• Scam Alert. Members are reminded to NOT send money to buy anything. Don't buy things remote and have it shipped - go get it yourself, pay in person, and take your equipment with you. Scammers have burned people on this forum. Urgency, secrecy, excuses, selling for friend, newish members, FUD, are RED FLAGS. A video conference call is not adequate assurance. Face to face interactions are required. Please report suspicions to the forum admins. Stay Safe - anyone can get scammed.

CNC Router alignment

Oh that's interesting. I have been cautious about adjusting motor parameters, since they were set by someone who obviously knows more than me, and frankly the CNC works already.
The mismatched master/slave accel's I found the other day has made me question that assumption.
Can you think of any down-sides if acceleration or speed are reduced too far?

(Aside from rapid free moves taking longer, sigh)
 
Is it possible that one of the set screws on a drive motor is a *little* loose, causing the shaft to just barley rotate before the gear "catches" the shaft

You could also forget about runing your slave on a seperate channel, daisy chain the step/dir pins between your two drivers, they would be getting the same signal, it would eliminate any software/configuration problems. That could help you narrow it down to a software vs a hardware problem
 
SparWeb said:
Oh that's interesting. I have been cautious about adjusting motor parameters, since they were set by someone who obviously knows more than me, and frankly the CNC works already.
The mismatched master/slave accel's I found the other day has made me question that assumption.
Can you think of any down-sides if acceleration or speed are reduced too far?

(Aside from rapid free moves taking longer, sigh)
Click to expand...
The only down side is that on wood projects if the max speed is too low you can't hit the optimal feed rates. But that's really only a concern on big machines. I have my machine set to 10,000mm/min max speed. But it took a lot of tuning to get that high.
What are the max speed and max accel set at now?
 
I suggest a big drop in acceleration and speed to start to see if that is the problem, if it is then keep increasing and re-testing testing. Slippage in the drive mechanism - that's another good thing to look for. That bit me too. set screws like ryan said. gears slipping, belts slipping...
 
So many suggestions!

Work holding.... is it solid?

And finally simplify your testing. Carve a straight line from one end of the bed to the other, move over 1", then carve back to the start. A flat end U shape. Measure that. It should start and stop in exactly the same place and length. Do the same for the other axis. Let us know!
 
When in doubt, see what the experts say. This is a good time to consult the big-name brand CNC builders because they publish a lot of good info about troubleshooting and maintenance.

Here's a valuable hint from the HAAS website:
IMPORTANT: If your application involves moving a single axis repeatedly back and forth over a small area of the ballscrew, the ballnut will heat up the ballscrew and cause thermal expansion. It will also not lubricate correctly because of the short stroke. Every few minutes, it is necessary to move 80% to 90% of the axis travel in order to cycle the grease throughout the ballnut. This is common on smaller machines with a smaller work envelope.
Click to expand...
Um, yeah, that's exactly what my machine's been doing for weeks. Yesterday was probably the first full-stroke of the X and Y axes since I bought it.

There are several procedures on their webpage that I'm going to try out.
"https://www.haascnc.com/service/tro...shooting/Ballscrew_Troubleshooting_Guide.html"

So hang on guys, I'll get to it all... I'll get to it...
gimme time
:)
 
Today and yesterday I had some time to work on the CNC. The main improvements are three-fold:
- relubrication of the X-axis linear guides
- cleaning the ways for the linear guides and the lead screw
- pumping fresh grease through the X-axis ball-nut

Each of these tasks weren't quite so simple because, for example, the grease nipples were too small and fell out as I used them! WTF. I replaced them with the correct SAE size and continued on.
I should have cleaned the ways before relubricating because fresh grease was mixing with old gunk. So I cleaned the ways again, more thoroughly, and then used the grease gun a few more times.

