Turning tool table toolturn.trn (#50 / #4-03-1)
Application
The turning tool table toolturn.trn contains the parameters specific to turning tools.
Related topics
- Editing parameters in tool management
- Tool parameters
- Milling-turning operations on the control
- General parameters, regardless of the technology
Requirements
- The Turning (#50 / #4-03-1) or Adv. Spindle Interpol. (#96 / #7-04-1) software option
- Turning tool is defined in TYP column of tool management
Description of function
The file name of the turning tool table is toolturn.trn and this table must be stored in the folder TNC:\table.
The values of the parameters ZL, XL and YL go from the tool tip TIP out to the tool-carrier reference point. The algebraic sign of, for example, XL depends on whether the tool tip is to the right or left of the tool spindle. If the tool is oriented and tool tip is to the right of the spindle center, enter a negative value for XL.
For YL the algebraic sign depends on whether the tool tip is in front of or behind the center of the tool spindle. If the tool tip is in front of the spindle center, enter a positive value for YL.
Parameters of the turning tool table toolturn.trn
The toolturn.trn turning tool table provides the following parameters:
Parameter | Meaning |
---|---|
T | Row number in the turning tool table The tool number allows you to identify each tool unambiguously (e.g., for calling a tool). Using TOOL CALL to call a tool You can define an index after the period. The row number must match the tool number in the tool.t tool table. Input: 0.0...32767.9 |
NAME | Tool name? The tool name identifies a tool, for example when calling it. Using TOOL CALL to call a tool You can define an index after a period (i.e., name.index). Input: Text width 32 |
ZL | Tool length 1? Length of the tool in the Z direction, with respect to the tool carrier preset Input: –99999.9999...+99999.9999 |
XL | Tool length 2? Length of the tool in the X direction, with respect to the tool carrier preset Input: –99999.9999...+99999.9999 |
YL | Tool length 3? Length of the tool in the Y direction, with respect to the tool carrier preset Input: –99999.9999...+99999.9999 |
DZL | Oversize in tool length 1? Delta value of tool length 1 as a compensation value in connection with touch probe cycles. The control enters compensation values automatically after measuring the workpiece. Touch-probe cycles for workpieces Is added to the parameter ZL Input: –99999.9999...+99999.9999 |
DXL | Oversize in tool length 2? Delta value of tool length 2 as a compensation value in connection with touch probe cycles. The control enters compensation values automatically after measuring the workpiece. Touch-probe cycles for workpieces Is added to the parameter XL Input: –99999.9999...+99999.9999 |
DYL | Tool length oversize 3? Delta value of tool length 3 as a compensation value in connection with touch probe cycles. The control enters compensation values automatically after measuring the workpiece. Touch-probe cycles for workpieces Is added to the parameter YL Input: –99999.9999...+99999.9999 |
RS | Cutting edge radius? The control takes into account the cutter radius for tool tip radius compensation. Tool radius compensation (TRC) with lathe tools (#50 / #4-03-1) In turning cycles, the control takes into account the cutter geometry to prevent damage to the defined contour. If the contour cannot be machined completely, the control will display a warning. Mill-turning cycles (#50 / #4-03-1) For the cutter geometry, the control also considers the parameters TO, T-ANGLE, and P-ANGLE. Input: 0...99999.9999 |
DRS | Cutter radius oversize? Delta value of cutter radius as a compensation value in connection with touch probe cycles. The control enters compensation values automatically after measuring the workpiece. Touch-probe cycles for workpieces Is added to the parameter RS Input: –999.9999...+999.9999 |
TO | Tool orientation? From the tool orientation, the control determines the position of the tool tip and, depending on the selected tool type, additional information such as the tool angle direction. This information is necessary, for example, for calculating the cutter radius compensation, milling cutter radius compensation, plunge angle, etc. Tool radius compensation (TRC) with lathe tools (#50 / #4-03-1) Machine Refer to your machine manual. The control displays the tool orientations that are possible for each tool type. The machine manufacturer can change this assignment. In turning cycles, the control takes into account the cutter geometry to prevent damage to the defined contour. If the contour cannot be machined completely, the control will display a warning. Mill-turning cycles (#50 / #4-03-1) For the cutter geometry, the control also considers the parameters RS, T-ANGLE, and P-ANGLE. Input: 1...19 |
