Thread: Hole interpolation accuracy with endmill

Originally Posted by cgrim3

Damn 1800 bucks! That seems like a lot of money to spend on that every year

While it can be a great piece of data to have and collect, very few shops actually need an annual ballbar test. Again, lookup how to check for lost motion. That is good enough for 99% of applications.

Originally Posted by cgrim3

Damn 1800 bucks! That seems like a lot of money to spend on that every year

That's about six bone plates.

Originally Posted by boosted

While it can be a great piece of data to have and collect...

It's not just data collection; they adjust the backlash compensation and the error mapping to minimize the error in the machine.

So I guess tolerance is tolerance.... 1.002" seems an odd size though? Is it a slip fit on a 1" pin? If you can get a 1.002" and not a 1.003" I'd say you are good to go, or as you said a bore mic, averaging the reading (1.0021-1.0025" etc).... I don't think .0003" out of round is bad on 23007 machine at all. And as mentioned, need better - tenth set boring head....

Originally Posted by mhajicek

It's not just data collection; they adjust the backlash compensation and the error mapping to minimize the error in the machine.

Again, the backlash comp can be achieved with just standard lost motion checks and adjustments.

I do like ballbar tests, they are great for tracking long term accuracy, trends, etc... If I had a fleet of similar machines we would definitely ballbar all of them annually. It's just not a necessity for most environments. Most of us don't have machines and processes that are consistent enough that measuring and tuning circular motion at very high accuracy will be critical.

We did a few studies on this for a military/ aerospace company I had the misfortune of working for. They insisted on using circular interpolation for holes rather than reamers or boring heads. (They are the reason I prefer not to fly).

You can comp in any hole to make it seem like it's to dimension if you are using a pin gauge, but as you found it is not necessarily round. A hole that passes a pin gauge may very well fail in a CMM or an optical system... the inverse is also true (set comp with a CMM and then have the customer reject the part with a pin). If you choose to make parts using this method, it pays to know how the customer will be qualifying the parts.

I found that I could achieve better circularity by helically boring the parts with the tolerance set very tight. This broke the code into very small line segments rather than using a G02/G03. I would love to go back and revisit that theory if I ever have time and the appropriate test equipment sitting around.

Boosted, sorry if this comes off as a noob question, but how do you do lost motion checks and adjustments? I am not entirely sure what lost motion checks mean.

When you say lost motion, do you just mean backlash?

Originally Posted by cgrim3

When you say lost motion, do you just mean backlash?

Guessing here, but "lost motion" may also include stiction, belt stretch, etc., where backlash might just be the loss of contact from one element/group of elements (bearings) from another.

Just my WAG...

I don't know why you guys even consider this stuff .... if you want a round hole, a boring bar is dependent on the spindle bearings. Interpolated hole depends on spindle bearings, end mill concentricity and cylindricity, axis accuracy and backlash and velocity and position control.

No contest.

So this morning, we checked the backlash of the machine in the x, y, and z. I was pretty surprised it was out so much. Backlash in the Z is .0004, the Y is .0005, and the X is .0003. I am going to get somebody in here to do a ball bar test or calibrate the machine. You all think this is too much? I know I can probably do a backlash comp in the controller but I want to make sure nothing else is going on which would cause this much backlash (such as a bent ball screw, bad bearings, etc).

Originally Posted by cgrim3

So this morning, we checked the backlash of the machine in the x, y, and z. I was pretty surprised it was out so much. Backlash in the Z is .0004, the Y is .0005, and the X is .0003. I am going to get somebody in here to do a ball bar test or calibrate the machine. You all think this is too much? I know I can probably do a backlash comp in the controller but I want to make sure nothing else is going on which would cause this much backlash (such as a bent ball screw, bad bearings, etc).

