[Smooth90]

I am running a very basic setup with my fireball v90 but a slight problem has hit me and I'm entirely convinced that it is because of emc.

I have a powerful stepper setup with a 40v power supply. The machine also has anti backlash nuts.

My problem is that my machine is consistently cutting things to smaller dimensions than they should be.

Here is my G code

( Made using CamBam - http://www.cambam.co.uk ) (

That code SHOULD* make a 1x1 square with two holding tabs, and .52 inches deep (two .26in passes). However no matter how many times I look at the g code and verify it the machine never cuts it correctly. I have made about 10 (1x1 squares) and every single one of them measures .975 x .990 inches. No matter what I do I cannot get 1.000 x 1.000 which is what I want and the code says.

The machine is practically brand new (2 months) and has had very little work through it. Although I have had a few nasty collisions with the bit/step blocks. The bit snapped every time and didn't hurt the machine. Other than that it is new. I looked into backlash being the problem but these cuts are too consistent and too large for that to be the case (plus I have anti backlash nuts).

Meshcam seems to do better than Cambam and gets closer to the dimensions think 1.000 x 1.010. The only reason for this is that meshcam is for 3d and does lots of little moves to accomplish the same square rather than long stretches like cambam does (faster) (2.5d). Meshcam takes 3 - 4 times longer to cut the square than cambam does.

This makes me think that emc is having an error somewhere inside it where it is not timing something correctly resulting in bad dimensions.


So what could be wrong with emc that is causing it to do this??

ANY help would be greatly appreciated I am in a bind here and have no idea what to do/try!!!

[wendtmk]

Incorrect tool offset? Incorrect tool diameter? Are you sure the scale for each axis in your ini file is set correctly? Could be a number of things.

Mark

[lerman]

Who configured EMC for you?
Did the system ever work?
If yes, when happened immediately before it stopped working.

Some possibilities:
1 -- If it never worked, look at the timing of the signals to the stepper. (That's why the who configured question is important.)

2 -- Check that the "anti-backlash" nuts aren't too tight. That could cause the stepper to miss steps.

3 -- Try decreasing the feed by a large amount. A factor of five or ten would make for a good test. If it works then, it is probably a mechanical problem.

Talk to the people on the emc-users irc channel.

Ken

[Smooth90]

1. I used the step config menu and followed the instructions they had on their website.

FireBall V90 EMC2 Step Conf

My latency test comes out to around 10,000 - 12,000 ns at the absolute max.

I am going to go play around with the step time and space settings to see if they have any effect on the issue.

If did in fact work a little while ago I have a video on youtube that proves it.

[nomedia="http://www.youtube.com/watch?v=2lb1T2k6d5M"]YouTube - Fireball CNC V90 Lexan Milling[/nomedia]

The coins fit perfectly and the square measured exactly 3.000 x 3.000 inches when it was complete.

2. I will remove the lead screws on the x/y axis and completely reassemble the anti backlash nuts. Clean them out to as I think that some mdf dust may have gotten in them.

3. Once I have finished the above I will try to heavily reduce the feedrate and see where that gets me.

Thanks for the reply's!

Will post back in a few hours with results.

[MrWild]

If you have two different dimensions for a square pocket, chances are you have developed lash. If EMC worked, there is no way that I know of that it would start causing problems. About the only place EMC might give a hiccup of this nature is if the steps per inch were changed some how in the step config file. Open your config file and see.

[Smooth90]

So I just finished tearing down the X, Y, and Z axis. Everything was cleaned, inspected, and reassembled. The backlash nuts look fine. I compared the X axis nut to the Y axis nut and couldn't tell the difference. They were dirty and had mdf dust inside them as I had thought and now they are clean. The only real problem/issue I noticed was that the x axis nut block underneath the machine was a bit loose. I fixed that and its perfect now.

The machine runs great on all axis's now and has very smooth motion.

Once I connected it all up I ran another 1x1 block test with some .35in thick LDPE plastic. I chose to use slow feed rates this time.

The first test I did was at 25 ipm.

The block came out to be.

X axis - > .994 in

Y axis - > .990 in

Then I cut a second block at an even lower feedrate 10ipm.

X axis - > .994 in

Y axis - > .995 in

After cleaning out everything it seems to be working better but remember I also heavily reduced the feedrate. I don't think it is lash at this point because lash that is .005 - .010 inches is pretty bad especially at such low speeds. On top of that its practically a new machine, with anti backlash nuts again very unlikely that I've developed such bad lash.


