Change Fanuc 10T from Metric to English

TimD · Dec 5, 2013

Picked up a used lathe with a Fanuc 10T control. Anyone know what parameters to change for it to display in inches? I assume I'll also have to update the parameters for soft limits and such?

Thanks
Tim

angelw · Dec 5, 2013

TimD said:
Picked up a used lathe with a Fanuc 10T control. Anyone know what parameters to change for it to display in inches? I assume I'll also have to update the parameters for soft limits and such?

Thanks
Tim

Hi Tim,
You do this by executing G20 (Imperial Designation) in either MDI or via a program. The machine will power up in the the last executed G20/G21 mode.

1. Its a safer practice to include G20/G21 in a typical safety block at the very beginning of all program. This safeguards against running a program, the units of which contradict the Imperial/Metric system setting of the machine. Things will get a bit untidy if a machine set in Imperial Mode is fed a Metric Unit program. Z-50.0 (mm) will be interpreted as Z-50.0 (inches) in an Imperial set machine; that scenario will most likely end in tears.

2. G20 and G21 must not be switched during the normal running of a program. That is, you can't have both Imperial and Metric units in the one program and switch between the two using G20/G21.

3. When the machine unit and the input unit systems are different, the max error is half the least command increment and does not accumulate. See parameter 1004 for Least Command and Least Input Increments.

4. When switching between G20 and G21, the Work Coordinate System Shift must be reset, but Tool Offset values are automatically switched between inch and metric.

Soft Limits are normally not affected, but any Stored Stroke limits to define forbidden areas turned on and off by G22/G23 respectively, should be looked at.

Regards,

Bill

machtool · Dec 6, 2013

angelw said:
Things will get a bit untidy if a machine set in Imperial Mode is fed a Metric Unit program. Z-50.0 (mm) will be interpreted as Z-50.0 (inches) in an Imperial set machine; that scenario will most likely end in tears.

Yes indeed. The probability of having a crash goes up 25.4 times when that happens.

Regards Phil.

TimD · Dec 6, 2013

Bill, Thank you for the info. I've said it before and will say it again you have shared a wealth of knowledge on this forum and it is much appreciated.

Gave the G20 from MDI a try and got this error:

PS010 IMPROGER G-CODE

Gave G21 a try as well and got the same error.

Any other ideas?
Tim

beege · Dec 6, 2013

Sometimes G70/G71 have been used for metric/inch.

TimD · Dec 6, 2013

Well took a look at the programs that were in the machine from previous owner. The programs certainly appear to be in inches and there is a G20 in the program. Tried to execute the G20 via program and still get the same error. Makes me think that the dealer had to reload parameters and didn't get them all right :angry:

I think there was a parameter print out. I guess I'll start paging through that...

angelw · Dec 6, 2013

TimD said:
Bill, Thank you for the info. I've said it before and will say it again you have shared a wealth of knowledge on this forum and it is much appreciated.

Gave the G20 from MDI a try and got this error:

PS010 IMPROGER G-CODE

Gave G21 a try as well and got the same error.

Any other ideas?
Tim

Hi Tim,
Beege is quite correct. There are 3 "G" Code systems available, A, B, and C. Overwhelmingly, System "A" is the norm, but given the alarm that you've listed, its likely that your machine is equipped with System "C". Take a look at parameter bits 7 and 6, the two left most bits of parameter 2400. If set to 1 and 0 respectively, then your control is set to System "C".

"G" Code System "C" is an Optional function. Unless you have a particular reason for wanting to use the machine with "G" Code System "C", I'd suggest setting the parameter so that the control uses System "A". You will find that there will be more people able to answer your questions, should you have any, about System "A" than for "B" and "C", but particularly System "C". Apart from the "G" Code to switch from Imperial to Metric, or vice versa, there are many other "G" codes that are different to System "A".

To select "G" Code System "A", parameter bits 2400.7 and 2400.6 should both be "0".

Regards,

Bill

TimD · Dec 6, 2013

Tried G70/71 and got the error:

PS067 G70-G73 AT FORBIDDEN MODE

Parameter 2400 bit 7 and 6 are both 0
00010010

angelw · Dec 6, 2013

TimD said:
Well took a look at the programs that were in the machine from previous owner. The programs certainly appear to be in inches and there is a G20 in the program. Tried to execute the G20 via program and still get the same error. Makes me think that the dealer had to reload parameters and didn't get them all right

I think there was a parameter print out. I guess I'll start paging through that...

