I followed flashsolutions video for adjusting backlash and found that my machine had .007 backlash. But really claiming .007 is questionable as I am not sure that can be accurately measured on the machine. I input the .007 in the backlash setting and found that it did very little for correcting my egg shaped circles. What it did stumble onto was when I jog the x axis .050 and what my dial indicator set up showed for actual movement were completely different. In my video I start off by doing an x axis calibration, the. I perform a series of .050 jogs. You will see that the machine only moves about .020. After I set a .030 backlash, the machine then moves .050(roughly) when a .050 jog command is given.
Maybe someone can shed a light on my findings.

 

I'll give it a try. After I did the backlash adjustment my circles are concentric. All this came on when my machine developed a problem with accurately returning to zero on the y axis after long machining cycles. X and Z have amazing accuracy . Short cycles, it has no problem. I think my Y stepper is having issues, it started unlocking again.

 

Thanks Mark
I'll get it taken care of. My machine normally runs accurate with no issues but I have noticed a couple of times over the past month it " slipping". So now in retrospect I think that stepper was acting up when it happened.

 

I could not solve the un-round circle yet. All my cuts are not accurate. I calibrated so many times the pp had sent me an email complaining about boredom. I used a 1,2,3 block to measure the travel and the backlash. I used a dial indicator and it showed zero backlash on all three axis' yet I still have consistent inaccurate cuts.

In the pic below all edges in the red circles are identical. When I cut the parts out of 1/2" ply using the multipass the edges on the left where smaller than the edges on the right. I had to sand down the long edges.

When I drill four holes, in a circle at 90° to each other, three come out perfect on is off a bit. CONSISTENTLY. Same spot every time. I had that problem when I cut the parts for my outrunner spindle. And no, it's not a mistake in SU,, I've checked it three times.

I know that if I hold the chuck at the end of the spindle I can move the whole gantry. Not a lot but I can but not with just a light pull, a very strong pull and shove (while the steppers are under power). It's not that the bearings don't sit tight on their guide, they do. I've checked it a few times. It's just that the whole gantry has an inherent play. At the end of the bit maybe 0.1" maybe 0.2" Attached files

 

I would like to clarify something. The PP was designed to cut foam. That was the main and original drive behind Mark's thinking. The PP cut foam just as it was designed to do as you can see in the pics above and in the pics bellow, which I had cut today. The circles are near perfect as far as I can tell without measuring it. On the right the circles are cut in segments and on the left with the radius command.

The problem is that idiots like me can't leave well enough alone and try to do things that were not meant to be done in the first place. Having said that, did Evil-Tunes try to do these cuts in MDF or plywood? I'll be interested to see if he will get the same results as the cut in the foam Attached files

 

Tigerpilot

The J-peg you attached. did that come from google sketch-up? If you have a .dxf file, I can extrude it in Solidworks, then generate the code in MasterCam. Maybe see if its a code problem. I don't really know how you are generating the code but it maybe how the CNC USB software is interpreting the file that may be the problem. PM it if you want me to look at it. The only other thing I can think of being a problem is the stepper motor loosing steps. A problem I have been running into.
I had some head slop on my machine until a did a little modification by making a slot out of the right guide roller bolt holes. Making the right guide rollers adjustable. It does take a little special technique to get the roller tension right so there is no slop.
The phlatprinter will cut wood, you just have to do it slow (15 IPM) and make multiple cuts under .040 deep.

 

dhc8guru, the picture is a screenshot from SU. I have generated the code in SU and I use Mach3 not the CNC USB.

You are right, of course, that the cuts have to be made slower. I think that that is one of my problems. I used 20ipm and I think I should use 15ipm and cut less than 0.04. I'll see how it goes that way it will report back.

 

One thing I've learned about the pp is you might want to recalibrate
the machine for running different materials each time you run a new material.
Foam has very low resistance to the router, wood has high resistance.

Each time you calibrate the machine, save the settings file (usb-cnc card) with the name
of that material for the settings file. I do this, and I also keep the settings written down
just in case I should loose the file. When you change materials, just import the settings
file for that material.

When I was cutting my edge lit clock project I had to cut Oak and Plexiglass.
The settings I used with the Plexi did not work with the oak.
I found this out by experimenting on a scrap peace of wood and plastic.
I just engraved a 1" and 2" square and circle and then measured each.

I also had to experiment with feeds and speeds to get good clean accurate cuts.
My pp runs true, and is pretty tight on all three axis. If you know your
pp is put together correctly, then try saving a few setup files for each
material you are cutting and see how that works.

Another thing that might also be helpful is adding material guides to the deck of the
pp. It keeps the material from shifting left or right on the Y-Axis.
Guides can also help against rotational forces that try to twist the material in the machine.

