Pieces cut cut too small

[Mikehell]

If I cut a piece in MDF with a profile toolpath,, using the conventional setting, they come out 1/16th too small. Using a climb cut, they come out correct. I know this is probably more of a "doctor, it hurts when I do this" situation, but I'd really like to find the root cause.

My first thought is to replace the collet and collet nut. Asked the boss "when is the last time the collet and but we're replaced?" His answer "the what?". So, yeah, probably been years and years. Unfortunately, it's a Perske spindle (as far as I can tell) and the collets aren't as easy to find so it'll take a week or so to get one.

[bravesoul]

To me the most common reason for your issue is bit deflection which is why it works in the opposite direction. I always try to take small amt each time (4 - 6 steps) to help minimize this and also use .02 allowance and reverse direction for the final cut.

Joe

[Adrian]

When you change the cut direction it changes which side of the cut the "pull" is applied so if the bit or machine is deflecting then the deflection will either be towards the piece or the waste depending on the direction of the cut.

Definitely should have the collet replaced by now. I cut 20 to 30 sheets of MDF a week plus 10 to 20 sheets of recycled plastic and I generally replace the collet every three months.

[Mikehell]

To me the most common reason for your issue is bit deflection which is why it works in the opposite direction. I always try to take small amt each time (4 - 6 steps) to help minimize this and also use .02 allowance and reverse direction for the final cut.

Joe

Tried various bits. Same result. Slowing down the cut didn't seem to fix it either. Not wanting to go too slow, as production times will be affected.

[Mikehell]

When you change the cut direction it changes which side of the cut the "pull" is applied so if the bit or machine is deflecting then the deflection will either be towards the piece or the waste depending on the direction of the cut.

Definitely should have the collet replaced by now. I cut 20 to 30 sheets of MDF a week plus 10 to 20 sheets of recycled plastic and I generally replace the collet every three months.

Collet and but replacement is a no brainier. It's gonna happen. I'm probably the first guy they've hired that has even a clue about CNC. When I was shown how to use the machine, they were cutting MDF at 60ipm at something like 20,000rpm with a straight flute bit. The bit was literally black and duller than a butterknife. MDF looked like it was being torn, not cut.

I'm currently using an Onsrud 60-113mw compression bit, so I don't really want to slow it down so much as to affect the bit life.

"Mike, you're cutting that at 5 inches per second? That's 5times too fast!".

"No, it's 10 times too fast, I'm doing it in a single pass"

[scottp55]

Mike,
Don't forget to acetone the spindle cone itself, until paper towels/Q-Tips come out spotless....also blow out spindle cone/collet/collet nut at every tool change.

On of the better ways to measure a bit to enter in data base...is to Cut the material you'll be cutting, at a depth you normally use...and then measure the cut carefully several times. A good real world measurement.

scott

[tomgardiner]

That deflection is huge. Is the error consistent in both the x and y axis? I would be looking for machine play when the runout is that large. Collet wear would lead to chatter, vibration and loose bits.

[GEdward]

That deflection is huge. Is the error consistent in both the x and y axis? I would be looking for machine play when the runout is that large.

I agree. I suspect the there may be a fair amount of backlash in the system. Does your control system have backlash compensation capability? If so you might want to check that out and compensate accordingly.

Ed

[Mikehell]

That deflection is huge. Is the error consistent in both the x and y axis? I would be looking for machine play when the runout is that large. Collet wear would lead to chatter, vibration and loose bits.

.error is the exact same in both X and Y dimensions.

Machine play most likely not an issue, as this thing is built like a tank. Can't budge it by hand, so no noticable slop in either direction.

[tomgardiner]

I figured that if it had a Perske spindle it is a big machine. Have a look at the wear to belts (if there are any) and pinions
Is this an ATC machine?

[Mikehell]

That deflection is huge. Is the error consistent in both the x and y axis? I would be looking for machine play when the runout is that large.

I agree. I suspect the there may be a fair amount of backlash in the system. Does your control system have backlash compensation capability? If so you might want to check that out and compensate accordingly.

Ed

Honestly, I don't know. It has a proprietary controller designed and built in the Stone age. I have a folder full of pdf documentation for it that tells me everything EXCEPT anything I really need to know.

[Mikehell]

I figured that if it had a Perske spindle it is a big machine. Have a look at the wear to belts (if there are any) and pinions
Is this an ATC machine?

Yes, the machine is a big monster. It's not an ATC. Pretty sure they got it second hand somewhere, as there seems to be a mist option that was disconnected and partially removed. Machine is pretty much overkill for what we use it for. Cutting rather basic shapes out of 1/2" MDF.

If it was a belt problem, would the problem be the exact same in both X and Y ?

[tomgardiner]

It would be unlikely that both axes would have the same wear but if this machine hasn't had routine maintenance then it would be wise to look into replacing the drive components susceptible to wear.
I am not the right person to advise on this, others on the forum or on a machine specific forum such as cnczone will know what to look for.
What is the machine and control?

[GEdward]

Regardless of what the problem is, it is not Vectric software related. Cutting 1/2 inch MDF in a single pass with a 1/4 inch bit is pretty ambitious IMHO. But if you are managing the chip load and evacuation well enough to avoid introducing re-cuts at the cutter-material interface then why not. If the error is the same regardless of the size of the part then the problem is deflection and mechanically related. If the error grows with increased size of the parts then the problem is likely firmware related in that the pulse count of the encoders or step/micro-step count of the step drives are not set right. You might have better luck finding a solution in a forum that is specific to your machine and or operating system. In the meantime, as long as your finished product turns out correct when you cut them out with a climb cutting strategy then I would go with that.

Ed