Rounding corners

Discussion/questions about software used with your CNC Shark and programming issues

Moderators: al wolford, sbk, Bob, Kayvon

User avatar
Kayvon
Posts: 552
Joined: Tue Oct 21, 2014 11:46 pm

Re: Rounding corners

Post by Kayvon »

MQUICK wrote:Checked square corners.
I thought this meant you'd already checked that box. What were you checking instead?

You're right about the post processors: contour for 3d, arcs for everything else. The contours file relaxes the precision between points slightly, which allows the machine to go a little faster on 3d cuts. For 2d parts, the precision is often more important and the operations aren't as inherently slow as 3d movements.

Rando
Posts: 757
Joined: Tue Jan 06, 2015 3:24 pm
Location: Boise, ID
Contact:

Re: Rounding corners

Post by Rando »

The differences between the two are actually very small, and appear to only be about the accuracy of the cutting. If you make useful changes to your post, I'll recommend these three things:

First, use that My_PostP folder. Put just the post files you want in there, and those are the only ones you'll see in Vectric's pulldowns.
Second, make copies of the post files, and edit at will. They're not that complicated, and once you learn the GCode (it's really quite simple), you can add useful operations. For example, I add an M06 T01 "tool change" right before the start of the moves, so it pauses and waits for me to make sure everything is up and running.

And finally, I added/modified this command to all my Shark post files:

G64 P0.001

Okay, maybe 0.001 is a bit excessive. This command sets the "path tolerance" of the CNC movement system. The value sets the maximum allowed deviation from the programmed path. If this isn't set, the assumed value can be quite large, rounding off corners of rapid travel, and potentially even gouging the workpiece. Note that the various and many simulators / back plotters don't seem to predict that path-rounding, and so many times won't warn about tool/part/vise/clamp collisions. Typical values are 0.001 to 0.010. The values in the CNCShark-USB files is either 0.1 (3dcontour) or 0.01 (Arcs). Thus, the Arcs will be seriously more accurate. I'd modify them BOTH down to 0.005" or less, and my values are 0.001", as part accuracy is important to me.

Regards,

Thom
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)

User avatar
Kayvon
Posts: 552
Joined: Tue Oct 21, 2014 11:46 pm

Re: Rounding corners

Post by Kayvon »

Rando wrote:The values in the CNCShark-USB files is either 0.1 (3dcontour) or 0.01 (Arcs).
Yikes. I had forgotten what the actual values were. I think I'll create a third file to use when accuracy matter a lot (e.g., when I'm cutting all the clock gears I just finished cutting :( ).

User avatar
Kayvon
Posts: 552
Joined: Tue Oct 21, 2014 11:46 pm

Re: Rounding corners

Post by Kayvon »

For those interested, here is a modified post-processor file that uses 0.002" precision rather than 0.01" precision. In all other aspects, it's identical to the arc-inch post processor.

Be sure to check this and any post processor file before using it. Just because it works for me doesn't mean it's right for you. It must be renamed from .txt to .pp in order to use.
Attachments
CNCShark-USB_FineArcs_inch.pp.txt
(5.18 KiB) Downloaded 345 times

User avatar
bill z
Posts: 342
Joined: Fri Sep 25, 2015 9:09 am
Location: Spring, Texas USA

Re: Rounding corners

Post by bill z »

I think I really misunderstood this thread. Probably my dyslexia.

I was having some problems where Aspire showed square corners but the Shark cut rounded ones only on one side of the cut. Actually the corners were 135 degrees. Strange, because all of the 90s really did come out square.

Anyway, I changed to 3D because of what I thought was being suggested. and that really rounded everything even though Aspire showed square corners. Not what I wanted at all. Doesn't seem to happen all of the time, that I notice, like with other projects.

I even redrew the project not using any circles in the design, just squares and rectangles. To get the angles, I rotated squares. When I look at the nodes, everything was sharp angles. Still the cut is rounded on angles larger than 90. I even slowed down the cut to 45%.

