Manager File New 5. Use the Profile option to describe the corner round form tool shown below (use tool ID 999) Add New Tool Mill ID=999 Description=CORNER RND EM Add Cutter. Profile Add - adds Point X=0.0000 Z=0.0000 Grid Size = .5 Pick point 1 grid right from the tool origin point. (Note that GridSize is .5, also the current cursor position is indicated next to the ZX axes.) Point X=0.5000 Z=0.000 appears in the profile list. Arc Pick arc center point at X=1.0000, Z=0.0000 Pick arc end point at X=1.0000 Z=0.5000 Pick point at X=1.0000 Z=1.0000 Pick point at X=0.5000 Z=1.0000 Pick point at X=0.5000 Z=1.5000 (VERICUT will automatically add point X=0.0000 Z=1.5000 to close the cutter profile on the tool centerline) Flute Length=1.0 OK 6. Describe the 3.0 diameter holder of tool ID 999, then add tool to the library Add Holder. Profile Add - adds X=0.0000 Z=0.0000 Pick point at X=1.0000 Z=0.0000 Pick point at X=1.5000 Z=0.5000 Hint: It might be necessary to Zoom Out or Pan on the grid to see the next point. After picking, use Fit to see the entire profile. Pick point at X=1.5000 Z=3.0000 OK In Tool Display right-click Fit, if necessary. 7. Save the tool in a Tool Library file named special.tls and close the Tool Manager File Save As Shortcut=Working Directory File Name=special.tls, Save File Close, Yes 8. Override tool changes to make Tool Library tool 999 the active tool Setup Toolpath Tool Override=999, OK 9. Cut the model- how many errors were detected? Play to End Select Info Status - Errors=7, the portion of the cutter exceeding the Flute Length generates errors when in contact with the material. Close 10. Use tool holders, then reset and cut the model Setup Motion Select Display Holders in Workpiece View, OK Reset Model , Yes Play to End 11. How many and what type(s) of errors were detected? Select Info Status - Errors=16 Scroll up the Message Area to see the error messages 12. Add tool 998 to the Tool Library to represent the carbide insert shell mill shown below (use the holder from ID 999) Cutter: Setup Tool Manager Add New Tool Mill ID=998 Description=4.0D .25R SHELL MILL Add Cutter. Profile GridSize=.25 Pick point atX=0.0000Z=.2500 Pick point at X=1.5000 Z=0.2500 Arc, ArcDir=CCW Pick arc center point at X=1.7500 Z=0.2500 Pick arc end point at X=1.7500 Z=0.5000 OK Shank: Add Holder. Profile GridSize=.25 Pick point at X=0.0000 Z= -0.2500, then edit Z= -0.2500 = -0.3000 Pick point at X=1.7500 Z= -0.2500, then edit Z= -0.2500 = -0.3000 Pick point at X=1.7500 Z=1.0000 Pick point at X=0.5000 Z=1.0000 Pick point at X=0.5000 Z=1.5000 OK Reference the holder in tool ID 999: Add Holder. Reference Reference ID=999 OK In the view below you can see the non-cutting collision zone under the tool. An error is caused if that portion of the tool assembly removes material. To see this on your tool assembly use Dynamic X (or XY) Rotation. 13. Save the Tool Library, set tool Override to tool 998 , then reset and cut the model File Save File Close Setup Toolpath Tool Override=998, OK Reset Model Play to End Note the error Error, HOLDER removed material . issued by VERICUT when the shell mill plunges into material. Session 10T- Turning Tool Profiles（ cls 文件 刀具设计） This session shows how to use VERICUTs Tool Manager to define a tool assembly (cutter and holder) via profile descriptions. The Tool Manager allows tools having almost any shape to be easily defined. For simple profiles, the points can be sketched directly on the tool manager profile sketcher. For more complex shapes, points can be obtained from a CAD system and entered manually. Session Steps: 1. In VERICUT, open the sample vcturn3.usr User file File Open Shortcut=CGTECH_SAMPLES File Name=vcturn3.usr, Open If prompted, respond as follows: Reset cut model? Reset / Save changes? No 2. Access the Tool Manager and create a new Tool Library file Setup Tool Manager File New 3. Use the Profile option to describe the rough turning tool shown below (use tool ID 1) Add New Tool Turn Description=.06RAD OD CUTTER Add Insert. Profile Add - adds Point Z=0.0000 X=0.0000 Because of the small scale of certain points, it will be easier to edit the added points rather than to set a small enough grid Edit the values for the first point to Z=0.0270 X=1.0000 Add Edit the values for the new point to Z=-0.0590 X=0.0050 Arc Add Edit the values for the new arc to Z=0.0000 X=0.0000 Radius=0.0600 Arc Direction=CCW Add Edit the values for the new point to Z=0.0250 X=-0.0540 Add Edit the values for the new point to Z=1.2500 X=0.5200 Add Edit the values for the new point to Z=1.2500 X=1.0000 Press OK 4. Use the Profile option to describe the