Use the Tool Properties dialog to define further details about a tool, such as its program point.
To display this dialog, click the Tool Properties button on the Tool Data dialog.
The following settings are available:
Program Point — Use these options to specify the tool's program point. The program point is a point on a tool that is referenced in the NC program. Select one of the following options to specify the location of the program point:
- Tool Zero — Select to set the program point at the tool zero point.
- Nose Center — Select to set the program point at the center of the tool nose radius.
- Add Tool Shifts — Select to set the program point to be a point that is shifted away from the tool zero point (using the X, Y, Z values in the Tool Shifts area of the dialog).
Tool Shifts — Use the X, Y, and Z values to shift the program point. Tool Shifts are used for Swiss-type lathes in Stock Motion Simulation. The Z value specifies the distance between the common plane (where Z=0) to the programmed cutting edge of the tool.
- Set Default Z-Shift — Click to set the default tool shifts for Swiss-type lathes, as required for Stock Motion Simulation.
Tool Head Properties
- Mini-Turret Index Angle — If you are using a mini turret, enter the angle of the mini-turret attachment used on Tool Head. The corresponding reserved word in ConfigPost is <mini-turret-angle>.Note: This option is displayed only for PartMaker/Turn-Mill and PartMaker/SwissCAM.
Inclined Tool Properties — Turning Tool Inclination
- Shank Inclination Angle — Enter the turning holder inclination angle for the Tool Head.
The corresponding reserved word in ConfigPost is <b-angle>.
- Use B-angle for Toolpath Calculations and Simulation — Select this option if you want PartMaker to rotate the tool by the Shank Inclination Angle before it calculates the toolpath. If selected, PartMaker displays the rotated tool during simulation and toolpath verification. If this option is not selected, then the Shank Inclination Angle is used only as a reserved word in ConfigPost.
B-axis inclination is not available for Back Turn tools.
These options are displayed only when using PartMaker/Turn-Mill, PartMaker/SwissCAM, and PartMaker/Mill.
In PartMaker/Mill, inclined turning is supported only for Head-Table machines where the tool head remains in the ZX plane while rotating about the Y-axis.
Inclined Tool Properties — Live tool Inclination
- Programmable Tool Inclination — Select this option to specify an inclination plane and tool axis direction for use in Full Machine Simulation and post processing. This option is applicable only for live, fixed-angle tools for machines that do not have an articulated Tool Head. Such tools can be used on Turn-Mill or Swiss machines.
The inclination angle for such tools is defined using the Inclination Angle (B) field on the Face Options dialog.
The corresponding reserved word (which includes both the Tool Plane and the Tool Axis Direction parameters) for post processing is <inclined-tool-region>. The post processor outputs these into the required coordinates in the NC program file.
- Tool Plane — Select which plane is used as the tool plane. The plane is constructed through two lines: one line coincident with the tool axis and another line coincident with Z-axis. PartMaker supports only ZX and ZY planes:
ZX — Select if the tool rotates about the Y axis and is parallel to the ZX plane when cutting.
ZY — Select if the tool rotates about the X axis and is parallel to the ZY plane when cutting.
- Tool Axis Direction — Select the direction of the tool axis in reference to the Z axis. The values available depend on the Tool Plane selected:
When the Tool Plane is a ZX plane, you can select:
X+ — Select if the direction of the tool axis is towards the positive X coordinates.
X — Select if the direction of the tool axis is towards the negative X coordinates.
When the Tool Plane is a ZY plane, you can select:
Y+ — Select if the direction of the tool axis is towards the positive Y coordinates.
Y– — Select if the direction of the tool axis is towards the negative Y coordinates.
These options are displayed only when using PartMaker/Turn-Mill and PartMaker/SwissCAM.
- Tool Plane — Select which plane is used as the tool plane. The plane is constructed through two lines: one line coincident with the tool axis and another line coincident with Z-axis. PartMaker supports only ZX and ZY planes:
Use as Cut-off Tool — Select this option if the tool is used as a cut-off tool. For Bar-Fed Mill machines that cut off with a saw, selecting this option ensures that PartMaker handles this type of cut-off tool correctly during simulation and post processing.
Output Coordinates Shift — Select this option to insert Tool Shifts into the NC program file for machines that support Tool Shifts.
Negative Diameter — Select this option if the tool requires a negative diameter to be used in the NC program.
Feed and Speed Factors — Click to display the Feed and Speed Factors dialog.