Machining Plastics?

[AARONIS]

I work with wood all day long but I've never machined any plastic. I'm taking a part that I designed to be made out of solid wood and transfering to white nylon. Other than the obvious feed rate modification is there anything else I should watch out for? Do I need to turn down my RPM's so I don't melt the nylon?

[Elad]

You wont melt the nylon as long as you will use you coolant and keep straight strong emulsion while cutting.

There sould be no problem.

Keep in mind that plastics are not stable and after you take it out from the machine it will be perverted.

[richardtraver]

NYLON ISN'T HARD TO WORK WITH BUT, THERE'S OTHER PLASTICS THAT LOOK BETTER WHEN MACHINED LIKE DELRIN. I CUT MOST PLASTICS ON A MINIMILL AND THE NORMAL SPEED IS 60 IPM @ 6000 RPM FOR TOOLS BETWEEN 3/16 - 1/2 BY 1 OR 2 DIAMETERS DEPTH OF CUT. 3/8 - 1/2 CAN USUALLY HIT FOUR DIAMETERS FULL WIDTH AT THAT SPEED. FOR DRILLS I SLOW IT DOWN TO 2500 RPM @20 IPM FOR ALL DRILLS.

[AARONIS]

I'm not so interested in the look but rather the usefullness. I need something that will hold up to abuse. I'm using it to machine some vacuum pods. There other thing is that I don't have a flood/coolant system. The only thing that I could do is hold air on the part/tool to keep them relatively cool.

[Guest]

What kind of tooling are you using?

[Guest CNC Apps Guy 1]

You should be using HSS because your tools have to be SHARP and carbide just is not sharp enough.

 

JM2C

[AARONIS]

I will be using mainly carbide endmill's.

[Guest CNC Apps Guy 1]

You'll be sorry. You're going to melt that stuff and make a mess.

 

Experience is what you get when you don't get want the first time.

[Dan_AKA_ROY]

quote:

---

You should be using HSS because your tools have to be SHARP and carbide just is not sharp enough.

---

Learn something new everyday. HSS sharper than carbide. Never knew that or to think to give it any thought. When machining renwood, especially on flat surfaces, it pits if you don't slow down you feed rates. I've machined various plastics on my router over here and had always used carbide bits. It does melt if you don't constantly cool it and sometimes melts a little anyways.

 

I would take James advice on this one. He knows a little bit about this kind of thing!

 

I wonder if changing from carbide to HSS while machining renwood, I can increase the feeds without pitting? I'll have to experiment on that one.

[Philcott]

Aaron,

 

Check out this thread. Some really good nylon info.

Nylon

 

Phil

[AARONIS]

Am I going to melt it because I don't having a cooling system or because I'm using carbide?

[Guest CNC Apps Guy 1]

Both. The reason the carbide will melt it reason 1 is because of the nature of carbide, carbide is "Powdered Metal", even the finest micro-grain carbide money can buy is still substantially "duller" (is that a word???) that HSS because HSS is actually steel that has and can maintain a razor edge, which with nylon is ctitical. NOw the heat, because carbide is essentially "rubbing" the material off, it generatea a lot of friction.

 

JM2C and HTH

[Travis_Buchanan]

Not to dispute, but I cut some seaboard the other day using a solid carbide router bit. It did very well. 9000rpm 200imp conventional cut. chip load cools tools. Router bit geometery differs from endmills. Relief angle is greater resulting in less rub. at least IMHO.

[Guest CNC Apps Guy 1]

Relief is very critical. If you absolutely positively have to use carbide... gotta be High Shear...

[Lucky]

Use Delrin as your material. It is much more forgiving than other plastics of "bad" technique. You can use standard carbide tools with no coolant and get excellent results. I love the stuff.

