Deviation when milling a circular pocket.

[zvika-g]

Hi,

I have a replica of IH mill that I converted to CNC.
I have a very strange problem. When I'm trying to make a circular pocket, it always made a little bit narrower then the plan. In my attempts, I was rying to make a pocket of 19.05mm (3/4"). The pockets final diameter are 18.6-18.7mm. I'm testing it with a digital caliper that seems to work well. When I mesure the endmill diameter I can see that it is exactly 10mm. The G-code was generated by MasterCam and it looks good, i.e. when calculating the diameter of the G2 command the diameter result is correct.
I have a DRO installed on my mill and while making the pocket, I can see thatthe table moves to the right position (when the X,Y axes reaches the pocket edges), but still, the result is smaller pocket.

I'm at a loss and desperate. Do you have any idea?

Thanks in advance,
Zvika

[Matt McColley]

no expert here but I have a couple ideas for you....

1.) have you check the hole sizes with a bore guage?

every caliper I've ever seen has a slightly flate section on the measuring edges (i.e. they're not sharpened to a knife edge, but have a small flat) ..... which will introduce some error and an ever so slight undersized reading.

2.) how do linear machined features measure on the mill? spot on? or a hair light?

Maybe your calibration is ever so slightly off.

3.) Any back-lash on your screws/nuts.... that would also introduce some error

Sounds like you have a great set up... should be able to get it figured out.

[TOTALLYRC]

Backlash in the system normally results in the circular feature being out of round at the compas points. Using a good dial indicator, I would verify that the dro and the computer are actually calibrated correctly. If you have set them up based on the mathimatical values of the steps per rev and the tpi of the screw or their metric equivilents, you can sometimes come up short or have the wrong values. My machine should have bben 20k steps per inch based on what I thought I had, but I needed 21937 or some such thing to make Mach3 give me good readings on the dial indicator. I can now command a .001" move and it will match the indicator for full 1" travel of the indicator.

Small variations can be caused by using a caliper instead of a micrometer to measure the end mill, machine flex or endmill flex. When talking about .01mm (.001") or less, making adjustments is part of being a machinist. Learn how to apply tool offsets in the cnc control to compensate for tool wear or part out of tolerences when machining.

Mike

[Superman]

Before you pull things apart, to find the problem.
Does it happen at a low feedrate ( 50mm/min ) as well ?

Try this first in Mastercam, break the circle into 2 ( at 0 and 180 degrees), so that the NC-code has a different target instead of doing a full circle. use "ramp" ,by depth of 2mm,

If this improves the sizes across the quadrants, then your machine has past it's feedrate limit to control the tool accurately ( machining full circles a no-go )

If problem is fixed, them your mastecam Machine Definition file, on how it handles arcs, needs to be modified to "break full circles at 180 degrees".

many older machines can travel fast in a straight line, but fail miserably when they hit the bend ( change direction )

A good analogy,
while walking, you can turn sharp when going around a corner,
now do it while running flatout ( that sharp turn is not so sharp now ), but put a waypoint that the tool should pass through would help

[zvika-g]

First of all, Matt, Mike and Superman, thank you very much.
your willing to help and your very smart advices is admirable.
Unfortunately, I already went through most of your suggestions.

I think that my measurements are correct (I verified it). In addition, I don't think that it is a backlash issue since the backlash is cancelled by software and it seems to work well. Further more, I think that the step/movement ratio is also correct since when I move the table for a large distance, the DRE readouts are matched.

As I wrote, I couldn't find any logical explenation for this strange problem.
I've continued investigating it and I may have found the problem (actually, by accident). At a very specific point (of the X axis), When the table crosses this point, the DRO readouts jumps 0.1mm. This is another strange problem that I can't explain yet. It can be a DRO problem but it can also be a problem with the screw. I'll try to verify it with a dial indicator.
This new finding can't fully explain the original problem since the pockets diameter is fixed and it is not an ellipse.

I'll keep you posted.
Thanks again,
Zvika

[pete from TN]

I am also converting a RF style milling machine to cnc control. Do you have a build thread here on the zone? I would love to see some pictures of your setup and your machine running. I am not experienced enough yet to help with your problem but it sounds like you might have found the problem there. Did you go with a stepper based or servo based system? It also sounds like you are trying to get some feedback thru the use of dro linear encoders, is this correct? I am interested in hearing what your software and hardware setup is on this... Thanks and good luck...peace

[Hirudin]

If possible wouldn't it be better to cut a circular profile rather than a pocket? The profile would be easier to measure accurately.

