Engraving Parameters
Use the Engraving parameters tab to set the parameters of your engraving toolpath. You can set the toolpath to roll around sharp corners, wrap a toolpath on a curved surface, filter points from the toolpath for smoother motion, specify the number and type of depth cuts, and re-machine the toolpath.
If you use a flat cutter to machine out a cavity and plan to re-machine the corners, you can enter an Angle for flat cutter offset that will offset the tip of the straight (flat) bit to match the V-groove tip position of the engraving bit or chamfer bit so that the roughing operation does not gouge the engraved edge.
When you open a Mastercam 2020 or older part file containing an Engrave toolpath, you may notice changes in the motion when you regenerate the toolpath. This is due to a change in the algorithm. The motion is still correct.
Absolute
Absolute values are always measured from the origin 0,0,0. If you were to translate geometry associated with a toolpath, and the toolpath depth were set to an absolute value, the tool will try to cut to that same absolute depth value no matter where the geometry is located.
Incremental
Incremental values are relative to other parameters or chained geometry.
For most Mill and Router toolpaths, Depth and Top of stock parameters are relative to the location of the chained geometry. Clearance, Retract, and Feed plane are relative to the Top of stock.
Clearance
Sets the height at which the tool moves to and from the part. Select the checkbox to activate the clearance height. If it is not selected, the Retract value is used as the clearance plane. Click the button to set or change the height. You can select a point on the geometry or enter a value.
Use clearance only at the start and end of operation
Rapids to the clearance plane only at the start and end of the toolpath.
Retract plane
Sets the height that the tool moves up to before the next tool pass. Select the checkbox to activate the retract plane, then click the button and select a point on the geometry or enter a value. This option is off by default. The retract height should be set above the Feed plane.
Feed plane
Sets the height that the tool rapids to before changing to the plunge rate to enter the part. The tool also moves to this height between operations if you do not enter both the clearance height and the retract height. Choose the Feed plane button and select a point on the geometry or enter a value.
Top of stock
Sets the height of the material in the Z axis. Many other toolpath parameters are measured from this position in Incremental mode, such as Clearance, Retract, and Feed planes. Select the checkbox to activate the retract plane, and then click the button and select a point on the geometry or enter a value. Incremental values are measured from the chained geometry.
Depth
Determines the final machining depth and the lowest depth that the tool descends into the stock. The default Depth is the depth of the first chain selected. Select the checkbox to activate the retract plane, and then click the button and select a point on the geometry or enter a value. Incremental values are relative to the chained geometry, not the Top of stock.
Climb
Cuts in one direction with the tool rotating in the opposite direction of the tool motion.
Conventional
Cuts in one direction with the tool rotating in the same direction as the tool motion.
Roll cutter around corners
Generates arc moves in the toolpath when sharp corners are encountered. Select None to guarantee all sharp corners; select Sharp to only roll the tool around sharp corners (135° or less). The radius of the arc equals the radius of the tool.
XY Stock to leave
Leaves material in the X and Y axes for finish passes, while allowing Mastercam to display the correct tool diameter.
Angle for flat cutter offset
If you use a flat bit to rough out a cavity and plan to re-machine the corners, enter an angle that matches the V-groove tip. This will offset the flat bit to match the position of the engraving bit so that the roughing pass does not gouge the engraved edge.
Depth cuts
Select the checkbox to divide the total depth into multiple depth cuts. Click Depth cuts to configure the cuts.
Filter
Select the checkbox to eliminate unnecessary tool moves in the toolpath to create smoother movement. Click on the Filter button to configure toolpath filtering options.
Remachining
Select the checkbox to enable the Remachining button and activate default parameters for cleaning out remaining material. Click the Remachining button to set remachining parameters.
Wrapping
Select the checkbox to enables the Wrapping button and activates default parameters for wrapping a toolpath onto surfaces or between two curves. Click Wrapping to set wrapping parameters.





