Daniel's Work Thread: Toward a Hackerspace Scanner

[rob]

I think you may end up having to post your problem in the Mach3 forums. I read the first post you linked to, from 2007, and it looks like the guy never had his problem solved. Surely the situation has gotten better in the intervening five years?

In any case, CV and sharp corners shouldn't be a problem. Because the tool has a radius, the toolpath is going to be a quarter-circle around a corner anyway, and as long as you don't have the feed rate set so high that you whip around that arc, acceleration should be low enough that you won't have a problem. That's geometry.

And here's math:

Let your feed rate be F inches per minute. And let your tool diameter be 1/4", because I know that's what we're using. A quarter-circle of radius 1/8" around the corner will let you make a sharp corner. The acceleration towards the center of that circle is just v^2/r, so 8 * F^2 inches per minute per minute. So if your feed rate is 220 ipm (or 3.67 ips), then your acceleration around that corner is 387,000 inches per minute per minute, or 108 inches per second per second (2.7 m/s^2, or about a third of a g). Is your machine capable of doing that?

If not, you may need to change your feed rate around corners to be slower, which is what the ShopBot does. It's the max feed rate on straight cuts, but it has to slow down around corners (and so it does, making perfect sharp corners).

Now, as to why you're getting rounded corners in some directions and sharp in others... is it possible that the machine is stiffer in one direction than in another? Make some test squares to see.

And finally, I am mystified by the advice to turn arcs into polygons. To me, anyway, arcs would be much easier to accelerate around. Polygons are all sharp angles, which would seem to make the moves less smooth?

[daniel_reetz]

And finally, I am mystified by the advice to turn arcs into polygons. To me, anyway, arcs would be much easier to accelerate around. Polygons are all sharp angles, which would seem to make the moves less smooth?

The thing is, circles can be represented by a G-code for arcs, or they can be represented by a bazillion tiny line segments. When represented the second way, they can really mess up motion control algos and cause shuddering and all manner of problems. I saw this in person with my last set of cuts. So the fewer vertices, line segments, etc, the better. I pre-emptively despise this fact even more than you will.

Thanks for the crisp-and-clear math, Rob. I'll be cutting squares all weekend until this is FIGURED OUT.

[daniel_reetz]

It turns out that VCarve can output with apostprocessor designed for Mach3, and it can output arcs instead of line segments. I'll be using the "Mach2/3 Arcs(inch)(*.txt)" output settings for my test today.

The test piece is a 6" square with .2" support tabs. I will cut it and modify machine settings until it cuts square.

[daniel_reetz]

Square testing Gcode attached.

Feedrate 100ipm (too slow for my bit, unfortunately, but I can't really run my spindle slower than 12krpm as it is air-cooled... will have to work on this).

[daniel_reetz]

Alright, following all the info in the threads, and Rob's math, and everything, I got it to work - at least for squares.

I cut the squares at 50, 100, 200, 250, and 300 Inches Per Minute feedrate. I have to say I'm pretty impressed with this machine in that respect. On the 6" squares I cut, the machine spent most of its time near or around 300IPM, so it's definitely going to haul if I can consolidate lines in future GCode.

The finish is about as good on any one piece, maybe a hair better on the slower ones. I'll chisel the tabs off and take a closer look at them and then try cutting an entire scanner for the Paper Upgrade project.

[daniel_reetz]

These are my Mach3 settings and motor tuning settings.

[daniel_reetz]

Cutting out a machine now at 250IPM.

Lessons learned so far:

1. It pays to be aggressive with tab thickness. Too-thin tabs can disappear if the wood bows up during cutting. Corollary: buying truly flat plywood is DEFINITELY worth the money. .2 inches is minimum. "3D tabs" as setup in VCarve are worth it.

2. Ramping into plunges, especially in pockets, is worth the extra time.

3. Part spacing is important.

This won't turn out to be a full scanner due to mistakes on my part.

[daniel_reetz]

Postmortem: this unoptimized cut took 1 hour, 10 minutes. That's pretty solid and I think I could shave off the ten extra minutes easily. That also says to me that with optimized sheets containing many parts, I could probably get the total cut time with loading and unloading the machine to around an hour per machine. Considering that I want to spend exactly one day per week on this, I feel that this is all now in the realm of possibility.

Good.

Bad things - many parts were not sufficiently tabbed. This was due to three factors, one being that the wood was warped and so some tabs were lost due to lifting. Another was due to some parts being too close to each other, so that the tabs were not holding on to a substantial piece of material. Third was that some parts just didn't have enough tabs.

Some parts, especially the handlegrip holders and button-pressers, have arcs that gave my machine fits and need to be re-drawn.

All my parts had a relatively poor quality bottom finish. This may be due to the bit I currently have in the machine. I will try a different (new) bit as soon as I can get one.

I will post a more detailed post-mortem as soon as I can.

[daniel_reetz]

Decided to do a video. Post-mortem uploading now.

[daniel_reetz]

Post mortem uploading here. I'm off to get some tacos. I'll get another sheet of plywood today and try for a complete cut by the end of the day.

ETA:2 hrs