Fadal 4020 backlash and interpolation

[SigurdACVW]

I have a job on our Fadal 4020 that is a series of blind .7500" holes, .875" deep. I've programmed them in Mastercam using the Helix Bore toolpath. 2000rpm, 35ipm. Inspecting the hole with an indicator and Indicol, the machine is cutting it round, but at the 2:00 and 8:00 positions, there is a .002" divot outward. It's not an oval; just a bump outward in those two spots. If I put my hand on the table while it's running, I can feel it bumping.

Now, if I turn the feedrate down to 10ipm, the hole comes out perfect. What could be going on here? Is this a backlash issue? Wouldn't it be doing it at all feedrates?

 

[Orange Vise]

What's the size of your endmill? Guessing maybe 1/2" with a .125" toolpath radius?

35ipm is pretty quick with such a tight R. On higher end machines, high accuracy mode needs to be turned on to stay on size at those parameters.

Doesn't sound like backlash as you've stated. In any case, backlash is pretty easy to diagnose with an indicator.

Do you get the same issue with holes at different locations?

 

[mhajicek]

Sounds to me like you have some mechanical backlash that the machine is compensating for. It takes time for the servo and screw to reverse and take up the backlash, which is why it can't do it perfectly at higher speeds.

 

[SigurdACVW]

What's the size of your endmill? Guessing maybe 1/2" with a .125" toolpath radius?

35ipm is pretty quick with such a tight R. On higher end machines, high accuracy mode needs to be turned on to stay on size at those parameters.

Doesn't sound like backlash as you've stated. In any case, backlash is pretty easy to diagnose with an indicator.

Do you get the same issue with holes at different locations?

1/2" 2-flute Dapra endmill with a backdraft insert. I've only done the first hole. Second one when I get in today.

 

[SigurdACVW]

I spoke too soon. I never checked the slower feedrate with an indicator; only by watching the Dykem disappear. The indicator shows that the dip is lessened, but still there. Could this be a Format 1/Format 2 problem? Or a G8/G9 problem?

 

[mmurray70]

Cant ream it? or bore it?

 

[dandrummerman21]

I have the opinion that most people who say "I just interpolate holes instead of reaming them" think their machines are gonna be making holes that are round within .0002, and when I see it, I either think they have a brand new high end machine, or full of it.

I think it is generally unrealistic, especially on older machines, or non-high end machines, to expect interpolation with an endmill to be better than .0005 or so for the size that you are trying to accomplish.



Making a 3/4 hole at 35ipm with a 1/2 endmill is way too fast. And I would expect that .002 error. I would be finishing at 10ipm or so like you said you changed to. And I still would expect greater than .0005 error.


If a clearance hole, or dowel hole (press or slip), I'd say "good enough". On a hole that takes a bearing or something that needs to be round, I wouldn't mess around with interpolating to finish. I would just ream or bore it.


I don't think there's a problem with your machine, other than it's not a high end machine, don't expect high end results.


Ballscrew/thrust bearing wear can contribute. But even with everything mechanical in brand new condition, the electronics have response times and such, and it's very difficult to get perfection from older hardware.


FWIW the newest mill in the shop I work at is a 2005. We have 10 mills and only 2 are newer than 2000, the oldest being 1993.