tool offset cancel problem

[zoeper]

Hi,

I have got a funny problem on a Victor tns turning center with fanuc 10t controll.

All runs well, but whenever you cancel the tool 4 offset (T0400) the machine will wait for the command to finish..and wait.. and wait. The only way to get it to continue is to spin the chuck a couple of times by hand. It seems like it is waiting for a signal from the spindle encoder??
If anyone can shed some light on why this would only happen with the no. 4 tool i would be most gratefull to hear your theory.

Thanx
Pieter

[Karl_T]

If you can get to usenet, find the group alt.machines.cnc

There's a couple of real sharp Fanuc folks that hang out there.

Karl

[zoeper]

Karl T,
I heve never used usenet before, and cannot post any questions, Am i missing something? and where do you go for usenet?
Thanx
Pieter

[timlkallam]

http://groups.google.com/group/alt.m...n&lr=&ie=UTF-8

[Dan Fritz]

Is it possible that you're in G99 (feed per revolution) mode when you're canceling this offset? That's the only reason I can think of for the control to wait for the spindle encoder.

If you were in a feed motion (G01) and in feed/rev. (G99) at the same time, the axis motion can't happen unless the spindle rotates. If you look at the command screen, you should be able to see what G-codes are effective. Look for a combination of G99 and G01. If the tool offset motion in X-Z can't finish, because the spindle is stopped, then the control will just stop and sit there. The next time you have to manually rotate the spindle, watch the position display and see if X or Z moves as you turn it.

If you inspect your program, you will probably see some difference between how you're stopping the spindle and cancelling the offset for tool 4 and the way you're doing it for the rest of the tools. Even if you do it the same way, your spindle may be coming to a stop a bit quicker on tool 4, stopping the axes before the motion is complete.

[zoeper]

Dan,
Thanx for your thoughts. I do not think the G99 is the cause of the problem, as the command normally preceding the tool offset cancell is G28U0.W0. M05(home command)
As G28 happens at the rapid feedrate there should be no reason at al to expect movement. This also happens in MDI mode
Further, we are talking lathe here and the problem occurs only on the 4 tool (reagrdless of the weight of the part) so stopping should be consitent throughout.

All the more reason for calling it a weird problem???

[Dan Fritz]

zoeper:

Please post the segment of your program where the hangup occurs. About 5 blocks before & after the offset cancel is enough.

The G28U0W0 command does cause a rapid move, but it's not modal. If you're in G01 and G99 before the G28, you'll still be in that mode after the axes go home. Try putting a G00 in there with the G28 command and see if that fixes it.

Also, cancelling a tool offset on a lathe is very different from cancelling an offset on a mill. Fanuc lathes will actually move when you give it the T-command to activate or deactivate a tool offset. Your offset may be very small, but that won't matter.

Fanucs have a very small "in-position" zone, and if a feed motion is not completed so all axes are within this zone, then the control can't execute the next block.

A big clue would be to find out if the X or Z axes move (at all) as you manually rotate the chuck.

[zoeper]

We're onto something here,
It took me a long time now to simulate the problem. I ran the same program i did the other day when it happened, except for changing the spindle speed to 1000rpm(instead of 2500) to avoid having to warm the machine up. As these things go i had a hell of a time to get it to create the same problem. It did eventually once i upped the speed again and as predicted, there was movement on the x axis as as the spindle rotated.
Combination of momentum, braking etc etc. I am nut sure that this is normal, but i should be able to avoid getting the problem in future.

Thanks for your input
Pieter

[Karl_T]

Originally Posted by zoeper Karl T, I heve never used usenet before, and cannot post any questions, Am i missing something? and where do you go for usenet? Thanx Pieter

Usenet FAQ:

http://www.faqs.org/usenet/