cutter compensation not working.

[jerrybentley]

I have used the radial compensation on this machine before but not with fusion 360. It seems to me the program and code is correct, But looking to be confirmed on this??  The program does run but  don't obey the the offset

I am attaching the gcode in this post and tiring to attach the file. I have a Milltornics machine with a centuion 6 control. It always runs flawlessly Any ideals??

O5000 (FL ROLLER FIXED)
(T6 D=0.47 CR=0 - ZMIN=-0.875 - FLAT END MILL)
N10 G90 G94 G17
N20 G20
N30 G32
(2D CONTOUR2)
N40 T6 M6
N50 S2425 M3
N60 G55
N70 M8
N80 G0 X-1.8623 Y-1.5499
N90 G43 Z0.6 H6
N100 G0 Z0.2
N110 G1 Z0.0394 F9.2
N120 Z-0.828
N130 X-1.8621 Y-1.5497 Z-0.8333 F11.5
N140 X-1.8614 Y-1.5492 Z-0.8385
N150 X-1.8602 Y-1.5483 Z-0.8435
N160 X-1.8587 Y-1.547 Z-0.8484
N170 X-1.8567 Y-1.5454 Z-0.853
N180 X-1.8543 Y-1.5435 Z-0.8573
N190 X-1.8515 Y-1.5414 Z-0.8612
N200 X-1.8484 Y-1.5389 Z-0.8647
N210 X-1.8451 Y-1.5362 Z-0.8678
N220 X-1.8414 Y-1.5334 Z-0.8703
N230 X-1.8376 Y-1.5304 Z-0.8724
N240 X-1.8337 Y-1.5272 Z-0.8738
N250 X-1.8296 Y-1.524 Z-0.8747
N260 X-1.8255 Y-1.5207 Z-0.875
N270 G41 X-1.6304 Y-1.6916 D6
N280 G3 X-1.5809 Y-1.2674 I-0.1874 J0.2369
N290 X-2.1691 Y-1.7326 I-0.2941 J-0.2326 F9.2
N300 X-1.5809 Y-1.2674 I0.2941 J0.2326
N310 X-2.0051 Y-1.2179 I-0.2369 J-0.1874 F11.5
N320 G1 G40 X-1.8838 Y-1.447
N330 X-1.8879 Y-1.4503 Z-0.8747
N340 X-1.892 Y-1.4535 Z-0.8738
N350 X-1.8959 Y-1.4566 Z-0.8724
N360 X-1.8998 Y-1.4597 Z-0.8703
N370 X-1.9034 Y-1.4625 Z-0.8678
N380 X-1.9067 Y-1.4652 Z-0.8647
N390 X-1.9098 Y-1.4676 Z-0.8612
N400 X-1.9126 Y-1.4698 Z-0.8573
N410 X-1.915 Y-1.4717 Z-0.853
N420 X-1.917 Y-1.4733 Z-0.8484
N430 X-1.9186 Y-1.4745 Z-0.8435
N440 X-1.9197 Y-1.4754 Z-0.8385
N450 X-1.9204 Y-1.476 Z-0.8333
N460 X-1.9206 Y-1.4762 Z-0.828
N470 G0 Z0.6
N480 M9
N490 G32
N500 G28 G91 X0 Y0
N510 G90
N520 M30

[MoshiurRashid]

Hi

Thanks for posting. We have a manufacture forum for CAM and CNC related posts. @seth.madore  Will help you by moving your post in that forum.

Stay safe!

[seth.madore]

The compensation codes are there:

With Control comp, if it's not being obeyed, that means your holes are .470 larger than expected?

[mathew.hutton · Accepted solution]

Hi @jerrybentley 

Have you specified you want to apply radial wear compensation in the toolpath? It will only apply Z axis wear offset when set to default which is "in computer". I have attached an image of where to locate the compensation type drow down selection. You can also mess around with tool compensation by toggling with the "stock to leave" option as shown in the other attached image, this may be easier for you rather than applying wear offsets to each tool in your machine. This is how i tend to use it for cutting to specific sizes or tight tolerances.

Hope this helps

Mat 

[jerrybentley]

not sure I understand  your reply. I don't think the wear offset or stock to leave will help .  the compensation   seems to be ignored .  I have a .75 hole in the part,  but I'm cutting near a 1" hole.  It don't seem to make a difference what value I put in the radial offset on the machine.

[jerrybentley]

I don't understand what you mean ,   With Control comp, if it's not being obeyed, that means your holes are .470 larger than expected?   I don't understand how you figure this,  hope you are right, but could you explain more?

[alan]

Hello,

I know that we have to use "wear" not "in control" on our Haas machines.  The other issue is we have to have out tool diameter offset at 0.0

Fusion is great but you have to get to know it.

[seth.madore]

In your offset page on the control, you should have fields for length and diameter.

Control compensation requires that you input the radius (or diameter, depending on control) of the endmill into the diameter column of that tool. 

If your machine isn't recognizing the control comp, is your hole coming out oversized?

[jerrybentley]

My holes are coming out oversized.

[seth.madore]

How much oversized?
Are there any values in the diameter offset column?

Does your tool measure .470 in actuality?

[jerrybentley]

I have .470 in the diameter offset slot,  my machine does call for diameter ,  but I have entered less than 470 but don't seem to make a difference.   I am getting a cut of about 1"  I forgot  exact hole size  but near 1".   Its hard for me to say exactly what its doing,  because that size does not support that it is cutting on the z axis center line.   The real tool size is .473

[seth.madore]

Modeled hole size is .75". Endmill size is .473". If cutter comp was being ignored entirely, you should have a hole size of 1.223" (hole size plus endmill size).

Looking at your code, we have:

N280 G3 X-1.5809 Y-1.2674 I-0.1874 J0.2369
N290 X-2.1691 Y-1.7326 I-0.2941 J-0.2326 F9.2
N300 X-1.5809 Y-1.2674 I0.2941 J0.2326
N310 X-2.0051 Y-1.2179 I-0.2369 J-0.1874 F11.5

To check that the post processor is giving us correct data, we take the square root of I squared plus J squared, which does give us a radial value of .37496.

Because your code also does have a G41 D6 as I posted earlier, there has to be something going on with either the tool or the offset column.

To be close to the diameter you are getting, it seems to me that your machine wants to see full diameter values, not radius of tool, as that is approximately the difference that you are off

[jerrybentley]

I am interring the full diameter of the tool and also have tried  the radius.  Unless someone gives me a better ideal,  when I go to the machine again in a day two,    I will do some  more test I will test od profile and see what happens .  I will also go with different sizes until I find out what the machine is cutting or really doing.   I will post back then.

[jerrybentley]

I see in the program the option for wear offset,  I never new that was there , I never noticed.  With the stock to leave option you are talking about , I can't make adjustments after the frist try without  re posting can I ?

And if I choose the  wear option,  do I still enter the to diameter in the tool offsets?  The full size or just a small negative,  could you explain a little more?? Thanks

[seth.madore]

Traditionally speaking, a Wear Offset would start off with zero in the respective column. It is important that the tool is defined correctly. 

I personally prefer to use Wear. It's a lot easier to just leave everything set to zero and make small adjustments from there.

[jerrybentley]

This worked for me.  I created the program and done a contour   and then picked wear as compensation type ,  then set my tool offset to 0.0 on my machine radial tool size,  then at the end  to get  the correct size I ended up with -.006 that made the prefect size.

Thanks for the help

JB

[mathew.hutton]

Hi @jerrybentley 

Perfect, glad i could be of assistance! Let us know if you need any more help

Mat