外文翻译=配置模拟G代码的刀具加工轨迹=5000字符

外文原文 Session 25- Configure to Simulate a G-Code Milling Tool Path This session shows how to configure VERICUT for processing a G-Code tool path file . The sample 3axtltip.mcd G-Code tool path file to be simulated has been programmed to drive the tool tip. The tool path is destined to be run on a 3-axis vertical mill similar to the one shown below. A Mazak Mazatrol M-32 CNC milling control interprets the G-codes for this milling machine. Sample 3-axis vertical mill: The Machine Simulation system provides many sample machine and control configurations which users can choose to simulate their NC machining environment. This session demonstrates how to create a User file for a specific NC machine and control combination for simulating the G-Code tool path. The basic requirements for G-Code tool path simulation are the same as for any other tool path type (stock, tool path, and cutting tool descriptions), however, there are additional considerations: Tool descriptions are not typically present in a G-Code tool path file. A Tool Library is typically used to supply cutter descriptions. VERICUT must have knowledge of the NC machine kinematics & control capabilities, as well as job-related data such as: the initial machine location prior to G-Code processing, offset register values entered at the NC control, etc. With the Machine Simulation system, this information is stored as follows: - kinematics properties of an NC machine are stored in a Machine file - information about the capabilities and methods of how an NC control interprets G-Codes is stored in a Control file - job-related data, as well as the names of the above mentioned Machine and Control files are stored the User file Session Steps: 1. Start a new VERICUT session in Inch units File Properties Default Units=Inch, OK File New Session If prompted, respond as follows: Reset cut model? Yes / Save changes? No 2. Add a 5 x 6 x 2 inch block stock model View Axes Select Model and Driven Point Zero Close Model Model Definition: Model tab Type=Block Length(X)=5, Width(Y)=6, Height(Z)=2 Add Fit Cancel 3. Specify the sample 3axtltip.mcd G-Code tool path file to be simulated Setup Toolpath Toolpath Type=G-Code Data Add Shortcut=CGTECH_SAMPLES File Name=3axtltip.mcd, OK OK 4. From the CGTech library, use the g3vmtt.mch generic 3-axis mill with mazm32.ctl Mazak Mazatrol M-32 CNC milling control Setup Machine Open Shortcut=CGTECH_LIBRARY File Name=g3vmtt.mch, Open Setup Control Open Shortcut=CGTECH_LIBRARY File Name=mazm32.ctl, Open 5. Specify that tool tip programming is used for this tool path Setup G-Code Settings: Settings tab Programming Method=Tool Tip OK 6. Orient the tool path origin to the top left corner of the stock, as shown below Setup required for tool path 3axtltip.mcd: Setup G-Code Settings; Tables tab Add/Modify Table Name = Program Zero Select From/To Locations From, Name = Tool To, Name = Stock Click on the selection icon on the To row Click top left corner. (value should be 0 0 2) Add Close OK Reset The 3axtltip.mcd tool path contains T words which specify the tool number of the cutters used to machine the part. The 3axtltip.tls Tool Library file contains cutter descriptions that correspond to the tool numbers referenced in this G-Code tool path. 7. Configure VERICUT to use cutting tools stored in the sample 3axtltip.tls Tool Library file Setup Tool Manager File Open Shortcut=CGTECH_SAMPLES File Name=3axtltip.tls, Open Tool Manager: File Close, Yes 8. Cut the model Play to End Session 26- Use a Tool List and Master Tool Library This session shows how to use VERICUTs Tool Manager to define cutter shapes and store them in a master Tool Library file for easy access by everyone. Master tool libraries typically have tool identification (ID) values that differ from the T numbers in the G-code tool path file. A tool list is used to cross-reference（交叉引用） G-code tool change blocks to access tool descriptions stored in the Tool Library file. This feature makes it possible to define a single Tool Library file containing all available tool descriptions, and have all users use this file as a source of tool descriptions for VERICUT. Session Steps: 1. In VERICUT, open the bars.usr User file File Open Shortcut=CGTECH_SAMPLES File Name=bars.usr, Open If prompted, respond as follows: Reset cut model? Reset / Save changes? No File Properties Default Units=Millimeter, OK This assures that the units for a new Tool Library are set to millimeter. 