fanuc illegal plane error

[cruzila]

I read on the internet that threading and a "K" value can conflict with G17. But our issue is the first position line after the safety line has G17 and "A" value which causes 0021 alarm. We have other machines this runs just fine. (Move the "A" to the next line and it runs fine)

I guess my question is has anyone had this issue and resolved it with a parameter change? It"s a Doosan and I see 5109#0 is referenced on their website but I'm not the best FANUC guy.

[crazy^millman]

1 hour ago, cruzila said:

I read on the internet that threading and a "K" value can conflict with G17. But our issue is the first position line after the safety line has G17 and "A" value which causes 0021 alarm. We have other machines this runs just fine. (Move the "A" to the next line and it runs fine)

I guess my question is has anyone had this issue and resolved it with a parameter change? It"s a Doosan and I see 5109#0 is referenced on their website but I'm not the best FANUC guy.

Get a hold of Ellison and have them help you out. PAnderson on the forum works for Doosan look him up and PM him to help.

[cncappsjames]

On 4/27/2022 at 9:05 AM, crazy^millman said:

Get a hold of Ellison and have them help you out. PAnderson on the forum works for Doosan look him up and PM him to help.

If they even have somebody that KNOWS. I spend 25% of my time correcting bad information competitor AE's have given my customers on their other equipment (that has never worked right) then they try to do that on our equipment....

I'm not sayin'.... I'm just sayin'.

[crazy^millman]

5 minutes ago, cncappsjames said:

If they even have somebody that KNOWS. I spend 25% of my time correcting bad information competitor AE's have given my customers on their other equipment (that has never worked right) then they try to do that on our equipment....

I'm not sayin'.... I'm just sayin'.

Dealing with that right now on a some machines. Needed to get Fanuc involved and go around the OEM to get the machines running correctly.

[cncappsjames]

4 minutes ago, crazy^millman said:

Dealing with that right now on a some machines. Needed to get Fanuc involved and go around the OEM to get the machines running correctly.

Hate when that happens. Ben had to deal with that a while back too. He sent me the machine parameters and I looked at them and there were some issues. I offered to help the builder just because it was the right thing to do and I was told I didn't know **** about it. :rofl: Alrighty then. Never mind I've put my hands on more 5-Axis machines in Southern California alone they they have 5-Axis machines on the planet. But hey... no problem. I've got plenty of other things to do so no sweat off my back. :rofl:

[crazy^millman]

26 minutes ago, cncappsjames said:

Hate when that happens. Ben had to deal with that a while back too. He sent me the machine parameters and I looked at them and there were some issues. I offered to help the builder just because it was the right thing to do and I was told I didn't know **** about it. :rofl: Alrighty then. Never mind I've put my hands on more 5-Axis machines in Southern California alone they they have 5-Axis machines on the planet. But hey... no problem. I've got plenty of other things to do so no sweat off my back. :rofl:

Yeah we got that one sorted out, but amazing the arrogance of some of the people. Glad I am dumb as a box or rocks with moss growing on my back because I am so slow at getting things taken care of.

[PAnderson]

On 4/27/2022 at 10:22 AM, cruzila said:

I read on the internet that threading and a "K" value can conflict with G17. But our issue is the first position line after the safety line has G17 and "A" value which causes 0021 alarm. We have other machines this runs just fine. (Move the "A" to the next line and it runs fine)

I guess my question is has anyone had this issue and resolved it with a parameter change? It"s a Doosan and I see 5109#0 is referenced on their website but I'm not the best FANUC guy.

Sorry, I just saw this. I'm not visiting that much now since we are swamped getting ready for IMTS. Cruzila, I will need more info if you haven't resolved this by now. Lathe? Right? Which one and how old? What control? Send the program and show where the issue happens.

I don't do turning much, enough to do with milling and 5 axis but I can ask our turning AE's. We have really good guys here in NJ and hate to see us lumped in with certain Ellison divisions, good or bad.

