Make Corners Sharp - Unchecked - Doesnt produce arcs in lathe gcode.

[changedsoul]

I seen a post in here where a person wanted the corners not rounded and their output had arcs on the entry and exit of the chamfers.

Well this is actually what I want, but my output is all linear moves around the corner.

X0.1973 Z-0.0388
X0.1987 Z-0.0405
X0.201 Z-0.0419
X0.211 Z-0.0469
X0.2119 Z-0.0474
X0.2166 Z-0.0494

 This is supposed to be a chamfer with corners not sharp, but there are no arc moves in it.

Is this an issue with the post? I'm using the stock Haas Post.

[DarthBane55]

It is a bit difficult to answer your question with just the info provided.  Could you include a snapshot of the toolpath please?  If possible the project as well, but if not possible, another snapshot of the "passes" tab?

If you can't really show the part, zoom in on 1 section of the path, so we see where it should have a radius, without anyone being able to see the whole part.

[changedsoul]

Yeah sorry about that.

Highlighted #7 on the View tool path pege clearly shows an arc move.

Here is the Code that gets output:

G1 Z0.0031 F0.0025
X0.211 Z-0.0021
X0.201 Z-0.0071 F0.0015
X0.1987 Z-0.0085
X0.1973 Z-0.0102
X0.1969 Z-0.012
Z-0.037
X0.1973 Z-0.0388
X0.1987 Z-0.0405
X0.201 Z-0.0419
X0.211 Z-0.0469
X0.2119 Z-0.0474
X0.2166 Z-0.0494
Z-0.0594 F0.0025

And here is the post dump section...It shows its got arc moves in it, so I don't know why its not getting output.

413: onMovement(MOVEMENT_LEAD_IN /*lead in*/)
413: onLinear(0.10547545012526624, 0, -0.0020502525286411675, 0.002500000079785745)
414: onMovement(MOVEMENT_CUTTING /*cutting*/)
414: onLinear(0.10047544644573542, 0, -0.007050252688212658, 0.0015000000185384525)
415: onCircular(true, 0.10542519449249027, 0, -0.01200000014830762, 0.09842519685039369, 0, -0.01200000014830762, 0.0015000000185384525)
  direction: CW
  sweep: 44.999997deg
  normal: X=0 Y=1 Z=0 (ZX)
  radius: 0.007
416: onLinear(0.09842519685039369, 0, -0.03700000094616507, 0.0015000000185384525)
417: onCircular(true, 0.10542519449249027, 0, -0.03700000094616507, 0.10047544644573542, 0, -0.04194974899291992, 0.0015000000185384525)
  direction: CW
  sweep: 45deg
  normal: X=0 Y=1 Z=0 (ZX)
  radius: 0.007
418: onLinear(0.10547545012526624, 0, -0.04694974797917163, 0.0015000000185384525)

[DarthBane55]

I'm sorry, I didn't realize it was a lathe issue, I'm gonna step out as I don't know much about lathes, but ya, it looks like the post is wrong according to your data.  Anyway, sorry, I will leave the lathe experts jump in.

[Anonymous]

@changedsoul 

Maybe I have something different to you but without a file it is hard to get to exactly what`s wrong.

I made a small test file that I hope is close to yours and generated a toolpath with the "Make Sharp Corners" both checked and unchecked and Posted out using the HAAS Turning PP, seems to work OK on my file but again not having yours makes it difficult, here is an image of what I drew up.

Below is the generated code for both checked and unchecked, you can see that there are circular movements in the unchecked part of the code and none in the checked part of the code, this to me is correct so I don`t know what else to say.

%
O1001 (MAKE SHARP CORNERS UNCHECKED)
N10 G98 G18
N11 G20
N12 G50 S6000
N13 M31
N14 G53 G0 X0.

