Error from Kmotioncnc

I get an error from Kmotioncnc during test cutting a part. This is maybe a fault from the cam program. Running with Mastercam x4. Cutting tool is 25 mm dia.

Attach a pic from screen.

Attachment 274696

Any idea as to why i get this. Something set wrong in cam or Kmotioncnc? Hope someone can steer my in the right direction.

/Lars

Go to the machine type tab menu in mastercam and select machine definition manager. At the top of the window there is a icon for control definition. Select that. On the left under control topics select arc. Under arc center type change the xy plane to unsigned incremental. Then check out of that screen and hit yes to save. Check out of the next screen and hit yes to save again. Then repost your code and see if that fixes your problem.

Ben

Thank you!

Have reposted the code and will try again. Fingers crossed.

/Lars

Sorry to say that it did not work... get another error now.

Attachment 274776

Attachment 274776

/Lars

Sorry it didn't work. I was having the same issue and that's how I fixed it. If you want to post a picture of a few of your screens I'll compare to mine and see if there are any obvious differences. The same screen where you adjusted the arc settings and also the tolerance screen in the same area.

Ben

Also what post processor are you selecting? I am using inch not metric but I'll try a similar metric post to yours and see what I can come up with.

Ben

I guess a better question then what post is what are you selecting for machine type?

Ben

I have to get back to you on that. Not at the shop now. I think i have picked some standard 4 axs mill vmc. Cannot remember the exact name. I will post some screenshot later today.
Thank you for your help!

Im a beginner on all this.

/Lars

For Mastercam, I use the default router post, and it works perfectly save for some stuff that I have to delete prior to running. The only time I have seen an error like that is when I have tried to run a program from the middle without starting from the beginning.

I did the math for the incremental IJ needed for KMotionCNC. The radius is way off. As absolute IJ the Gcode doesn't make sense either.

Code:

---

Start        IJ        Center        End        cent to end
-53.77        6.406        -47.364        -23.199        24.165
11.611        24.165        35.776        -6.149        -41.925
                               
        Radius beg                        Radius end
        24.999681218                        48.3906277083

---

You might look at the CAM data and determine what it is trying to do. What kind of arc should be generated? Where would be the center? What would the radius be? Then you could probably look at the GCode and see what was wrong. A GCode Arc is pretty simple. The last coordinate is the starting point of the arc. The IJ is where the arc center is relative to the starting point (so add IJ to startxy to get the center). The specified XY coordinate is the end.

HTH
Regards

Here is some screenshots from the settings pages you wanted.

Attachment 274854

Attachment 274856

The Machine type selected is MILL 4 - AXIS VMC MM and the Postprocessor is Generic Fanuc 4X Mill.

I have not changed any settings in here except those you mentioned, the Arc one.

Maybe its the wrong postprocessor?

/Lars

Ah I just noticed changing the sign of J in the GCode (from 24.165 to -24.165) makes the beginning and ending radii equal.

Is there an "incremental signed" option?

Regards

Hi!

Yes there is.

Attachment 274862

What does all this mean? If there even is a easy way to explain this :)

Well, Signed radius is an option, shown in the Pic

I changed Control file to DEFAULT.CONTROL and Post-processor to MPFAN.PST. Now the error has gone away when simulating in KmotionCNC. The machine is at work so I cannot test run it until tomorrow.....

Hopefully this works!!

ARC center type now states: Delta start to center, what ever that means :)

Hi Lars,

Yes I was just about to suggest "Delta start to center". It means exactly that :)

(it means that IJ specify how far to go in XY from the arc's starting XY point to get to the XY center of the arc)

Good chance if it works in simulation it will work on the machine. I'm not sure what other differences are between the two different "posts" so the other option is to go back to the other and make that one change.

Good Luck
Regards

Problem solved!

Using another postprocessor made the trick!

Thnak you all for givning me the advise!

/Lars