Anything that you can add safely to the machine to help get the job done right is a good thing.

Hope this helps.
George

 

So the corner radius are intentionally a different size. I thought they were all the same radius and the ones in the red circles were coming out wrong.
MDF is hard as a rock. I would start with 7 IPM and increase it until you see issues. What are you using for a mill? A three flute end mill is ideal with wood.
Are you using an adjustable speed router? If you are running the original router, it spins at 15,000 rpm. At about 10ipm you may see chatter. Also put some masking tape to the back of the MDF for the rollers to bite into.
The last thing would be a small test to try. Take a full sheet of foam and set zero at one corner. Then make a hole there. Manually jog the machine to the diagonal corner. Then tell the machine to return to zero. And see how accurate it is returning to zero. If it's say, more then a 1/16 off on x or y, the stepper motors are missing steps. I can jog my machine within 12 inches of zero and have it return spot on with no issues. Jogged anything beyond that and the return accuracy decays on the Y axis only. Which tells me my stepper motor has issues.

 

I finally build my Phlatprinter.
I quickly measured backlash and it was .006" on X and .004" on Y axis. This was just quick measurment to get approximate value.

 

Kroko, I'm surprised that you have backlash on the y axis. Most people have no backlash on the y axis, me included.

Evil-Tunes, what kind of spindle speed did you use to cut it? I tried the stock spindle and it burns the material with the 1/8" bit. I have to use 0.730" or smaller bits for my cuts. I hope that once I have my outrunner up and running again I'll be able to cut with bigger bits.

dhc8guru, the problem was not the radii, the problem was that the strait line from the radii to the long line on the y axis was shorter on the left side than on the right side, even though they are the same length in SU. As I've said, I may have used a way to high cutting speed. I will try 10ipm and will report back. I have to cut a part tomorrow and we'll see. BTW, the parts in the picture were not cut from MDF, I cut them form 1/2" plywood using a single flute 0.730" bit. The reason I used this bit is that it is the only one I could find that has a cutting depth of more than 1/2" and is still just over 1/16". I need my cuts to be made with a thin bit, if possible. I have a three flute 1/8" bit but it's cutting depth is only 1/2" and that is cutting it to close, pun intended.

Second BTW, I use for all my wood cuts a piece of form as a carrier. I use spray glue to hold the wood to the foam. It works great. No need for tabs.

 

I see in your photo you have little notches in each circle. When it was cutting did you notice the little y axis bump it gave at the 12 'o'clock position on the circle? That is the latest mystery stumping a few of us.

 

That's pretty close to what I got when I changed my stepper settings to micro step. Before micro step I had .040 on the X and .020 on the Y. Which is strange because I would think the Y axis would have more backlash being the fact that it runs on a long belt that can stretch.
Tigerpilot
You will burn the material @15000 rpm running 10-30 ipm. Even with an 1/8 bit turning 15k, you need to be moving atleast 200 ipm.
I crank my pony router down to it's lowest setting 6000 rpm to run 10 ipm cutting light ply and laminates. Which doesn't burn. If your burning your material your also wearing your bit out prematurely.

 

I know all of the above. As I've said, I have the original router and flexshaft. I have to replace the bearing in my outrunner and than I'll have great speed control.

The notches that E-T has are only in the MDF and not in the foam. I think those are the bumps that comes where the bit is descending in the multipass. I've mentioned it a few days ago and Randy said that it happens in his shop on their expensive machine too. It has something to do with the bit loading on the down-cut or something like this.

 

When bit bites into material it is pulled into and this can cause notches. To prevent this you can use ramp moves which don't move bit directly down. Or in above circle code use helical path where Z moves down gradually whole time during cirles.

 

Kroko, how do you make it to cut a helical path? What is the command? We'll have to enter it manually since it is not in the SketchUCAM.

 

Standard code goes like this:
[pre]%
G20
G0 X0 Y0 Z0
G3 X0 Y0 I0 J1
G1 Z-0.1
G3 X0 Y0 I0 J1
G1 Z-0.2
G3 X0 Y0 I0 J1
G1 Z0
%
Same thing but with helixes goes like this:
%
G20
G0 X0 Y0 Z0
G3 X0 Y0 Z-0.1 I0 J1
G3 X0 Y0 Z-0.2 I0 J1
G3 X0 Y0 I0 J1
G1 Z0
%[/pre]

 

Today I cut some circles.

Without setting backlash circles were not correct. Then I measured backlash again with more precision. X=0.35mm (0.0138"), Y=0.08mm (0.0031"). After setting these backlash values circles looked perfect.

I still need to calibrate and finetune machine but for now everything seems to be working fine.