(Profile Roughing1)
N15 T101
N16 G99
N17 M22
N18 G97 S1096 M3
N19 G54
N20 M8
N21 G0 X2.2874 Z0.1969
N22 G50 S5000
N23 G96 S656 M3
N24 G0 Z-0.189
N25 X1.4528
N26 G1 Z-1.8189 F0.03937
N27 X1.5472
N28 G0 Z-0.189
N29 X1.3583
N30 G1 Z-1.8189 F0.03937
N31 X1.4528
N32 X1.5315 Z-1.7795
N33 G0 Z-0.189
N34 X1.2638
N35 G1 Z-1.8189 F0.03937
N36 X1.3583
N37 X1.437 Z-1.7795
N38 G0 Z-0.189
N39 X1.1794
N40 G1 Z-0.2657 F0.03937
N41 G18 G3 X1.189 Z-0.2835 I-0.0307 K-0.0178
N42 G1 Z-0.4803
N43 X1.1887 Z-0.4834
N44 X1.1751 Z-0.5614
N45 Z-0.8136
N46 G3 X1.189 Z-0.8346 I-0.0285 K-0.0211
N47 G1 Z-1.8189
N48 X1.2638
N49 X1.3425 Z-1.7795
N50 G0 Z-0.189
N51 X1.095
N52 G1 Z-0.2218 F0.03937
N53 X1.1682 Z-0.2584
N54 X1.1743 Z-0.2619
N55 X1.1794 Z-0.2657
N56 X1.2582 Z-0.2263
N57 G0 Z-0.5614
N58 X1.2223
N59 G1 X1.1751 F0.03937
N60 X1.1333 Z-0.8
N61 G3 X1.1751 Z-0.8136 I-0.0076 K-0.0346
N62 G1 X1.2538 Z-0.7742
N63 G0 X1.5472
N64 Z-0.189
N65 X2.2874
N66 Z0.1969
N67 G97 S1096 M3

N68 M9
N69 G53 X0.
N70 G53 Z0.
N71 M30
%%
O1001 (MAKE SHARP CORNERS CHECKED)
N10 G98 G18
N11 G20
N12 G50 S6000
N13 M31
N14 G53 G0 X0.

(Profile Roughing1)
N15 T101
N16 G99
N17 M22
N18 G97 S1096 M3
N19 G54
N20 M8
N21 G0 X2.2874 Z0.1969
N22 G50 S5000
N23 G96 S656 M3
N24 G0 Z-0.189
N25 X1.4528
N26 G1 Z-1.8189 F0.03937
N27 X1.5472
N28 G0 Z-0.189
N29 X1.3583
N30 G1 Z-1.8189 F0.03937
N31 X1.4528
N32 X1.5315 Z-1.7795
N33 G0 Z-0.189
N34 X1.2638
N35 G1 Z-1.8189 F0.03937
N36 X1.3583
N37 X1.437 Z-1.7795
N38 G0 Z-0.189
N39 X1.1794
N40 G1 Z-0.264 F0.03937
N41 X1.189 Z-0.2688
N42 X1.1889 Z-0.482
N43 X1.1751 Z-0.5612
N44 Z-0.7994
N45 X1.189
N46 Z-1.8189
N47 X1.2638
N48 X1.3425 Z-1.7795
N49 G0 Z-0.189
N50 X1.095
N51 G1 Z-0.2218 F0.03937
N52 X1.1794 Z-0.264
N53 X1.2582 Z-0.2246
N54 G0 Z-0.5612
N55 X1.2223
N56 G1 X1.1751 F0.03937
N57 X1.1334 Z-0.7994
N58 X1.1751
N59 X1.2538 Z-0.7601
N60 G0 X1.5472
N61 Z-0.189
N62 X2.2874
N63 Z0.1969
N64 G97 S1096 M3

N65 M9
N66 G53 X0.
N67 G53 Z0.
N68 M30
%

HAAS Turning PP used is attached

[changedsoul]

Interesting, maybe I am using a dated haas post.

I also could not find this post on the autodesk list of haas posts. Is what your using a modified post?

Edit: ID10T Error on the post, I was looking for "PP" in the name when it hit me just after posting, it stood for Post Processor, lol.

This is the one I am using. Ill try a fresh one off the autodesk site as well as the one you attached and see if I can find out why mine is not working.

[changedsoul]

Ok, well it behaved the same as the post I have. I am doing an ID chamfer and noticed your doing an OD, so I changed my OD to roll around the corner and its working.

