[WarrenW]

Hi,

I just about finished my first wood cnc router and am just curious what people cut foam for? What is it used for? I can understand the wire for cutting foam for stuff like model airplane wings, etc. But to use a router, what is the foam shapes then used for?

Warren

[JPMach]

I've cut a couple of big pieces of foam in my vmc. The guy I made them for wanted to proof out a computer model of a bike seat and make sure the fit was just right before spending a lot of money on an expensive mold. The foam comes out to less than half the cost of aluminum and you can pretty much go full speed at some incredible depths of cut (.5"+). It is fun to machine but a real mess to clean up.
I get my foam from goldewest mfg out in CA.

JP

[ViperTX]

You could also use foam for "lost foam casting"...check out http://www.buildyouridea.com

[JPMach]

here are some pics of foam being machined

JP

[plexer]

We use foam in school in our cnc router as an inexpensive material for the students to use we got our current stock of it for free and it machines fast so not much waiting around.

Ben

[Geof]

You could also use foam for "lost foam casting"...check out http://www.buildyouridea.com

The foam used for making prototypes such as JPMach shows is most likely polyurethane which can be made in a variety of densities and machines okay.

The foam used for lost foam casting is polystyrene, this quote was copied from a website describing industrial scale: "Lost foam casting is a process in which a polystyrene pattern of a component is produced, coated with a refractory, placed in a flask and surrounded with loose molding media (such as sand) to stabilize it. Then, molten metal is poured into the flask, vaporizing the polystyrene pattern and replacing it to form its exact shape."

[JerryFlyGuy]

Glad to find this thread! I'm actually building a router for only cutting foam. However I'm no machinist and don't really know what feed speeds to design for. Someone passed a link on to me for General Plastics which showed that you could mill their foam at up to 250 ipm. Is this really a realistic number to shoot for? How fast have you guys gone to w/ your systems? Any guess as to a safe number to plan for? Would a 250 ruff cut and 400 ipm rapid machine be ridiculous? The foam I plan to mill is slightly different from the general plastic's stuff [ however I may be doing some of that also] but is should be pretty close to this, its only 2# density].

JerryFlyGuy

[JPMach]

I rough cut 20# density foam with a .75 4 flute @ somewhere around 3500rpm and close to 300 ipm with a .500" depth of cut. I think my finish pass was around 4500 rpm and just under 300 ipm. So you can see that with these chiploads at the spindle speeds you could run in a router you could run around 600-800 ipm. I did hear though with some of the foams that at higher spindle speeds you risk melting the foam and ruining everything.
I have to cut some again in a week or two and am going to try higher speeds and feeds, will let you know how fast I get it to. I think it can handle a pretty fast speed it's just my heart that might not be able to. With that kinda feed in foam you get a pretty thick and long rooster tail coming off the bit. It is also a real mess to clean up as it clings to everything. The higher the chipload you can handle the more the dust turns into shavings that aren't so bad to clean.

JP

[Geof]

JPMach;

Have you ever used a two flute cutter? Double your chipload for the same speed and feed and maybe reduce the dust level? Also if the heavier chip carries off the cutting heat more effectively as it does with solid plastics maybe run both speed and feed higher?

[JPMach]

I haven't yet tried a two flute but I might. The one problem I did notice before is that if you try to get to high of a chipload it is very easy to get chipping on the edge of a part, so you have to watch what you're doing.

JP

[JerryFlyGuy]

I rough cut 20# density foam with a .75 4 flute @ somewhere around 3500rpm and close to 300 ipm with a .500" depth of cut. I think my finish pass was around 4500 rpm and just under 300 ipm. So you can see that with these chiploads at the spindle speeds you could run in a router you could run around 600-800 ipm.


JP

JPMach, so during these cuts what was your step over? Or were you going the full 3/4"? This is just what I wanted to hear.. I was starting to think that my system was way over on the speed and way under on power to put the tool through the foam.

Can you tell me what your system is running as far as stepper power [ or servo] and your screw pitch as well as is it acme, ball or what ever else type of screw? I can then figure out how many # force it is taking you to push the tool through the foam, I suspect its very little but I just want to confirm this.

Thanks!!
JerryFlyGuy

[JPMach]

My machine is a Haas Vf-4 with 20 hp spindle with two speed gear box. Although when cutting foam the load meter barely moves. It runs on linear ways with ball screws. I believe the ac servomotors are rated for 2500 lbs but they rarely get to full power except when rapiding. As for how much power they were using while cutting I couldn't tell ya but I know it wasn't much. The stepover I was taking I believe was about .730" just enough to ensure a clean cut. I probably could have taken deeper depths of cut but I didn't want that big of steps left on my 3-d surface. I think the ball mill I used for finish was running about .030" step over. Then with just a light hand sanding it was as smooth as glass.

