Vcarved letters - More smoothing

[Bob Savage]

Alright, I got a good shot of the "chatter" I'm talking about. There are a boatload of forums here now, so know where it goes, I don't, but it's a sign so here it is.

This picture depicts the smoothing issue I mentioned in the WinCNC smoothing thread. I was mistaken about this issue being only on curves. As you can see, the P, A, K and E in this picture also exhibits the problem.

I have not tested slowing down the rate yet, per Guy's suggestion, but will next time I cut lettering. I will say, that I see many people posting about cutting letters over 180-220 IPM without issue, but nonetheless, if it fixes it, that's good.

Any other input, now that I have a good shot posted?

[mezalick]

Bob, I am certainly no expert on this topic but my first responce would be tha the step over is too large.
The points on the top of the letter when the bit starts to cut are closer together than where the bits stop cutting, at the bottom of the letter, thereby causing the ridges.
I think.
Michael

[Bob Savage]

Hi Michael,

I've got my vcarving clearance pass at 24% and final pass is 2%. Do those seem reasonable?

[mezalick]

I'm not sure Bob.
I assume you are using a ball end bit ?
If so the bit can't cover all of the area on the sides of the letters.
Maybe if you used a V bit and ran it around the edge of each letter, like a profile line.
That would need a bit more room between each letter and it may not look as nice.
Hand sanding or using a Dremil may also help, but it's more work.
michael

Originally Posted by Bob Savage

Hi Michael,

I've got my vcarving clearance pass at 24% and final pass is 2%. Do those seem reasonable?

[mezalick]

Bob, '
The more I look at your pic I come up with more questions.
There appaears to be no lines on the beveled edge. Are you using the same bit for that as well as the letters?
Michale

[Bob Savage]

Originally Posted by mezalick

Bob, '
The more I look at your pic I come up with more questions.
There appaears to be no lines on the beveled edge. Are you using the same bit for that as well as the letters?
Michale

Hi Michael,

I'm using a 1/2" 60 degree Vbit for the lettering and a 1/4" endmill for clearing.

[Joey Jarrard]

Bob,
Frank has looked at your ini file you have sent us in the past and he has some adjustments that should correct the problem you are having. Please call the shop and talk to him if he has not e-mailed you already.
Thanks,

[Bob Savage]

Originally Posted by Joey Jarrard

Bob,
Frank has looked at your ini file you have sent us in the past and he has some adjustments that should correct the problem you are having. Please call the shop and talk to him if he has not e-mailed you already.
Thanks,

Hi Joey,

Frank did send me an updated WinCNC.ini file. I'll call him shortly.

Thanks for the quick support turnaround!

[mezalick]

Would it be possible to discribe the problem and how it was fixed?
I would be interested in case I run into the same problem.
Michael

Originally Posted by Joey Jarrard

Bob,
Frank has looked at your ini file you have sent us in the past and he has some adjustments that should correct the problem you are having. Please call the shop and talk to him if he has not e-mailed you already.
Thanks,

[Bob Savage]

Originally Posted by mezalick

Would it be possible to discribe the problem and how it was fixed?
I would be interested in case I run into the same problem.
Michael

Michael,

I just spoke with Frank and here's what he's done. There are two problems that he addressed, one of which I did not mention in this thread.

For the smoothing, Frank increased the g09 smoothing setting. The machine came stock at s15, I had increased it to s20 and Frank brought it up to s35.

[*************Adjust Smoothing as Needed**********]
g09=s35 [a45 [S#smoothing/A#angle][Wincnc Manual pg51]

Additionally, he increased the resolution of the resolution of the arc_err value from .010 to .005.

[Arc Settings]
[g2modal=1
arc_err=.005

And finally, I initially had an issue with my Z0 reference being lost during machining, causing the bit to plunge too far into the material during Vcarving. This was resolved by decreasing the acceleration setting on my Z axis. Having dived into my first 3D work yesterday, I again encountered the issue which caused the Z axis to dive .150" deeper than it should have, about 3/4 of the way through the job.

Frank decreased the X,Y and Z acceleration a bit more, indicating that due to the extra weight of the X3 gantry/tools, the machine requires a slower acceleration than a single head machine.

I'm planning on running this file again tonight and will let you know the outcome.