Cutter Comp

Nowadays, almost every machine control provides the functionality of automatic cutter compensation. This is a function that lets the control calculate the offset toolpath based on the profile that is specified in the NC code. The offset amount (tool radius) is normally specified somewhere in the controls memory ( compensation register), often together with other tool related data. The big advantage of this approach is that changes to the offset value are done directly on the machine without editing the NC code. This is very practical when making adjustments to compensate tool wear or switching to a tool with different diameter.

The Cutter Comp setting in EZCAM is used to activate cutter compensation on the control by posting the corresponding commands (G41 - comp left/ G42 - comp right / G40 - cancel comp, or equivalents) in the NC code at begin and end of the machined profile. If you plan to use this function please read the paragraph below carefully.

Rules that apply when using cutter compensation:

• Typical controls need linear moves at begin and end of the machined profile (curve) to activate and cancel cutter compensation. In addition the length of these moves has to be bigger than the tool radius. Best is to use EZCAM's Lead-In and Lead-Out options to create these moves automatically.
   

• Ensure that the specified path curve does not include any undercut areas or arc moves that are smaller than the tool radius. Some modern controls may be able to handle such cases, but all others will most likely return some kind of compensation error message during machining.
   

• The EZCAM system only posts the coordinates of the machined path curve without any offsetting or undercut checking.
   

• Ensure that the operator specifies the correct offset value (tool radius) in the right place (offset register) of the machine controls memory.
   

• Never use Cutter Comp in combination with multi-pass contouring (Total Stock, Cut-Step).