There are 5 different Mastercam Cutter Compensation Types in the Mastercam 2D toolpaths. Computer, Control, Wear, Reverse Wear, and Off.
Compensation is only available in the 2D tooplaths that have a finishing pass such as Contour, Dynamic Contour, Pocket, Peel Mill, Blend Mill, Slot Mill, Circle Mill, Helix Bore, and Thread Mill. Only the finishing portion of these toolpaths would have access to the compensation settings.
Compensation is not available in the roughing specific toolpaths such as Dynamic Mill, Area Mill, and Face Mill. It is also not available in Drill, Engrave, or any of the Wireframe toolpaths.
Compensation is used to offset the toolpath from the selected geometry depending on the diameter or radius of the cutter. The tool can be offset to the left or the right of the geometry relative to the direction of travel. Typically, on CNC machines, a climb milling cut is preferred. This is achieved by offsetting the tool to the left of the geometry.
Computer. With this setting Mastercam will create the toolpaths position relative to the center of the cutter when the cutter is on the selected geometry. No cutter compensation gcodes will be output into the gcode so the radius/diameter values in the control will have no effect on the tools motion. The same sized tool that was used in Mastercam must be used on the machine.
Control. Control compensation will output cutter compensation into the gcode, G41 or G42 based on the offset direction (typically CNC use a climb cut which is offset left, or G41), and the positions in the gcode will be that of the selected geometry (not center of tool as Computer was). This allows adjustments to the cutter size being used as well as adjusting the parts final size if the tool wears during production. Using Control requires that the tools diameter, or radius depending on your machine, needs to be input into the offsets for this tool. Different tool diameters can be used with the program now, not just the size that was used in Mastercam. We could cut this feature with a half inch endmill, or even a reground tool that might be 0.603 diameter, as long as that is input into the geometry field in the offset for this tool. The wear field can also be used to make fine adjustments to the final size of the part. Putting in a negative wear value will result in more material being cut, a positive number will be less material cut
Wear. This kind of combines Computer and Control. This will generate tool positions relative to the center of the tool but will also include compensation code being output (G41/G42). Since this toolpath is generated at the center of cutter, the same tool used in Mastercam must be used on the machine but since we have the addition of the compensation, we are able to use the wear field. On your machine control, you would set the tools geometry to 0 and then the wear field can be used to adjust the final size of the cut feature. For Wear, inputting a negative wear value will cut more material, a positive will cut less material.
Reverse wear. Reverse Wear is the same as wear except it will compensate to the opposite side of the toolpath. Here, a negative wear value will cut less material and a positive offset will cut more material. Keep in mind the geometry field for Reverse will be set at 0 as well.
Off. With this setting Mastercam will not compensate at all for the tool being used. The path generated is relative to the geometry selected. Posting G code shows no output of G41 or G42 either. Values input into the diameter or wear offsets will not affect this toolpath. Typically, application of this setting would be for engraving when offsetting of the toolpath is not desired.
A few things to keep in mind when using compensation…1-it is very important that no matter the compensation type chosen, the diameter and wear offsets on the cnc machine must be setup relative to the compensation type used. 2-Some machines will not allow compensation to be applied to a G2 or G3 arc move, you may need to ensure the first move the cutter makes is a straight line. This can be controlled on the lead in lead out page. 3-When using Control compensation, some machines will also require that the first line movement while applying the compensation is at least as big as the radius of the tool. For example, if your using a 1-inch cutter the line of code applying the G41 or G42 must make a move that is at least half an inch long.
See other blog posts
blog.caminstructor.com
Check out our website
caminstructor.com
#Mastercam #LearnCNC