[rweaver5302]

Cutter Comp Help Requested


I'm running Dolphin Partmaster V13 along with Mach3 on a 3 axis bridgeport style mill and I can't seem to get Dolphin to output a file using G41/G42 when using the post processor for Mach3 on a 2D profile - or any profile for that matter. I'm not cutting a pockect - use a regular profile cut.

I'll set up a profile to cut using the "goround" command and select "Use part surface programming", and yet no G42/G41. If I switch to a different post processor - something other them Mach3 - with the same cutter path, Dolphin includes G41/G42 in the G-code program when posted.

I'm thinking it is a problem with the post processor since I can get G41/G42 when I select a different post processor.

Any one else run into a similar problem?


Thanks in advance.

Randy

[andre-dolphin]

Hello,

Yes, you're right, for some reason the cutter comp has been switched off in the post M_MACH3.

I have attached a zip file contains a modified version called M_MACH-CC

Instructions below on how to import the post after it has been unzipped.

Run the Post processor from the desktop.
From the startup menu choose Import Post and browse the the location where the post was unzipped
The post processor will be imported
From the toolbar choose Compile.
Exit the post module.

The new post will available when you next run CAM.

Don't forget to choose the new name from the pull down list

ATB
Andre

[rweaver5302]

Thanks for the quick response, I'll give it a try.

I plan on putting it right to use -

Thanks again,

Randy

[mmmilligan]

Output of Cutter Radius Comp codes (typically G41/G42) depends on the configuration of the Post Processor file.

Many posts are configured only to output CRC code when the option 'Part Surface Programming' is selected in the Options tab of the Goround feature.

Basically Dolphin Partmaster can output one of two Toolpaths i.e.

1) The fully offset path of the cutter centre complete with corner rolling & span elimination as required.

2) The path of the original un-offset geometry (referred to in dcam as 'Part Surface').

With option 1) all offsetting is handled by dcam so G41/G42 is not required, although some Clients still prefer it to be output to compensate for tool wear.

With option 2) the CNC Control is presented with Part Surface Geometry and is responsible for all offsetting, in this case G41/G42 is required to activate compensation.

If a post is not outputting the required CRC codes it is usually because it is configured to only output these codes when Part Surface is selected and the Client is not selecting this option.

If anyone is experiencing difficulty with this please contact me direct ( [email protected] ) and I will modify their post .ppr file accordingly.

Michael
Dolphin Cad Cam Systems Ltd