[jay_dizzle]

Hello everyone, im trying to machine a large radius into the face of a steel plate and im having trouble getting BobCAD to output some decent looking code.

i have drawn the plate as a solid and then drawn a cylender as a solid and subtracted the cylinder from the plate. i am using a planar function to try and cut the contour into the surface of the plate.

instead of outputting smooth G02 and G03's i am getting a bunch of choppy G01 moves. i have selected the arcfit box and it doesnt help. the only thing that seems to help is if i increase the arc tolerances and the machine tolerances,

and even then it still has some short choppy sections please help!

-OSP200M post processor
-V26 BobCAD

[RAF.]

Hello everyone, im trying to machine a large radius into the face of a steel plate and im having trouble getting BobCAD to output some decent looking code.

i have drawn the plate as a solid and then drawn a cylender as a solid and subtracted the cylinder from the plate. i am using a planar function to try and cut the contour into the surface of the plate.

instead of outputting smooth G02 and G03's i am getting a bunch of choppy G01 moves. i have selected the arcfit box and it doesnt help. the only thing that seems to help is if i increase the arc tolerances and the machine tolerances,

and even then it still has some short choppy sections please help!

-OSP200M post processor
-V26 BobCAD

Maybe your problem? 3D large Gcode
2D smaller Interpolated Gcode

[jay_dizzle]

thank you for the reply, i am currently using the 3 axis selection.

also, i am cutting a radius out of the face of the plate... like a skateboard half pipe... or like a valley that travels along the y axis...

[SeanDa]

Jay,

Does your machine support G131/G130?

[jay_dizzle]

Jay,

Does your machine support G131/G130?

no it does not...

[SeanDa]

Jay,

With Okumas, you would need to enable the high speed option on the machine. I know in newer machines, its G131/G130 to enable/disable the high speed contouring option. This would eliminate your issue. Do you know if you machine has any high speed option?

[jay_dizzle]

Jay,

With Okumas, you would need to enable the high speed option on the machine. I know in newer machines, its G131/G130 to enable/disable the high speed contouring option. This would eliminate your issue. Do you know if you machine has any high speed option?

i dont believe it has anything to do with the machine, i can read the code that BobCAD is putting out and it is a bunch of small segments of straight lines that are mixed in with the occasional G02/03.
the machine is doing exactly what the code is telling it to do.

all of my okumas are less than 10 years old, osp200 controllers, G131/G130 arent listed in the program manual nor are they listed in the interactive machine menu. high speed cutting is enabled/disabled within the parameters.

[RAF.]

Can you Zip and Post the file

or maybe just a pic of the solid

[SeanDa]

Jay,

For any 3axis toolpath, you are going to get G01 movements from point to point, with the exception of when arc fit is enabled, which creates arc segments where possible based off the defined tolerance. If the machine is running choppy when running these toolpaths, that is because it accelerates,decelerates while going into and out of the segment. This can be resolved by enabling the high speed option through the code, or by modifying the tolerance of the high speed function of the machine.

[SeanDa]

Jay,

Here is the manual I am referencing for the Okuma where I saw the G131.

[jay_dizzle]

i understand the high speed machining function, and i believe it is set up properly on the machine side. my issue is BobCAD outputting G01 movements where there should be arcs.
the part i am trying to machine has a very very simple radius cut into its face in the G18 plane. this radius should be one simple movement from one point to another, there is no need to break the arc into segments of straight lines.

[SeanDa]

Jay,

Upload the .bbcd file in a zip folder and we can take a look and see if we can get you those G02 movements. Also upload the post processor you are using.

[jay_dizzle]

here ya go, look forward to hearing from you!

[SeanDa]

Jay,

I updated your post processor and increased the arc fit tolerance. This reduced the number of linear segments, while also making the arcs larger. Your post will also now output G18/G17 when it is required.

[SeanDa]

Jay,

Also just a note. Your stepover is greater than half of the selected tool. This can be problematic from a left over island standpoint. You should set the stepover to .5 at most for the tool size you are using to get a better finish. Your machining tolerance is also way to larger. The machining tolerance should never exceed .0015 or else your part may not cut correctly.

[jay_dizzle]

when i try to open the provided BobCAD file it says "cam tree loading fail" and BobCAD crashes

[SeanDa]

Jay,

This means my version of V26 is greater than yours. As far as the arc fit, I do not recommend increasing the tolerance after looking at it. It causes a major gouge on a section of your part. Do use the updated post, as it will atleast allow G18 arcs, which your old post would not. Do you have a g-code list for that machine by chance?

[jay_dizzle]

Jay,

Also just a note. Your stepover is greater than half of the selected tool. This can be problematic from a left over island standpoint. You should set the stepover to .5 at most for the tool size you are using to get a better finish. Your machining tolerance is also way to larger. The machining tolerance should never exceed .0015 or else your part may not cut correctly.

yes i agree, these were just things i was messing with to try to get the program to output properly

[jay_dizzle]

i had been manually entering the G18 command in the past in order to have the code run

[SeanDa]

Jay,

Just looking at the positions in Predator, the code seems to be running OK, without it being choppy in Predator. Try that new post with an arc fit tolerance of .005 and a machining tolerance of .0005 and stepover over .5 or less and see how it works with the new post outputting the correct arc plane. That may have been the issue possibly the entire time.