What's new
What's new

Gibbscam, Surfacing a radius with g18/g19?

dandrummerman21

Stainless
Joined
Feb 5, 2008
Location
MI, USA
I have a solid file, that has 15mm and 20mm radii on some islands. I would like to surface them with a ball endmill, but I would like to be able to switch the machine to G18/G19 (depending on their orientation; this file would need G19).

Right now, the best I can figure out is to surface them using the surfacing operation, but it cuts up the code into .01-.03" long. That leaves a surface that is faceted, kind of looks bad. It isn't the end of the world with this part (black delrin, tolerances are not tight either), but if I knew how to make gibbs Change to G19 and use g2/g3 JxKx, it would be a lot smoother.

I could figure how to program it manually, but this comes up from time to time and would rather know how to do it quickly than do it manually (this part has 4 islands, 2 different size radii)

FYI the machine is a mid 90's Leadwell 760, with 0m control, so no smoothing out by the control like some new controls have.

The code I get looks as follows (very truncated, this code takes up 450k of memory, I'd have to drip feed this):
...
G1 Y2.8111 Z-.0384
Y2.8041 Z-.0463
Y2.7985 Z-.0538
Y2.7929 Z-.0627
Y2.7883 Z-.0715
...

zXT9Y8l.png


lFfHHGa.png



Ideas?
 
I am not sure how Gibbs handles this, but there should be an option somewhere to turn an ARC filter on. Also the post your are running would need to be setup for this posting G18 / G19 arcs. With the correct post and arc filter turned on, you should get the G18 / G19 you are after...

Question, if you ramp or helix are you getting a G17 G02/G03 XYRZ currently?
 
My post supports g2/g3 just fine in the normal g17 mode.

I don't believe it is related to my post specifically. If i run the machine simulation for the part in gibbscam, you can see the facets the machine programs, rather than a smooth radius that results when doing a radius in the xy plane. This suggests that gibbs is processing it as lines, and it has nothing to do with the postprocessor.

I tried searching the help documentation, but it only mentions g18/g19 is possible with CS selection. I tried changing my CS to the yz plane, it just posted out code that pretended i was machining it from the side, not above.

0je6075.png


I did run the program that gibbs gave me, it actually looks better in delrin than the simulation does, even when the machine wouldn't go faster than 50ipm because it was starved for data (9600 baud rate). I recently made a similar part out of stainless, and because it is shiny, you could see the facets, it looks like they are spaced .100" apart. It was good enough, but again, it should have been posted as a radius instead of line segments, ideally.

That cimco program looks cool, and if it works like it says it does, that would be cool. However, this doesn't come up enough for me to have the company buy a program, that this 10k$ program (gibbs) should post out for me. Besides, I have a way around it (drip feeding), so that is another reason to avoid that program. Still cool tho.
 
I find it very hard to believe you can swing a g18 g19 with gibbs on a 3d surface....

What version are you running and what toolpath are you using?
 
Many years ago, I machined a one off part that required an arc to be machined in the XZ plane.

The program was written manually with circular interpolation using a 1" ball mill and try as I might, the arc never came out exactly as I wanted. (It had to match a partially milled radius done in the XY plane).

From what I can see, to get a true radius with a ball end mill, the tool path is NOT a series of arcs, but rather more complex as the software maintains tangency with the required surface.

So, I don't think it is simply a matter of Gibbs switching planes for you.
 
The radius can be programmed with a ball mill, without several g2/g3 moves, but simply one arc move.. It is no different from circular interpolation in the xy plane; you still have a round tool (ball endmill) and a round part (radius in the yz plane), so it can be programmed as such.

To get my 15mm radius with a .250 ball endmill, lets suppose the center of the radius is at x0y0z0, I could do the following:

...
G19
G0X0Y-.4655
G1Z-.125
G3Y.4655J.4655K0
G1X.01
G2Y-.4655J-.4655K0
G1X.02
G3Y.4655J.4655K0
.....
etc.

This will create a 15mm radius along the x axis (interpolates yz, with x stepover)

That is exactly the type of code I'd expect it to give me, not 200 moves per x stepover.

If it isn't possible for gibbs to figure it out, fine, but the very little documentation relating to G18/G19 in gibbs seems to suggest it supports it, but it gives no examples or specifics. If nobody here has done it, fine, the parts needing this are almost done, I've got a few more to run on Monday. Thankfully drip feeding exists.
 
I was able to it this.


First I chained the wireframe for the radius, for the contor toolpath.
Then I transformed"copied" the tool path for the .02 stepover x however many time to cover the surface
1.jpg

I then selected to comp the toolpath from the right plane. like using a right angle head
2.jpg

posted with G19
Capture.JPG

would not be able to zig zag the toolpath though, just one way climb
 

Attachments

  • 4.JPG
    4.JPG
    53 KB · Views: 366
I understand why the 3D CAM software will not post a single arc movement. The toolpath that is generated is linear interpolated, then what happens is an acr filter is run on all the line segments to "fit" arcs based on a tolerance. In your case, you are looking for 1 ) less code 2) smoother finish. Using arc fit would accomplish this.

This is how you turn on this option in BobCAD CAM


I have a really hard time thinking Gibbscam doesn't offer this option. They must! It's just a matter of finding it...
 
To get rid of the facets you'll need to decrease your cut tolerance. Even .001" will produce faceting similar to what you've described. We typically use .0002" for general purpose surfacing. Your processing time will increase as well. You can also fit arcs but a post modification is required to get it to work. If your post doesn't support fit arcs it will post as usual.

I recently tested 40 or so haas posts looking for one that would output arc code but I couldn't find one.
 
Hi, If you go into the plug-ins tab. scroll down you will find under toolpaths HSM(high speed machining). Click on that and you will Arc segmentation. It is set to default but if you click arc tolerance yo can change the min. tolerance for you arcs. The bigger the number the less line segments you get. That is as close to the Mastercam arc/filter I could find so far. I am also new to Gibbscam.
 








 
Back
Top