I have access to ShopBot Desktop at work and I decided to build a big slow flying foamie to bring fun to the office (small coaxial helies other guys are flying are pretty lame).

So, I made a simple vacuum table to hold foam sheets and tried milling a paper backed foam board from Dollar Tree store, before risking good Depron sheets. The vacuum table worked remarkably well, but the cuts came out pretty poorly, the surface quality is nowhere near what I expected... I used a quarter inch bit spinning at 12,000 RPM with 6 in/sec move speed and 4 mm cut depth (being new to CNC, I'm not sure if I'm using the right terms).

What should I do to mill Depron better? Should I increase the spindle RPM? I guess I can go as high as 25,000 RPM. Or reverse the travel direction to ensure downcut operation?

Looking forward to your tips,
Boris

Hi Boris. If you're really moving at 6in/sec (360 inches/minute or IPM as it's commonly referred to), that's extremely fast, and I suspect you're tearing the foam more than you're cutting it. If it's good, uniform texture foam (e.g. not something with "chunks" like plain old styrofoam), you should be able to get it milling fairly well, but you'll want a much lower movement speed (this is usually referred to as "feed rate" in the CNC world, while "speed" is your spindle RPM). 12K RPM should be okay but you need to crank the feed rate way down - try something like 60-70 IPM. I'm assuming you have a nice, sharp bit in your spindle, carbide is best but high-speed steel would probably work fine as long as it's sharp. Good luck, let us know how it goes!

-John

A plain router bit made for cutting wood is ok, if sharp. Usually they are harder to find in small sizes. I often use the Rotozip 1/8" bits since they are easy to find locally. The tile cut bit works good. Also I have had good results with the Sabercut bits in foam. I usually mill with these bits at about 7,000 rpm, and 70 inches per minute. Depends on the foam. I usually set the feed to 70 ipm, since that is the fastest I want to run the machine. Then do a test cut, and turn the rpm down until the foam cutting sounds good, (sort of a slicing sound). To much rpm for the feed rate, and it melts the foam. Not good since it builds up on the bit, and makes a ball on the end of the bit.
http://www.homedepot.com/h_d1/N-5yc1...&storeId=10051
Here is a video of my mill with the 1/8" Saber bit milling Owens Corning XPS pink foam.
http://www.rcgroups.com/forums/showthread.php?t=1427681

Thanks a lot for all the suggestions!

I'll try reducing feed speed first, then will switch to 1/8" bit and lower RPM.
All our bits are brand new (we've just got the machine and my vacuum table was the first real part made with it) and I can order others.

Boris

Your router might be limited to the lowest rpm it can run at. If you have to run a high rpm you might need to get some much smaller router bits. I use many small sized fishtail chipbreakers. they cut like the foam is not there. This company sells good endmills.
http://www.precisebits.com/products/...s/fcrouter.asp

I tried cutting Dollar Tree foam (without paper backing) at 1 in/sec feed rate, 12,000 RPM speed, and the same 1/4" straight bit. The cut is much better quality than before! The bit is clean, no molten plastic--so far, so good.

I will try some bits from PreciseBits next.

Thank you for your help,
Boris

Originally Posted by bluesky123

I tried cutting Dollar Tree foam (without paper backing) at 1 in/sec feed rate, 12,000 RPM speed, and the same 1/4" straight bit. The cut is much better quality than before! The bit is clean, no molten plastic--so far, so good.

I will try some bits from PreciseBits next.

Thank you for your help,
Boris

was this done using climb milling or standard? when milling depron the direction is critical to the finish. if this was using climb milling try the same settings and standard milling.

Also, I use dedicated bits for foam use. they must be sharp to achieve a decent finish. Check out Onsrud for downward spiral bits for cutout toolpaths. I use 4 flute un-coated for milling.

Originally Posted by RCROBBY

was this done using climb milling or standard?

Not sure, the tool path was generated by Autodesk's online CNC Utility, http://www.123dapp.com/, and I haven't look at it closely... Will do this next.

Check out Onsrud for downward spiral bits for cutout toolpaths. I use 4 flute un-coated for milling.

Which of the many bits on this page would you recommend for depron:
http://www.cncroutercentral.com/CNC-...ts-Downcut.asp

Which tool diameter do you use? It looks pretty small on your picture...
Why using small diameter bit is advantageous? I though that, if the large fillet at the corners isn't a problem, bigger bit would be better, since the cutting speed will be higher. Or do we want to have as low cutting speed as possible, thus small tool adds to this?

Sorry for all these silly questions, I'm so new to this whole CNC milling... But I love it so much--your 3D model is converted to a real thing with such high precision!

Thank you,
Boris

Originally Posted by bluesky123

Not sure, the tool path was generated by Autodesk's online CNC Utility, http://www.123dapp.com/, and I haven't look at it closely... Will do this next.


Which of the many bits on this page would you recommend for depron:
http://www.cncroutercentral.com/CNC-...ts-Downcut.asp

Which tool diameter do you use? It looks pretty small on your picture...
Why using small diameter bit is advantageous? I though that, if the large fillet at the corners isn't a problem, bigger bit would be better, since the cutting speed will be higher. Or do we want to have as low cutting speed as possible, thus small tool adds to this?

Sorry for all these silly questions, I'm so new to this whole CNC milling... But I love it so much--your 3D model is converted to a real thing with such high precision!

Thank you,
Boris

Here is the Onsrud bit I use for cutting: http://www.cncroutercentral.com/CNC-...its-57-600.asp

the bit in the picture is one of my milling endmills. I think it was 1/4". Your design will depict the maximum size endmill you can use. My spindle can be setup to take 1/8" shank up to 1" shank though most of my tooling is 3/8". I have milled foamies (the pockets) at over 120IPM no problem though I usually keep it about 80 IPM. I also set up index marks so I can mill on the CNC and final cut on the laser .

I have milled alot of foam. Rohacell, Herex, XPS, etc. Normally I feed at around 80-120ipm depending on the foam particulars. I always try to cut with a 1/4 tool, typically a four fluted radiused endmill. Alot of the advice above could have saved me much grief over the years... used dedicated bits, downspirals for cutouts, etc.

My mill spends most of its time at lower RPM settings in foam, like around 8k. If you go much higher and don't increase your feed rates, you are probably burning and melting the foam as much as cutting it.

I get alot of bits from lakeshore carbide... www.lakeshorecarbide.com. They have a great selection, decent pricing and excellent service.

Tom,
100 ipm -> 2.5 meters per minute? A did so for a long time and it's way too slow for me.
Now having a new fast machine I go up to 6 meters per minute.
Btw how do you find milling the Herex in comp with Rohacell and XPS?

I have to keep a sharper tool. Rohacell can be miller even with dull tools for good results. Herex can tear and chunk.

Originally Posted by ViktorF

Tom,
100 ipm -> 2.5 meters per minute? A did so for a long time and it's way too slow for me.
Now having a new fast machine I go up to 6 meters per minute.
Btw how do you find milling the Herex in comp with Rohacell and XPS?

Your correct at the math. I wish I could run as fast as your machine. My mill has to much mass. I can feel the house shake when it turns around at 150 ipm. So been limiting it to 70 ipm.

I had to build light belt driven cnc router. Trading the stiffnes and precision for speed. No need big precision for foam.

Thank you all for good advice!

I bought a downspiral bit, switched to upcut path, and reduced the feed rate to 2 cm/sec. The results are amazing, 3 mm Depron cut with 0.3 mm remaining layer.
I'm a happy CNC-er now!

Boris