One surprise: The roller chain holding the X-axis cable bundle proved to be too short and came up tight a couple of inches before the end of the travel. Like I said, I have used this machine only for small parts so far. Running the X-axis across the whole width as I did the other day, I didn't realize I'd bent a bracket on the back! So I spent a few hours adding new links to the rollerchain to make it longer, shifting cables to get more slack, and relocating the end-stop limit switch. I now have 50" to work with!

With the ball-nut released from the carriage, I slid the carriage across the gantry and at first felt lots of little bumps and grabs along the way. At the end of all this work, it was very satisfying to pull the carriage across and feel nothing but smooth motion. Ahhhhh.

One possible concern: The ball-nut has a bit of play sideways. This might not be an issue (maybe normal for all I know) since the ball-nut only needs to be rigid in the longitudinal direction. I set up the dial indicator and found a fair bit of play side to side, though not any more than the lead-screw will move when pushed by hand. I can't measure any free play longitudinally on the ball-nut pushing by hand so I'll be satisfied with that, for now.
 
I ran some more trials today and yesterday, but I haven't seen much change in the results.
All point-to-point operations are 1:1 or near enough that I could leave them as they are.
The circular arcs continue to be egg-shaped, however.

I have changed the size of the circles, partly because it was good advice to see if this mattered, and partly because the big circles were wasting more material.
I did one test piece with the straight 1/4" cutter and added some finishing passes, cutting only 0.015" engagement of the cutter and 0.050" depth of cut, and its egg-shape was nearly identical, though +45 degrees, not -45 degrees.
I did another test piece with the v-groove cutter and made several circular passes. One of them was generated by V-Carve as a carving pass, which produces G01 commands in line-segments, and the other one I manually set up to use the same v-groove cutter to cut G03 arcs. Both of these also suffer from the egg-shaped lobes, although I should also say that I accidentally ran the v-groove cutter too fast through the aluminum and the cut surfaces were terrible. Despite this, the lobes are unmistakable when measuring carefully.

The test pieces were secured in various ways during these tests. Sometimes held down with screws directly to the spoilboard bed, other times wedged in against the fence boards on the X- and Y- table edges. This didn't seem to matter.

Here is an example of the "egg-shape" that I'm talking about. It's a plot of the error from nominal size. This particular circle is typical of the others. Though the absolute magnitude of the error is different at times, the relative error (greatest deviation too big MINUS greatest deviation too small) is always in a range of 0.010" to 0.015". It happens to be 0.013" in the example below.

Imagine turning a bushing on the lathe that is 0.013" out-of round, and then trying to push it into a circular hole. Obviously, a CNC router is definitely not a lathe, so I can't expect it to be as accurate as a lathe.
But is this all I can reasonably expect?

Squareness_Check.webp
 
SparWeb said:
Something doesn't look right on the X-Axis bearing mount. I'll be examining that carefully soon.
Thanks for the other good ideas - I'll try some other circle sizes to see if the error scales up or not.
Profiling in a circle is turning out to be more useful as a diagnostic than I thought.

To answer the other questions: Yes all of the steppers are the same NEMA style.
I've been using just one feed rate so far - trying a different rate also sounds like it will reveal more information. I haven't set up any finishing passes.
For a little while I will be reluctant to change the cutting program because that would make it hard to compare "before and after".
But I agree that some of the irregularities could be natural results of these roughing passes, and not due to misalignment or problems in the NC machine itself.

I haven't mentioned it yet, but I also realized that this 1/4" cutter is actually cutting like its diameter is 0.255" or more. But when I measure the cutter's blades I get 0.249" So why would a nominal 5/16" slot be 0.325" wide?
I'm not sure if that mystery is related to the suspected backlash. I'm going after the backlash issue first. If I discover what's causing the overcutting in the process, then all the better. Otherwise by fixing backlash I'll be in a better position to figure out why it's cutting over-size. For the record, Mach 3 is using the tool at nominal 0.250" diameter, and has no offsets or tool wear adjustments that I can find.
Click to expand...
Two things might cause the oversize. TIR, or deflection, vibration. Maybe measure the TIR for one, and then compensate the oversize by offsetting your toolpath and add 0.001 / side for benching if its critical
 
SparWeb said:
I ran some more trials today and yesterday, but I haven't seen much change in the results.
All point-to-point operations are 1:1 or near enough that I could leave them as they are.
The circular arcs continue to be egg-shaped, however.

