Komacell Feeds & speeds 1/8 in sheet

[dubliner]

I nned to cut as many 9"x6" parts out of .125" 4 x 8 Komacell, with a .125 bit , need tight 125 radius corners. Trying to come with a time & yield per sheet, anyone recommend a fed & speed and bit type? TIA Dubliner

[widgetworks_unlimited]

Hi Neville... Can't wait to get back to Austin and eat at that fish place you took us to during last years Maker Faire

I'm not sure how Komacell cuts compared to other foamed PVC/soft plastics, (like Polyethylene) but I've had trouble getting clean cuts with these materials in the past. Regular 2 flute bits and even Osrude 0 flutes (both 1/8" and 1/4" diameter) were leaving some welded chips. The manual clean up really sucked!

After running the same parts with this problem for 2+ years, I finally tried the Onsrude O-flute bits designed specifically for SOFT plastic. What a difference! No more melting/welding! I can't describe the differences in bit geometry, but there significant/obvious - you can pick out the right O-flute for plastic/metal without looking at the label.

I also increased my feed rates to up the chipload and switched from a roughing/cleanup cut strategy to a single cut at full thickness depth. I know that sounds backwards, but the results don't lie.

Fingers crossed that I never have to deal with those headaches again!

[dubliner]

So what are your F's & S's?. I'll be using an Alpha & Spindle.

[bruce_taylor]

Neville,
I have the best luck with onsrud 56-612 it's straight so it doesn't lift the material . I go 1 ips to 1.3 ips at 7700 rpm. Faster makes it to hot and melts. It cuts back onto itself but comes off like crust but not welded together. I hope this helps, The cut is fairly good but we still sand a little to get all the tooling marks out. Most applications wouldn't require much sanding. If you find something that works better. I would love to find it. I have an alpha with colombo spindle. Been cutting sintra all day and will be for the next several days.
Bruce

[widgetworks_unlimited]

I couldn't find my last cut file for Sintra, but I used the same bits with great results on 1/4" thick, medium density Polyethylene.

1/4" diameter single 0-flute upcut specifically designed for soft plastics = 6 ips feed, 3 ips ramped plunge at 22.5 degrees, PC router at top speed (rated at ~20k rpm)

1/8" diameter bit = 3 ips feed, 1.5 ips ramped plunge...

Both bits cutting 0.260 depth, 1 pass - no clean up, to make sure chipload was high.

You may be able to go faster with the 1/8" bit - I don't think I tried to really push it. You could probably slow the RPMs down as well, to improve chipload - though I did get good cuts with what's listed above.

All other bits that I've tried have always left welded hairs on UHMW and the "crust" that Bruce mentions on Sintra.

[bruce_taylor]

Most of my parts are 4x4 or less and hold down was a problem with the upcut even though they produced the best cut. Your peices are bigger so you might not have the hold down issue.The straight cut doesn't lift the material and the crust is more chips packed together tight and helps to hold the parts together and cleans very easy. I go a little slow but this works for our application. I have tried a multitude of bits,

[larry_r]

Neville,
I just cut some 1/8" Sintra which I believe is the same as what you are using. I did use an upcut 1/8". I used vacuum and screwed down the outside of the work piece. The key was cutting it in multiple cuts. In this case 2. First, was .08" and second was through. Worked very well. I also used the 3d tab feature, 0.5 x 0.1. When I tried to cut it with one pass it was a mess.

Good luck
Larry

[larry_r]

Feed for 1st cut was 3.6 in/sec. Second cut 3.1. I am certain you could increase the feed of the first cut quite a bit. Router speed was 13,000.