Deburring Process

The Deburring Process cleans up selected edges of parts. The user must first create a tool and select a face and the edge to machine before using this plug-in. While any tool can be used (the tool will be considered a sphere with a diameter equal to the tool's diameter), it is recommended that a form tool (like the one shown at the right) be created to represent the most accurate rendering of the part. Using an endmill may show a collision that does not actually occur.

Select the tool to be used and the face and the edge to be machined and run the plug-in. Double-click the Deburring Process Tile to bring up the Deburring Process dialog.

Cutting Depth

This value represents the size of the chamfer (as the graphic in the dialog illustrates) and specifies how deep the tool will penetrate into the material. The distance is measured along the normal to the selected face.

Overlap

This item specifies how deep the tool will move inside the opening. The value must always be smaller than the tool's (or the tool shank's) radius, or else the tool shank will collide with the part.

Lead In/Out Line

This value represents the length of the lead in and lead out moves, or the length of the tangent line to be used with a 90 degree arc to approach and exit the deburring operation. Enter a value of zero for an arc move.

Lead In/Out Radius

This value represents the radius of the circular lead in and lead out moves; in other words, the radius value for the 90 degree arc following the tangent line. Enter a value of zero for a straight line move.

Approach

This item determines the length of a linear approach or retract move, parallel to the normal to the selected face at the start or end point.

Entry Z

This value represents the Z value at the start of the operation (Z CP2).

Exit Z

This value represents the Z value of the end of the operation (Z CP3).

Feedrate

This item determines the feedrate value in part units.

Spindle RPM

This item determines the spindle rotation in revolutions per minute.

Tolerance

This value specifies the tolerance used to approximate the edge.

Reverse Direction

Select this checkbox to reverse the calculated toolpath.

Click Close in the dialog and then Do It in the Machining palette to create the deburring operation.

The image to the right illustrates practical use of the Deburring Process. The spherical tool approaches a hole in the part, feeds onto the edge cuts around the select edge, pulls away, and the retracts.