2. Access the Tool Manager and create a new Tool Library file Setup Tool Manager File New 3. Add tool ID 101: 15 dia., 150 ht., 118 deg. drill Add New Tool Mill ID=101 Description=15D 150H DRL Ensure Units=Millimeter Right-click Cutter Drill Diameter (D)=15, Drill Point Angle (A)=118, Height (H)=150 OK (the drill is displayed) 4. Add tool ID 201: 25 dia., 150 height, flat bottom endmill Right-click New Tool Mill ID=201 Description=25D 150H FEM Right-click Cutter Flat Bottom End Mill Diameter (D)=25, Height (H)=150 OK 5. Add tool ID 501: 60 dia., 3 cr., 25 ht. end mill Right-click New Tool Mill ID=501 Description=60D 3R 25H EM Right-click Cutter Bull Nose End Mill Diameter (D)=60, Corner Radius (R)=3, Height (H)=25 OK 6. Save the tools in a Tool Library file named master.tls and close the Tool Manager File Save As Shortcut=Working Directory File Name=master.tls, Save File Close, Yes 7. Build a tool list that cross-references G-code tool numbers to tools in the Tool Library as follows: T1M6 uses ID101, T2M6 uses ID201, T3M6 uses ID501 Setup Toolpath Tool Change By=List Use Tool list Make sure Prompt for Optipath is NOT selected Build Tool List - scans the tool path and generates the following tool list based on tool pocket numbers: With Event 1 (T1M6) selected, enter Cutter ID=101 Select Event 2 (T2M6), Cutter ID=201 Select Event 3 (T3M6), Cutter ID=501 OK, OK 8. Cut the model Reset Model Play to End Session 27- Use OptiPath Manager to Create an OptiPath Library This session shows how to use the OptiPath Manager function to define the OptiPath records required to optimize cutting in H13 tool steel (approx. 200 HB). Once defined, the OptiPath records are stored in an OptiPath Library file. The following session (Optimize Tool Path Feedrates via OptiPath tool list method) demonstrates how to configure VERICUT for optimizing a G-code tool path file, including using the OptiPath Library created during this session. Session Steps: Define OptiPath Records 1. Start from a new Inch User file File Properties Default Units=Inch, OK File New Session If prompted, respond as follows: Reset cut model? Yes / Save changes? No 2. Access the OptiPath Manager OptiPath Manager Optimization settings will be established differently to accommodate the different cutting performed by each tool (see below). The part will be cut on a 3ax vertical mill in a rigid setup. Cutters Used by Tool Path op_mold.mcd: Tool 1 (T1): Description: .625 dia. 4 flute carbide flat end mill Operation: planar milling not to exceed .5 depth, 1200 RPM Feedrates for this tool will be established from a known successful cutting condition: assume the cutter is successful cutting full width in .3 depth passes at 8 IPM feedrate. The feedrate used to enter material should not be more than 8 IPM. Tool 2 (T2): Description: .75 dia. 4 flute carbide ball end mill Operation: semi-finish profile milling (kellering/lacing)（仿行铣） The light cuts performed by this tool will be optimized by constant volume combined with chip thickness. This method of optimization varies feedrates based on the volume of material removed. Assume volume removal rates are not known for this tool; OptiPath record will be copied from the Ingersoll OptiPath Library. Configure Optimization Settings for the .625 dia. Flat End Mill: 3. Add and identify a new OptiPath record for the .625 dia. flat end mill as follows: Stock material to be cut= H13 Tool Steel Machine that will cut the part= 3ax Mill Tool description= .625D 1.50H FEM, Carbide #Teeth= 4 Add Click in the field under the Material heading, type:H13 Tool Steel Under Machine type: 3ax Mill Under Tool Description type:.625D 1.50H FEM, Carbide Under # Teeth type:4 OptiPath Cutter Shape Flat Bottom End Mill Diameter(D)=.625, Height(H)=1.5 OK 4. Configure a known successful cutting condition for this cutter Axial Depth=0.3(Value can be adjusted with the slide bar or typed) Radial Width=.625 Feed Per Minute=8 Spindle Speed=1200 Select Spindle Speed (when selected, optimized spindle speeds are supplied along with corresponding optimized feedrates) Under these conditions, Volume Removal rate is 1.5 cubic in. per minute. 