Announcements
Attention for Customers without Multi-Factor Authentication or Single Sign-On - OTP Verification rolls out April 2025. Read all about it here.

Need help with Fanuc 21iTB post processor CAN Cycles

lethal375
Enthusiast

Need help with Fanuc 21iTB post processor CAN Cycles

lethal375
Enthusiast
Enthusiast

I have a Clausing Lathe with a Fanuc 21iTB control.

If I post NOT using CANNED cycles everything seem to work fine but when using CANNED cycles I get errors in the G71-76

If I post in A B & C then compare the G71 lines there is no difference but get errors when it gets to those lines.

I went to the manual and went through each line of the G71 cycle, all seems to be correct.

Probably something simple.

Any help or suggestions are greatly appreciated   

 

0 Likes
Reply
Accepted solutions (1)
461 Views
6 Replies
Replies (6)

serge.quiblier
Autodesk
Autodesk

Hi @lethal375 

 

Looking at the partial code nothing seems strange, but we can't see the last two line N46 and N47.

As they are part of the path used for roughing, are they correct?

Can you tell us what is the error message on the controller?

It may help us diagnose.

It can be the G18 code (that is correct, but may not be desired) or a trouble with the arc interpolation, but it's hard to tell.

 

Regards.

 


______________________________________________________________

If my post answers your question, please click the "Accept Solution" button. This helps everyone find answers more quickly!



Serge.Q
Technical Consultant
cam.autodesk.com
0 Likes

lethal375
Enthusiast
Enthusiast

Sorry I forgot to include that Alarm "65"

I did have a chance to go back and try running it again.

Simulation is good but on the machine it appears to be going to final roughing pass and not starting at the outside 

0 Likes

lethal375
Enthusiast
Enthusiast

Here is the part

Stock is 4 inch diameter

0 Likes

serge.quiblier
Autodesk
Autodesk

Hi @lethal375 

 

Error 65 seems to be cause by the following situation

65 - ILLEGAL COMMAND IN G71-G73 (T series)

Alarm Description

1.) G00 or G01 is not commanded at the block with the sequence number which is specified by address P in G71, G72, or G73 command. 2.) Address Z(W) or X(U) was commanded in the block with a sequence number which is specified by address P in G71 or G72, respectively. Modify the program.

 

Can copy the gcode file to another file and hand edit it.

Then change the line N47 X4 to N45 G1 X4.

And test it again.

I don"t remember having this kind of trouble before.

The rest of the code look correct.

 

On an older controller, I would have questioned the G71 one line version against the two lines version.

But it's Fanuc 18, and that was more a Fanuc10/11 trouble.

 

Regards.

 



Serge.Q
Technical Consultant
cam.autodesk.com
0 Likes

lethal375
Enthusiast
Enthusiast
Accepted solution

I found the problem in the manual under the "notes" regarding G71 

No "Z" movement can be in the G0 rapid move line after the G71 lines

Line N39 I had to remove the "Z" move.

 

Thanks

0 Likes

serge.quiblier
Autodesk
Autodesk

Hi @lethal375 

 

after checking a Fanuc manual, effectively, the G71 can have 2 variants.

Type I that cannot plunge in groove, the shape should be monotonous.

Type II can machine if grooves are present.

Type II is a cost option, that your machine doesn't seem to have.

 

Regards


______________________________________________________________

If my post answers your question, please click the "Accept Solution" button. This helps everyone find answers more quickly!



Serge.Q
Technical Consultant
cam.autodesk.com
0 Likes