Lathe Drilling operation not working

[Carbidecnc]

Hi

I have an error hoping up on my machine programmed axis not available.I am trying to run a drilling cycle in fusion lathe all my WCS look good i have attached the code, have no idea why its doing this is there something I'm missing for the drilling operation like tool orientation

[LibertyMachine]

Please export and share the Fusion .f3d file so we have a better idea of what is going on: File > Export > Save to local folder. Return to thread and attach the .f3d file in your reply.

What post processor are you using and what is your controller?

[Carbidecnc]

Hi Seth

Here is the file thanx

[LibertyMachine]

And what is your machine and controller?

[Carbidecnc]

Siemens 808D

[Carbidecnc]

This is my modified PP

[LibertyMachine]

Well, tool orientation is not needed if you are drilling in the same orientation as your Setup, which you are. However, turning off tool orientation produces no difference in posted code. I guess the question is; What does your machine want to see for a drilling cycle? Are the posted values correct, but causing an issue? More exploration on your end as to what is causing this issue (in the code) is needed, I suspect. Once we determine what is triggering this alarm we can start looking at the Fusion or the .cps file and determine where to go from there.

Block 72 is your drilling cycle: 

N72 CYCLE83(5, -1, 5, -28, , -7.25, , 0, , , 1, 0, , 6.25, 0, 0, 0)

What does your manual or other programs show for formatting?

[Carbidecnc]

HI Seth

Just looked in the Siemens manual and they use a Cycle 81

[LibertyMachine]

Now the Cycle81 is going to be a one-shot drilling cycle with no retract, right? Side-note; My lathe experience is limited to begin with, and even more so as it's only Fanuc knowledge....

The G81 (fanuc) is a drill to depth and rapid out. The G83 (again, Fanuc) is a peck drilling cycle with return to clearance plane. How does this concept translate over to Siemens? Is there letter addresses you can place inside the Cycle81 that will give it a pecking function?

Selecting "Drilling - Rapid Out" will give you a Cycle 81 from Fusion

[Carbidecnc]

Hi Seth

Yes you are absolutely right its the same for Siemens I am peck drilling so its Cycle 83 the formatting in my manual looks the same as posted code

[LibertyMachine]

So, I guess you are going to have to do some trial and error and determine what is actually different between output code and what the machine wants. Sorry I can't be of more help 😕

[Carbidecnc · Accepted solution]

Hi Seth

I managed to get the drill cycle working I had to put a G17 in there, also do you know how I could add a variable in my PP to let my turret do a tool change at the home position,I have a few long tools and the home position setting in the work setup is not enough clearance for me before it hits the limit switch in the Z so  to move up in the x as well would be ideal

Regards

Dave

[Carbidecnc · Accepted solution]

oK ALL SORTED

[Anonymous]

Hi, I'm having a similar problem to the one you describe here.

Setting up a post processor using a modified version of the generic Siemens lathe post. I have everything working well with the exception of drilling cycles. 

Just to clarify, you added a G17 to the drilling cycle and that cured your problem?

Thanks

[Carbidecnc]

yes just add a G17 to G code just before the spindle turns on 

[Anonymous]

Brilliant, Thanks! 

All working perfectly now, just swapped out the G18 for a G17 in the intro to the code. Now all drilling cycles work with no effect on other operations. 

The thing that confuses me is why? If its a turning post why don't the cycles work in XZ ? 

[Anonymous]

G17 plane not generated 

Please suggest how do i change in dafault PP

[Carbidecnc]

Hi Take a look at this post

https://forums.autodesk.com/t5/hsm-post-processor-forum/siemens-turning-802d-omit-g97-and-change-g18...