You can't really adjust real mechanical backlash out of a machine in hopes of getting rounder holes. The backlash basically mucks with the PID setting of the servos, meaning the parameters have to be set 'looser' because the servo loop cannot be as tight as a theoretical zero backlash. Servos find position by cutting the error in half many times over (very quickly) which involves decelerating to an exact stop at exactly the right position. It might be tuned to do this electronically so far as the encoders are concerned, but if your machine rapidly stops a heavy table, and real backlash exists, then that table position is going to be undefined within the range of backlash. The servo will have to hunt in both directions and settle on the best average it can find. That would be for positional moves. Imagine the complexity of the servos passing any quadrant line and trying to tune out that table inertia and the ballscrew backlash and getting it perfect at the quadrant line. Slim chance. In Z axis of a vertical mill, you've got significant weight bearing down consistently, so backlash comp could work pretty good there because the head will never find itself 'above' the backlash.

If you want round holes, bore 'em.

If it were me I would be happy with 3 tenths on that machine and bore anything that needs to be held tighter.

Often it is more valuable to know what your machine can and can't do than to have a machine that can do almost anything.

Originally Posted by cgrim3

we are using smoothing and feed optimization. We are using fusion 360. The tolerance set for smoothing is .00001

Feeds and speeds: 2000 rpm, feedrate of 10 ipm. It is aluminum and we could have gone faster. The machine has an 8000rpm spindle so we try not to go too fast. This is a one-off part so we didn't apply super super fast feed rates for production.

I do not know how to apply look ahead in fusion or on the machine. How do you do this?

Why would you use smoothing on a round hole? That makes no sense. I would recommend breaking your arcs into quadrants and using G60 (exact stop positioning)so you can see where the problem is.

Coronavirus, I'm not entirely sure how to do that in fusion. I don't think fusion gives you that level of control but I might be wrong

Originally Posted by cgrim3

Coronavirus, I'm not entirely sure how to do that in fusion. I don't think fusion gives you that level of control but I might be wrong

Try selecting a sketch of the circle rather than the solid. Back when I was playing with it that made a huge difference on the toolpath. IE it would output 1 arc rather than linear moves or a ton of tiny arc

To interpolate a circle with an endmill, I generally use the circular or the bore function for interpolation, then use a contour toolpath for finishing. These toolpaths don't give you an option to select a point. You must select the sketch of the circle.

Anyhow, we are having somebody coming out here to calibrate the machine. It's funny because our daewoo Puma lathe is from 1998 and that has like 30 millionths backlash in the X and Z. This daewoo mill is newer and has backlash in y of .0005

Originally Posted by cgrim3

Coronavirus, I'm not entirely sure how to do that in fusion. I don't think fusion gives you that level of control but I might be wrong

Me either. I have never used fusion, but I would try drawing arcs instead of circles if fusion does not have a break arc feature when posting.

Originally Posted by cgrim3

To interpolate a circle with an endmill, I generally use the circular or the bore function for interpolation, then use a contour toolpath for finishing. These toolpaths don't give you an option to select a point. You must select the sketch of the circle.

Anyhow, we are having somebody coming out here to calibrate the machine. It's funny because our daewoo Puma lathe is from 1998 and that has like 30 millionths backlash in the X and Z. This daewoo mill is newer and has backlash in y of .0005

It's been a while but I seem to remember being able to select the edge of the solid with contour which is not what you want. You want to hide the solid and make the sketch itself visible and select that. Maybe it's changed since I last used it since the bastards were making changes every week when I used it.

Originally Posted by EmanuelGoldstein

I don't know why you guys even consider this stuff .... if you want a round hole, a boring bar is dependent on the spindle bearings. Interpolated hole depends on spindle bearings, end mill concentricity and cylindricity, axis accuracy and backlash and velocity and position control.

No contest.

No contest indeed. I sometimes get a print and model at 5pm, and put the part on the engineer's desk by morning. I can throw an endmill in and get it done; I don't have a full set of boring bars for all length and diameter ranges. 99% of the time the hole will be a locating bore or a press fit for a pin, so if the gauge pins say it's good, it's good.