|
There are two ways to program cutter compensation ... program the print dimensions and use the full radius of the cutter as the offset value ... or program the center line of the cutter and use only the compensation amount as the offset value. We choose to use what has proven for us over the years to be the best method ... programming the center line of the tool and only inputting the comp amount into the offset table.
CONVERSATIONAL MENUS :
KipwareM® conversational menus always create G code using the center line of the cutter. If you look at the dimensions in the G code you will see that they reflect the center line of the cutter not the part dimensions. This allows the user to only have to enter the compensation amount into the offset value in the tool table for the tool. For example ... if the slot cuts to small by say .005" ... the user can enter .0025 into the offset value ( .0025 for each side = .005 total ) in the tool table for the cutter. If the slot cuts to big by .005" ... the user can enter -.0025 into the tool table.
This method causes much less "overcutting" alarms than entering the full radius of the tool into the offset table and program print dimensions. Using a smaller cutter comp offset allows for more intricate, smaller moves when they become necessary for clearance or other restrictions. Because one of the cutter comp rules is that any move made must be greater than the radius of the tool as entered in the offset table ... when they are not the overcutting alarm will be generated.
Note that this method also allows the user to enter a POSITIVE or NEGATIVE number into the offset table ... allowing for easy compensation in both directions and the smaller value is easier to determine as it is only based on the amount of compensation needed regardless of the radius of the cutter.
SketchPad :
The use of cutter comp when using the SketchPad depends on the specifics of the Sketch.
(1) Some users prefer to draw the actual workpiece profile using actual workpiece dimensions. In this instance ... as the SketchPad will create a toolpath using the elements of the Sketch ... the radius / diameter ( depending on your machine specifics ) of the cutter should be entered into the offset table at the machine. This method uses the machine's cutter comp feature when machining the shape.
(2) Some users prefer to offset the actual workpiece profile using the radius of the cutter that will be used. In this instance ... as the SketchPad will create a toolpath using the elements of the Sketch ... a zero offset value should be entered into the offset table at the machine to start. If an adjustment is required ... then only the amount to be adjusted needs to be entered into the offset table at the machine. Plus or minus values can be input depending on the offset direction required.
|