There is also more evidence that I've thought of which disproves it being a hardware malfunction. The machine obviously cut the piece in the video perfectly....now it can't do that.....why???? Well the only thing that happened which was stressing to the hardware between now and then was a bit snapping off. This bit snapped while it was being pushed by the X AXIS. So if that movement/snap damaged anything it would be the X axis and the Y axis would have been completely left alone. However we not only see incorrect dimensions on both axis but there is greater slop on the Y axis the axis that was not subjected to high stresses.


At this point I am thinking that the settings from probotix need to be tweaked or that my computer is the issue. I am running on a laptop and have read that power saving features can interfere with emc trying to use the parallel port.

Two more things to try

Tweak the settings

EMC on a desktop


Will post back soon when I have tried these things.

[ninefinger]

Did you check the couplers for the screws to the stepper? If a set screw is a bit loose on a flat it can present itself as backlash. Ask me how I know.

Mike

[MrWild]

You got rid of .015 and .020 in lash. If it had been the fault of EMC there would have been NO change from your efforts. What you have here is a "Carburetor problem." What's that? Well, a carb problem is where you don't know how one works so any problem a motor has, you are sure has to be in that blasted carburetor. I know this sounds like a simplistic answer, but after seeing it time and again (the mind set) I can only make one suggestion to you. Buy yourself a copy of Mach. You aren't going to be happy until you do, and will just keep blaming EMC. Heck even after Mach forces you to tune the last of the lash out of your system you will still tell folks how EMC let you down.

Once you have Mach installed, try running your square pocket in the other direction. I predict interesting results. Don't bother trying this with EMC as the results you get, will cement your conviction it is a EMC problem for sure. What to expect with Mach running in the opposite direction is a larger pocket. Say 1.015 x 1.020.

Don't assume a crash in just one direction only screws up your machine in a single axis. It sounds like the Z has a problem as the lash seems to be equal for X and Y. It sounds like the Z axis slide has gotten loose, the acme nuts or thrust bearings are loose, or the spindle has gotten loose. By using the lash compensation in Mach you will be able to dial all of your problems away and then can trash EMC for all that listen. Of course I'd tighten up all slides/screws and check the spindle for looseness before I blamed EMC, but the lash compensation in Mach will let you not worry about machine looseness.

It's time to buy a new carburetor for your motor because until you do, you won't look for the real problem elsewhere.

[Smooth90]

I had never made flats on the motors so I went ahead and did that today then set the screws on the flats. Right now they are perfect well connected and secured no way there is any movement.

So I did another 2 tests after this and found that at 10ipm I got very close to perfect. It was .996 x .998.

I am probably just going to switch to mach 3 now (trial version) and see how it runs. If I can compensate for the lash and get down to +- .001 inches it will be fine.

Thanks for the input!

Will post back after I've tried mach 3.

[ninefinger]

The only real problem/issue I noticed was that the x axis nut block underneath the machine was a bit loose. I fixed that and its perfect now.

I don't think it is lash at this point because lash that is .005 - .010 inches is pretty bad especially at such low speeds. On top of that its practically a new machine, with anti backlash nuts again very unlikely that I've developed such bad lash.

There is also more evidence that I've thought of which disproves it being a hardware malfunction. The machine obviously cut the piece in the video perfectly....now it can't do that.....why????

You found one mechanical problem and it solved a bunch of your missing travel (ie not software), .005 to 0.010 lash is not that much for a machine with acme screws and anti-backlash nuts to develop. The machine hasn't been static since that video - it wasn't you making the video was it? If not then I'm guessing the machine was purchased and shipped from one place to another.

Sounds like you need to do a bunch more investigating of the mechanical aspects of the machine before chasing software gremlins.

Start by measuring backlash - not a cut. As Mr Wild pointed out a cut can have other variables at play that can affect the cut ( sloppy z axis travel, undersize cutter, loose spindle bearings...) Use an indicator to measure the backlash.
Other sources of "backlash" - the bearings supporting the screw - can the screw move back and forth at all?
Being a stepper machine it can loose steps too. That is why there are recommendations to slow it way down. IF its loosing steps going slower will usually help. If its loosing steps then you need to look for why - is there binding in the travel? Are the nuts too tight? Are the slides clean? etc.

[Smooth90]

I went and ordered a pci card adapter so that I can use one of my beefier computers with mach 3.

I also ordered a dial test indicator w/stand that is accurate to .0005" this way I can test to see if runout is the problem whether it is in the collet, collet nut, bit, or spindle bearing I will find it.

