Machining a Foam Mold

I have a project that I need to get started soon. I will be machining a mold out of a 24"x24" foam block. The foam is 15 lb/cf density. I will be cutting it on a Doosan 5700 with a 12K rpm spindle and I can get whatever tooling is recommended. The machining will be roughing, then 3d surfacing. The end product will be a mold for carbon fiber layup so I would like to get a decent surface finish so there is minimal sanding involved. I have experience with almost every type of material but foam, so I would like everyone's input on speeds and feeds or any tips that the collective has.

You can run the spindle as fast as it will turn. Keep a decent feed at least 0.005fpt. Biggest problem we have had is cutters getting dull and Z axis depth. (Machining foam you could have a cutter 2' long if you had the travel).

706jim said:

d Z axis depth.

Click to expand...

Z axis won't be a problem, the block is 2" thick and the mold at it's deepest point is roughly 1.5" deep. Sounds like the foam is fairly abrasive on the cutters?

Hi lastrada:
Do you know what kind of foam it is?
There are a lot of different foams with a lot of different properties, so it's worthwhile to know what you're up against.
Also you will need to find out if it's open cell or closed cell foam, and how you manage it will depend on what it is.

I assume you don't get to pick what material...if you did, I'd recommend considering a product called Renshape.
It's used to make foundry patterns and mills like a dream but makes a helluva lot of dust..
It's also more rigid and dimensionally stable than foams tend to be and holds detail better.

Last, you might need to get a cold air gun or knock together an air blast nozzle...if you just flood cool it you're gonna make one helluva mess, and if you run it dry you might end up with a big melty blob on the end of your cutter.
There are lots of foams that can be cut dry at reasonable feedrates but not all of them.
You might also need to bodge together a vacuum system to suck up the crap as you make it...if you don't your co-workers may never forgive you.

The very last point; if the material turns out to be abrasive enough to be a problem, you could look into PCD cutters or diamond coated cutters like the guys who cut graphite EDM electrodes use.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Flute count, dust evacuation, thermal growth control or adjustment if precision is needed.

Don't air blast, try to set up some vacuum hoses that travel with the head (get the routing right!) to pick up dust as you go.

And no coolant. Disconnect the pump so you can't accidentally turn it on. If you must have it on due to spindle cooling, turn off all the head nozzles or in some other way protect the part.

Yes abrasive wear on the cutters. Another vote fro Renshape if you were given the option. It cuts beautifully but is god awful expensive.

implmex said:

Hi lastrada:
Do you know what kind of foam it is?

Click to expand...

The foam was supplied to me so I don't have a choice there. Here is what I'm working with.

https://nebula.wsimg.com/cc8a1a379f...C6B26FE864D509590&disposition=0&alloworigin=1

Milland said:

Don't air blast, try to set up some vacuum hoses that travel with the head (get the routing right!) to pick up dust as you go.

Click to expand...

I'm working on a vacuum system right now as I definitely don't want any foam or dust to get into my coolant system. I have a standard shop vac I'm trying to incorporate into my mill. I also thought about taping some plastic sheeting inside to help out there.

Also I'm here looking at the Onsrud cutter website, there is a lot to choose from. Up-cut, down-cut, flute count, like I said I have no experience with foam, what works better? More flutes, less flutes? Does the up-cut help with chip evacuation? I'm treating this as a learning process

Hi again lastrada:
I've never used that product but it sounds like a standard urethane prototyping board.

What surprises me most about the block chosen by your customer is its low density.
The "Butterboard" I'm most familiar with is about 48 lb/cubic foot and is pretty good to machine.
Renshape 460 is about the same and is also urethane based.

I don't think you'll have any issues at all; use whatever cutters you have in stock (brand new and sharp is helpful to get a nice finish) and just go to town.
Disregard all my blather about needing a cold air gun but definitely invest effort in sucking the dust up as you make it.
If you run aggressive chiploads you can get it to make more chips than dust so play with it in the roughing until you're happy.
Look up some UTube videos to get you into the ballpark for speeds and feeds.
Here's one:
CNC Router Making Molds - YouTube
I think he's going a bit pathetically slowly in the roughing but it's a starting point.
Just remember though, that you can break out chunks if you push it too hard, so if you have little details or unsupported ribs and thin walls, prepare to go gently there and you'll be fine.

Cheers

Marcus

Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

One trick if you have to do some sanding-type handwork is to use a piece of the same foam instead of sandpaper. It's a lot easier to control the rate of material removal. That is a fairly lightweight foam for molding purposes. If your customer is also new to this game, I would make sure you have some good indexing features in case you have to put it back on the machine to re-machine the cavity, coat with Featherfill and re-machine that to get the finished surface restored.

I'd suggest more flutes, as you're likely limited by RPM rather than HP or materials cut properties. With a tooling material, you can get away with a weaker flute that's part of a higher tooth count with bigger gullets, if the option is available in your needed configuration.

Large Square edge for roughing, bull (with a largish radius) nose for semi or finishing, and a ball for detail finish if needed. It sounds like you can use a bull unless you've got fine details or geometry requirements that call for a ball.

A hard coating that still leaves the flutes sharp will be good, DLC if possible. I think you won't need a PCD cutter unless it's a glass-filled material, which it doesn't sound like.

I machined some stuff like that, but it was cores for composite parts, not molds. So it was lower density. I think the 'heavier' stuff was 6 lb/cf. It cut nice with 2 flute carbide, and I'm sure HSS would have done just fine as well. I don't remember it being 'abrasive'.

Here are some ideas to consider:

Creating High Quality, Reusable Molds with CNC Machined Foam and Stretchelon Bagging Film – aka “The Method” | Better Living Through CNC