Milltronics Lathe Post Processor

[Anonymous]

I am trying to get a good post processor for my milltronics lathe, In another Post it was suggested to use a generic fanuc Post Processor  It works ok most of the time, but I am having a threading issue In the Generic Fanuc Post processor, that I downloaded and renamed, Milltronics Turning, the threading feedrate defaults to .040. I have changed the pitch on my tool in the tool library, as well as set it in the threading box if fusion. all looks good until I post it then I get a feedrate of .040 instead of the .083333 that I require. I posted it for my Haas CL-1 lathe and it posts out perfect.

below is a link to the other post that I have been describing my issues in. there you will find the actual post processor and file that I am using to sort this out.

Any help is sure appreciated 

Thank you

https://forums.autodesk.com/t5/fusion-360-computer-aided/post-processor-for-a-milltronics-lathe/m-p/...

[seth.madore]

You need to be setting your Pitch at the toolpath level, not insert:

That yields this toolpath: 

N14 T0400
N15 G54
N16 M8
N17 G99
N18 G97 S500 M3
N19 G0 X4.3 Z0.1969
N20 G0 Z0.1
N21 G92 X1.984 Z-2. F0.07874
N22 X1.968
N23 X1.952
N24 X1.936
N25 X1.92
N26 G0 X4.3 Z0.1969

[Anonymous]

---

@seth.madore wrote:

You need to be setting your Pitch at the toolpath level, not insert:

That yields this toolpath: 

N14 T0400
N15 G54
N16 M8
N17 G99
N18 G97 S500 M3
N19 G0 X4.3 Z0.1969
N20 G0 Z0.1
N21 G92 X1.984 Z-2. F0.07874
N22 X1.968
N23 X1.952
N24 X1.936
N25 X1.92
N26 G0 X4.3 Z0.1969

---

please notice the screen shot below, I have the thread pitch set correctly but am still getting the same result

---

---

[seth.madore]

Alright, sorry, I missed that. Please share your post processor here. What I posted above was the generic Fanuc turning post. You should be getting the same. Since you aren't I'd like to see why...

[Anonymous]

Good Morning;

Sure I'll attach it below.

I have tried to post the same path out for our Haas lathe and it posted correct. in fact i copied and pasted it into my milltronics program and it work fine other than I had to add an M6 for the tool change.

Thanks Again

[seth.madore]

Alright, I found the culprit. When it's "Use Cycle", it posts out the correct feedrate. When it's not "Use Cycle", it defaults to a 1mm feedrate. I've notified the post team and will post back shortly with a solution

-EDIT#1- This exists in your post only, not the current Fanuc Turning Post. If you haven't done any other changes to the post, I'd just suggest grabbing that one.

-EDIT#2- Your post hails from Oct. of 2013... The new Fanuc post was last updated on 12/2018. Suffice to say that there have been more than a few upgrades..

[Anonymous]

Well, turning the cycle on only made 1 threading pass and didn't actually cut anything, but I just downloaded the newest fanuc post and it looks better , Im getting ready to go try it out now and will update you. 

[Anonymous]

Well that didnt work, I left out my m6's for my toolchange and added a G28 U0. that gave me an error.  Threading pass looks good tho.

[seth.madore]

Well, we can add an M6 callout, that's not issue.

Did you want it like:

N48 T0400

M6

N49 G54

and then at the end of the toolpath, what are you looking for?

[Anonymous]

M06T404

[seth.madore]

ok... and what about at the end of a tool cycle, you do not want it to go home. What then?

[Anonymous]

The book says

X to tool change (G48)

 The G48 function will retract X to the tool change position. This position is set by the machine tool builder But may be change by editing the Tool Change Coordinate Parameters

Same for Z

 So I guess it would be

G48

G49

in that order

[seth.madore]

Do you have working code for your machine? Anything that's been run with success?

[Anonymous]

My Bad,

 should be

G48

G47

G48 for X

G47 for Z

[Anonymous]

Yes Sir; 

I am currently running the 1 attached below

[seth.madore · Accepted solution]

Sorry for the delay, it's been a busy day in the shop. Give the attached post a shot. It's the generic Fanuc with a couple tweaks;

No G28 U0. or W0., using G47 and G48 instead

M6 at every tool change

Test carefully. Not responsible for any undesirable results 🙂

[Anonymous]

Im running a little behind myself, lol, i tried out that post processor yesterday, and it seems to work great. Didnt have any hicups at all. I want to thank you for all your help. Pat Burden Sektam of Independence Inc. Www.sektam-indy.com