Trouble cutting circles with mach3

[billwann]

Hello

I was hoping some one here could help , I am having trouble cutting circles in acrylic with Mach3 . what is happening is there is a small flat spot where the cutter enters and exits the cut . I remember someone telling me that there was a way to make the cutter cut past the spot where the cutter started the cut to make it completely round . kinda like extending the cut to clean it up . does any one have any ideas ?

Thanks BIll

[Walky]

What you're looking for are probably "lead in - lead out" and "overcut" options (or something like that) in your CAM software. If you're using one of the Mach3 wizards, then I don't know really, since I haven't used those. Also, check that your Z axis is perfectly at 90º relative to both the X and Y axis.

[CarveOne]

Try slowing down the Z axis plunge rate to see if it helps. If plunging too fast the cutter may be walking around in a larger circle than the diameter of the cutter as it enters the material. That would typically be caused by flexing in your Z axis if it is not as stiff as it needs to be, or some backlash in the X or Y axes.

Mach3's Tools menu has a final step-over setting that may help clean up your problem.

CarveOne

[DonFrambach]

Here's a snippet of g-code to cut a small circle. Since it plunges to the desired cut depth and then moves to the edge, you shouldn't get a flat spot.


(cut circle) (radius = .125 )
(depth =-.1 )

G01 X0 Y0 (zero X & Y)
G01 Z-.1 (bring cutter to cut level)
G01 X .125 Y0 (move to start position)
G02 X0 Y-.125 R .125 (quadrant 4)
G02 X-.125 Y0 R .125 (quadrant 3)
G02 X0 Y .125 R .125 (quadrant 2)
G02 X .125 Y0 R .125 (quadrant 1)

[AiR_GuNNeR]

I would simply make the first cut .005" (.010 on diameter), oversize, then do a second pass at diameter. I do this for any finish cut where I need a nice finish.

[ger21]

I cut circles using helical cuts, so there is no plunging.

[HPbyGD]

An other option is to drill a hole that is 1/16" smaller than the cutter right where the cutter is going to plunge so that as it plunges into the material is cutting very little material.
Gary :-)

[jsheerin]

Like Gerry said, don't plunge your cutter straight in. Ramp it in to the cut at a low angle, like 5 to 10 degrees. Do this while you're going around the circle. Plunging straight in is hard on your spindle bearings.

What cam software are you using?

[Cheeta]

I have a similar issue. I am using IJ code to plunge a 21/64 bit into 3/4" plywood. I am cutting a matrix of 1inch holes. Every single hole looks as if the path was followed perfectly through 3/4 of the circle then the last 1/4 of it takes on a different radius and leaves a flat spot in the circle.

I checked all backlash and then ran a pocket cutting wizard from Mach3 which used the radius command and spiraled a perfect 1 inch hole. I tried all the usual suspects IE incr, CV, abs and nothing affected it. Tried feeds so slow i almost started a fire and still the exact same pattern.

I tried the same file on a different machine(same style) with different bit (1/8") and faster computer. Holes were good. It got late so I havent tried fast computer on the first machine.

1. Could the computer be choking on the interpolation and deceleration?
2. Should I be pocketing all small holes?

Any ideas?

[ger21]

Is the problem visible in the toolpath display?

Can you post the g-code?

[Cheeta]

Gerry,
Funny you should mention toolpath. Les Newell also told me that everything in that path is exactly what gets thru the P port. I ruled out backlash but started looking into flex. My machine is very stiff, however with the z-axis it is difficult to keep it stiff and nimble at the same time. It turns out that I had a tool crash once and scorched my bit. I didnt think it was a big deal but it really dulled it. I was getting more flex from the dull bit. I put a fresh one in and also added a ramp to the approach and the circles came out perfect. Remember your father telling you never use a dull blade...nobody ever gets hurt with a sharp blade. I think he knew more than I thought ha ha.