Printable View
my V30 with okuma osp200 post processor is outputting an arc calculation error, ive used this post hundreds of times and never had an issue, anyone have any insight on this? where to start looking? its a large program and i couldnt possibly track down the error and make the corrections manually. thanks.
Does it error when running in Preditor Editor Backplot ?
If so that would be it where it stops
Or does it error only at the machine ?If so that part of the program where it goes screwy should point to it
Do you not have any line numbers in program ?
What kind of part you running.An engraving ?
Engraving of .dxf files can sometimes give problems
Track down with Preditor when and where it happens
Sometimes it is just a slight drawing error
Couple things.
Did you set arc fit at the feature level?
There are a couple places in the post processor to set arc handling that can help with large calc files.
As jr mentioned, geometry can be the culprit.
Where in the chain is the error? Ie; upon caculation, simulation, posting, at the machine control, etc.......
i tried to chase down the problem manually but gave up. i tightened up the arc fit and it is now running, the new problem im having is the machine will stop momentarily everytime it switches between a G01, G02, G03 command and being that the program is now broken down into tiny line and arc segments, the machining process looks like sh*t.....
i suspect this is something in my controller that i need to address? a look ahead parameter or something of the sort?
Is it a 3d tool path,engraving ???
can you share a file,,or pm it
I assume the machine is a mill...Quote:
Originally Posted by jay_dizzle
... small linear moves are what is creating the stutter ( executing the moves faster than what the program can be read... a standard issue ) (Adjusting or turning OFF tolerance control in the machine may improve smoothness ... if you have it )
look to see if the CAM system can "fit arcs" to the calculated paths to minimise the point-to-point programming..... Maybe something related to "tolerance" or "fit arc tolerance"
.... some CAM systems output small line segments on splines, you may have to replace splines with arcs before creating the toolpaths.
it seems as though i need to change the arc fit tolerance in the CAM system to match the maximum allowable deviance that is set in the machine parameters, this would give me the smoothest machining operation while still staying within the allowable amount of arc calc error.Quote:
Originally Posted by Superman
it was a 3D tool path, unfortunately, i deleted the file (i had a bit of a temper tantrum) and started fresh, i messed with the arc fit tolerance and matched them to the machine parameters, the process got a lot smoother and the alarms are no longer an issue.Quote:
Originally Posted by jrmach