Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Can't turn off C axis with ST20Y Post

14 REPLIES 14
Reply
Message 1 of 15
derekmillright
821 Views, 14 Replies

Can't turn off C axis with ST20Y Post

I have the Haas ST20Y post processor from the post library. I can not find a way to command it to use just the Y axis and leave the C Axis alone. There are times when it is useful, but sometimes you just want to use the Y. What am I missing?

For what it is worth, it is not a matter of deleting a G112 (cartesian to polar). Everything is written to the C axis. Everything is well in range of the Y.

 

Thanks

14 REPLIES 14
Message 2 of 15

There was some discussion a few months back about this. It seemed that in some cases, the Haas didn't react well to crossing below the Y axis C/L, thus the change to this mode. However, I also thought they implemented a method to get around that...

 

Looking in the post, I see this:

if (!longDescription) {
  longDescription = subst("Preconfigured %1 post with support for mill-turn. You can force G112 mode for a specific operation by using Manual NC Action with keyword 'usepolarmode'.", description);
}
 

Seth Madore
Customer Advocacy Manager - Manufacturing
Message 3 of 15

Thanks for the reply. 

 

That seems to do the same thing as selecting the option "use polar interpolation" = "Yes" in the post settings.

 

That will write G112 and X and Y values. I do not want that because it is still going to engage the C axis (by way of the G112) and I'm doing the same thing. If I kill off the G112 and from a g code program posted as such then my X axis looks to be 1/2 the distance they need to be... like a radius versus diameter program.

 

 

Message 4 of 15

im on a has st30-y and I can confirm this.

 

trying to figure out why my feed rate changes so dramatically when it uses the C axis to interpolate. im messing with it now. wish me luck.

Message 5 of 15
k.m.urbanczyk
in reply to: Ketherton21

I have exactly the same problem.

 

Did you figure something out?

 

G112 with X and C axis in some cases leaves me with not good enough surface finnish.

 

I can of course program this manually on the maschine, but the point of Fusion is that i don't have to program parts on the machine.

Message 6 of 15

I am having the same issue with my st20y. I'm trying to simply use a axial live endmill to buzz out a small counterbore at the end of a part and the c axis along with the speeds are all over the place. I could figure out another way very simply, however, I'd like fusion to work correctly for this. 

 

 

let me know if anyone figured this out. 

Message 7 of 15
BlastedBilly
in reply to: seth.madore

Hi

This thread is 4 years old and we are still having this issue. Is there no solution to this?

Message 8 of 15

@BlastedBilly you're trying to get a toolpath on the main spindle that doesn't involve a whole lotta -C- axis moves, right? The issue is this; historically, Haas has had a not insignificant issue with the live tool going below centerline. As such, any toolpath that does will be forced into an X/C motion. There are ways around this:
1) There's a user property for "X axis Minimum" change that to a negative value (at your risk, and it's also in metric)

2) "useG112" property


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 9 of 15
BlastedBilly
in reply to: seth.madore

Seth,

Can you please elaborate on "not insignificant issue"? This is a brand new lathe so software should be up to date. My issue I'm running into currently when I force a G112 is Error 9971 - Excessive Speed or Acceleration. This happens as soon as there is an x and y move on the same line. Slowing down feedrate changes nothing.

 

 

Message 10 of 15
seth.madore
in reply to: BlastedBilly

Bear in mind that I do not have access to a Haas lathe, so this is all second-hand knowledge. As it was explained to me (and my old memory recalls), Haas had an issue with X negative movements resulting in crashes, as the control just couldn't calculate the position. Now, this is what I recall as the issue, but cannot confirm one way or another.

 

Are you certain there is no mechanical interference going on? I had a part on my Doosan not too long ago that was leaving a little mark on a milled feature. I couldn't figure out for the life of me what was happening, as everything seemed to clear just fine. It wasn't until close examination revealed that the adjacent toolholder was "kissing" the chuck when my Y axis was extended, resulting in a bit of deflection. A little creative grinding to the tool holder and the issue went away.


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 11 of 15
BlastedBilly
in reply to: seth.madore

Update:

I just had the lathe software updated to the latest version 100.23.000.1010 released July 10, 2023, and it has resolved that alarm. 

 

Directly from their release notes:

 

Lathe: 9971 Excessive speed Alarm in G112 - Updated the G112 model to reduce the impact of numerical noise and to increase reliability for low C-axis acceleration.

 

 

Message 12 of 15
seth.madore
in reply to: BlastedBilly

So no more issues?


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 13 of 15
BlastedBilly
in reply to: seth.madore

No more 9971 alarm. I was able to dry run cutting a square with an axial live tool with x and y, but it still seemed to move c. I'll report back.

 

Tomorrow I will have more time to see if the feedrate issues are corrected like Ketherton21 mentioned.

 

Seth,

Is there a difference between manual nc action "us3polarmode" vs "useg112" property vs just checking the g112 box in the post?

 

Also, where do I find this "x axis minimum" property?

Message 14 of 15

The "usePolarMode" is typically used as a Manual NC Action when you don't want every toolpath possible to be posted out in G112 mode. Conversely, using the G112 mode in the post settings will make every toolpath post out in G112 mode.

 

The X-axis minimum setting is here:

2023-07-18_17h40_16.png

 


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 15 of 15
BlastedBilly
in reply to: seth.madore

Ok first a little background...

Machine is a 2022 Haas ST-30LY. I have been having various issues including acceleration errors, stuttering/jerky c axis movement, and greatly reduced feedrates.

 

I am hesitant to say this since I have not had much time yet to evaluate, but the latest Haas software update from July 10, 2023 seems to have fixed all of my issues. 

 

Here's the quick test I was able to do today. It's just a hex with a chamfer and then parted off.

1000014460.jpg

 The part on the left used c and x, and the part on the right is everything the same but with the "use g112" box checked. It used c, x and y. The finish is significantly better, and both toolpaths ran much faster than similar toolpaths did pre-update. C axis also appeared to move smoothly.

 

Seth,

Thank you for the suggestions. It turns out I dont have much travel in the x negative direction with the way this bmt65 turret is set up so I haven't messed with that yet.

 

I'm not sure why more people with haas lathes aren't complaining more unless they're just doing traditional turning.

 

I will continue messing with this and report back if I run into issues again.

 

Thanks

Billy

 

 

 

 

 

 

 

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report