Todd,
The is a field set aside in the Planner for
"Finish Allowance" in the following operations:
Rough Milling
Face Milling
Copy Milling
Surface Milling
This value is not actively used by SmartCAM straight
out of the box but can be accessed by using the jos
data tag "cutfin".
To output this value to code with the template file
you need to assign the value to a template variable.
i.e. #EVAL(#V0=jos(cutfin))
Then use the template variable to output the value
in the desired format in the @START, @TOOLCHG and
@STEPCHG template sections.
i.e. ( OVERBURN = #V0 )
You can also use this data tag in the various control
panels for creating meshes or surface machining. You
would type in "jos(cutfin)" the field for finish
allowance and it would extract the value from the
Planner.
You could also use the "File - Keep Defaults" function
to have the tag as a default entry in the panel.
=============================================
Fred Lauzus, CAM Programming Coordinator
High Steel Structures, Incorporated
mailto:[EMAIL PROTECTED] http://www.highsteel.com
=============================================
-----Original Message-----
From: D G Bowen [mailto:[EMAIL PROTECTED]]
Sent: Wednesday, November 29, 2000 9:15 PM
To: Todd Crosby; SmartCam
Subject: Re: [mfg-smartcam] FINISH ALLOWANCE ?
> Hi all ,
> When creating cutterpath for electrodes from models (mesh or surface
> machining) I typically use a negative finish allowance to create desired
> overburn. Does anyone know of a way to get this finish allowance value
> into the posted program? Is it even saved anywhere ? By the time the
> trodes are ready to burn I never remember what was used.
>
> Todd Crosby
Todd,
One way would be to go into the planner and manually enter the info into the
Step Notes. Then you can output the info in your posted file using the
#TLCMT variable.
I don't have any idea where the info might be saved. I doubt that it is.
I have a question for you: do you know a trick to surface machine using a
negative finish allowance greater than the tool radius? I need to cut
multiple surfaces .150" undersize with a 1/8" ball mill.
Gene Bowen
======================================================================
To find out more about this mailing list including how to unsubscribe,
send the message "info mfg-smartcam" to [EMAIL PROTECTED]
======================================================================
======================================================================
To find out more about this mailing list including how to unsubscribe,
send the message "info mfg-smartcam" to [EMAIL PROTECTED]
======================================================================
