Router chatter

[speedrider]

We have a motionmaster 4 foot by 8 foot router with a 7.5 HP motor. It has a top RPM of 18,500. We cut plywood and 3/16 " plastic. We are getting real bad chatter marks on the edges of the plastic. I checked backlash and it is fine. The motor is new and the collet runs true. Any othe ideas that could cause this?
Thanks

[jeffrey001]

Are you using climb milling or conventional.

Or this can be caused by or due by a bad way to hold material or you material is vibrating during machining.

Jeff

[lancut]

Increase chip load on the tool, by either increasing the feedrate, or decreasing tool rpm, In some cases a climb cut helps with the finish cut. Hope this helps.
BR

[MarkT]

Use the largest diameter tool you can for the application. Mount that tool in the collet so that the flute of the cutter is as close as possible to the collet without going inside the collet. Run the low end of the sfm calculation (rpm), recommended from the tool manufacturer, and high end of the chipload calculation (rpm x load per flute x # of flutes). Insure your material clamping method is rigid. Less efficient but alternate process is to add rough pass leaving material around the pheriphery cut ( 1-2mm ~.04-.08 inch) and come back in with a lighter load finish pass.

Hope this helps

Mark T.

www.cnccustomservices.com

[speedrider]

Originally Posted by jeffrey001 Are you using climb milling or conventional. Or this can be caused by or due by a bad way to hold material or you material is vibrating during machining. Jeff

I am climb cutting.
The pattern is very equal. In other words it is like a gear. I check the run out of the tool and it had about .003 one tooth to the other. They have been cuttin g these things for years at the same RPMs and feed rates. It only started doing this about 4 months ago. We put on a new motor after that because we thought the bearings were going in the spindle, but that did not fix the problem.
I also just found out that they have not been greasing and oiling the leadscrew and ways for years. They were dry as a bone.

[ger21]

Originally Posted by speedrider I check the run out of the tool and it had about .003 one tooth to the other.

That'll do it. Although a pic would help us see what you mean by "real bad".

[speedrider]

Originally Posted by ger21 That'll do it. Although a pic would help us see what you mean by "real bad".

[Boots]

You should be Conventional cutting man made materials.

[beege]

I disagree on the Conventional. The only reason to use conv. is if your machine is loose (play in the axes).

You should be using a down-cutter, Left hand spiral, right-hand cut, to push the forces into the bed, instead of away. What kind of cutter are you using?

[speedrider]

We are using a straight 2 flute carbide router bit. The same as they have used for years. They even tried a couple new ones.

[lancut]

Speedrider, I just look at the picture, and I from what I see the combination of feed rate, rpm, and the depth of the finish cut are not correct. Try lesser cut about .025" and slow the feedrate a little, climb cut, and you should be able get better result. I don't agree with someones comment about conventional cutting a plastics. Any kind of steel, titanium, I agree. Aluminum, plastic etc give much better results climb milling and routing. Actually I have better luck with slightly dull endmill as far as finish cut goes. If the machine is loose, spindle bearings shot, good file maybe good option.
Hopefully this help.
BR

[Boots]

Well, if one way does not work then one has to try a different way,,,, NO?
I cut 1/4 in. thick Plexiglass for Sedwick Townhouse to cover their windows. I used a 1/4 in. Straight 2 flute carbide tool cutting at 240 IPM running at 16,000 RPM in 2 passes in the Conventional direction, ramping in. I tried Climb cutting with BAD results in the finished edge.