Steady Rest Point (Mill-Turn)
Use this dialog box to create operations for a turret-mounted steady rest in Mastercam Mill-Turn.
Each steady rest point operation can contain a number of individual events, such as linear moves, rapid moves, and clamp/unclamp events. Most steady rest point operations are one of the following types:
-
Operations that clamp the steady rest. These typically include one or more linear or rapid positioning moves preceding the clamp event, but these are not required. The clamp event is always the last event in the operation.
-
Operations that unclamp the steady rest. These typically include one or more linear or rapid positioning moves following the unclamp event, but these are not required. The unclamp event is always the first event in the operation.
-
Operations that move the steady rest, but do not clamp or unclamp it. For example, after creating an operation that clamps the steady rest, you might choose to create an operation that moves the steady rest so that it follows the tool or other turret.
Build your operation by adding points and events to the Motion Points window. Expand the section below to learn more about working in the window, or see Creating a Steady Rest Operation: Mill-Turn to learn more about creating a steady rest point operation for a turret mounted steady rest.
You will do most of the work of creating your operation in the Motion Points window. This is where you assemble the sequence of events that will occur in the operation.
Right-click in a blank area of the grid or use the buttons below it to add points to the operation. The instructions in this topic use the right-click menu but you can also perform the steps with the corresponding buttons.
To add a new point, follow these steps:
-
Right-click in an empty area of the grid (not on an existing point) and select Create new point.
-
Click in the Type cell and select the type of motion. You can choose from G0 (interpolated rapid move), G0 - Break (dog-leg rapid move), or G1 (linear move at feed rate).
-
Enter the destination coordinates directly in each cell. You can also specify a Dwell time and, for linear moves, the Feed Rate.
Follow these steps to clamp the steady rest:
-
Create points for any desired positioning moves that precede the clamp event. These are optional—if the steady rest is already at the proper position, you do not need to create any additional points.
-
Right-click in an empty area of the grid and select Create new clamp.
-
Enter a Dwell time if desired.
The clamp point must be the last point or event. Mastercam will not let you add any additional points.
-
Once you create a clamp point, the Utilize boundary in collision detection option will be enabled. When this option is selected, Mastercam collision checks against the steady rest's boundary when you create subsequent operations. Read more about this option in the Parameters section below.
Follow these steps to unclamp the steady rest:
-
Right-click in an empty area of the grid and select Create new unclamp.
The unclamp event must be the first point or event. Mastercam will not let you unclamp the steady rest if you create any other points first.
-
Create any additional points to move the steady rest away from the part or to its home position. These are optional, you do not need to create any additional points.
Mastercam gives you several ways to add points by selecting them from the graphics window.
To add a new point, do either of the following:
-
To add a new point at the bottom of the grid, right-click in an empty area of the grid and select Create new point from selection.
-
To insert a point in the existing list, right-click on the number in front of an existing point. Mastercam will insert a new point below it.
To reselect the coordinates of an existing point, right-click on the number in front of an existing point and choose Reselect point.
Mastercam Mill-Turn supports steady rests in two different ways:
-
Steady rest operations are used to program standalone steady rests.
-
Steady rest point operations are used to program turret-mounted steady rests.
Steady rest operations in Mastercam Lathe are different than Mill-Turn steady rest operations. See Lathe Steady Rest to learn more about Lathe steady rest operations.
Steady rest display window
This window displays the available steady rests. If more than one steady rest is available, click the one you would like to use for this operation.
Tool number
For most applications, this will be equal to the turret index position in which the steady rest is mounted. This field is disabled when the Tool number equals index position option is selected as part of the turret properties in the machine definition:
Offset number
The offset number associated with the steady rest.
Motion Points grid
Displays the programmed points and other events that are contained in this operation. See the main body of this topic for more information.
Utilize boundary in collision detection
Select this option to have Mastercam collision check against the steady rest boundary when creating subsequent toolpaths. This option is available once you have created a clamp point in the grid. The setting is applied as long as the steady rest remains clamped.
-
Mastercam always collision checks against the steady rest component models when you are running Simulation. The option on this page is applied while Mastercam is generating subsequent toolpaths.
-
The boundary used by this feature is a 2D wireframe boundary that is specified as part of the component properties of the steady rest. See Component Geometry: Mill-Turn Steady Rest to learn more.
-
You can select or deselect this option as the default for your part on the Work Support page in your Job Setup.

Axis combination/Spindle origin
Click this button to select the desired spindle origin. Mastercam opens the Axis combination/Spindle origin dialog box, where you can select the spindle origin from the list. Typically this will let you select the left or right spindle. For most machines, this will also determine which work offset is used.
Comment
Enter comments for the toolpath. Comments help identify the operation in the Toolpaths Manager. These can be output in the NC file when you post if you select the proper option in your machine group properties.





