PDA

View Full Version : Diameter offset



qmas99
03-23-2008, 05:55 PM
Hi,
Is there any way that I can change tool diameter offset same as tool length offset, instead of 50+?
Thanks

Adam Hubert
03-24-2008, 08:31 PM
I'm assuming that you might be talking about lines such as:

T1 M06
G43 H1 D51 G0 X5.0, etc - you want the D51 to Be D1

Please note that many don't believe in putting the D number on a line such as the one above. Not a big deal but what if you aren't using compensation in that operation.

Therefore many do not put the D number on that line but instead only put it in when compensation is checked in the Operations dialog box such that the output is the following:

G41 D1 X0, etc.

Configured properly the SolidCAM post output can be setup either way.


This behavior is driven by some logic in your *.mac file. Either in the @change_tool call or the @compensation call. The makeup of some controller offset register tables sometimes does not allow the T, H, and D values to be the same. Therefore you sometimes see D values coming out the the 30's, 40's, or 50's.

If you open up your *.mac file and go to the @change_tool area or the @compensation area you will very likely see some instructions that are forcing this to happen. Hard to tell exactly what or where due to the fact that the words and structure of GPPTool language can vary dramatically from post to post.

Perhaps you will see something in @change_tool like the following. For T1 it outputs D31, T2 it outputs D32, etc. Of course the +30 is causing this.

{nb, 'G'gcode, ' H'tool_number, ' D'(tool_number+30), ' '}


Another one in @change_tool looks like the following:For T1 it outputs D1, T2 it outputs D2, etc.

{nb, 'G'gcode, ' H'tool_number,' D'(tool_number),' '}


Another looks like the following. This one only outputs the D number not from the @change_tool call but from the @compensation call when compensation is checked in the Operation dialog box.

in @change_tool {nb, 'G'gcode, ' H'tool_number' '}
in @compensation {nb, 'G'gcode, ' D'(tool_number),' '}




Hi,
Is there any way that I can change tool diameter offset same as tool length offset, instead of 50+?
Thanks