What's new
What's new

Fadal tolerance and roundness issues

sortafast

Aluminum
Joined
Jul 22, 2011
Location
hillsboro OR
So I got a 2002 4020HT With the MP control a month or so ago. It needed ball screw thrust bearings so I went all in and did all of the axes, replaced seals, disabled the cool power to the ball screws (and looped it all back together so the spindle is still connected), I replaced the coupler discs as well so that I wouldn't have to do that crap again later and set the backlash comp. I went through and tuned the axis drives per the doc on fadalcnc's site as the X axis servo was making some noise and I just wanted to make sure everything was fine there. Machine is level. Used my Starrett level that was spot on. So I ran some parts and they fell within the tolerances but they were fairly simple with strait lights and drilled holes etc. Measurements were consistent and most everything was with in a thou and seemed good to go. Now I am moving on to a part with some slightly more complex contours and such and now its getting weird. There are two 0.590" OD circles that it has to cut and those circles are coming out about 0.004" out of round and undersized. The best I can describe it is that at the spots exactly 45degree to the X and Y axis in all 4 quadrants of the circle it is larger in diameter then at the point of the axis it is smaller in Diameter. Slowed the feed down a bunch, didn't really help the out of roundness. Started at 140ipm, went all the way down to 25ipm and same thing. This is in 6061 with a 1/2 Destiny Viper. At the faster speeds it would make the part smaller in the areas that were rounded or contoured. With the first parts at the faster speeds it was like 0.010" to 0.015" undersized on the contour. Slowed the feed and it got better tolerance wise, but even at 25ipm it still undersized the round parts of the contour by about 0.003" on the diameter, but all of strait lines were spot on dimensionally. So its doing something when it transitions from axis to axis like it just can't process fast enough or something. I am not sure where else to look. Could it be a ball screw binding? I am checking the gibs and straps now, but they seem ok. Seems like the issue is in the electronics somewhere and its driving me nuts. Is there a parameter or setting that I am missing or need to check? Need to get this thing spot on so I can get on with some jobs.
 
Did you do the backlash using the factory program or using the jog handle? Did you tune the drives using all 3 axis running or just one? 140ipm using a 1/2 emill to get a .590 hole... ...
 
Did backlash using both the program and the jog wheel. Got the same results. Have checked and rechecked the BL just to be sure. Did the servo tuning with the program running all 3 axes at the same time. Tuned the gain to 1.470 then balanced it.

As for the .590, its an outside profile. Even slowing things waaaaay down it doesn't get any more round, maybe by a thou but thats it. Dimensionally it tightens up a little, but at a 140ipm rough with a 90ipm finish it's way undersizes the diameter by like 5-8thou. With the finish at 25ipm it still undersizes by 2thou on the contoured path while the strait line are right on the money. Like a steering wheel down my pants, its driving me nuts.
 
Not electronic. Backlash in the ballscrews. If you want a round hole, you bore it ...

Ovality between the 1st/3rd and 2nd/4th quadrant can absolutely be "electronic". In fact it almost certainly is, considering OP mentions tuning the drives, and mentions nothing of steps at the quadrants which is the first sign of lost motion.

If the velocity and balance is mismatched between the x and y axis this is the result.

Edit: just reread the OP. If the out of roundness is symmetric about x and y then what I wrote above is not the cause.

You said it cuts bigger at 45 degrees to the axis that it does along the axis. Which one is closer to the right size?
 
Sounds like servo miss match. Renishaw term for the axis can position accurately but when working together to make a circle or radius one of the axis is lagging behind or one is going too fast to their points.
I dont know how to adjust this on a Fadal but it sounds like what is going on.
 
Ovality between the 1st/3rd and 2nd/4th quadrant can absolutely be "electronic". In fact it almost certainly is, considering OP mentions tuning the drives, and mentions nothing of steps at the quadrants which is the first sign of lost motion.

If the velocity and balance is mismatched between the x and y axis this is the result.

Edit: just reread the OP. If the out of roundness is symmetric about x and y then what I wrote above is not the cause.

You said it cuts bigger at 45 degrees to the axis that it does along the axis. Which one is closer to the right size?

Based on the under cutting on the curved profile, I would say it closer to spec at the x and Y points not on the 45's. But I could be wrong. This whole thing makes my brain hurt and I need to stop and think about it and measure the parts for the eleventieth time. Also, one thing I forgot to mention is that on the +X side of the circle there is a flat facet that is noticeable, maybe 10 thou wide. The thing with it is that the OAL of the part is 0.002" short but the width on the flat sides in the y is right on the money. I will take a pic of the part as I think it will be easier to explain. But it either the Y is jumping the gun when it is transitioning to the X or something. I am thinking that the X and Y aren't very well sync'd up at this point. At least when they are doing continuous movements.
 
I'm learning what it's reasonable to expect of the 1998 4020HT/CNC88 new to my shop. Where can I get away with profiling, what has to be bored or reamed. Yes it makes 4 lobed holes. To the best of my gaging ability the radius deviation is about +/- .0002". That's finish passes at 20 to 40 ipm. Haven't had the occasion to check holes cut at higher feeds.

