Probing within g code program on a Fanuc I series

[Glang]

I set up an operate a Doosan DNM 750 II. We have the renishaw probing package.I currently probe each part prior to running by using the controller GUI interface. Rather than using the Interface, I would like to add them macro probing code to the beginning of my program so it is all automated. I don’t have any access to manuals. Can anybody help with the auto macro probing cycles? Thank for reading!!!

 

[sinha]

Do you have some knowledge of Custom Macro B?

 

[Glang]

Not much, I thought the programs were already written and I would just have to edit the variables

 

[pato]

The base programs should be there, but you should probably find or download the manuals to know what probe cycles to call and what variables control what in that cycle. You may be able to copy the output from the GUI into your program as well, but you should have a basic knowledge of what it is doing which you can get from the manuals.

A basic probe blank for center in X program would look something like this(I think, it's been a little while since I ran anything with a Fanuc control)

T100M6(PROBE)
G90G00G54X0Y0
G65P9832 (PROBE ON)
G43H100Z3.
G65P9810 Z.2 F250. (PROTECTED MOVE TO Z.2, WILL ALARM OUT IF PROBE HITS ANYTHING)
G65P9812 X2. Z-.5 R.2 S1(PROBE 2" WIDE WEB, OUTPUT TO G54, S2 WOULD BE G55, ECT...)
G65P9810 Z3.
G65P9833 (PROBE OFF)
ECT.....

 

[13engines]

If you have the Renishaw probing software, then you have the manuals, as they come with the software. If your boss doesn't have the manual, I'm sure you can download it as has been suggested.

Regardless, if all you're after is mostly work offset setting, you can use the simple Go Probe part of the software. (G65 P9901) (Look for it on your control) The various probing cycles embedded in the Go Probe software store their result directory into work offsets, and into known variables that you can access and use, if you need to add a few Macro B program lines after the initial probing cycle. It would do you good to work with the Go Probe cycles regularly. They're simple and logical enough that in a short amount of time you can have most of them memorized. If memorizing isn't your thing, there is a phone app that can supply you with the command line for all the various cycles. Your particular variables can be input into any of the Go Probe cycles. And no I don't work for Renishaw. I just use it a lot. :-)

 

[AMeador]

Hey man. Doosan did things a little different. G Codes won't trigger the probe because they use M Code M165 to do this. M165 P9XXX will trigger the different cycles.
I have the Doosan manual showing the different cycles & steps at work. If no one has uploaded it by in the morning I'll attach it for you. But basically you can run what Pato said, just change G65 to M165.

Best of luck!
A. Meador

 

[Glang]

Hey man. Doosan did things a little different. G Codes won't trigger the probe because they use M Code M165 to do this. M165 P9XXX will trigger the different cycles.
I have the Doosan manual showing the different cycles & steps at work. If no one has uploaded it by in the morning I'll attach it for you. But basically you can run what Pato said, just change G65 to M165.

Best of luck!
A. Meador

Thanks, I was gonna do some more research tomorrow but I think got it right! I experimented with the G 65 a while ago and couldn’t get anything to work. I any help would be greatly appreciated, we don’t have the manuals at work or they’re on the lock and key and I’m unaware.

 

[Glang]

The base programs should be there, but you should probably find or download the manuals to know what probe cycles to call and what variables control what in that cycle. You may be able to copy the output from the GUI into your program as well, but you should have a basic knowledge of what it is doing which you can get from the manuals.

A basic probe blank for center in X program would look something like this(I think, it's been a little while since I ran anything with a Fanuc control)

T100M6(PROBE)
G90G00G54X0Y0
G65P9832 (PROBE ON)
G43H100Z3.
G65P9810 Z.2 F250. (PROTECTED MOVE TO Z.2, WILL ALARM OUT IF PROBE HITS ANYTHING)
G65P9812 X2. Z-.5 R.2 S1(PROBE 2" WIDE WEB, OUTPUT TO G54, S2 WOULD BE G55, ECT...)
G65P9810 Z3.
G65P9833 (PROBE OFF)
ECT.....

Thanks

 

[DouglasJRizzo]

The Renishaw cycles are imbedded in the control, standard.
So, if you wanted to probe during a part cycle you would:

Call up the probe.
Set probe conditions
Call probe cycle.
Retract probe.
Shut down probe.
Call next tool.

It's in the additional Renishaw manual.
If you don't have it, PM me.
These cycles are standard.

 

[LockNut]

M165 is indeed the method used by us (Doosan) to call Inspection Plus routines from the GUI software. It covers all but the multi-axis probing routines from Inspection Plus.

Paul

 

[MaxPrairie]

You may not have physical Renishaw manuals, mine were given to me as a pdf on a usb drive.

 

[Glang]

If you have the Renishaw probing software, then you have the manuals, as they come with the software. If your boss doesn't have the manual, I'm sure you can download it as has been suggested.

Regardless, if all you're after is mostly work offset setting, you can use the simple Go Probe part of the software. (G65 P9901) (Look for it on your control) The various probing cycles embedded in the Go Probe software store their result directory into work offsets, and into known variables that you can access and use, if you need to add a few Macro B program lines after the initial probing cycle. It would do you good to work with the Go Probe cycles regularly. They're simple and logical enough that in a short amount of time you can have most of them memorized. If memorizing isn't your thing, there is a phone app that can supply you with the command line for all the various cycles. Your particular variables can be input into any of the Go Probe cycles. And no I don't work for Renishaw. I just use it a lot.

Thanks

 

[Glang]

Thanks for the reply’s everyone, I was able to turn the probe on and off with G65 P8501 (on)
G65 P8053 (off)
I cannot tell what other Macros would be used. The program numbers y’all have suggested don’t work or don’t exist on my drive. Or I can’t locate them.

 

[LockNut]

Keep in mind that the GUI covers most of the Inspection Plus routines. Having the normal Inspection Plus in addition to the GUI means you will have to calibrate for each. It is much easier and less painless than trying to maintain both sets of calibration data. The GUI macros are stored in the macro executor memory of the machine, not in the standard CNC memory.

 

[LockNut]

Thanks for the reply’s everyone, I was able to turn the probe on and off with G65 P8501 (on)
G65 P8053 (off)
I cannot tell what other Macros would be used. The program numbers y’all have suggested don’t work or don’t exist on my drive. Or I can’t locate them.

They won't be on your drive because Doosan stores them in the macro executor area of machine memory not in standard program memory. This saves valuable memory area for programs.

 

[Glang]

Here is a snapshot of the directory where 8501 and 8503 reside.

 

[Glang]

Here is a snapshot of the directory where 8501 and 8503 reside.

 

[Glang]

File too large arghhh

 

[Glang]

They won't be on your drive because Doosan stores them in the macro executor area of machine memory not in standard program memory. This saves valuable memory area for programs.

Ok this makes sense as to why I can’t see them. Wow without the manuals Iwill not be able to figure this out. Thx

 

[LockNut]

Ok this makes sense as to why I can’t see them. Wow without the manuals Iwill not be able to figure this out. Thx

Email me at [email protected] and I will send them to you.