[Bruce Caulley]

I machined plastics exclusively for nearly 10 years. Use air to remove the chips from your job if you dont have coolant. A spray bottle is a good idea if your machine is open and you need some coolant on your drills. Tip when drilling is to spin it slow eg 1200 rpm and 700mm feed with a 4mm peck. This will work all day long with no coolant. If you are making vacuum pods for a router I would not suggest using delrin. I have used these on a morbidelli router as well as milling machines and they always ended up cracking after repeating loadings with heavier full sheets of material. Nylon is fine as long as does not have a filler to complicate things. HSS definitely works better, but if this is not a production run don't worry about it. Carbide woodworking routers can be usefull but you might need to increase the relief a bit.

[AARONIS]

I was given another alternative material recently....(UHMW) Ultra-High Molecular Polyethylene. Good/Bad. It seems to have a higher melting point and possibly higher tensil strength.

[Gary]

cut delrin most of today. 9600 rpm and 300imp with 3/32 2 flute carbide ball em. stuff cuts like butter dry or wet. Nylon is not near as cutter friendly also watch how you enter exit the part so it doesn't chip your part.

[billystein]

I have found that drilling is better if you double your normal chip load. It seems to evacuate the chips better. If the chips don't come off of the tool they will cause many problems.

[Bruce Caulley]

UHMW is very soft. Cuts like butter.

[AARONIS]

I machined the nylon the other day and it wasn't as bas as I thought. I was running 18,000 RPM with a slow FR. Came out great, no problems what so ever. I also received some billet UHMW and will machine it later today.

[mold100]

quote:

---

running 18,000 RPM with a slow FR.

---

Can I ask why a low feed rate, or why such High rpms, maybe small cutter?

 

I prefer delrin over most other materials, 2 flute high shear tin coated HSS is preferable, with air 3/8 dia in old matsurra at 7800 rpms 75 ipms .1 to .3 doc for roughing / semi.IMO (whatch leads ((in and out)) for chipping)

[AARONIS]

Well the main tool I'm using a 12mm 2 flute endmill solid carbide, the part is detailed and needs to be fairly precise. Other than that the machine is capable of high rpm's and gives me a clean cut. Also the low feed rate has to do with the vacuum table. The parts tend to break the seal if my feed rate is too high.

 

I've been looking into delrin, nylon and uhmw polyethylene. I've been told that the uhmw is going to have relatively slick surface.

[Jim at Gentex]

AARONIS,

I cut plastics almost every day. There is some good advice in this thread I would like to elaborate upon.

 

As mentioned, Delrin is an excellent material choice for stability, durability, and machinability. The 500 grade is nearly as tough as nylon without the machining drawbacks. We use Delrin 100 and 500 for probably 80% of our prototyping needs in our R&D shop.

 

That said, if you MUST use nylon, be careful. As advised here, melting is an issue. Not having a coolant system on the machine is a real drawback. I have a cheap little pneumatic mister that I use for Bridgeport work that needs a bit of coolant. I just fill a coffee can with Hangstefer's and the mister spritzes it onto the tool with a low volume air flow. It's a bit messy, but it works well. Blowing air on the cutter will help, but you really need the liquid coolant to keep the tool and the nylon temps in check. Obviously I always try to do my nylon work on my CNC's with flood coolant whenever possible.

 

James Meyette's observation about HSS cutters is accurate. They do seem to hold up a bit better than carbide, and they need to be SHARP to cut nylon properly. You will see your dimensions go south in a hurry when the tool gets dull, especially a carbide tool. I would add that the TiN and TiCN coated cutters seem to hold up better over the long run and are worth the few extra bucks if you need to machine a quantity of parts.

 

Lastly, a word about dimensional stability. I don't know what kind of tolerance you are looking for, but if it is an issue then you should know that nylon is notoriously finicky when it comes to close tolerance work. Especially in the area of drilling / reaming close tolerance holes. I will almost always mill and bore a close tolerance hole whenever possible rather than drilling and reaming. No matter what you do, it seems as though the hole contracts the second the drill or reamer withdraws resulting in an undersize hole. Even with a brand new drill and reamer it seems to be a challenge to hold size accurately. If tolerance isn't an issue then you needn't worry about it...I just thought I'd mention it. Good luck with your project.

[AARONIS]

Thanks everbody for the help.....