Use this tab to enter settings for an Auto
Drill or Start Holes operation. You can also use this tab to modify
settings for Solid drill operations.
Absolute
Mastercam measures absolute values from the origin 0,0,0. If you translate geometry
associated with a toolpath, and the toolpath depth is set to an absolute value, the
tool tries 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.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.
NOTE
This option does not result in incremental coordinates being output in
the NC program; use the Control Definition Manager to determine that.
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 clearance height. You
can select a point on the geometry or enter a value. Note that, for multiaxis toolpaths, Clearance is always an incremental distance from the
current tool position.
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
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. If you do not enter a Clearance height, the tool will move
to the retract height between operations.
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. Click Top of stock 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. Click Depth and select a point on the geometry or enter a value. Incremental
values are relative to the chained geometry, not the top of stock.
From top bottom of arc
For holes in solids, select which set of arcs to use as the baseline for an incremental
depth.
Tip compensation
Select to turn on tip compensation so that the tool drills all the way
through the stock. Click Tip compensation to open the Drill Tip Compensation
dialog box to enter a breakthrough amount and tip angle.
Machine group
Tell Mastercam the name of the machine group in which to store the new operations.
Select a name from the drop-down list or enter a new name in the field to create
a new group.
3 axis
Creates 3-axis drill toolpaths for the selected points and/or arcs. Uses the G100
code in the NCI file.
Use arc views
Select to create toolpaths for all selected arcs. If not selected, Mastercam
filters out any arcs that are not in the current tool plane.
No sorting or grouping
Creates drill operations in multiple planes in no particular order. Only available
if you select the Use arc views option.
Sort by plane
Sorts drill operations according to the plane. Only available if you select the Use
arc views option.
Group by plane
Creates a new machine group for each pane and places drill operations in these groups
according to the plane. Only available if you select the Use arc views option.
5 axis
Creates 5-axis drill toolpaths for the selected points and/or arcs.
Tool library
Displays the tool library name where Mastercam selects tools for the toolpaths.
Diameter match tolerance
Mastercam uses this value to determine how closely the diameter of the tool and the
hole must match before selecting an appropriate tool.