Hi Tim,
If you're lucky, there should be an Executive Tape with the machine that's used to load all the parameters. If not, and you have a printout of the parameters, you will find it easier and less error prone, to type all the parameters using a Text Editor/Communication software package, and reload the parameters via RS232. Check first with your list, that there are many to change first though.

If you choose to download them form a PC, they have to be in a particular format. You can determine this format by Uploading the current parameters of the control to the PC and copying the format for those you want to Upload.

Of course, you will have to manually set the parameters for RS232 comms with the control before being able to Up and Download to the control.

Regards,

Bill

angelw · Dec 6, 2013

TimD said:
Tried G70/71 and got the error:

PS067 G70-G73 AT FORBIDDEN MODE

Parameter 2400 bit 7 and 6 are both 0
00010010

Hi Tim,
That's a bit of a worry. Normally all controls have System "A", even if equipped with the Option Function System "C".

Try setting "1" below for parameter 2400 and then try to execute G20 again. If still an error, try setting "2" and execute G70 to see if that still gives an error.

Make sure that you document all that you change so that you can get back to square one if required.

1. 01010010

2. 10010110

Regards,

Bill

TimD · Dec 6, 2013

Tried both setting 1 and 2 with there respective codes are received the same errors. Have returned param 2400 to original state.

The parameter list that I have shows 2400 originally as 00011010 but was hand corrected to 00010010

The live tooling and c-axis seem to function fine so I wasn't too worried about having issues when I inspected. Would seem odd that those work but this is a bit wonky. Thought I would mention it.

Thank you again for all your help so far Bill. It's greatly appreciated.

Also begee I have to thank you as well. I remembered that PWE was 8000.0 but it wouldn't let me change it. It was a post of yours I found that pointed out it needed to be changed in settings so thank you for that!

Tim

angelw · Dec 6, 2013

TimD said:
The parameter list that I have shows 2400 originally as 00011010 but was hand corrected to 00010010

Hi Tim,
Bit 3 of parameter 2400 shown above in Red is irrelevant, and has no function with this control. Accordingly, it can be set either way.

If you're fortunate to still have the Control Specification sheet with the machine, check to see if the machine was supplied with "G" Code System "C" or not. If yes, and you're suspicious that the parameters may have been lost, then this "G" Code System will have to be reinstated via an Option Parameter. These should also be listed in the Spec sheet. However, System A and B are basic functions and should be available whether or not the control has the Option Function "G" Code System C.

TimD said:
Tried G70/71 and got the error:

PS067 G70-G73 AT FORBIDDEN MODE

Parameter 2400 bit 7 and 6 are both 0
00010010

When either "G" Code System A or B is selected, "G" codes G70 through G73 can only be executed in Memory Mode. Accordingly, write a one line program of G71 and with parameter 2400 set for either "G" Code System A, or B, execute it in Memory mode. You will get some errors, because its not being used correctly, but as long as you don't get a P/S 010 alarm, you will be progressing in the right direction.

Regards,

Bill

TimD · Dec 6, 2013

angelw said:
Hi Tim,
If you're fortunate to still have the Control Specification sheet with the machine, check to see if the machine was supplied with "G" Code System "C" or not. If yes, and you're suspicious that the parameters may have been lost, then this "G" Code System will have to be reinstated via an Option Parameter. These should also be listed in the Spec sheet. However, System A and B are basic functions and should be available whether or not the control has the Option Function "G" Code System C.

Thought I had a spec sheet but upon inspection it's for a completely different machine, a mill with a 6M...

angelw said:
When either "G" Code System A or B is selected, "G" codes G70 through G73 can only be executed in Memory Mode. Accordingly, write a one line program of G71 and with parameter 2400 set for either "G" Code System A, or B, execute it in Memory mode. You will get some errors, because its not being used correctly, but as long as you don't get a P/S 010 alarm, you will be progressing in the right direction.

Spot on. Executed a G71 from memory with a missing P and Q error, for obvious reasons.

