Tool Diameter Compensation
In ECAM there are 3 compensation mode available :
Within CNC Mode and Tool Wear Mode , a linear approach movement is automatically added at start and at the end of toolpath.
This is necessary to enable machine tool compensation.
In the output code are visible codes for enabling / disabling cutter compensation (usually G41/G42/G40).
The linear approach movement is 5% larger than the tool diameter.
Computer Mode
This is the most compatible mode, since the final path is calculated automatically. The output code don't contains any command related to compensation ( usually G41 - G42 )
It's not possible adjust the toolpath from the machine tool table. You don't have to worry about setting tool diameter in Tool Diameter register.
It's not indicate if you have to keep tight tolerances in your workpiece.
See at bottom page for info about output code .
Computer Compensation Mode:
CNC Mode
This the least compatible mode. The output path reflect exaclty the geometry profile. All the offset distance and effective toolpath are calculated by cnc machine.
With this mode is necessary define tool diameter in cnc machine tool table. Is possible adjust tool wear value in order to compensate possible tool deflection.
The toolpath preview and simulation always show the uncompensated path. This issue can be visually misleading to the user.
The toolpath will be compensated in cnc machine, so there you'll get desired toolpath.
CNC Compensation Mode:
Tool Wear Mode
The offset diameter is calculated by the computer, but you can also adjust the toolpath editing the machine tool wear table .
This permits to have less incompatibility issues with cnc.
Tool Wear Compensation Mode:
Both in CNC Compensation and Tool Wear compensation, if toolpath engine can't create proper lead in / lead out movement, an error is raised.
If this happen, try to reduce the approach radius value , under the finishing operation
Output Code
To help the machininst have clear what compensation is enabled and what values has to insert in cnc tool registry, in the output code are visible all this information.
Both in tool summary and when the tool is actually called.
Computer Compensation Example :
In Tool Summary :
(#7 - END MILL D 8MM COMP COMPUTER - RADIUS COR VALUE 0)
On Tool Called :
N5 (POCKET - FINISHING) (COMP COMPUTER - RADIUS CORRECTOR VALUE 0) (END MILL D 8MM)
CNC Compensation Example :
In Tool Summary :
(#7 - END MILL D 8MM COMP NCCONTROL - RADIUS COR VALUE 4)
On Tool Called :
N5 (POCKET - FINISHING) (COMP NCCONTROL - RADIUS CORRECTOR VALUE 4) (END MILL D 8MM)
Tool Wear Example :
In Tool Summary :
(#7 - END MILL D 8MM COMP TOOLWEAR - RADIUS COR VALUE 0)
On Tool Called :
N5 (POCKET - FINISHING) (COMP TOOLWEAR - RADIUS CORRECTOR VALUE 0) (END MILL D 8MM)
In this way , directly from gcode , you can see what compensation mode is going to be activated , and what value have the machinist have to insert in the machine tool table.
From this comments ,you have to set the tool diameter only with CNC Compensation, with the other two modes you have to set to 0 the tool diameter.