B-Axis Contour Turning
Use the B-Axis Contour Turning function panel to create a finishing toolpath that follows the contour of the chained geometry while simultaneously allowing for B-axis rotation. You can:
-
Select automatic mode to compute the optimal B-axis angles for all points along the toolpath.
-
Select manual mode to define the B-axis angles based on selected tool axis control lines.
Before you can create a B-axis Contour Turning operation, you need to:
-
Complete the Mill-Turn job setup. For more information, see Performing a Mill-Turn Job Setup.
-
Set the tool for the operation to center compensation.
For 2D tools, set the compensation on the Parameters page of the Define Tool - Machine Group dialog box.
For 3D tools, set the compensation on the Compensation page of Tool Assembly in the 3D Tool Designer function panel.
Each page in the function panel contributes to a top-down structured workflow for programming a B-Axis Contour Turning operation.
Follow the guidelines below to create a B-Axis Contour Turning toolpath.
-
Select the Tool page to select a tool and set your feeds and speeds.
-
Select the Machine page and define the machine settings for this operation, such as the axis combination and the tool's orientation. Unlike other turning toolpaths, you do not need to define an angle for the tool axis or a cutting direction because the B-axis Contour Turning operation will derive them for you.
-
Select the Operation page and define operation settings such as reference points, or add a toolpath comment.
-
Select the Geometry page to view or edit the contour chain. Choose the compensation direction and adjust the stock to leave.
-
Select the Lead In page to control how the tool approaches the part. These settings eliminate the need to create extra geometry for the lead in movement. You can also set an entry feed rate and extend or shorten the start of the chained geometry.
-
Select the Lead Out page to control how the tool retracts from the part. This eliminates the need to create extra geometry for this purpose. You can also set an exit feed rate and extend or shorten the end of the chained geometry.
-
Select the Basic Motion Control page and choose a tool axis control method. B-axis Contour Turning offers two methods for controlling the tool axis:
- Automatic mode creates safe B-axis angles for all positions along the chained contour based on the shape of your tool insert and holder. The Tool Angle Limits define the range of angles (degrees) that Mastercam is allowed to assign to the tool along the contour.
- Manual mode allows you to select lines to define the tool axis vectors along the contour. Tool Offset Angle allows you to define an offset angle for the selected lines. The Tool Offset Angle makes geometry creation easier by allowing you flexibility in how you draw the tool axis control lines.
- Select the Advanced Motion Control page to access settings that give you greater control over your tool and toolpath. These settings include:
-
Cut tolerance: Adjust the maximum value by which the toolpath is allowed to deviate from the chained contour. A smaller Cut Tolerance value leads to a more accurate toolpath, but too small of a value will increase toolpath generation time.
-
Maximum distance between points: The maximum distance allowed between the points from which the toolpath is made and which occur in the posted code. Not all points will be the same distance apart; rather, no points will be farther apart than the distance specified in this field. To display the points in Classic Backplot, enable Show end points.
- Maximum angle step: The maximum angle by which B-axis rotation may change between two points. If there is a need for a greater angle change between two points, Mastercam will add an intermediate point so that the Maximum angle step value is respected.
-
Holder clearance: The value by which the holder boundary is offset, prior to Mastercam computing the toolpath, to create a gap between the holder and the stock.
Holder clearance of 0.0 Holder clearance of 1.0
NOTEIf the Holder Clearance value is less than double the Cut Tolerance, Mastercam will use double the Cut Tolerance as the Holder Clearance value to keep the holder from contacting the contour.
-
Maximum insert depth: This value controls the maximum amount of the insert allowed to contact the contour. Entering a value of zero or less allows the toolpath to use all of the exposed portion of the tool insert. The method by which the Maximum insert depth is applied depends on the tool type:
-
Grooving/parting tools apply the Maximum insert depth value from a line along the plunge direction, at the distance the user has entered. The resulting portion of the insert is allowed to contact the contour.
Grooving/parting tools: Maximum insert depth of 0.0 Grooving/parting tools: Maximum insert depth of 2.0
-
Boring bars, general turning, and custom tools use the Maximum insert depth value as follows:
-
For a Maximum insert depth value that is less than the tool nose radius, Mastercam applies the same method as is applied for grooving/parting tools.
-
For a Maximum insert depth value that is greater than the tool nose radius, Mastercam computes the allowable contact portion of the insert by creating a circle with a radius that is the Maximum insert depth value and with a center point at the center of the tool nose radius. Any portion of the insert contained within the circle will be used for cutting. Any portion of the insert outside of the circle will act as part of the holder.
Boring bars, general turning, and custom tools: Maximum insert depth of 1.5 Boring bars, general turning, and custom tools: Maximum insert depth of 0.25
A setting of 0.0 will allow the entire cutting portion of the insert to contact the contour.
-
-
- Select the Stock page to control how Mastercam updates the stock definition between operations.
- Select the Settings page to adjust tool display settings.





