poor circle cutting

[chunkstyle]

Hi everybody,
Yesterday afternoon I cut a part out of mdf on my prs standard. It was .75" MDF that was getting some small 3/8" diameter holes drilled thru the panel. On the top side there was also a 1" D counter bore 1/8" deep. The counter bore was for the heads of some t-nuts that are going into the panel. When I installed the t-nuts it became obvious that the holes were very sloppy. Not at all concentric. The good news was they were consistently out of round.
The tool paths were created in partworks and the bit was a 1/4" down spiral bit running at 2"/ sec. The cut was a climb cut.
Would someone have any suggestions on what to look for or change? The motors are all tight and the machine is cutting square.
Thanks for any advice,
Tim

[clueless]

I can't speak from a technical standpoint, just a general observation from being around CNC machines for a long time, 2" per second (120 ipm) is crazy fast for trying to do a small hole. The machine has to ramp up to speed and ramp down to stop, and in your case, it's cutting a circle that's .75" in diameter (cutter makes it the 1" finished diameter), so that's a circumference of 2.35 inches. You're trying to make a rack and pinion system with stepper motors go from 0 to 2" per second and back to zero in about 1 second. There's not enough time for the machine to gain speed and stop in that 1 second, so it's trying to do the best it can, which leads to a odd shaped hole.

My guess would be to try it down at .5" per second range and see if that helps.

That's all my gut feeling about it, someone might post something that completely proves me wrong, but that's what I think is happening. Just not enough time to speed up and slow down in that time frame.

[chunkstyle]

Thanks Steve,

I've gone back and looked at the tool paths and noticed that the "ramp plunge moves" was not selected. I'm wondering if the start and stop of the bit, instead of a smooth plung, could also have caused it.
Your observation about the feed speed makes sense also. I thought, though, that the SB control software had the ability to slow down the cutting speed with a change in direction? Maybe a diameter doesn't work this way. If not, your suggestion to slow the feed speed may be the answer.
It does bring up the question of how you would compensate for a tool path that has both straight and circular paths within it. Would you have to look at the slowest speed that would work within a tool path in determining feed speeds?
Thanks for the advice,
Tim

[wmcghee]

It could also be a set screw loose holding one of your pinion gears on. I think theirs 2 screws in each gear so check them both.I've had that happen to me a couple of times. They seem to get loose over time.

[knight_toolworks]

the speed is not that bad but you want to ramp the holes. I cut holes that fast without a problem. but I pretty much ramp everything.

[clueless]

Ramping the holes changes everything, instead of trying to do all that in 2 inches, it's doing all that in many times that (however many times you make it go around the hole to get to depth), which gives it time to get to speed and maintain it during the cut.

[myxpykalix]

Tim I kind of agree with steve on the speed issue however even if you had the speed higher the machine can only get up to a certain speed given the area it has to move.

To make it a little faster overall I would go back and retoolpath by selecting all your straight lines for one toolpath at a higher speed and all your circles at a lower speed. That way it isn't jumping from fast to slow, slow to fast, ect.

[chunkstyle]

Thanks all,

I re-ran the file and added the ramping feature. It really helped it out a lot.
The holes much improved. The one thing I have to check on is that the counter bore is concentric to the thru hole. I will try some more test cutting tomorrow and will lower the feed speeds for the circular pocket cuts. I assume that the larger the diameter the faster the acceptable feed speed?
I can see that it's going to take time to get a feel for this new tool. liking the results I'm getting now, though.

Tim

[erik_f]

How far out of round are we talking here 1/8" or .015"? I would say if your +/- .015-.020 then it is speed and direction related. I hardly ever use climb cut since it seems to be less accurate than conventional cutting. Yes, in an ideal world both should cut the same...but since we are cutting using large tinker toys...I stick with conventional...also if I need things to be dead on...I cut no more depth than the width of the bit...usually I stick to 0.2" per pass for stuff I need highly accurate. If you are off greater than that you have something mechanical going on.

[John David]

You can run the feed at 100" per second and if the line is only .25" long the machine will never get to speed due to the ramp speed set, i actually use the ramps and speed combination to smooth things out in other Motion Control applications