This has me stumped

[lkenney]

Running a 1997 5020 with 5 vises on it. Programing with SurfCam Velocity 5.1 using Mpost to create Gcode.

On Monday i wrote a program using TrueMill and started a part that uses 4 of the vises so that we put in raw stock and take out a finished part everytime the machine stops. We went gangbusters all day Tuesday.

On vises 1 and 2 I use the same program to cut both sides of the part. I use E1 on Vise 1 and E2 on Vise 2 etc.

I run the 4 programs as subs under a master program whose sole purpuse is to call the next program.

Yesterday after a few catchup and setup runs with single programs to get my parts all at the same point.

I fired off my master progrma nad had a failur on the very first cut. It said that I had an error in my programming that I could not use a G3 on a fixture call or close I am at home right now and don't have my notes with me.

I went back and recreated the G-Code, Same error, I then ran the program for the other side that is done in Vise 2, exact same code except for name and location it ran fine.

Using NCeditor I compared the two programs they are exactly the same except for name and location.

Finally I changed Vise1 to be called by E5 and the program ran as it had the day before so we are making parts but I am puzzled as to why that happened and what is going on.

Thanks for any Ideas.

Lowell

[DareBee]

Usually I fix this error by going into the fixture offsets and deleting any A axis offsets that are present.

Don't ask me why this causes an error.
I NEVER use or input an offset into A - so I have no idea where or how they get there.

Neal can explain this issue (that still makes no sense to me).
Hope this works, otherwise I am out.

[lkenney]

I did notice that there was a 0.0250 in the B axis but since we don't have any boards forthe B I could not see where that would hurt us. I will look at it again.


thanks
Lowell

[Neal]

Explanation is this: When you are in Format 2 each individual axis offset in only applied when the program call for that specific axis to move. In Format 1, ALL fixture axis offsets are applied at the same time when ever the Fixture offset number is stated in the program.
If you ARE IN format 2 and have, for instance, a fixture offset value in the fixture table for the "B" axis but you do not call for any "B" axis movement AND the program calls for a G3 or G2 move you will get the error "FIXRURE OFFSET MUST BE APPLIED WITH G0 OR G1". This is termed a "pending" offset". One that have been called BUT not yet applied.
To correct this problem either call for a "B0" when you call the "E" code or remove the "pending" offset value from the fixture table.

I hope that answers the issue!

Neal

[lkenney]

Thank you, that makes sense, I guess. It does give me a way to cure the problem. These forums are great.

Lowell