[kentavv]

Tonight was the first time that I have attempted 3D milling on my IH mill. The piece below was cut from 2x2x1 aluminum using a 3/8" ball end mill held in a collet. Overall I am fairly pleased but I do see one problem. Namely, the flat area is 7 thou higher at the beginning than at the end. This creates an edge that is easily seen when holding the part in your hand and may be noticeable on the right side in the picture below. The end mill might have slipped though the cuts being made were very light. Might there be other reasons? Is it even reasonable to expect better from this mill? I have never measured any backlash in the X and Y but have measured (and attempted to correct in Mach3) .002 backlash in the Z. Though, I don't think this is a backlash problem. What else should I consider to try to isolate this error? Perhaps unrelated but I also often have an edge formed at the beginning/end of an outside contour.

[judleroy]

Try slowing down the cut or better yet a smaller tool 1/4" maybe. Also if you stopped and retracted during the cut where the line starts you may have lost position for some reason.

[kentavv]

The only retract away from the part was at the end of the finish pass. Of course while cutting the part generally all three axises were moving at once. Cuts alternated from starting at the top and then the bottom of the hemisphere... Imagine a zig-zag pattern radially arranged. If the end mill slipped, it slipped down. There seems to be at least two "lines." The obvious one that separates the beginning from the end and another at about 135 degrees which starts a region that is about 2 thou deeper. How might position might be lost on this mill? I am certain that the Gecko drives never faulted because that would have caused a major problem. How might a smaller cutter help?

[philbur]

It's my understanding that you should avoid backlash compensation if possible. I would try again with it turned off. Also your described contouring problem could, I think, indicate backlash in x and/or y, although you can get a "mark" at the start of a contour due to the longer residence time of the cutter at that location during a plunge operation.

Just some thoughts from a novice CNCer.

Regards
Phil

Tonight was the first time that I have attempted 3D milling on my IH mill. The piece below was cut from 2x2x1 aluminum using a 3/8" ball end mill held in a collet. Overall I am fairly pleased but I do see one problem. Namely, the flat area is 7 thou higher at the beginning than at the end. This creates an edge that is easily seen when holding the part in your hand and may be noticeable on the right side in the picture below. The end mill might have slipped though the cuts being made were very light. Might there be other reasons? Is it even reasonable to expect better from this mill? I have never measured any backlash in the X and Y but have measured (and attempted to correct in Mach3) .002 backlash in the Z. Though, I don't think this is a backlash problem. What else should I consider to try to isolate this error? Perhaps unrelated but I also often have an edge formed at the beginning/end of an outside contour.

[srmaietta]

Is that one side meeting the other at a lower level, or is it a groove from a single pass that was too deep?

congrats on a cool 3d part! Polish her up!

~Steve

[philbur]

It looks like a Z issue. You can see the step on horizontal portions but not on the vertical section. If you study the step closely you should at least be able to determine which axis are involved in the error.

Regards
Phil

Tonight was the first time that I have attempted 3D milling on my IH mill. The piece below was cut from 2x2x1 aluminum using a 3/8" ball end mill held in a collet. Overall I am fairly pleased but I do see one problem. Namely, the flat area is 7 thou higher at the beginning than at the end. This creates an edge that is easily seen when holding the part in your hand and may be noticeable on the right side in the picture below. The end mill might have slipped though the cuts being made were very light. Might there be other reasons? Is it even reasonable to expect better from this mill? I have never measured any backlash in the X and Y but have measured (and attempted to correct in Mach3) .002 backlash in the Z. Though, I don't think this is a backlash problem. What else should I consider to try to isolate this error? Perhaps unrelated but I also often have an edge formed at the beginning/end of an outside contour.

[kentavv]

Yes, the sides have different height. However, this was not intentional. Please see the attached image. The finish pass starts at the "point" of the hemisphere initially traveling along the 0 degree line and then "zig-zags" counter-clockwise up and down the hemisphere. There are two marks - one near 135 degrees (counter-clockwise) and the other at 360 degrees. The first mark delimits sides with .002 error (measured with a mic from the bottom of the piece) and the second mark delimits sides with .007 error. It is as though the Z position was slowly being lost as the mill traveled around the hemisphere. the chip loading was in general quite low while finishing especially in the area with the most error. The part was mist cooled the whole time. I'll give it another go using an endmill holder.

Is that one side meeting the other at a lower level, or is it a groove from a single pass that was too deep?

congrats on a cool 3d part! Polish her up!

~Steve

[kentavv]

Yeah, I think there is an issue with the Z axis as well but I am not sure how to go about identifying the actual cause. I have measured the head height using a height gage resting on the table and with .002 backlash comp all is fine. I am pretty sure that if I disable backlash comp that passes will alternate in depth by .002 (the backlash amount). The error might have occurred if the part lifted on the right side as the tool as going around but it would had to have been pretty gradual and gosh the cuts were really light.