If runout is not the the issue then I will have mach 3 to compensate for backlash and if that works then backlash would have been the problem from the beginning.

Now I just have to wait to get the stuff but the problem should be resolved.

[MrWild]

Well, no... The problem itself will be masked, but not resolved. Still, if it makes you parts that pass inspection at the end of the day, then that's good enough. Be careful about lash compensation in Mach. You can use it to such an extent the entire machine becomes sloppy. The indicator is a tool you should have already. It'd have pinpointed the problems without the need of a Mach Motion purchase.

[chester88]

EMC does simple backlash compensation and sophisticated mapped compensation (which requires homing to a accurate consistent point).
little bit about it here: Basic Configuration[AXIS]-section

Chris M

[rvt]

If you need to test a cut, then it's best to create a square (or other shape you can measure) by hand coding the G-CODE instead of letting a CAM tool create it.
This way you also know what's in the file and know how it's going to work.

[jmelson]

I have made about 10 (1x1 squares) and every single one of them measures .975 x .990 inches. No matter what I do I cannot get 1.000 x 1.000 which is what I want and the code says.

Are you absolutely sure you know what the pitch of the leadscrews are? Are you sure you have correctly entered the right values in the .ini file?

Meshcam seems to do better than Cambam and gets closer to the dimensions think 1.000 x 1.010.

Well, this is very suspicious! Why should EMC be the culprit when two different CAM programs produce different results?

Do you have any measuring tools there? Dial indicator, caliper, etc.? First, you should use them to check that the commanded moves produce the right movement distance. You can then do repeatability tests. Move to coord. zero, and set up the dial indicator to read zero. Then, move away slowly and back, and see if you get back to the zero dial reading. then, move faster and faster, and see if at some point it doesn't return to the same point. That would indicate the steppers are losing steps.

Jon

[sansbury]

I have used both EMC and Mach, so I don't have a dog in this fight. I agree with the other posters that you need to isolate the mechanical part of the problem. Test cuts introduce too many other variables to diagnose your issue.

Here is how I have done it with similar machines. I'm assuming a dial indicator with at least .500" of travel, but you could do the same with a .015-0-.015 indicator, just adjust the distances accordingly:

1. Mount a dial indicator on the table with the plunger against some flat, stable part of the spindle assembly or router mount.

2. Jog the spindle in towards the dial indicator by .100" or so to absolutely positively take up any backlash. Zero the indicator or note the reading to use as a zero point.

3. Using the MDI, jog another .100" in the same direction at a feed rate of 5IPM or so. The indicator should show .100" of movement since there should be no backlash. If there is any difference, write it down. This could be due to a number of things, we'll get back to it later.

4. Then, jog the machine .100" in the opposite direction. With no backlash, it would return to the zero point set in step 2. Most likely, it will stop short of the zero point by some amount. Note the amount.

5. Zero the dial indicator or note the position and jog another .100" in the same direction. If it is off, note how much.

6. Jog back to the zero point. Again, it will likely stop short, so note the difference.

7. If you want, repeat the whole process once or twice to confirm your readings. You could also move to a different part of the machine if you want, since you're only testing a small part of the overall travel.

This test looks at two different things: backlash and screw pitch deviation. With no backlash, in steps 3 and 5 you should get exactly the movement commanded by the PC. If you get a small amount more or less than .100" in both steps 3 and 5, it would suggest you have the steps-per-inch setting incorrect, or a pitch deviation in the screw. If the errors are different (by more than .001" or so) then you may have a local deviation in the screw pitch. I would test at multiple spots along the travel of the axis to see what I found.

Second, look at the travel errors noted in steps 4 and 6. They should be within .001" or so of each other. That is your mechanical backlash.

If you want to be absolutely, positively sure it is mechanical, another way to test this is to set up the indicator as I described, and turn the stepper by hand with the power off. The best way to do this is with a handwheel mounted on the back of the stepper. Put some masking tape on the motor and the handwheel and draw a line across it to use as an alignment mark. You can either do the test by turning the motor one full revolution (if your indicator has enough travel), or count the steps, which you can feel as little "clicks" as you turn it, even with the power off. Practice turning it one click at a time, then test moving it 10 or 20 steps forward and back. Repeat a couple times to make sure you're counting accurately as the detent torque is pretty light on smaller steppers like yours.

If you do this and the errors come out the same as when you do the tests with the power on, then it would prove without any doubt that they are mechanical. I may have made it sound complex but it shouldn't take you more than 15-20 minutes.