JP

[JerryFlyGuy]

Thanks JP, I can see that figuring out how much force it would take would be pretty tough, does the 2500lb's mean thats how much force they can deliver? or is that some type of torque number? I would guess however that if I can produce say 25% of what your's can [ assuming thats 2500lbs force] that it should create no problems in running at a similar speed! Theoretically mine should be able to produce 800# force in the x and 400 in the y and the z all during a 400ipm rapid. I don't plan on having as big a spindle as you do, I was thinking more in the 2-3hp Variable speed router this to could have some effect, I would guess, on the feed speed.

Jerry

[JPMach]

According to the Haas website that is 2550 lbs max thrust rate on X and Y and 4200 lbs max on Z. With rapid travels of 1000ipm and a max load of 3500 lbs on the table I would say they would be fully loaded.

JP

[Geof]

Quote from JPMach; "My machine is a Haas Vf-4 with 20 hp spindle with two speed gear box".

It is pretty safe to say this machine is not working hard machining foam

Jerry;
If your drives can give you rapids of 400ipm with acceptable acceleration; i.e. you don't reach the end of the travel before you get to speed, they will have plenty of push for foam. As JP says the servoes only get near their maximum load during acceleration, cutting is always much lower. Also if you are climb milling the work is pulled into the cutter (well with Aluminum that is the case with foam probably less so) so your feed drive is actually holding back sometimes rather than pushing.

JPMach;
Did you notice any difference in edge chipping between climb and conventional milling? I am picking brains here because later this year I will probably be doing some large vacuum forming or fiberglas layup molds in foam on a GR510. It is much more efficient to learn from another person's experience

[ger21]

I cut wood, but at work we cut up to 1" thick partical board and mdf at 400ipm. I could probably cut foam twice as fast.

[JPMach]

Geof;
You're right when you've got a machine that can handle mold steel with ease, it doesn't even know its cutting anything when running foam.

As far as chipping I didn't notice much difference but it seems to me that conventional caused more as it forces the chip out in more of a pushing action when leaving the foam. When entering the foam it seemed like just the oppisite was true. You either have to spend a lot of time programming to get around it or just leave a little more for finish than normal and it should clean up. The best thing I found so far is to start with a piece that is plenty big enough then if it does chip it doesn't matter cause you're coming back later and removing it any way.

Just my two cents
JP

[JerryFlyGuy]

Jerry;
If your drives can give you rapids of 400ipm with acceptable acceleration; i.e. you don't reach the end of the travel before you get to speed, they will have plenty of push for foam. As JP says the servoes only get near their maximum load during acceleration, cutting is always much lower. Also if you are climb milling the work is pulled into the cutter (well with Aluminum that is the case with foam probably less so) so your feed drive is actually holding back sometimes rather than pushing.

Geof;
Well the platform for my system is 20' x 10' so hopefully it will get to rapid speed before the end Actually if I calculated things correctly and I keep my gantry under 350# overall it should go from 0 to 400ipm in 0.25 seconds.. the bigger question is if the rest of the structure can take it.. It's all fab'd from [ the gantry] 3" and 4" sqr tubing. The main bed sits on the floor and is from 5 x 3 .250 HSS tubing with channel cross stringers. The gantry runs on 24 bearings running on the age old angle iron rails [ on each side of the bed rails -4 angle irons total] however if this turns out to be no good, I plan to mount 3 x 1 CRS and use that as a rail. The motion side is all rack/pinion style stuff the other question I'm working through is weather I'm gonna blow my pinion due to overloading it when I rapid or do really heavy cuts.. [ not likely to happen in foam but possibly in wood/MDF if I ever do any] I'm going to most likely anchor it to the floor [temporary until I get my work shop built- then it will be leveled, grouted and anchored]. What do you feel would be an acceptable accel rate for 0 to 400? I'm no machinist so.. I just built the biggest, badest & strongest I could afford... not nowing what an acceptable limit would be.

JP;
Thanks for all the help! I've finally got some great answers that I'd been searching for, for a while now. I'll have to post some pic's some time when I get this thing all built..

Also another question for you guy's, any of you use CAM systems that will let you "over" cut your part [ not "undercut"] so that the part is actually smaller than the model you pulled it from, and needs to be built back up? Weird question but.. this way I can put a finish on my foam and re-machine it to its proper size and have a nice sealed, hard and durable finish. I've been looking at onecnc but have never check to see if it can do this yet.. gotta get my demo booked

Jerry

[ger21]

Also another question for you guy's, any of you use CAM systems that will let you "over" cut your part [ not "undercut"] so that the part is actually to small, and needs to be built back up? Weird question but.. this way I can put a finish on my foam and re-machine it to its proper size and have a nice sealed, hard and durable finish. I've been looking at onecnc but have never check to see if it can do this yet.. gotta get my demo booked

Jerry

Just tell it your tool is smaller than it really is.

[JerryFlyGuy]

Just tell it your tool is smaller than it really is.

That's 1 way of doing it, however I could see that producing other issues due to tip radious of the ball end etc, might work.... however I was thinking more of a setting.. I looked at visual mill's demo, you can specify in it how much you want to leave for your finish work, so normally you'd enter..say 0.010 or something.. could you enter -0.010? or would that produce an error?

Jerry