finish turning tool ID 2 Add New Tool Turn Description=.03RAD OD CUTTER Add Insert. Profile Add - adds Point Z=0.0000 X=0.0000 Because of the small scale of certain points, it will be easier to edit the added points rather than to set a small enough grid Edit the values for the first point to Z=0.1910 X=1.0000 Add Edit the values for the new point to Z=-0.0290 X=0.0060 Arc Add Edit the values for the new arc to Z=0.0000 X=0.0000 Radius=0.0300 Arc Direction=CCW Add Edit the values for the new point to Z=0.0110 X=-0.0280 Add Edit the values for the new point to Z=1.2500 X=0.4800 Add Edit the values for the new point to Z=1.2500 X=1.0000 Press OK 5. Create a 1/2 dia. drill ID 3 Add New Tool Mill Description=.5DIA. DRILL Add Cutter. Drill Diameter(D)=.5, Drill Point Angle (A)=118, Height=2, Flute Length=1.75 OK 6. Use the Profile option to describe the Inside Diameter rough turning insert tool ID 4 Add New Tool Turn Description=.06RAD ID CUTTER Add Insert. Profile Add - adds Point Z=0.0000 X=0.0000 Because of the small scale of certain points, it will be easier to edit the added points rather than to set a small enough grid Edit the values for the first point to Z=0.0050 X=-0.7500 Add Edit the values for the new point to Z=-0.060 X=-0.0050 Arc Add Edit the values for the new arc to Z=0.0000 X=0.0000 Radius=0.0600 Arc Direction=CW Add Edit the values for the new point to Z=0.0250 X=0.0540 Add Edit the values for the new point to Z=1.0000 X=-0.4000 Add Edit the values for the new point to Z=1.0000 X=-0.7500 Press OK 7. Use the Profile option to describe the Inside Diameter finish turning insert tool ID 5 Add New Tool Turn Description=.03RAD ID CUTTER Add Insert. Profile Add - adds Point Z=0.0000 X=0.0000 Because of the small scale of certain points, it will be easier to edit the added points rather than to set a small enough grid Edit the values for the first point to Z=0.1360 X=-0.7500 Add Edit the values for the new point to Z=-0.029 X=-0.0060 Arc Add Edit the values for the new arc to Z=0.0000 X=0.0000 Radius=0.0300 Arc Direction=CW Add Edit the values for the new point to Z=0.0110 X=0.0280 Add Edit the values for the new point to Z=1.0000 X=-0.3800 Add Edit the values for the new point to Z=1.0000 X=-0.7500 Press OK 8. Create the rough OD grooving insert tool ID 6 Add New Tool Turn Description=.03RAD GROOVING TOOL Add Insert. Profile （ groove insert） Square,Single End Width(W)=.25 Length(L)=1 Thickness=0.1 Radius (R)=.030 C =.175 D =0.75 OK 9. Use the Profile option to describe the Inside Diameter finish grooving insert tool ID 7 Add New Tool Turn ID=7 Description=.03RAD ID GROOVING TOOL Add Insert Profile Add - adds Point Z=0.0000 X=0.0000 Because of the small scale of certain points, it will be easier to edit the added points rather than to set a small enough grid Edit the values for the first point to Z=-.0625 X=-0.7500 Add Edit the values for the new point to Z=-0.0625 X=-0.0300 Arc Add Edit the values for the new arc to Z=-0.0325 X=-0.0300 Radius=0.0300 Arc Direction=CW Add Edit the values for the new point to Z=-0.0325 X=0.0000 Add Edit the values for the new point to Z=0.0325 X=0.0000 Arc Add Edit the values for the new arc to Z=0.0325 X=-0.0300 Radius=0.0300 Arc Direction=CW Add Edit the values for the new point to Z=0.0625 X=-0.0300 Add Edit the values for the new point to Z=0.0625 X=-0.75 Press OK 10. Save the tool in a Tool Library file named turn_profile.tls and close the Tool Manager File Save As Shortcut=Working Directory File Name=turn_profile.tls, Save File Close, Yes 11. Set VERICUT to change tools based on tool number and cut the model Setup Toolpath Tool Change By=Tool Number OK Reset Model Play to End Session 11- Control a Tool Path Simulation（ cls文件） This session shows how to control the simulation of an APT tool path file. Full control is provided over the interactive simulation enabling users to interrupt the simulation at any time by pressing Stop or the Escape key. In addition, VERICUT can be configured to stop tool path processing based on a variety of conditions, including: when errors are detected, after tool changes, after a specified number of cuts have been performed, etc. This session demonstrates practical use of VERICUT simulation controls. Session Steps: 1. Open the rib.usr User file File menu Open Shortcut=CGTECH_SAMPLES File Name=rib.usr, Open If prompted, respond as follows: Reset cut model? Reset / Save changes? No 2. Open the Status window to monitor the machining operation Info Status 3. Configure VERICUT to use only the cutting portion of the tool during the simulation； cutter descriptions are to come from CUTTER