5. Select to optimize by Constant Volume, use 150 IPM feedrate for cuts in air Select Volume Removal Clear Air Cut Feed Rate: Default Enter Air Cut Feed Rate=150 6. On the Optimization Settings tab, specify settings for the following conditions: Settings tab Add More Cuts Clear all Default checkboxes (4 places) Minimum Feedrate Change=3 (minimum change required to output a different optimized feedrate) Clean-up Feedrate=85 (spring pass) Minimum Cut Feedrate=1 (okay as is) Maximum Cut Feedrate=80 Circle Feedrate=Optimize (okay as is) 7. Set an Entry Feedrate to enter material with 8 IPM feedrate (to begin .1 before contacting material - till .1 cut into material), then apply the optimization settings Entry/Exit tab Entry Feedrate=Feed/Minute: 8 Clearance Distance= 0.1 Cut Distance=0.1 Apply, enters all the above settings to the selected Optipath record 8. Test how optimization will be performed under various cutting conditions 调整优化结果 Testing ensures that optimization will be performed as expected. If unsatisfactory results are experienced, adjust optimization settings and re-test until satisfied. Feed/Speed Tab Enter various cut depths and widths, then observe the optimized Feed per Minute and Feed per Tooth values Example: Axial Depth=.1 = (Feed per Minute= 24) Radial Width=.5 = (Feed per Minute= 30) Configure Optimization Settings for the .750 dia. Ball End Mill: 9. Add a new OptiPath record for the .750 dia. ball end mill, edit the new record name as follows: Stock material to be cut= H13 Tool Steel (same as previous record) Machine that will cut the part= 3ax Mill (same as previous record) Tool description= .750D 1.50H BEM, Carbide #Teeth= 4 Add Tool Description = .750D 1.50H BEM, Carbide Teeth= 4 OptiPath Cutter Shape Ball Nose End Mill Diameter(D)= .75, Height(H)=1.5 OK 10. Configure a known successful cutting condition for this cutter Clear Volume Removal checkbox Axial Depth=1(Value can be adjusted with the slide bar or typed) Radial Width=.125 Feed Per Minute=12 Spindle Speed=1200 Select Spindle Speed 11. Configure OptiPath settings for this tool to be the same as for the previous tool, except optimize by Constant Volume and Constant Chip Thickness (continue to add more cuts when needed) Select Volume Removal (1.5 cubic inch/minute) Select Chip Thickness (.0019 chip/tooth load) Settings Tab Notice that all the settings defined for the first record have been carried when adding this record. Apply 12. Test how optimization will be performed under various cutting conditions 13. After satisfactory test results, apply any changes made, then save an OptiPath Library file named optipath.olb Apply OptiPath Manager: File Save As Shortcut=Working Directory File Name=optipath.olb, Save This session demonstrated how to create an Optipath Library that can be used to optimize cutting by different tools. Session 28- Optimize Feed Rates via Tool Library Method This session shows how to configure VERICUT for optimizing a G-code tool path file by adding references to OptiPath records to tools stored in a previously defined Tool Library file. The sample G-code tool path file to be optimized uses 2 cutting tools: T1, T2. The tools have been defined and stored in the Tool Library file that will receive the OptiPath record references. The demonstration shows how to link cutting tools in the Tool Library file with OptiPath records in an OptiPath Library file, as well as optimize the tool path file motions and review the optimized tool path file. See also: Session 29- Optimize Feed Rates via OptiPath Tool List Method Session Steps: Optimize an Inch Tool Path Cutters used by sample tool path op_mold.mcd: 1. In VERICUT, open the sample op_mold.usr User file File Open Shortcut=CGTECH_SAMPLES File Name=op_mold.usr, Open If prompted, respond as follows: Reset cut model? Reset / Save changes? No 2. Use OptiPath Control to reference the optipath.olb OptiPath Library file, and indicate cutting H13 tool steel on the 3-axis mill machine OptiPath Control: Settings tab OptiPath Library, Browse Shortcut=Working Directory File name=optipath.olb, Open, (If optipath.olb