Lathe Stock Advance
Use the Lathe Stock Advance dialog box to create a stock advance operation to reposition the stock in the spindle or to control a bar feeder.
Before programming a stock advance operation, you need to have defined the stock and chuck boundaries in the Stock Setup tab.
Stock advance operations have the following general components:
If your bar feeder is not capable of measuring how far it has advanced the stock, use the Toolpath parameters tab to select a tool to stop the stock from advancing, or to pull the stock to its new position.
If your machine has two spindles, select the active spindle for the operation.
Then, enter the original and new positions for the stock. You can choose From stock face to use the currently calculated stock location, or click Select to return to the graphics window and pick a location. The point you choose does not have to be on the face of the stock. You can choose any convenient reference point.
Finally, choose how the stock will be advanced: pulled, pushed, or stopped by a tool.
You can also move the chuck along with the stock by selecting Chuck position.
Choose Transfer geometry
to create a copy of your part geometry aligned with the transferred
stock, leaving the original geometry unchanged. Click Select to return to the graphics window
and pick the specific entities or chains that you want to copy.
Active spindle
These options are enabled only if the stock boundary is defined for both the left and right spindles. Select the spindle for which this component or operation is being created.
Transfer geometry
Select to make a copy of your part geometry aligned with the new stock
model. Click Select to return to the graphic window and pick the geometry
to be copied.
Blank original geometry
Select to remove the original geometry on the screen from view. Mastercam does not delete the entities from your part file, so you can Unblank them later to see and work on them.
Keep the same
Places the transferred geometry on the same level as the original geometry.
Copy to level
Lets you specify on which level you want to place the transferred geometry.
Offset by
Mastercam calculates a destination level based on the level number of the original geometry plus the number you enter here.
Stock position: Original position
Enter the coordinates of a reference point on the original stock or click Select to pick a point. Mastercam moves the stock so that this point is positioned at the location entered in the Transferred position Z field. Enter a value or choose Select to pick a point.
From stock face
Select to automatically use the Z coordinate of the face of the stock as defined in the Machine Group Properties. Mastercam adjusts the location if the stock has been affected by any machining operations since it was defined.
Stock position: Transferred position
Enter a value or choose Select to pick a location to which the stock's original reference point will be moved.
Push stock
Select to use a bar feeder to push the stock to its transferred position.
Use tool stop
Select to use a tool to stop the bar feed at the advanced position. Use the Toolpath parameters tab to select the desired tool. Selecting this option enables Stock clearance and Tool X position.
Pull stock
Select to use a tool to pull stock to its transferred position.
Stock clearance
Determines the distance between the tool pulling the stock and the stock. This option appears only if the Pull stock or Use tool stop option is selected.
Grip length
Enter a value to determine how much of the stock the tool puller will grip before it pulls it to its advanced location. This option appears only if Pull stock is selected.
Tool X position
Enter the tool position's X coordinate. This option appears only if Pull stock or Use tool stop is selected.
Custom Parameters
Select to apply the values for any custom parameters that have been defined for this operation. Click to see or edit the custom parameters. Use the Lathe Part Handling section of the Text page in the Control Definition Manager to define the custom variables.
This operation is only used in Mastercam Lathe. Mastercam Mill-Turn uses Bar Feed instead.





