[Chriseg1]

I am trying to circle mill a small hole with a 1/8" end mill using live tooling and the y axis.

the hole is centered the the c axis and is 0.31" diameter.

the problem I am having is that the hole is not round. its is oval. its 0.2905" x 0.273"

any thoughts?

CAM is OneCNC

G28 U0. W0.
G56
T1010
M154
M133 P3000
M08
G98
M14
G17
G00 X0. Z1.75 Y0.
Z1.55
G01 Z1.375 F9.
X0.004 F18.
G03 Y0.0259 X-0.0219 I-0.0259 J0. R0.0259
Y0. X-0.0478 I0. J-0.0259 R0.0259
Y-0.0478 X0. I0.0478 J0. R0.0478
Y0. X0.0478 I0. J0.0478 R0.0478
Y0.0696 X-0.0219 I-0.0696 J0. R0.0696
Y0. X-0.0915 I0. J-0.0696 R0.0696
Y-0.0915 X0. I0.0915 J0. R0.0915
Y0.0915 X0. I0. J0.0915 R0.0915
Y0. X-0.0915 I0. J-0.0915 R0.0915
Y-0.0269 X-0.0828 I0.0457 J0. R0.0457
G00 X-0.0828 Z1.625 Y-0.0269
X0. Y0.
Z1.425
G01 Z1.25 F9.
X0.004 F18.
G03 Y0.0259 X-0.0219 I-0.0259 J0. R0.0259
Y0. X-0.0478 I0. J-0.0259 R0.0259
Y-0.0478 X0. I0.0478 J0. R0.0478
Y0. X0.0478 I0. J0.0478 R0.0478
Y0.0696 X-0.0219 I-0.0696 J0. R0.0696
Y0. X-0.0915 I0. J-0.0696 R0.0696
Y-0.0915 X0. I0.0915 J0. R0.0915
Y0.0915 X0. I0. J0.0915 R0.0915
Y0. X-0.0915 I0. J-0.0915 R0.0915
Y-0.0269 X-0.0828 I0.0457 J0. R0.0457
G00 X-0.0828 Z1.625 Y-0.0269
X0. Y0.
Z1.345
G01 Z1.17 F9.
X0.004 F18.
G03 Y0.0259 X-0.0219 I-0.0259 J0. R0.0259
Y0. X-0.0478 I0. J-0.0259 R0.0259
Y-0.0478 X0. I0.0478 J0. R0.0478
Y0. X0.0478 I0. J0.0478 R0.0478
Y0.0696 X-0.0219 I-0.0696 J0. R0.0696
Y0. X-0.0915 I0. J-0.0696 R0.0696
Y-0.0915 X0. I0.0915 J0. R0.0915
Y0.0915 X0. I0. J0.0915 R0.0915
Y0. X-0.0915 I0. J-0.0915 R0.0915
Y-0.0269 X-0.0828 I0.0457 J0. R0.0457
G00 X-0.0828 Z1.625 Y-0.0269
X0. Y-0.0602
G01 Z1.55 F9.
Z1.17
X-0.019 Y-0.0863
G03 Y-0.0925 X0. I0.019 J0.0261 R0.0323
Y0.0925 X0. I0. J0.0925 R0.0925
Y-0.0925 X0. I0. J-0.0925 R0.0925
Y-0.0863 X0.019 I0. J0.0322 R0.0323
G01 X0. Y-0.0603
G00 Z1.625
Z1.75
M15
G18
M09
M135
M155
G99
M01
G28 U0. W0.
M30
%

[KenFoulks]

From the Haas Factory Applications Department:

There are couples of thing you can do to correct this problem:

1. There are IJK and R in every G03 line, prefer to use IJK, it is more accurate.
2. You should be able to use one line of code, e.g. (G03 I-0.0925) to cut a full circle for Y axis machines.
3. If you want to hold the tolerance better than 0.0005, I would suggest using the C axis tool path, rotate the spindle around the cutter, since this hole is in the center of the lathe spindle.
4. Check X&Y axis tools center line, the closer the better, and avoid using cutter compensation if possible.
5. Add a finish cut to avoid a tool deflection.

[Chriseg1]

Thank you Ken,

I would love to use the C axis for this, and other parts. but I have a problem on the software side. i have contacted the publisher and worked with them extensively to resolve the posting issue.. but, long story short, I can ether post so as to use the XY, or post to have the machine convert XY to XC. I cannot do both in one post.

I can post XC, but If I post with C, the C commands are posted to the 4th decimal and the machine will error. The publisher has said they could not fix that and that I should post for the machine to convert XY to XC. but doing that on center line does strange things. the hole is clean, but the C axis back spins at uncontrolled points.

Is there a way to have the HAAS control ignore or round the 4th decimal place number?

[KenFoulks]

Please send us an email, include:
Serial Number
Contact Information
Your contact at OneCNC and his/her contact info
Part Print
Full Program

apps (at) haascnc.com

[Matt@RFR]

Check X&Y axis tools center line, the closer the better, and avoid using cutter compensation if possible.

Ken, can you elaborate on why this was suggested?

[Chriseg1]

I will get the info to you as soon as I can, but I am at a different location today.

Thank you for your help.

[KenFoulks]

Ken, can you elaborate on why this was suggested?

Cutter comp has tool offsets and other factors that can complicate troubleshooting. Many CAM systems didn't do Y-axis lathe cutter comp very well in the beginning and there were some software issues with earlier versions of Y-axis software.

[Chriseg1]

Update:

the problem is entirely software. we did have a tech come and check the machine for another issue, but had him look at this issue as well. he did find and couple small 0.0002 -0.0006 misalignments and dialed it all in. it did not make a difference on the hole shape.

after a lot of back and forth with the software tech, he finally admitted that there is an issue in the soft ware that prevents it from outputting 3 decimal for the C axis without also limiting all axis to 3 decimals. Also, the software is limited in that you can either do one of three types of face machining, and you need a different post for each one. 1: you can do XY to XC conversion in the controller. 2: you can do true XY movements. 3: you can do XC movement, but only if all axis are reduced to 3 decimals.

you cannot switch between these in one program, you must change what post is being used for each tool group and either post them separately and edit them together in a text editor, or set them up as sub programs and call them up in the order needed.

we have been able to produce round holes now with each of the option above, but not at all happy with the limitations of the software. Looking at MasterCam now.