Having built 5 machines with Mach 2, Mach 3, and EMC, what I have found is that software malfunctions cause large and variable errors, while mechanical or configuration problems cause small(er) and consistent errors. I've used a variety of steppers and drivers, and have never had small step losses or that kind of thing--either the machine drove through or stalled and howled badly. Long story short, everything you've said smells to me like mechanical, not software issues.

[Smooth90]

I got my dial indicator yesterday and did a few tests on my spindle.

First I measured the runout inside the hollow spindle of the router.

It came out to be a bit greater than .0005". This is pretty good for the router
and means that the bearings in the router shouldn't be the problem..

Then I put on the precisebits 1/8in collet/collet nut with a 1/8in blank in it.
I measured the runout near the bottom of the blank.

It came out to be around .0025 - .0030" which is pretty bad.

I then put in the 1/4in precisebits collet and tested that. The only 1/4in
tooling I had was a 1/4in drill bit but it did have a flat surface at the top.

Once again the runout came out to be around .0025 - .0030" same as the 1/8in
collet.

Thinking that maybe the stock collet was better I put that on with a 1/4in drill
bit and tested that.

It was the worst out of everything measuring in at more than .005".

______________________________________________

Essentially my tests showed that when I am cutting with my normal bit my runout
is .0025 - .0030" which is pretty bad.
______________________________________________


At this point I think runout could be a legitimate problem and possibly
compounded by very minor lash.

I'm not sure how to see lash because the indicator only has a travel of .03" so
any move has to be very minor. I tested it will .0005" moves and as far as I
could tell it was spot on.


__________________________________________________ __________

I'm going to go pick up another router now and test the runout on it if that
fixes the problem then it was the router (although my test showed it was fine).
If it doesn't then I will have to go order a new collet/collet nut from precise
bits. I have to order bits from them anyway........................

[sansbury]

A .030" indicator should work fine, just do .010" moves instead of .100" ones.

The runout on the tool isn't going to help you but if it was the only thing going on, your test squares would be square, not rectangular. Runout is a constant error and will have the same effect on both X and Y.

My other thought is that if your test cuts were done with a .125" tool, then tool flex could be an issue unless you took at least one spring pass with it. I would stick to the .250" bit as that won't flex much if you're cutting anything softer than aluminum. All of which is why measuring with the indicator is better for tuning purposes....

[Smooth90]

I was able to get some 99% perfect cuts by looking into emc backlash compensation.

I set the X axis to have .014" backlash compensation and the Y axis to have .011" of compensation after tinkering with it for a while. Then I did a test cut at 24ipm and 56in max acceleration. The square came out to be 1.000 x 1.000 which is perfect for my applications.

The 1% error comes from a slight bevel between the first/second passes on one side. I think I need to either tune the backlash compensation some more on that axis or add holding tabs on that side.

I didn't know emc could do backlash compensation so I don't need mach 3 now...........neither will my wallet be out $175. Not that I am against mach 3 its just that if there is a free linux based alternative why dump cash on it?


I will buy some 1/4in bits next time, the reason I like 1/8in bits is because I can cut smaller features.

[Smooth90]

I replaced the anti backlash nuts a week ago and the problem persisted. This ruled out backlash. Finally I called probotix and talked to someone about the issue. We went through my setup and almost immediately he pointed an issue with my cutting.

I was using a .125in endmill to take .26in passes through mdf. He told me the rule of thumb is to take passes less than or equal to your bit diameter. So I simply changed the pass depth to .075in and tried that. To my surprise the square I cut came out to .998 x .998.

Once I saw this I knew that the remaining .002in was a constant error (runout) so I called precisebits. I talked to Ron Reed and he told me that the bit snapping off could have damaged one of the leafs on the collet. So I ordered a new 1/8in pg collet and collet nut (just to be sure) along with some bits.

In the mean time I was able to get a replacement router (I thought my bearings may have been slightly damaged). The new router didn't changed anything it still had the .002in runout.

My new collet arrived today and I set it all up. It made the runout disappear and go below .001in.

Now I am cutting perfect squares......perfect parts....and for the first time I'm actually building something with it.


________________


This whole ordeal cost me two hundred dollars after all the stuff I bought but you know what now I've got a real slick setup and I know the machine inside out.

Now I have a computer controlled spindle (on/off), mushroom e stop switch, dustbox, lighting system. Check it out....not a bad little home cnc setup



By robofreak at 2011-02-21