It looks like a Z issue. You can see the step on horizontal portions but not on the vertical section. If you study the step closely you should at least be able to determine which axis are involved in the error.

Regards
Phil

[youngfg]

Were the cuts getting deeper? If so I would say the end mill slipped down in the collet. I have had that happen to me several times.

[kentavv]

I use ETM end mill holders and Lyndex collets. This is R8 tooling. In this particular case I used a collet. Is there something better that I could be using? I have had end mills complete fall out before when taking massive side milling cuts. That's when I switched to the end mill holders. But there are those that say the end mill holders are junk because they put the tool off center. Never had an end mill slip in a holder though

[youngfg]

I have had .25" endmills slip down while slotting steel. They would slip down enough that the endmill would break from the cut getting so deep.
I have been using endmill holders so the mill can't slip.

[philbur]

I think the slipping endmill is probably a red herring if you were take very light cuts.

Regards
Phil

I use ETM end mill holders and Lyndex collets. This is R8 tooling. In this particular case I used a collet. Is there something better that I could be using? I have had end mills complete fall out before when taking massive side milling cuts. That's when I switched to the end mill holders. But there are those that say the end mill holders are junk because they put the tool off center. Never had an end mill slip in a holder though

[philbur]

I found this on the Yahoo mach1mach2cnc site:

"The trouble with full CNC (multiple axis) is that during the steps that the
backlash is being taken up, the other axis are still moving. "

You maybe should do a search of "backlash compensation" on the Mach site and read about the issues.

Regards
Phil

I use ETM end mill holders and Lyndex collets. This is R8 tooling. In this particular case I used a collet. Is there something better that I could be using? I have had end mills complete fall out before when taking massive side milling cuts. That's when I switched to the end mill holders. But there are those that say the end mill holders are junk because they put the tool off center. Never had an end mill slip in a holder though

[philbur]

A different machining strategy, such as waterline, might allow you to turn the Z axis backlash compensation off, as all Z moves would be only up or down but never both.

Regards
Phil

I found this on the Yahoo mach1mach2cnc site:

"The trouble with full CNC (multiple axis) is that during the steps that the
backlash is being taken up, the other axis are still moving. "

You maybe should do a search of "backlash compensation" on the Mach site and read about the issues.

Regards
Phil

[kentavv]

I have had .25" endmills slip down while slotting steel. They would slip down enough that the endmill would break from the cut getting so deep.
I have been using endmill holders so the mill can't slip.

I like using end mill holders. Unfortunately lots of end mills, especially carbide cutters, don't have the Weldon shank. Is it fine in those cases just to tighten the screw down on the round shank?

[holbieone]

I'm assuming the way you mapped it out the the error is mostly in one quadrant

if yes it looks like a backlash problem in the axis reversals

also if you had more then .02 left for you finish pass some of that near the end could be shadowing from the extra stock

each pass would get less and less tool engulfment causing the tool to relax and cut deeper

I'd run the part again with a new piece of stock and then run a dry pass and see if it cleans up better

[judleroy]

I cut steel all day long 1/4" peck depth with a 1/2" endmill at 26ipm using a cat 40 spindle. The tool has
no flat and is held with a cap screw. The tool has never
slipped. I always use 5ipm for plunge speed. I have over
the years had many router bits slip up and down in there collets. I've also had endmills come all the way
out of R8 collets. Always while cutting plastic. I'm thinking to much load or too much speed is the culprit.
Try it again sometimes you just never know just what caused a problem until you do it again and see what happens the second time.

[kentavv]

I cut the part again tonight with the tool in an end mill holder. There is still a small error but 2 thou is better than 7 thou. Interestingly 2 thou just happens to be the backlash comp I currently have set. I'll give it another go with backlash comp turned off as well. Looks like the greatest error was from a slipping tool. Amazing the tool slipped with these light cuts.

[holbieone]

i don't know how much material you had for your finish pass

if it was a lite cut just using the ball to cut ,that wouldn't pull the tool out(unless you had it way too loose in the holder)

[kentavv]

i don't know how much material you had for your finish pass

if it was a lite cut just using the ball to cut ,that wouldn't pull the tool out(unless you had it way too loose in the holder)

About the curvature there was at least .005 and probably .050 on average. In the "flat" areas I would say the average was .100. I say "average" because of the nature of the roughing operation. Yes, only the ball was engaged with the material. I can assure you the drawbar was tight but given this problem is not uncommon to me I wonder if the collets are not great or the spindle does not have correct taper. The collets are Lyndex but I suppose even they can make a bad collet from time to time. I am considering getting a set of ER collets and a collet chuck and hopefully solving this problem.