ORI | Angle of spindle orientation? Angle of tool spindle for aligning the turning tool Input: –360.000...+360.000 |
SPB-INSERT | Angular offset? Angular offset for recessing and threading tools, spatial angle B Input: –90.0...+90.0 |
P-ANGLE | Point angle In turning cycles, the control takes into account the cutter geometry to prevent damage to the defined contour. If the contour cannot be machined completely, the control will display a warning. Mill-turning cycles (#50 / #4-03-1) For the cutter geometry, the control also considers the parameters RS, TO, and T-ANGLE. Input: 0...179.999 |
T-ANGLE | Tool angle In turning cycles, the control takes into account the cutter geometry to prevent damage to the defined contour. If the contour cannot be machined completely, the control will display a warning. Mill-turning cycles (#50 / #4-03-1) For the cutter geometry, the control also considers the parameters RS, TO, and P-ANGLE. Input: 0...179.999 |
CUTLENGTH | Cutting length of recessing tool Usable length of the cutting edge of a turning or recessing tool. The control monitors the usable length of the cutting edge in the turning cycles. If the programmed cutting depth is greater than the usable length of the cutting edge defined in the tool table, then the control will display a warning and will automatically reduce the cutting depth. If you do not define CUTWIDTH, the control uses the usable cutting length to define the tool for the graphic representation. The control calculates the missing information from the CUTLENGTH, P-ANGLE and T-ANGLE parameters. If the usable cutting length is less than the actual cutting length, the graphic representation will not match the actual tool. Input: 0...99999.9999 |
CUTWIDTH | Width of recessing tool Cutting width of a turning or recessing tool The control uses CUTWIDTH for calculations within cycles and to exactly define the tool for the graphic representation. Mill-turning cycles (#50 / #4-03-1) Input: 0...99999.9999 |
DCW | Oversize f. recessing tool width Delta value of recessing tool width as a compensation value in connection with touch probe cycles. The control enters compensation values automatically after measuring the workpiece. Touch-probe cycles for workpieces Is added to parameter CUTWIDTH Input: –99999.9999...+99999.9999 |
TYPE | Type of turning tool Depending on the selected turning tool type, the control displays the suitable parameters in the Form workspace of the tool management. Turning tool types (#50 / #4-03-1) Selection by means of a selection window Input: ROUGH, FINISH, THREAD, RECESS, BUTTON, and RECTURN |
WPL-DX-DIAM | Compensation value for the workpiece diameter Compensation value for the workpiece diameter with respect to the working plane coordinate system (WPL CS). Working plane coordinate system WPL-CS Input: –99999.9999...+99999.9999 |
WPL-DZL | Compensation value for the workpiece length Compensation value for the workpiece length with respect to the working plane coordinate system (WPL CS). Working plane coordinate system WPL-CS Input: –99999.9999...+99999.9999 |
Notes
- The control shows delta values from the tool management graphically in the simulation. For delta values from the NC program or from compensation tables, the control changes only the position of the tool in the simulation.
- Geometry values from the tool table tool.t, such as length L or radius R, are not effective with turning tools.
- Assign unique tool names!
If you define identical tool names for multiple tools, the control will look for the tool in the following sequence:
- Tool that is in the spindle
- Tool that is in the magazine
- Machine
Refer to your machine manual.
If there are multiple magazines, the machine manufacturer can specify the search sequence of the tools in the magazines.
- Tool that is defined in the tool table but is currently not in the magazine
If the control, for example, finds multiple available tools in the tool magazine, it inserts the tool with the least remaining tool life.
- If you want to archive tool tables or use them for simulation, save them with different file names and the corresponding file extension.
- Use the machine parameter unitOfMeasure (no. 101101) to define inches as the unit of measure. This does not automatically change the unit of measure in the tool table!
- The columns WPL-DX-DIAM and WPL-DZL are deactivated in the default configuration.
In the machine parameter columnKeys (no. 105501), the machine manufacturer activates the columns WPL-DX-DIAM and WPL-DZL. The names of the columns may be different, however.