It seems then its an ID issue.

EDIT:

Ok well I dug into the post and placed a comment at the beginning of "OnCircular" and this never gets called on the ID tool path, but does on OD path.

How does the Post work exactly...what causes each function to be called, and why might this not be getting called for the ID, when the dump clearly shows its there.

OD Dump: 
415: onLinear(0.1779235441853681, 0, -0.023076456832134818, 0.002500000079785745)
416: onCircular(false, 0.16687500195240412, 0, -0.03412500141173836, 0.18249999819778082, 0, -0.03412500141173836, 0.002500000079785745)
  direction: CCW
  sweep: 45.000006deg
  normal: X=0 Y=1 Z=0 (ZX)
  radius: 0.015625

ID Dump:
791: onLinear(0.10047544644573542, 0, -0.007050252688212658, 0.0015000000185384525)
792: onCircular(true, 0.10542519449249027, 0, -0.01200000014830762, 0.09842519685039369, 0, -0.01200000014830762, 0.0015000000185384525)
  direction: CW
  sweep: 44.999997deg
  normal: X=0 Y=1 Z=0 (ZX)
  radius: 0.007


OD gcode:
X0.3558 Z-0.0231
(OnCircular_Called)
G18 G3 X0.365 Z-0.0341 R0.0156

ID gcode:
G1 Z0.0031 F0.0025
X0.211 Z-0.0021
X0.201 Z-0.0071 F0.0015
X0.1987 Z-0.0085
X0.1973 Z-0.0102
X0.1969 Z-0.012
Z-0.037

No OnCircular on the ID.

[Anonymous]

@changedsoul 

Not sure what is happening your end, works here on an ID Profile, see the Circular in the toolpath and see it in the code.

N65 G1 Z-0.5866 F0.03937
N66 X0.7559
N67 X0.6772 Z-0.5472
N68 G0 Z0.0236
N69 X0.9228
N70 G1 Z-0.0454 F0.03937
N71 X0.8826 Z-0.0655
N72 G18 G2 X0.8619 Z-0.0906 I0.0251 K-0.0251
N73 G1 Z-0.5866
N74 X0.8504
N75 X0.7717 Z-0.5472
N76 G0 Z0.0236
N77 X0.9951
N78 G1 Z-0.0092 F0.03937

P.S. IMHO no need to mess with the PP, works here !!

[changedsoul]

I appreciate your help in trying to figure this out.

I have narrowed it down I think to the tools corner radius.

I change my tool to a .015R and it output ok...I put it back to a radius of .007R and it went back to no arc outputs....even when the Fusion Tool path viewer shows arc moves in it, and the post dump shows arc outputs.

Can you confirm this with yours?

and if so...is there maybe a hidden setting for minimum radii?

EDIT: I found that a tool corner radius of .0128 will fail and have no arc output, but a tool corner radius of .0129 will succeed.

Not sure what to make of that.

[Anonymous · Accepted solution]

@changedsoul 

Then it is likely to be the Minimum Chord Length setting may be too high a value for the very small rads you are doing, in my ID Profile I get 7 circular movements in the toolpath but only 4 appear in the code, changed the default Minimum Chord Length of 0.25 to a lower value of 0.01 as in the image below and then all circular moves did appear in the code exactly as they should. Have a go with different setting to find the right one for you. Yes altering the TNR will allow the circular moves to appear but i don`t think that is the right way to go, no expert here but unless you have actual tool with the same TNR as the value you put in fusion will that not change the size of your part?

[changedsoul]

---

@Anonymous wrote:

@changedsoul 

... Yes altering the TNR will allow the circular moves to appear but i don`t think that is the right way to go, no expert here but unless you have actual tool with the same TNR as the value you put in fusion will that not change the size of your part?

---

 I thank you for your concern, but you misunderstood why I was changing the radius. It was only for experimenting trying to see why and when it would work or fail. I would never use a different nose radius then my actual tool unless there was a specific reason for it, which is extremely rare for me to do.

Changing that value fixed the issue though, so thanks for helping me out.