Yeah, getting hold of Ellison is your first choice, we get the overflow or more difficult ones from them anyway. You can call us here in NJ anytime no matter. No one gets turned away.

 

Paul

[cruzila]

13 minutes ago, PAnderson said:

Sorry, I just saw this. I'm not visiting that much now since we are swamped getting ready for IMTS. Cruzila, I will need more info if you haven't resolved this by now. Lathe? Right? Which one and how old? What control? Send the program and show where the issue happens.

I don't do turning much, enough to do with milling and 5 axis but I can ask our turning AE's. We have really good guys here in NJ and hate to see us lumped in with certain Ellison divisions, good or bad.

Yeah, getting hold of Ellison is your first choice, we get the overflow or more difficult ones from them anyway. You can call us here in NJ anytime no matter. No one gets turned away.

 

Paul

Hey, Thanks for the reply

It's a Mill actually. 2016 DNM5700 i control .. Not sure how much gcode will help, it's the  first move callout after tool change. not sure removing the plane callout from 4th axis post is a good idea. This works fine on our HMC another older Doosan and HAAS

 

G91 G28 Z0.
A0.
M01
N16 T16 ( T16 | 1/8 STUBBY DRILL )
M6
( DRILL )
G0 G90 G17 G54 X-1.0169 Y0. A0.

[gcode]

will this run if you move the A axis callout to the next line

[cncappsjames]

On 4/27/2022 at 7:22 AM, cruzila said:

I read on the internet ...5109#0 is referenced ...

On my machines that have done XYZIJK in G17, this is 0 - as are all bits on #5109.

FANUC 31i-B5 5-Axis VMC and FANUC 31i-B 4-Axis HMC are what I'm looking at at the moment.

I've got a few FANUC Manuals and none have 5109 listed that I can find. That Parameter Section however relates to Canned Cycles. So unless you're doing some sort of Canned Cycle, that parameter may not be the answer. I'll poke around and see what I can dig up.

Are you absolutely certain that machine has the Helical Interpolation Option?

[cruzila]

Got the info from the Doosan site I.E. 0021  All bits on #5109 are 0

Controller Alarm Guide | Doosan Machine Tools

Have not had a problem with helical before, we've done lot's of full 4th axis work on this machine, just not with MC.

In one of the ops it is doing G83 but there is no helical in that one. The rest is all milling 2d at rotations. Couldn't be more basic.

This would be nice to solve, but we have a workaround that is simple and easy.

 

[PAnderson]

Cruzila,

Your mention of threading threw me of, making me think it was a turning center. I agree with GCode. Your safety line should only contain G Codes and (M Codes?). You should not put any axis moves on that line. The DNM5700 lives in G17 and should not be needed but is not a bad idea to be redundant. You stated in the OP that moving the A Axis move to the next line lets it work. All of my showroom mills have #5109.0 set to "0". This seems like a programming issue, not a machine issue. Fanuc is a finicky beast. Drop all of the axis moves down to the next line.

 

Paul

[PAnderson]

Here is a sample program from a DNM5700 that I did a 4th Axis program on. It's at the beginning of the program and the second tool change.

G20
G0G17G40G49G80G90
(DRILLRIGHTSIDEJOURNAL)
T1M6
G0G90G59X1.125Y0.A90.S2037M3
G43H1Z6.
M7
G98G81Z1.3R2.6F24.22
G80
(DRILLLEFTSIDEJOURNAL)
A270.
G98G81Z1.3R2.6F24.22
G80
M09
M5
G91G28Z0.
A0.
M01
(ROUGHHELIXBORE1.250DIARIGHTJOURNAL)
T2M6
G0G90X1.125Y0.A90.S3056M3
G43H2Z6.
M8
Z2.6
G1Z2.5F25.
G3X1.1992Y.0742I.0371J.0371F55.01

[cruzila]

3 hours ago, gcode said:

will this run if you move the A axis callout to the next line

YES, that's the workaround.

 

[gcode]

2 hours ago, cruzila said:

YES, that's the workaround.

 

that's a very easy post edit.. make the edit and call it a day