Machining Solid Surface Material on the CNC

Advice on bits and feed speeds for milling solid surfacing. September 18, 2014

Question (WOODWEB Member) :
I run a Weeke bhp-008 5x10 nested base for a store fixture company. Tomorrow I have to cut out a top for a kiosk in sections that will be glued after machining. I have zero exp with solid surface materials. I've read a bit about feed speeds and bits in Dupont's Corian fab manual and set up 2 flute 1/2" 3deg downshear, spun at 12,000rpm and fed 10m/min for the programming to be done with. Today, the shop lead comes up to me asking about the tooling to be used and is adamant about me using a three or four flute bit at 18,000+ without compensating feed rates so he gets a glass smooth edge for his joints. I am concerned about the heat traveling up into the spindle and killing the bearings and re-welding the parts together with a melted chipload (more like powder Iím guessing). Does anybody have a solution?

Forum Responses
(CNC Forum)
From contributor T:
I would never use a downshear tool on solid surface. The chips will pack up and weld together. As for heat on the spindle I wouldnt worry about that. Heat should be kicked out with the chips. If the shop lead is willing to stand by what he wants, then do what he says. If heís the kind to throw you under the bus do what you think you know. Be ready to take the hit if it doesnít work. The guy is shop lead for a reason so itís best to run it as directed. If he's wrong, it's on him. Keep your hand on the feedrate overide and adjust as needed. It should be no big deal.

From the original questioner:
In my shop I'm responsible for the machine. Itís up to me and the shop manager to decide how to attack this. I neglected to mention the lead wants a three or four flute downspiral and slow feed rate, so the heat is going to load up in the bit badly. I'm betting it doesn't make anything close to the size of a chip, so like you mentioned I'm also concerned about welding the cuts back together, especially since the vacuum table doesn't help with extraction at all. I was wondering if anyone had a method to make the cuts with proper feeds using a true straight bit and then make a finishing pass of some sort that produces the edge the lead is after?

From contributor T:
I'd just use an o-flute (1/2 (2 flute) 18000 rpm 125-250 ipm). Depending on how deep you need to go you may need to step it down. In which case I'd leave the rough pass +.025-.05 stock and cut the final pass at depth and to size. Anything .500 or under just let it rip. I'm sure there are other opinions and variables on the subject that could affect how it works out. Something as trival as the color of your solid surface can affect how it cuts, such as the amount of decorative aggregate added. It would be a good idea to contact your supplier for info on your specific material. If you can start out cutting oversize and see how it goes. Considering the material cost I understand your apprehension. Just use your head and listen to the cut and you'll be fine. Feed rate override is your friend. As with most acrylics you have to push it a little to kick out the heat.

From contributor M:
Your lead guy there is simply incorrect. His method will result only in wasted time and material. If you cut Corian only occasionally, as I do and high throughput on this material is not a big issue, save money and material by using a 1/4" single O flute. 18000K and 180 IPM leaves a glass smooth finish on 1/2 inch material in one pass. Onion skin small or narrow parts, with the first pass 5 thousandths away and .48 deep. The second pass is on size and all the way through. I cut my material face down, not for reduced chipping but the smooth face holds better to the spoilboard. Also, for a nice finish be sure and use a new bit. If you have cut wood or plywood with it the edge will no longer be suitable for use on plastic.

From contributor L:
Don't you have some off-fall or scrap that you can do a test cut on? Three flute is probably more than enough, just lower the rpms to match the feed rate. Start with whatever the chart says then crank it up until you get a poor quality finish. I've used a low helix 2-flute down-shear o-flute 1/2" diameter and it seemed to cut fine to me, no welding but I take it in multiple passes. With that tool I take it 300ipm at 16000 rpm, .25 depth per pass. I've cut many tops that way without any problems. You could try doing a rough pass the way you want and leave about 1/32" or so stock, then come back and finish it off the way your guy wants.

From the original questioner:
The shop manager decided we would do mirror cuts at a bench for the glue joints to be done in house and postponed cutting until tomorrow to give me time to make test cuts and handle normal production for the day. He asked about using an upshear late in the day, and after reading others posts here, we will likely pursue that for future solid surface work. For now I'm using a 1/2" 2 flute o flute straight, no shear up or down (12,000rpm fed at 13-15m/min (500-600ipm)). I'll dial the feed in as the actual material has much larger aggregates in it than the test material. I plan to cut it in three passes as my dust collection is not adequate for full depth passes. I ran a perimeter cut as part of my testing at full depth and had enough chips flying out from under the hood to trip the optical sensors on the front of the machine and cause a feed stop. I finally got a "maybe we do need more extraction on this machine" out of that one.