Went through my entire list of parameters and don't see much amiss. There are a lot of differences in 9101-9102 but most everything else seems to match the sheets supplied by Wasino.

I'm starting to think I'm just missing something stupid... Going to go look for something stupid

angelw · Dec 6, 2013

TimD said:
Thought I had a spec sheet but upon inspection it's for a completely different machine, a mill with a 6M...

Spot on. Executed a G71 from memory with a missing P and Q error, for obvious reasons.

Went through my entire list of parameters and don't see much amiss. There are a lot of differences in 9101-9102 but most everything else seems to match the sheets supplied by Wasino.

I'm starting to think I'm just missing something stupid... Going to go look for something stupid

Hi Tim,
Parameters 9101-9102 are two of the Option Parameters. Make sure you have a copy of ALL the 9000 series parameters in case something diabolical happens and you lose them. As soon as you can, you should get communication set up between control and PC so that you can download the parameter set that you currently have. It makes reinstating them easier when you have a digital copy of them.

Regards,

Bill

TimD · Dec 6, 2013

Started a new thread as it seems that this one is starting to going a different direction. New thread:
http://www.practicalmachinist.com/v...-10t-won-t-allow-g20-21-a-276426/#post2174009

Looking through the MTB manually they indicate that G-code System A is standard. Machine can be switched to System B and that System C is not available. So at least those were the options from the factory.

Was able to transfer the programs just fine but the parameters seemed to transfer in a very odd format. I'm at home now but will take another look at transferring the parameters in the morning. Not as handy as the digital version but I did write down all of the parameters that were different from the print out.

Thanks again.
Tim

angelw · Dec 6, 2013

TimD said:
Started a new thread as it seems that this one is starting to going a different direction. New thread:
http://www.practicalmachinist.com/v...-10t-won-t-allow-g20-21-a-276426/#post2174009

Looking through the MTB manually they indicate that G-code System A is standard. Machine can be switched to System B and that System C is not available. So at least those were the options from the factory.

Was able to transfer the programs just fine but the parameters seemed to transfer in a very odd format. I'm at home now but will take another look at transferring the parameters in the morning. Not as handy as the digital version but I did write down all of the parameters that were different from the print out.

Thanks again.
Tim

Hi Tim,

If the RS232 parameters are set correctly, and the settings of the Comms software are set to match those of the control parameters, there should be no unusual Format. The Program, whether being Up or Downloaded should look the same at the Control and PC end. If you can do a Cut and Paste of the resulting code after transfer, Post it here for the Forum to see.

List the parameter numbers that are different. If you can make a digital copy, you can PM me a copy and I'll let you know if any are significant.

Regards,

Bill

TimD · Dec 6, 2013

Bill,

When do you sleep? What time is down under? :Yawn:

The programs were fine, just like expected. Going to double check the param transfer in the AM, maybe I was just looking at them wrong.

Unless something comes to overnight I may just take you up on the offer to double check the altered parameters.

Thanks again and get some sleep
Tim

machtool · Dec 6, 2013

TimD said:
When do you sleep? What time is down under?

Its just coming up 3.00 P.M on a beautiful Saturday afternoon here where Bill & I are. Another hour and I'm cracking a beer.

Bill's last post (#16) would have been at 2.00 P.M

Regards Phil.

angelw · Dec 6, 2013

machtool said:
Its just coming up 3.00 P.M on a beautiful Saturday afternoon here where Bill & I are. Another hour and I'm cracking a beer.

Bill's last post (#16) would have been at 2.00 P.M

Regards Phil.

Good one Phil, cheers.

TimD · Dec 7, 2013

Sent you a PM with the changed parameters. I feel like a broken record but thank you again.

The parameters were transferring just fine. Didn't have my thinking cap on and was thinking 0 series. It did only transfer up to param 2900. I'm assuming there is a setting for that, will crack my books open.

Change Fanuc 10T from Metric to English

Hot Rolled

Diamond

Diamond

Hot Rolled

Stainless

Hot Rolled

Diamond

Hot Rolled

Diamond

Diamond

Hot Rolled

Diamond

Hot Rolled

Diamond

Hot Rolled

Diamond

Hot Rolled

Diamond

Diamond

Hot Rolled

Similar threads