PDA

View Full Version : endmill specs for foam milling ?



max_imum2000
12-23-2006, 09:03 PM
i need so answers on these questions please

1. what are the best endmill i can use for foam milling ? ball, ..etc
2. how deep should go in each path ?
3. what speed should i use ? lower or higher is better ?
4. what travel speed it better ?

thank you in advance

afmcorp
12-24-2006, 05:43 PM
Hello

you forgot one more question and that is which type of milling. climb milling or conventional milling.

1. what are the best endmill i can use for foam milling ? ball, ..etc

well i would start with a 2 flute centercut for plunging. foam is plastic and is subject to heat. if you have any heat build up you will ruin the finish. the thing i would look at is using a HIGH VOLUME OF AIR to keep any chips from sticking to the endmill and clogging up the flutes. once the flutes are clogged you'll only be burning the foam. as for ball end or square end that will depend on what you're machining i.e. curved surface or flat or 3D. this will also dictate what size. you'll want the biggest endmill that you can use but your geometry will tell you the actual size. as for type of milling climb or conventional your material will tell you. make a few cuts to see how the foam comes off. does it leave a clean surface or is it raggity. so then you can program around that.

2. how deep should go in each path ?

don't be tempted to go too fast and too deep. use the same basic rules as you would for metal. go less than 1/2 the diameter for side milling and less than the diameter deep.

3. what speed should i use ? lower or higher is better ?
4. what travel speed it better ?

these 2 questions should be qrouped together. based on load per tooth and the rpm you will dictate what the feed rate is. rpm is judgement. take those test cuts and visually decide. too fast will burn too slow may rip so you need to do some test cuts. the foam material i'm assuming is not a tuff cut. so you can likely make a fairly heavy feed rate. i know that when i cut a solid plastic i run up to 3000 rpm with a 2 flute maybe somewhere between 10 to 20 ipm. just depends how much i have to do. these speeds are more for a smaller end mill say under 5/16" [8mm].

do your tests then decide. you might also check out the niagara endmill site. they may have a chart on your material.

good luck

fractaledge3
12-25-2006, 08:21 AM
Hi,

What type of foam you use? white or blue, also what type of milling? 3D or just cutting.
Then I can give you some surprising answers.

max_imum2000
12-25-2006, 03:16 PM
hello
and thanks for your reply.
by the way i have sent you an email before but i didnt get any answers from you, or maybe i did and i over looked it .
well
i use blue and white foam. (well anything i can find over here)
and i am using engraving , not cutting

actually i wanted to make a foam hot wire cutting and independent axis but i wanted to use a turn table to produce real 3D shapes, but i couldnt find any software to handle this.

so i went to making a foam milling instead

so what do u think ?

kol sana wenta tayeb, we 3eed sa3eed

fractaledge3
12-25-2006, 04:20 PM
Hello,

Kol sana wenta tayb, I received your Email and replied to you but I didn't get answer from you.
I am not using end mill for foam cutting or engraving , I am using a plane rod instead (like nail or end mill shank) with 20,000 router RPM , but when I need 3D milling I use rounded tip rod or V shape tip rod, also you can use wood carving tools (rounded or v shape).

swagman
12-26-2006, 04:41 AM
i use rotary burs . they give great finish and can be run quick.

fractaledge3
12-26-2006, 04:46 AM
i use rotary burs . they give great finish and can be run quick.

Hi swagman,
What rotary burs looks like

Sparktech
12-26-2006, 11:12 AM
Hi. I've found that standard metal cutting endmills don't have the correct flute geometry to do a real good job in foam (or wood). Foam and wood tools require a higher rake angle and smaller core. Look for some wood or plastic endmills, and they should work fine. I've never tried the routers, but I would think one of the single flute router type tools would also work. Hope this helps.

swagman
12-26-2006, 03:28 PM
i will try to get pic up for you. they work really well, don't rip up the foam.

fractaledge3
12-26-2006, 04:19 PM
Thanks Swagman.

swagman
12-26-2006, 10:13 PM
2 pics of rotary burs used for foam cutting.