records in the tool path file Setup Motion Clear Display Holders in Workpiece View 4. Configure VERICUT to stop after tool changes and when an error is detected Stop At=Tool Change Select Stop At Maximum Errors Stop At Maximum Errors=1 5. Configure VERICUT to issue an error if material is cut using a feedrate of 100 or higher Fast Feed=100 OK 6. Cut the model - why does VERICUT stop? Play to End - tool change with record 20: CUTTER/1.25,.19,0,0,0,0,2.5 (see Status window) 7. Cut the model - why does VERICUT stop? Play to End - Collision with clamp or fixture occurred at record sequence number 134 (see VERICUT window message area) Play to End - Fast feed rate removed material at record sequence number 292 8. Cut the model - why does VERICUT stop? Play to End - tool change with record 577: CUTTER/1.25,.19,0,0,0,0,2.5 (see Status window) Play to End - Fast feed rate removed material at record sequence number 618 9. Cut the model - why does VERICUT stop? Play to End - Fast feed rate removed material at record sequence number 771 Play to End - Fast feed rate removed material at record sequence number 799 10. Cut the model - why does VERICUT stop? Play to End - Fast feed rate removed material at record sequence number 945 11. Cut the model - why does VERICUT stop? Play to End - Collision with clamp or fixture occurred at record sequence number 955 12. Configure VERICUT to continue processing without stopping on errors Setup Motion Clear Stop At Max Errors OK 13. Cut the model - why does VERICUT stop? Play to End - tool change record 1356: CUTTER/1.25,.12,0,0,0,0,2.5 14. Configure VERICUT to continue process the rest of the tool path file without interruptions, then cut the model Setup Motion Stop At= End OK 15. Cut the model - how many errors did VERICUT detect? Play to End - VERICUT detected over 400 errors! Without VERICUT this NC programmer would be looking for a new occupation. 16. Use Feature/History to identify the tool path record responsible for cutting the upper clamp (see below) Analysis X-Caliper Feature/History Tab Click on machine cut in upper clamp - Record Number: 959 17. Review the motions that caused the collision with the clamp Analysis Toolpath Review Click on machine cut in upper clamp The block responsible is highlighted in the upper window； GOTO/12.7461,9.3317,-0.9500,0.0000000,0.0000000,1.0000000 right-mouse click with the cursor on the highlighted line Set Current right-mouse click with the cursor on fourth line above the highlighted line Set Start right-mouse click with the cursor on fourth line below the highlighted line Set End 18. Step (single block) through motions that cut the clamp In the Toolpath Review Window； Rewind (rewinds to the block assigned as start) Single Step Single Step (or pressing the Space Bar will repeat Single Step) Single Step You can also step backward with Step Backward Session 12- Standard vs. FastMill Simulation（ cls文件） This session demonstrates how to process VERICUT faster with different settings and with using FastMill- a verification method that cuts the VERICUT model very quickly without displaying tool motions. The FastMill cut mode is recommended for processing large amounts of tool path data intended for use on 3-axis mill machines where all cutting is on the Z+ side of the workpiece. Session Steps: 1. Open the sample idlerarm.usr User file File Open Shortcut = CGTECH_SAMPLES File Name=idlerarm.usr, Open If prompted, respond as follows: Reset cut model? Reset / Save changes? No 2. Configure VERICUT to stop after cutting the model with 100 cuts each time Play to End is pressed. Setup Motion Stop At=Num of Cuts Enter 100 in the field displayed to the right of the Num of Cuts option OK Configure VERICUT for maximum collision detection A major factor in the accuracy and performance of the VERICUT session is the Cutting Tolerance (ref. File menu Properties: Tolerance tab). This value is similar to specifying an INTOL/OUTTOL when generating a tool path. For maximum collision detection, the fixture holding the workpiece should be modeled in VERICUT, and descriptions of cutting tools should include the non-cutting portions of the tool: shanks and holders. Assuming shanks and holders are defined for the cutting tools in the simulation, using these provides collision detection of the non-cutting portion of the tool assembly against the stock or fixture. 