Home Positions and Reference Points
The Home position is where the tool spindle or turret typically travels for tool changes and at the end of the NC program. Reference points lie between the home position and the start or end of the toolpath.
Inch and metric values
If you are setting reference points for a machine definition, you should record separate sets of values for inch and metric operation. When working in the Reference Points dialog from the Machine Definition Manager, click the Convert to mm or Convert to inch button to automatically convert one set of values to the other units and write them to the proper fields.
This topic does not apply to Mill-Turn. To learn more, see the "Machine Reference Position Manager" link at the end of this topic.
Mastercam lets you control the home position from several different sources. You can:
-
Enter a default value for the machine definition, which is available to all operations created for that machine. Use the Machine Axis Combinations dialog box to enter a position for each axis combination. If you don't need to create axis combinations, enter the home position coordinates in the Default axis combination. Use world coordinates to enter the home position in the machine definition.
- Create an operation-specific default value and store it in the .DEFAULTS file.
- Store a home position for the tool as part of the tool definition that will be available whenever the tool is selected for an operation. (Lathe only)
Use the Tool page in the control definition to select which home position will be the default for new operations, as shown in the first image following. However, no matter where the default value is coming from, you can override it on the Toolpath parameters tab, as shown in the second image following.
The home position for each operation is expressed relative to the tool plane (Tplane) origin used for the operation.
If you create entry/exit or lead in/out moves for your toolpaths, the reference point is the starting point for the entry move and the destination point for a retract move.
- You can create separate reference points for approach and retract moves.
- For lathes, you can create separate sets of reference points for both ID and OD work. When you select From machine, Mastercam automatically selects the correct point.
- If the retract or approach reference point is not selected, the tool will rapid directly between the home position and the first/last programmed position in the operation.
|
|
Default reference points are stored in the machine definition as part of the axis combination settings, just like the home position. However, the process for selecting and using them is different.
- Use the checkbox in the Toolpath parameters tab to activate reference points for each operation.
- Click Reference point to select a point using the Reference Point dialog box. Choose From machine to read the value from the machine definition, or enter a new location for this operation.
You can disable the reference points feature using the NC dialog page in the Control Definition Manager. In this case, the user cannot use reference points, even if they have been defined in the machine definition.
World coordinates vs. part coordinates
Home and reference points saved in the machine definition are defined relative to the world coordinate system origin. Typically this is the center of the spindle nose for a mill, or the main spindle face on a lathe.
If you are setting reference points for a single operation, the points are defined relative to the tool plane used for that operation.





