What's new
What's new

Lathe program eliminating small fillet

Lotaxi

Aluminum
Joined
Jun 9, 2020
Hey all,

I have a small part I'm turning that is coming out with a sharp corner where there should be a 0.01 round. Looking closely at the physical movement of the lathe, the finish does seem to be running around that corner correctly, looking at the code I see the proper G02, and looking at the simulation in the controller I clearly see the theoretical movement, but I am somehow still left with a burr once the program completes. I spent about an hour and a half troubleshooting the issue yesterday with no luck. What the hell is going on?

Thanks
 
Would be helpful if you posted the code.
Here's the specific bit that's messing me up.
N108 G02 X.268 Z-.608 I0 K-.028
N109 G01 F.0005 Z-.655
N110 F.0005 X.304
N111 G02 X.34 Z-.673 I0 K-.018
N112 G01 F.0005 Z-.798
Code starts at a radius just outside the attached screenshot (a 0.02 radius that cuts correctly) cuts along the small diameter up to the shoulder, then runs up the wall and along the .010 radius at the outer diameter before cutting straight back for a bit.
 

Attachments

  • The Features in Question.PNG
    The Features in Question.PNG
    77.9 KB · Views: 25
Normally an O.D. radius is G3 if X is getting larger while Z is going deeper. At least on all the lathes I program.

X.212Z-.58
G3X.268Z-.608K-.028
G1Z-.655
X.304
G3X.34Z-.673K-.018F.001
G1Z-.798F.002
 
  • Like
Reactions: Ox
A tool above center line can cause a fussy burr on features this small.

Something as small as a different edge prep on the insert can change tool height a bit.
 
Normally an O.D. radius is G3 if X is getting larger while Z is going deeper. At least on all the lathes I program.

X.212Z-.58
G3X.268Z-.608K-.028
G1Z-.655
X.304
G3X.34Z-.673K-.018F.001
G1Z-.798F.002
Yes should be G3. The drawing is looking at the negative side of the ZX plane so circular interpolations appear backwards.
 
Normally an O.D. radius is G3 if X is getting larger while Z is going deeper. At least on all the lathes I program.

X.212Z-.58
G3X.268Z-.608K-.028
G1Z-.655
X.304
G3X.34Z-.673K-.018F.001
G1Z-.798F.002
Yes should be G3. The drawing is looking at the negative side of the ZX plane so circular interpolations appear backwards.

That would make sense, but I believe you're using a rear programmed lathe. Ours is front programmed.
A tool above center line can cause a fussy burr on features this small.

Something as small as a different edge prep on the insert can change tool height a bit.
Oh damn. This might actually be the issue. I didn't think about the tool height because it's just about never an issue for what I'm making.
 
That would make sense, but I believe you're using a rear programmed lathe. Ours is front programmed.

Oh damn. This might actually be the issue. I didn't think about the tool height because it's just about never an issue for what I'm making.
Not likely the issue as you would see a drastic dimensional difference between the smaller and larger diameters.

What brand of lathe is it?
For some reason I think a Haas TL series is programmed as if it had the turret in the back, even though it's on the front...
 
  • Like
Reactions: Ox
Not likely the issue as you would see a drastic dimensional difference between the smaller and larger diameters.
Damn. I guess this wouldn't be it, then. We are within about .0004 of the diameters we're aiming for.
What brand of lathe is it?
For some reason I think a Haas TL series is programmed as if it had the turret in the back, even though it's on the front...
It's a Milltronics ML-14 lathe
 
Change the G02 to G03. Ain't gonna get any simpler than that.
This crashes the tool. I'm moving toward the spindle and away from center where operator side is +X and left of the bed is -Z using a right handed tool. Seeing as the movement is physically clockwise, I programmed properly using a G02.

Part number on holder and insert?
Lets do the simple stuff first before we pretend to know the how and whys.
I hate everything. I went to go look at the insert box. Somebody put an insert in the wrong box. The tool I've been using has a radius of .015 and I didn't think to check because stupid me trusts labels. Won't be making that mistake again. Kill me.
 
I hate everything. I went to go look at the insert box. Somebody put an insert in the wrong box. The tool I've been using has a radius of .015 and I didn't think to check because stupid me trusts labels. Won't be making that mistake again. Kill me.

That's okay.
We will just tack your nuts to a telephone pole and push you over sideways for doing this.
We all have done such and hope to escape without pain.
 
Somebody put an insert in the wrong box. The tool I've been using has a radius of .015 and I didn't think to check because stupid me trusts labels. Won't be making that mistake again. Kill me.

Cool!
So with that problem solved, perhaps you should consider using tool nose radius comp on the machine instead of CAM.
Why?
Well, first, no, this would not have saved your butt here. Outside corners will always be generated fine, regardless of tool radius discrepancies.
But!
If it was in fact a fillet ( as it was incorrectly stated in the title ) and you've programmed one having a .008 radius, the control would have thrown an error before scrapping your part!
Same goes for turning accurate tapers as well.
 
Yeah that insert in the wrong box will get you every time.

So Lotaxi, in your sketch is positive Z to the left and positive X up?
 
Last edited:
The control would have thrown an error before scrapping your part!
How? I would imagine that machine comp would be like it is on the mill, no? Just offsets a tool location path by an input value defining the tool?

So Lotaxi, in your sketch is positive Z to the left and positive X up?
The screenshot provided is mirrored on a diagonal. Dunno why I made my screenshot like that, but I did.

Here's the part in the proper orientation. Spindle would be to the left, tool post coming in from the bottom (where the operator is), with +X mirrored from the origin shown in the screenshot. CAMWorks wants the part programmed with axes as shown, but our machine wants the post to mirror all X values.
 

Attachments

  • The Features in Question.PNG
    The Features in Question.PNG
    119.1 KB · Views: 10
How? I would imagine that machine comp would be like it is on the mill, no? Just offsets a tool location path by an input value defining the tool?


The screenshot provided is mirrored on a diagonal. Dunno why I made my screenshot like that, but I did.

Here's the part in the proper orientation. Spindle would be to the left, tool post coming in from the bottom (where the operator is), with +X mirrored from the origin shown in the screenshot. CAMWorks wants the part programmed with axes as shown, but our machine wants the post to mirror all X values.
So Z plus is to the right, correct? Is X plus up or down in this drawing?
 








 
Back
Top