[Superman]

What about getting rid of the circle , and program a 30mm square with 10mm corner fillets ?
and measure each direction with gauge blocks ( eliminate the measuring on an arc ).

This would check that each axis is correctly moving to scale, backlash etc.

Machining a cicle, the machine will have zero readout movement on the quadrant points for a minute segment to allow for change of direction

As for the jump, could you have too much backlash ?

[Robin Hewitt]

Could just be the tool bending. You might mod the G code so it takes a second identical go at the finishing pass, see if it removes any more metal

Robin

[BobWarfield]

Zvika, these things are always a bit of detective work, but we learn something interesting each time.

Circles are absolutely the hardest "torture test" for these machines.

Some things I have wrestled with:

- If you have servos (not steppers), tuning will affect your accuracy, at least on my system. I found that surprising given it is closed loop, but it was the case. BTW, the error corrected by retuning was less than the amount that would cause a fault, so maybe it isn't so surprising. Nevertheless, it was important!

- If you have servos or steppers, noise either on the step line or the for servos also on the encoder lines, can lead to errors. Your 0.1mm jump is really suspicious. Almost wonder if there is a loose connection that is bumped at that spot? Noise, unfortunately, is very tedious to identify and eliminate from your system. It is often unpredictable. For example, you may be measuring you machine accurately moving with the spindle off, but never realize when you turn the spindle on that there is all kinds of noise making the cut inaccurate.

- You are using backlash compensation. Lots of folks have found the Shuttle tuning parameter in Mach really matters a lot, particularly if you use compensation. Unfortunately, I can't advise you on how to adjust it unless you have a servo system. For servos, the recommendation is to set it as low as possible. Some research on the Mach3 support board (Yahoo) will tell you what to do for steppers.

- Any error you fix, will require you to recalibrate you steps/unit. Don't forget to at least check that!

- The size of your endmill is a touchy thing. You can measure it with a micrometer. I would not trust a caliper. Even the micrometer is not the best. My suggestion is to take a scrap of material. Use a micrometer to measure it's length. Cut it in half with your endmill. Now measure the lengths of the two pieces with the mic. The difference is your endmill's cutting width. Having done the experiment of calipers, mic'd the endmill, and then used this method, I got the best accuracy with this method.

- The state of tram of you machine will affect its accuracy. If the cutter is not presented to the cut exactly square, it changes the effective diameter of the endmill slightly.

- The state of adjustment of your machine's gibbs matters greatly. Also the lubrication of the ways.

There are probably many other things to check, but that is a start to think about. I will watch to see what the cure is and add it to my own list to test on my own machine!

Cheers,

BW

[sansbury]

- The size of your endmill is a touchy thing. You can measure it with a micrometer. I would not trust a caliper. Even the micrometer is not the best. My suggestion is to take a scrap of material. Use a micrometer to measure it's length. Cut it in half with your endmill. Now measure the lengths of the two pieces with the mic. The difference is your endmill's cutting width. Having done the experiment of calipers, mic'd the endmill, and then used this method, I got the best accuracy with this method.

Bob, this approach would also capture runout in the spindle/toolholder, which is sort of the point, right?

Another thing to watch is how your CAM package generates code for arcs. One catch that will make you pull your hair out is the different ways that I/J words are interpreted. Likewise, I get more accurate circular pockets from BobCad's G-code than I do when using the Mach 2 wizard. The wizard generates a continuous helical cut with a small finish pass, while BobCad generates a series of circles (like the rings in trees). I haven't bothered to figure out exactly what the difference is, but one gives me much better results than the other.

[BobWarfield]

Bob, this approach would also capture runout in the spindle/toolholder, which is sort of the point, right?

Another thing to watch is how your CAM package generates code for arcs. One catch that will make you pull your hair out is the different ways that I/J words are interpreted. Likewise, I get more accurate circular pockets from BobCad's G-code than I do when using the Mach 2 wizard. The wizard generates a continuous helical cut with a small finish pass, while BobCad generates a series of circles (like the rings in trees). I haven't bothered to figure out exactly what the difference is, but one gives me much better results than the other.

It captures runout, errors due to tram, and basically just creates a situation where the cutter diameter is measured according to a real cut.

RE CAM, there are some touchy issues. Most of the I,J stuff should be handled by your post, but there are subtleties. Make sure you have a good post. If you have any doubt about the CAM, NCPlot is a really nice g-code editor and simulator that makes it easy to step through and see what the CAM's g-code is really doing.

And yes, the wizards do a lot of things that are not very slick compared to really good hand code or CAM code.