is not available use CGTech sample op_mold.olb) Material= H13 tool Steel Machine=3 ax mill OK 3. Use the Tool Manager to link OptiPath records to cutting tools used by the tool path file, then save a new optipath.tls Tool Library file Update Tool 1 OptiPath properties: Setup Tool Manager In the tool list, select: 1 - .625D 1.50H FEM Click in the field under OP Description to highlight the record Click again to display the pull down list, select .625D 1.50H FEM, Carbide (4) Note: The window may require stretching to see all information. Update Tool 2 OptiPath properties: In the tool list, select: 2 - .750D 1.50H BEM Click in the field under OP Description to highlight the record Click again to display the pull down list, select .750D 1.50H BEM, Carbide (4) 4. Save a new optipath.tls Tool Library file Tool Manager window: File Save As Shortcut=Working Directory File Name=optipath.tls, Save File Close, Yes 5. Use OptiPath Control to create an optimized tool path named op_mold.opti OptiPath Control Optimized File=*.opti (OK as is. The * wildcard will be replaced with the op_mold tool path base file name to create an optimized tool path named op_mold.opti.) OptiPath Mode =On OK (Note the red OptiPath light on the VERICUT main window indicates optimization is on) 6. Open the Status window and configure to also show optimized feed rates and cutting time, as well as the Tool Use Graph Info Status Configure Ensure OP Time and OP Feedrate are selected Select Tool Use, Time interval=60 (minutes) OK During processing the Feedrate field displays the programmed feed rates while the OP Feedrate field displays the optimized feed rates. 7. Cut the model Play to End 8. Open the Log file window and review the OptiPath Summary, then close the Log file window Info VERICUT Log Scroll to bottom of file and search for the OptiPath Summary header. Sample Log File OptiPath Summary: Close the Log file window Session 29- Optimize Feed Rates via OptiPath Tool List Method This session shows how to configure VERICUT for optimizing a G-Code tool path file by building a Tool List to reference OptiPath records stored in a previously defined OptiPath Library file. The sample G-Code tool path file to be optimized uses 2 cutting tools: T1, T2. The tools have been defined and stored in a Tool Library file. The demonstration shows how to link cutting tools in the tool path file with OptiPath records in an OptiPath Library file, as well as optimize the tool path file motions and review the optimized tool path file. See also: Session 28- Optimize Feed Rates via Tool Library Method Session Steps: Optimize an Inch Tool Path Cutters used by sample tool path op_mold.mcd: 1. In VERICUT, open the sample op_mold.usr User file File Open Shortcut=CGTECH_SAMPLES File Name=op_mold.usr, Open If prompted, respond as follows: Reset cut model? Reset / Save changes? No 2. Use OptiPath Control to reference the optipath.olb OptiPath Library file, and indicate cutting H13 tool steel on the 3-axis mill machine OptiPath Control: Settings tab OptiPath Library, Browse Shortcut=Working Directory File name=optipath.olb, Open (If optipath.olb is not available use CGTech sample op_mold.olb) Material=H13 tool Steel Machine=3 ax Mill OK 3. Use a tool list to link OptiPath records to cutting tools used by the tool path file A tool list can be generated by scanning the tool path file. By default, the tool change events in the list represent the pocket numbers of cutting tools used by the tool path file. These events can also be linked to OptiPath records for tool path optimization, as described by the next step. Setup Toolpath Tool Change By=List Use Tool list Ensure Prompt for Optipath settings while building is cleared (NOT selected) Build Tool List - scans the tool path and generates the tool list In the fields under OptiPath Setting: - for event #1 o left-click to select: .625D 1.5H FEM, Carbide (4) - for event #2 o left-click to select: .750D 1.5H BEM, Carbide (4) Tool Change List window: OK Toolpath window: OK 4. Use OptiPath Control to create an optimized tool path named op_mold.opti OptiPath Control Optimized File=*.opti (OK as is. The * wildcard will be replaced with the op_mold tool path base file name to create an optimized tool path na