I have changed the size of the circles, partly because it was good advice to see if this mattered, and partly because the big circles were wasting more material.
I did one test piece with the straight 1/4" cutter and added some finishing passes, cutting only 0.015" engagement of the cutter and 0.050" depth of cut, and its egg-shape was nearly identical, though +45 degrees, not -45 degrees.
I did another test piece with the v-groove cutter and made several circular passes. One of them was generated by V-Carve as a carving pass, which produces G01 commands in line-segments, and the other one I manually set up to use the same v-groove cutter to cut G03 arcs. Both of these also suffer from the egg-shaped lobes, although I should also say that I accidentally ran the v-groove cutter too fast through the aluminum and the cut surfaces were terrible. Despite this, the lobes are unmistakable when measuring carefully.

The test pieces were secured in various ways during these tests. Sometimes held down with screws directly to the spoilboard bed, other times wedged in against the fence boards on the X- and Y- table edges. This didn't seem to matter.

Here is an example of the "egg-shape" that I'm talking about. It's a plot of the error from nominal size. This particular circle is typical of the others. Though the absolute magnitude of the error is different at times, the relative error (greatest deviation too big MINUS greatest deviation too small) is always in a range of 0.010" to 0.015". It happens to be 0.013" in the example below.

Imagine turning a bushing on the lathe that is 0.013" out-of round, and then trying to push it into a circular hole. Obviously, a CNC router is definitely not a lathe, so I can't expect it to be as accurate as a lathe.
But is this all I can reasonably expect?

View attachment 42620
Click to expand...
No you can expect good accuracy within the the rigidity limits of the machine.
My router will hold .002 accuracy but I have done a lot of work to get it there.
Have you calibrated the axis?
 
I might be way off in left field, but the math to draw an ellipse (oval) defines an offset of centers & radiuses as compared to a circle. Circle is x2 + y2 = 1. Ellipse is x2/b2+y2/a2=1. When you have an ellipse, the relative centres of x and y are offset. For example, If the ellipse is offset in the x plane the ellipse will be lower in x than the width of y. What direction is the ovality? If it's offset in both planes your oval will be at 45* offset.

Is the frame twisting when one axis moves?

CNX_Precalc_Figure_10_01_0032.jpg
 
Alrighty now....lets start with the x&y axis.

You have play in your system a whole lot of it, more in one axis than another. To make this easier to understand I'm going to use this as your leadscrew rates. 1 full rev is 0.100 inches, so 0.025 is basically 1/4 of a turn before movement engages. So simple test is to power everything down (so you can move the screws with your fingers), grasp the nut with one hand and rotate the screw with the other, note roughly how much you can turn before you feel movement in the this arrangement. Repeat for the second access. You found your play.....

Now elimination, keep repeating until you id the points of play, thrust bearings, nut, linkage between stepper/servo. Correct accordingly.

Z depend on type of set up, my guess is rack and pinion (larger error because of cutter down pull), same tests and fixes except you add more uplift tension to counter act play within reason (rack and pinion play is brutal to eliminate).

Hopefully this simple info gets you started in the right direction.

One final note, depending on you setup, do not do this powered up, at best you damage you system, at worst you damage yourself.
 
Are you cutting them in the same position? I’m wondering if they would change in measurement further along the x .
 
Thanks everyone. These are all interesting suggestions.
Right now it's frigidly cold and I can't heat up my shop enough to feel comfortable running the router. It's well below freezing and it's probably going to stay this way for a while.
Sorry, it means I have to put this on hold until things warm up enough.
 
You must log in or register to reply here.
Back
Top