fractaledge3
12-26-2006, 10:53 PM
Hi,
Many thanks. The photos show every thing I just can't get the meaning in English, Yes I used it before to engrave also in colored rubber foam.

swagman
12-27-2006, 07:21 PM
i use these to cut patterns for vac forming. we use poly styrene foam. we use epoxy resin and mat for the actual former. i cut at 4000 rpm with up to 500 mm per minute feed. they do exelant job.

thinkntink
12-27-2006, 10:18 PM
When you are cutting plastic foam, a great deal depends on the rigidity of the material being cut. High rigidity (like styrene and HDU) allows a cutter to develop high cutting shear at modest chiploads. Spongy, flexible foams need MUCH higher feedrates to achieve clean cutting.

Generally speaking, burrs do not have enough flute volume to allow debris evacuation at high chiploads. High rake 2-flute or 1 flute end-mills are by far the most effective tools for 3D foam carving.

Let's say you are carving a fairly large model so that you can use a 1/4" (6.35mm) dia ball cutter (picture attached). Also assume that you are plunging 20mm on each pass. If your spindle can turn 10KRPM you should cut styrene or HDU (high-density-urethane) foam at approx. 5 meters/minute. Anything much below this may melt the material to the bit and damage your model.

If you are cutting a more compliant material like ethafoam (polyethylene foam) or die ejection rubber foam with the same cutting parameters, you would want to use a feed rate of 10 to 12 meters/minute.

In any case, a VERY high shear cutter is called for.

It is pretty easy to determine the best feedrate to use with any soft material (not stone or metal). Go to:

http://www.precisebits.com/tutorials/calibrating_feeds_n_speeds.htm

Generally speaking, it is better to feed too fast than to feed too slow when cutting any thermoplastic material. For a case study on cutting a material similar to sheet styrene, go to:

http://www.precisebits.com/tutorials/machining_thermoplastics.htm

shrthang
12-28-2006, 12:49 PM
I've been custom cutting foam for over 10 yrs now and there is no question experience is the best guideline. For every material I cut, I've done trial runs to experiment with different feed rates and plunge depths. EPS is the common foam I use and I've run my 1" dia x 12" long 4 flute custom bit at 100% stepover at 6" deep, sometimes deeper. When you're manufacturing, cutting time is important. Hogging away as much material as you can with a large dia tool and then finishing with smaller tool is the way to go.

The two flute bits that thinkntink shows work great, but when you get into larger cuts, getting custom made bits designed for foam cutting is the smartest thing you can do.

If you want to see some interesting foam cuts, check out my site at www.revolutionaryminds.com.

If anyone has questions on hotwire cutting, I'm also very experienced in that department.

shrthang
12-28-2006, 12:57 PM
Rotary burs do work great as well for providing a very nice finish. Having a good vaccum system is very important when cutting foam, especially with rotarty burs because of the fine offcut particulate that will build up on your gantry and spindle because of the static build up. Ensuring that your table is excessively ground is a good idea. Foam can build up a tremendous amount of static when being cut and can cause your system to crash or even scrambles the program and can make your machine do some crazy and dangerous things.

When I first started cutting foam on a large custom built CNC table, it did some crazy things. It would race across the table and dive down through the bed. I was just lucky the custom bits were 1" dia and very durable. Once I got the grounding issue dealt with, I never had problem again. Foam building up on the gantry can be bad, because if it get into the teath for the cog and continually compressed, it turns to a hard plastic and keeps building up and puts torque onto the cog and it will eventually snap off.

thinkntink
12-28-2006, 02:41 PM
To Shrthang

Very nice models in your gallery. What feedrate and RPM (or chipload) are you using when doing deep hogging?

shrthang
12-28-2006, 04:33 PM
The feed rate when using the 1" dia 12" long 4 flute custom bit, was approx. 6000 rpm and the feed rate would be between 100 and 200 inchs per minute. If I dropped down to a 1/2" dia bit, I'd increase the rpms to 12,000 and the feed to 200 in/m.