Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Probing cycle is not writing to macros


Recommended Posts

Hi all,

I'm using a probing cycle that I've used before with no problems, but now the cycle is not writing to a macro. The macro just stays DATA EMPTY. Is it possible that I flipped a switch somewhere that doesn't allow probing cycles to write to the macros? Machine is a doosan dnm5700 with fanuc controls. If I haven't provided enough info, let me know. Also, #139 is a volatile macro, so I set #500 equal to #139 immediately.

Code;

N100
(2MM DIA PROBE)
(PROBE PART & ROTATE G54 OFFSET)
G0G20G17G40G49G80G90G53Z0.
T1M6
G0G54X3.873Y.09
G43H1Z5.0T2
M165 P9832(PROBE ON)
M165 P9810 Z1.35 F100.(SAFE MOVE)
M165 P9843 Y0. D1.3(MEASURE ANGLE TO #139)
#500=#139(SET #500 EQUAL TO #139)
M165 P9833(PROBE OFF)
G0G53Z0.
M01
Link to comment
Share on other sites
1 minute ago, JParis said:

So after you run your macro does #139 have a value?

I am thinking you're missing a definition of your 9843 call and #139 is just blank

#139 stays DATA EMPTY the whole time. 9843 has always written to this macro, now all of a sudden its not. No idea what changed.

Link to comment
Share on other sites
2 minutes ago, JParis said:

I look at this line and think it should be 9810 not 981


M165 P981 0Z1.35 F100.(SAFE MOVE)

 

 

It is P9810, I pasted the code in here without spaces added the spaces. That was a mistake just on this post.

Link to comment
Share on other sites

It has been a long time since i have worked on a Fanuc, but two things are coming to mind. First IIRC there is a parameter that makes the control retain #100+ variables after reset/M30. Second, it could be losing the values after the jump out of the 9843 program to the main. Try putting the #500=#139 at the end of the 9843 macro. Or look inside there to make sure it is not being cleared in there. 

Link to comment
Share on other sites
17 minutes ago, YoDoug® said:

It has been a long time since i have worked on a Fanuc, but two things are coming to mind. First IIRC there is a parameter that makes the control retain #100+ variables after reset/M30. Second, it could be losing the values after the jump out of the 9843 program to the main. Try putting the #500=#139 at the end of the 9843 macro. Or look inside there to make sure it is not being cleared in there. 

I don't believe I have access to those cycles. If I do, I don't know how to access them.

Link to comment
Share on other sites
18 minutes ago, YoDoug® said:

It has been a long time since i have worked on a Fanuc, but two things are coming to mind. First IIRC there is a parameter that makes the control retain #100+ variables after reset/M30. Second, it could be losing the values after the jump out of the 9843 program to the main. Try putting the #500=#139 at the end of the 9843 macro. Or look inside there to make sure it is not being cleared in there. 

I don't remember the parameter, but you are correct that there is one to reset the variables at M99 or M30.

Link to comment
Share on other sites
Just now, Sticky said:

I don't remember the parameter, but you are correct that there is one to reset the variables at M99 or M30.

Yes but I am not even seeing #139 update for even a fraction of a second. Right now I have to get the parts done so I am indicating each one. After, I will test this cycle out on something else. 

Link to comment
Share on other sites
3 minutes ago, Tinger said:

Yes but I am not even seeing #139 update for even a fraction of a second. Right now I have to get the parts done so I am indicating each one. After, I will test this cycle out on something else. 

You might not necessarily be able to see it. The PMC can process data way faster than it can update the HMI display. 

  • Like 1
Link to comment
Share on other sites
4 minutes ago, Tinger said:

Yes but I am not even seeing #139 update for even a fraction of a second. Right now I have to get the parts done so I am indicating each one. After, I will test this cycle out on something else. 

Run a few different cycles that also write data to #139 and see if any of them will still write. That will help you narrow your search down to a problem local to your program, or more global ie parameters.

1 minute ago, YoDoug® said:

You might not necessarily be able to see it. The PMC can process data way faster than it can update the HMI display. 

That's a good point, we have a 31i that way. I usually put a M1 in between my cycles and turn the block skip when trying this stuff out.

  • Like 2
Link to comment
Share on other sites
2 minutes ago, Sticky said:

That's a good point, we have a 31i that way. I usually put a M1 in between my cycles and turn the block skip when trying this stuff out.

Also, having #6001.6 = 1 helps the cause so it doesn;t disappear right after the cycle is complete.

  • Like 2
Link to comment
Share on other sites

All of our (Doosan) machines have an app in the control to simplify most Renishaw and Blum probing cycles. Mostly for setting work offsets and such. All of the probing macros are embedded in the macro executor and they cannot be accessed or edited. In addition to that, you can run most Inspection Plus macros by using M165 instead of G65. We did this partly so that all of the Inspection Plus macros did not have to be loaded into memory on low memory machines since Fanuc cheaps out on memory. In the config screen there is a setting whether or not to output values to the macro variables. It seems his was set to NO somehow. I'm almost sure this was the issue.

I responded because sometimes people don't come back to explain when a solution is found.

Paul

  • Like 1
Link to comment
Share on other sites
15 hours ago, cncappsjames said:

On a FANUC, Parameter #6001.6 = 1. This makes variables #100-#199 not reset until changed or control is powered off.

 

HTH

James, can that just be ran in MDI or do you have to go through the setting process?

14 minutes ago, PAnderson said:

...since Fanuc cheaps out on memory...

Just wanted to make sure everyone saw this.  You know, because the fire hasn't started yet.

  • Like 1
  • Haha 1
Link to comment
Share on other sites

Hello everybody, 

Sorry for wasting your time!! Paul is right. I had a simple setting set wrong. 🤦‍♂️

I haven't actually retried the program since I just indicated all the parts, but it's probably fixed... 

Go easy on me I'm only 22 🤣

  • Like 1
Link to comment
Share on other sites
53 minutes ago, Tinger said:

Hello everybody, 

Sorry for wasting your time!! Paul is right. I had a simple setting set wrong. 🤦‍♂️

I haven't actually retried the program since I just indicated all the parts, but it's probably fixed... 

Go easy on me I'm only 22 🤣

Tinger, not a waste of time. This is how we learn.

  • Thanks 1
  • Like 2
Link to comment
Share on other sites
8 hours ago, jlw™ said:

James, can that just be ran in MDI or do you have to go through the setting process?

Just wanted to make sure everyone saw this.  You know, because the fire hasn't started yet.

It's an actual parameter so you may need to enable parameter write

  • Like 1
Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...