Probe sets work offsets

[endmill]

Help! I have Fanuc 15m control one on Niigata one on a Daewoo. They both use probes to det work offsets. I can get all the probe macros to work on the Daewoo except for the macro that writes to the work offsets (G54-59) It all works fine on the Niigata. All the effective parameters are the same. Does this have something to do with ladder logic? I'm stumped..

[psychomill]

Have you done a file compare on the macro routines to see if any code (or variable used) is different? Don't change it necessarily, the machine may need it or use it in a different way. Just see if the subs (programs) are different. Just guessing here...

[endmill]

They are the same subs and programs

[psychomill]

Any alarms or just 'nothing happens'? Maybe the variable sets are different on the Daewoo for machine position and/or offset position. Will any of the macros (Bore/Boss, point, web etc) set any offsets? Or all of them work but won't set an offset?

[endmill]

All the probe macros call another to make the offsets. They all call the same macro to set the offsets. I am baffled no alarms no nothing. The program keeps running. It just doesn't make the offsets, thus it positions wrong after it exits probe routine, and goes back to the main program.

[psychomill]

May need to bust out the Daewoo programming manual (if you have one) and a probe programming manual (if you have one) and step through the macro. Verify that the variables its using to set the coordinates are correct for the machine. If you MDI the same variables for offsets will it set?

[endmill]

I've busted them out over thru and on the behind. It will set with a G10Pi just not with the macro. I should have time today to look closer at the daewoo manual. Fanuc told me nothing. Thanks for the ideas. The boss said to call Fanuc. I told him it was personal now, just me and daewoo.

[psychomill]

Try this in MDI....

G90
#5221=5. (Sets G54x)
#5222=5. (Sets G54y)
#5223=5. (Sets G54z)

You should see a "5." in G54 XYZ.

Now try this, move your machine to some position by jogging or handle. Make sure you move X,Y and Z. Now don't move the machine and in MDI try this:

G90
#5241=#5021
#5242=#5022
#5243=#5023

Now check G55 position. It should match your current 'machine position'.

[endmill]

I got it...In the ladder logic. G5.7 is a protect switch for key4 or on the pcdgn screen searchb for g5 this shows the bits bit 7 is off should be on. this is read from an eprom chip. Fanuc will have to burn a new eprom or we will have to manually set this at power on each day. I'll go with the Fanuc option.
Thank you for your help

[psychomill]

Wow! Thats unusual... Glad you found the problem. Most problems I've seen were up front.

[Al_The_Man]

Originally Posted by endmill In the ladder logic. G5.7 is a protect switch for key4 or on the pcdgn screen searchb for g5 this shows the bits bit 7 is off should be on. this is read from an eprom chip. Fanuc will have to burn a new eprom or we will have to manually set this at power on each day. I'll go with the Fanuc option.

Usually the machine tool builder is responsible for taking care of this (Daewoo).
You may have to get them to ship one out, and may be it was an oversight on their part originally.
Al.

[Eddieconklin]

I need some help,
I have a machine Job shop with 10 horizontals and 6 verticals. Our set-ups are slow and our operators have never worked with renishaw probes are non contact lasers. We have manual tool setter. We have a demand of about 50 set-ups a day with the average job box of about 7 pieces. Can anyone explain what the probes and laser can do to help me ? And are there any other things we can do to reduce our set-ups
Eddie