3. Specify .05 mm Cutting Tolerance（影响显示速度、影响显示质量不大） File Properties: Tolerance Tab Cutting Tolerance=.05 OK 4. Configure VERICUT to use tool holders defined for use in the simulation Setup Motion Ensure Display Holders in Workpiece View is selected OK 5. Fit the model in the view, then open the Status and Toolpath windows to monitor the simulation Fit Info Status (relocate window as desired) Info Toolpath (relocate window as desired) 6. Single step to create the model database, then cut the model with 100 cuts Single Step Wait for the BUSY light at the bottom of the VERICUT main window to go out before continuing. Press Play to End - note VERICUT processing time 7. How many errors were detected? Ref. Info Status: Errors field -9 errors Configure VERICUT for maximum collision detection - maximum speed For optimum performance, ensure axes are not displayed (View menu Axes), and close all VERICUT windows that are updated during the simulation (Info menu Status, Info menu Toolpath, etc.). Verification speed can be increased by turning the display of the tool off and reducing the size of the displayed models, since this reduces the amount of graphics activity that occurs in the VERICUT window. This is especially true when simulating 5-axis motions, displaying large cutters, or shanks and holders during the simulation. 8. Close the Status and Toolpath windows, then turn off the display of the tool Status window: Close Toolpath window: Close Setup Motion Tool Display=Off OK 9. Zoom out twice, then refine the display prior to cutting Press Zoom Out 2 times Refine Display 10. Cut the model with another 100 cuts Play to End - note VERICUT processing time Increase the Cutting Tolerance for faster processing Cutting Tolerance may be able to be increased while maintaining sufficient error detection results. Increasing the cutting tolerance increases the speed of the simulation, and requires less system resources and space to store the model database. However, the accuracy of cuts in the model is also reduced. The cutting tolerance also directly affects the results from AUTO-DIFF, OptiPath, holder collisions, Fast Feed errors, dynamic rotation speed, zoom speed, etc. In general, the value entered should reflect the accuracy needed for detecting cut-related errors and analyzing machined model features, such as required for model inspection by AUTO-DIFF, optimizing tool path motions with OptiPath, or exporting cut model data. 11. Reset the VERICUT model, then increase the Cutting Tolerance to .2 mm Reset Model , Yes File Properties: Tolerance tab Cutting Tolerance= .2 OK 12. Single Step once, then cut the model with 100 cuts Single Step Play to End - note VERICUT processing time Were the same quantity of errors detected as with the smaller Cutting Tolerance value? - Yes (ref. Info Status) Make sure to close the Status window when you are finished. Configure VERICUT to process fastest - reduced collision detection When checking for collisions with fixtures and the non-cutting portion of the tool assembly (shank/holder) are not required, remove these from the simulation to gain performance. In short- for optimum tool path verification speed simulate only what is required for the desired level of collision detection. 13. Reset the VERICUT model and blank (remove) the Fixture from the simulation Reset Model , Yes Model Model Definition: Component Attributes tab Select the Fixture model displayed in the VERICUT window Visibility=Blank OK 14. Use only the cutting portion of the tool in the simulation Setup Motion Clear Display Holders in Workpiece View OK 15. Single Step once, then cut the model with 100 cuts Single Step Play to End - note VERICUT processing time Note that since the fixture, shank and holder have been removed from the simulation, collision errors are no longer reported. However, the stock has been cut through where the cutter had previously plunged into the fixture (see below). At this level of verification, the cutter can be re-displayed with a minimal affect to performance. 16. Reset the VERICUT model, then turn on the display of the cutter and configure VERICUT to process the entire tool path file Reset Model , Yes Setup Motion Tool Display=Solid Stop At=End OK 17. Single Step once, then cut the entire model Single Step Play to End - note VERICUT processing time 18. Reset the VERICUT model, then configure VERICUT to process the tool path file without animation Reset Model , Yes Setup Motion No Animation OK 19. Single Step once, then cut the entire model Single Step Play to End - note VERICUT processing time Configure for FastMill verification Speed of verification is dramatically increased by using the FastMill cut mode. This verification method is designed for use with a fixed tool axis in a milling tool paths. 19. Reset the VERICUT model Reset Model , Yes File Properties: Tolerance tab Cutting Tolerance= .05 OK