The manual section for the M90-91-92 axis gain settings suggests 50ipm is the limit for accurate circular interpolation with default settings, and mentions the axes can overshoot if gain is set higher than the drives can handle at a particular feed rate. Someone prior to you could have set parameters that cause what you're seeing.

I have a lot to learn about this mill and control and am barely scratching the surface. So far it has exceeded my expectation in every way.
 
I'm learning what it's reasonable to expect of the 1998 4020HT/CNC88 new to my shop. Where can I get away with profiling, what has to be bored or reamed. Yes it makes 4 lobed holes. To the best of my gaging ability the radius deviation is about +/- .0002". That's finish passes at 20 to 40 ipm. Haven't had the occasion to check holes cut at higher feeds.

The manual section for the M90-91-92 axis gain settings suggests 50ipm is the limit for accurate circular interpolation with default settings, and mentions the axes can overshoot if gain is set higher than the drives can handle at a particular feed rate. Someone prior to you could have set parameters that cause what you're seeing.

I have a lot to learn about this mill and control and am barely scratching the surface. So far it has exceeded my expectation in every way.
Gain as set in the control is all set to normal for all axes. But I am wondering if there is another parameter that could be causing this issue. Because if stuff was just out a thou, I would be cool with that. I will trade a little accuracy for some speed. But 5-8thou is not acceptable. I dig the control on these. Once you know where stuff is, they aren't bad. I do wish it was more menu/soft key based like other controls, but for what it is, it works and gets the job done. Plus this one has handled some of the HSM stuff that I have thrown at it pretty well. I just wish on the small stuff like this that it could be both fast and accurate.
 
What did each axis backlash out at?

Have you tried cutting a circle-square-diamond test coupon?

What are the axis velocity values when moving at 45 degrees (they should be within 10 points)?

You said the X axis made noise, even after replacing the thrust bearings, have you given the motor a good once over?

I'm not sure if 2002 is DC or AC, but either will suffer performance issues if the motors are worn out (bearings, brushes, resolver or encoder bearings)
 
Ovality between the 1st/3rd and 2nd/4th quadrant can absolutely be "electronic". In fact it almost certainly is, considering OP mentions tuning the drives, and mentions nothing of steps at the quadrants which is the first sign of lost motion.
I meant backlash of the entire system, sorry. Fadals are cheap, they don't have resolvers on the far end of the ballscrews nor do they have scales, so they are depending on feedback info from non-rigid mechanical connections. When mill-boring was a new thing, people only used it for non-critical features for this reason. My guess is, this twenty-year-old inexpensive design is not up to the task of contouring truly round holes. Too much following error, servos are not stiff enough, feedback is too disconnected from true position.

Should have been more clear, I meant that I doubt that the problem is that the control can't do the math ...
 
Backlash is probably set too high as it always is by static (hand wheel) methods. (an easy but terrible method of backlash comp).
Never seen this number be right. I start with 1/2 of what the handwheel/indicator says.
OP does not have a tally-round or equal so hard to know the profile but high settings make 12,3,6,9 look smaller if the entry is not but the axis grabs the value and shoots in which is how the comp works. Now you measure the "inward" spots.
Other is servo timing to each other, 45 is where both axis must be at high speed and lockedstepped in time both behind the command by the same number of sample periods.

Cut the comp lower, see what happens.
Bob
 
So I got a 2002 4020HT With the MP control a month or so ago. It needed ball screw thrust bearings so I went all in and did all of the axes, replaced seals, disabled the cool power to the ball screws (and looped it all back together so the spindle is still connected), I replaced the coupler discs as well so that I wouldn't have to do that crap again later and set the backlash comp. I went through and tuned the axis drives per the doc on fadalcnc's site as the X axis servo was making some noise and I just wanted to make sure everything was fine there. Machine is level. Used my Starrett level that was spot on. So I ran some parts and they fell within the tolerances but they were fairly simple with strait lights and drilled holes etc. Measurements were consistent and most everything was with in a thou and seemed good to go. Now I am moving on to a part with some slightly more complex contours and such and now its getting weird. There are two 0.590" OD circles that it has to cut and those circles are coming out about 0.004" out of round and undersized. The best I can describe it is that at the spots exactly 45degree to the X and Y axis in all 4 quadrants of the circle it is larger in diameter then at the point of the axis it is smaller in Diameter. Slowed the feed down a bunch, didn't really help the out of roundness. Started at 140ipm, went all the way down to 25ipm and same thing. This is in 6061 with a 1/2 Destiny Viper. At the faster speeds it would make the part smaller in the areas that were rounded or contoured. With the first parts at the faster speeds it was like 0.010" to 0.015" undersized on the contour. Slowed the feed and it got better tolerance wise, but even at 25ipm it still undersized the round parts of the contour by about 0.003" on the diameter, but all of strait lines were spot on dimensionally. So its doing something when it transitions from axis to axis like it just can't process fast enough or something. I am not sure where else to look. Could it be a ball screw binding? I am checking the gibs and straps now, but they seem ok. Seems like the issue is in the electronics somewhere and its driving me nuts. Is there a parameter or setting that I am missing or need to check? Need to get this thing spot on so I can get on with some jobs.
You can PM me if you want a great fadal techs number. (Or anyone else that wants his number).