What I have not done yet is set use Kayvon'e post processor or to change precision to .002 from .01.

If anyone has another suggestion, I'd love to hear (or read) it.

User avatar
Kayvon
Posts: 552
Joined: Tue Oct 21, 2014 11:46 pm

Re: Rounding corners

Post by Kayvon »

Bill, does Aspire have the same problem in the preview, or only when you run it on the shark? If the problem appears in the preview, could you post an example file? Hopefully in something VCarve can load for those of us who have yet to upgrade.

User avatar
bill z
Posts: 342
Joined: Fri Sep 25, 2015 9:09 am
Location: Spring, Texas USA

Re: Rounding corners

Post by bill z »

In the Aspire preview to the cut, all looks OK. I can zoom in and it looks good.

Ah, but the cut, isn't what the preview indicates. Please know that I'm still a novice at this.

It may be ware and tare in the Shark. Even HDs get loose sometimes.

I'm open to suggestions.

I'm finding with the spring times honey Dos, I'm not getting as much CNC time as I want. I can use more time to clean, oil and tighten up some stuff. Maybe that may fix some of it.

I'm sorry if you are in the NE right now with feet of snow. But, down here in SE Texas, it is Spring, with robins and budding flowers.

Rando
Posts: 757
Joined: Tue Jan 06, 2015 3:24 pm
Location: Boise, ID
Contact:

Aside: why they used G64 P0.1 in the 3D postprocessor file

Post by Rando »

(Sorry to retrace back in the thread. Kindly continue with BillZ's issue :D )

I just now realized why the "contours" has such a large G64 (path interpolation) value. It is indeed so that 3D carvings come out correctly. But, not "correctly" in the way you and I think. When we say the toolpath acts correctly, we mean that it accurately matches what we told it to do. If we were to get out the calipers and measure some feature, why it should be what the model/design says it should be, right?

Yup, that's totally the way I see it too.

Except, what if the term "correctly" didn't really mean "accurately", but meant "without destroying the machine and breaking the bit and making a gawd-awful mess of the wood?" I mean, that's one form of "correct", right? Cutting aluminum all the time, I have more than my fair share of horribly broken end mills. By way of comparison, an off-sized part that finished being made is of more use and better than one that ruins the part, breaks a $50 bit, and makes me take a day to figure out how to prevent it from happening again. Right? That last part? That's the BAD stuff!

So if your goal in making the post-processor for 3D carving is to make the carving come out "close enough" dimensionally, but more importantly reliably "correct" in this new sense of not instilling panic in the user, then maybe having relatively loose path interpolation is actually a Good Thing. One easy way to do that might be to not allow the spindle to make "sudden moves". Because let's face it...when you're doing a VCarve/Aspire 3D Carve, it does raster-style, or planar (chew a little off the top each time). In planar, the "sudden moves" come in the XY plane, and that's perfectly normal, that won't too seriously affect the cut. But, check it out: in the raster-style, all of those "sudden moves" are at high-incline areas in that raster-line's path. Yeah...in the Z direction.

Plunging too quickly, trying to make walls too vertical, and edges too sharp, those are the things you're NOT going to have much success with a ballnose end mill. Sure there are some cases, but not like the raster mode Vectric uses. And so, they assume if you're going to take the time to do raster, there's significant detail in that...and you want it to come out properly.

One way to achieve it that doesn't require getting into the toolpath-generation guts of VCarve, it to just change how closely the CNC moves along the programmed path....which is conveniently what G64 does! In a raster toolpath, it essentially "rounds off" all those sudden moves up and down in Z. By effectively reducing that fast/sharp plunging, it would indeed have the desired effect of lowering the peaks in cutting stress. In aluminum, those stress-peaks spell destruction. In wood, often it just means a groaning noise that makes you look up, more hand-sanding in that area, and that's about it.

Maybe there IS a use for a G64 that large after all.

Now back to the new conversation....
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)

Post Reply