look ahead parmeter on a fanuc 31i control

[Guest CNC Apps Guy 1]

quote:

---

...Is Fanuc calling/treating this as a bug?

...

---

AFAIK, they are not because there is an "easy" solution I just cannot seem to recall what it is... at this moment in time.

 

You should get in touch with Henry.

[kenfromlodi]

Yes we tried everything mentioned and were only able to get it to work with an M0 as mentioned above. Hopefully the tech will solve the issue.. (not feeling to confident about that tho..)

thanks for all the input..

[Tim Johnson]

Please keep us posted. Rumor has it here we're going to replace half our 18i horizontals which will have the 31i.

[Guest CNC Apps Guy 1]

On Toyoda's with 31i's we use M20's in Custom MACRO's... Works like a charm... It's called "Buffer Protect".

 

 

>>>>>>>>I DO NOT reccommed using this code in a Robodrill unless first confirmed by reading the Machine's Operation Manual and checking the G and M-Code list. The key word here is "Buffer".

 

HTH

[Grumpy Guy]

Latest update!

We have a brand new Robo Drill on the floor, less than a month old. The macro works perfect in this control. I am going to back up the prams and compare them to the other "newer" 31i machines that are not working to see what is different.

[iowajim62]

Jerome,

Did you talk to Henry ?

Instead of just comparing, how about loading the working parameters in the machine giving ya trouble ?

[Grumpy Guy]

No I do not want to change the parameters. If any thing goes wrong out comes the knives for my neck! you understand I am sure.........

 

We have all been there done that!!!!

[Dhysta]

On 11/11/2008 at 12:39 PM, Grumpy Guy said:

Latest update!

We have a brand new Robo Drill on the floor, less than a month old. The macro works perfect in this control. I am going to back up the prams and compare them to the other "newer" 31i machines that are not working to see what is different.

Good day..

I'm having the same macro problem, could you please tell me what caused this problem to happen? 

 

Dhysta.

[crazy^millman]

5 hours ago, Dhysta said:

Good day..

I'm having the same macro problem, could you please tell me what caused this problem to happen? 

 

Dhysta.

Last time they were on the forum was about 10 years ago not sure they are going to get back to you. Have you reached out to the Machine Builder or AE staff?

[#Rekd™]

James has moved on and IowaJim passed away.

[Leon82]

1604 bit zero,  1 will turn it on automatically.

You can cancel it in the beginning of the macro program

[Zbuilder]

I am having a similar issue. I use #701 as an update counter for serial number engraving on a part. When I cycle start the tool at the beginning, it engraves only 2 blocks after plunging into the part then the #701 updates waaaay before going to the macro subprogram to do the serial number engraving, the +1 increment for the next part then M99. This was freaking me out until I realized the Matsuura 520 31i has about a 1000 block look ahead buffer. It remembers the original #701=2 an engraves the "2" but before the control ever gets to the subprogram #701 shows 3 on the offset page.

I thought it was going to skip 2 and do a 3. Took about an hour to finally understand it. I thought the macro was written wrong and then thought the control was messed up.

There is an M or G code I saw once upon a time in another macro on the machine. I'll have to look thru all of the macros to find it.
I hope it is commented as such or I'll never find it. I'll try the M20 first though.

If anyone needs this tip, I also remember seeing a parameter (forgot the number) to allow single block execution for macros, block by block (give or take), just like normal positioning moves. I turned this on for the Robodrills a few years ago.

[cncappsjames]

Parameters #3411 to #3420 specify which m-codes prevent buffering.

 

[Zbuilder]

Cool thanks.

Here are pics of those parameters. Are these one-shot M-codes, on a line by themselves ? And also, would these M-codes be described elsewhere and do something else I'm not aware of because I don't recognize these codes. except M6.

 

 

[cncappsjames]

Those M60-M62 are related to pallet changes. M06... y'all know what those are for.

In the empty ones, I'd create a new M-Code program in the library... O9020-O9029 Then find the open corresponding 6080-6089 parameter. 

%

O9020 (FOR EXAMPLE - M900)

G04X.1

M99

%

#6080=900

#3415=900

Then before your MACRO calls, command M900 and it should stop buffering.

Just some basic ideas...

 

Hope that helps.

[cncappsjames]

Some old topics have been resurrecting lately.

I wonder, do these topics show up in Google searches and that's what drives it?

[#Rekd™]

19 minutes ago, cncappsjames said:

wonder, do these topics show up in Google searches and that's what drives it?

Absolutely.

[crazy^millman]

19 hours ago, cncappsjames said:

Some old topics have been resurrecting lately.

I wonder, do these topics show up in Google searches and that's what drives it?

That is what the bots do when they create a login in and then start searching through the forums. They are data harvesting and then taking the key words and sending them back to the mothership. Google, Facebook, Twitter and the rest are not about free services they are all about data harvesting. People don’t realize we are in the matrix now just not using our bodies to produce heat and energy just pulling out data to use it against us. 
 

Wonder how many warning points I will get for going that far off OT?