Sent from my SM-N910V using Tapatalk
 
I am kind of scratching my head at this post..i understand the hole should be more round. but, are you like a fadal repair guy?
Man the stuff you did to that, i would have spent the money to have it tuned properly, by someone with the proper knowledge and equipment.
we have 5 fadals and it just is not a snap of the fingers to get the servo's tuned. and backlash set. even after all that if i want a round hole, i will bore it.
circle interpolation on a fadal is just good enough for a c'bore.
 
could be turcite worn or linear slides looseness problem.
.
i have seen old cnc roughers that remind me of 4 legged chair with one short leg often got a tilting problem of slides on reversing direction.
 
hey sortafast...try this....its a point to point machine...so with that in mind you do this....run program at 5.0 inches per minute (roughing)....then run program again this eliminates any backlash and or tolerancing and deflection...but run it at 3.0(finish pass)....now check roundness and size....and then run another boss at 3.5 inches per minute(rough)....and then same boss again at 1.2 inches per minute(finish pass)....all programs run twice and lower the values....the lower the feed the closer the part because its actually figuring out point to point and turning down feed makes the points smaller which is tolerancing and dimensioning tightening.....let me know how it does then.

PS...don't worry about time and speed just yet...that can be changed later
 
I agree with Johnny…Your interpolation speeds are way too fast! There are parameters that allow for the following and trailing and errors to get longer as feed rates go up. Plus the acceleration parameters extend as the speed increases too.

The reason for this is kind of obvious when you think about it because that’s a lot of mass to be throwing around and you wouldn’t want your servo’s and other mechanicals to tear themselves apart. A half inch EM trying to make a .590 circle is really ripping.

One other ‘long shot’ thought is… did you hand turn the ball screws after you replace the thrust bearings and just before closing the guards up to make sure the table moves smoothly in both axis? (With power off of course)

The reason I ask is I did see a problem like this once. The way lube lines were clogged. We believed what we were seeing was the ball screw shaft winding up a little during direction change because of the constant load caused by the way friction. This was a solid way machine though and I did not note what yours is.
 
Did some more playing around with it and more thorough inspection of the parts. It seems that it is putting flat spots on the OD circle directly in line with the x and y axes at all 4 sides. I ran parts at 75ipm and 45ipm with nearly no difference other than at the faster speed it was smaller in OD overall. I set the backlash comp to 0 on the x and y and there was no difference. I put in double what I had, no difference. I ruled out the program as the culprit. I even went into the Survey and moved the axis gain on the X and y to intermediate to see if that would help, and it did not. It almost seems like it's stalling one axis when the tool gets really close to the apex of the circle on that particular axis just a tiny bit prematurely. The Flat that it leaves at 75ipm is roughly .060 which would reduce the diameter of the circle by roughly 0.003" or .0015" per side. Even at 25ipm it still puts the flats there and is off by 0.0015" per side on those flats. The program calls out G2's and G3's where appropriate so it's not a segmented sort of HSM like path. Could it be some sort of pitch error on the ball screw thats messed up maybe or is there another parameter that I need to look at like the X-Y Aspect Ratio? This is driving me nuts, and I can't really swing bringing in a tech at the moment unfortunately.

I agree with Johnny…Your interpolation speeds are way too fast! There are parameters that allow for the following and trailing and errors to get longer as feed rates go up. Plus the acceleration parameters extend as the speed increases too.

The reason for this is kind of obvious when you think about it because that’s a lot of mass to be throwing around and you wouldn’t want your servo’s and other mechanicals to tear themselves apart. A half inch EM trying to make a .590 circle is really ripping.

One other ‘long shot’ thought is… did you hand turn the ball screws after you replace the thrust bearings and just before closing the guards up to make sure the table moves smoothly in both axis? (With power off of course)

The reason I ask is I did see a problem like this once. The way lube lines were clogged. We believed what we were seeing was the ball screw shaft winding up a little during direction change because of the constant load caused by the way friction. This was a solid way machine though and I did not note what yours is.

The Circle is an OD not an ID. On my old 1990 Tree 325J I could hold less than a thou at 50ipm doing this same op on this same part with no flat spots and everything looking super smooth. I have a hard time believing that this thing can't do it faster. Besides we have a 1990 Fadal VMC20 in here with it's DC servos that can hold better tolerance on this sort of cut at the same if not faster speeds. I also checked the ballscrews post bearing install and they turned fine so I am not super concerned there. But I may just tear it apart, again, and check everything just to be sure. But I am still of the mind that it is something in the control or the drives that is mucked up.
 
Sounds like someone needs to call a local ball-bar tester guy...

You're literally guessing at the problem, you should set backlash to zero, reset the axis tuning to conservative default values, then get it ball-bar tested. Those guys don't just give you a printout, they also give you a diagnosis as to common causes.
 








 
Back
Top