PDA

View Full Version : Machining Plastic (HDPE)



Buzz9075
06-26-2007, 11:22 PM
I am trying to figure out how to machine HDPE. The problem I keep running into is that the plastic gathers at the top of the cutter when I do plunging or drilling and then when it goes into future holes it melts and ater several holes cause marks in the top of the plastic I am machining. I am OK when I do linear movements but the plung causes the spirals of plastic to stay on the cutter.

Here is some tests I did tonight.

g01 Z.5 f25 with my router set to 1 spindle speed cause lots of small plastic piece to gather up on the cutter.
g01 Z.5 F50 does the same thing only the parts are better.
g01 Z.5 F120 gives me real nice plastic spirals but still bunches up at the top of the cutter.

Here is the cutter I am using tonight.. I have used a few similar cutters but they all do about the same thing.

http://www.leevalley.com/wood/page.aspx?c=1&p=30217&cat=1,46168,46171&ap=1

zenbot
06-27-2007, 01:39 AM
Try ramping in on the plunge. You will have to play with ramp angles to figure out which angle works the best. Ramping helps, but it still seems to wrap up from time to time. An air blast pointed at the cutter also helps to remove the wrapped up plastic.

CNC Pro
06-27-2007, 09:58 AM
I run this stuff almost daily, proper tooling is a good start. But most importantly air blast! Makes a world of difference!

Buzz9075
06-27-2007, 10:09 AM
When you say proper tooling can you eloborate on the appropriate cutters for HDPE. Thanks.

When you indicate air blast do you mean a continous air flow pointed at the cutter, or short blasts from time to time?

Thanks

CNC Pro
06-27-2007, 05:37 PM
My favorite choice of router bits for this application are produced by BELIN Yvon s.a. of France. I’m unsure of a source in Canada, but I get mine from Integra Tooling located in Poughkeepsie, NY. Their number is 1-800-633-6312 ask for Brian.
I run my routers with a continuous stream of air on the bit. A mister would also work, but you then have to contend with the mess.
I hope this helps.

billystein
06-27-2007, 05:47 PM
try a heavy load on your drill.
something like s2000 and f20. peck about .05 - .08
you should see the chips fly off of the tool. if it wraps around it will melt.

Buzz9075
06-27-2007, 06:25 PM
Thanks, I will check in with the supplier tomorrow.

I have tried to get the load higher on my cutter by my routers slowest speed is just under 10K RMP, for which I have tried freeds of 120IPM. Which do give me two nice plastic spirals out but no matter what I do they stay stuff to the router bit... air blasting them of tonight will be my next text. Then the cutters I will check tomorrow.

Present I use a small stick of MDF to knock them of between cuts PITA.

Buzz9075
06-27-2007, 10:23 PM
Do you have a specific model cutter u use? I check there web site they have a lot of cutters available and not really clear which ones are for plastic or not. This is there home page: http://www.integratooling.com/

I tried some cuts with my up flute cutter and the air only help when cutting a slot at f5, feeds like f30 the air was not removing much. What I did was hold the air noozle as close as I could to the cutter pointing in a downward direction (and few other directions but none seemed to work well).

FatChips
06-27-2007, 11:11 PM
Ramping should help as Zenbot pointed out.
If that is not possible maybe you could try to bump up your feed rates.
My theory is that the larger chips tend to behave more like metal chips which is what most of the drills I use are designed for.
Another thing you could do is rapid from hole to hole at about 1/2" or so above the material, this will allow you to stop the machine and blow the chips off as needed. If you are running a lot of parts you could also try a carbide drill, they have a low helix which helps a lot.

One of my favorite router bits is the 52-600 series from these guys.

https://www.onsrud.com/xpost

However I am going to try this one soon and see how it compares, the wui-201-08.

http://www.robbjack.com/pdf/wood_pg4.pdf

CNC Pro
06-28-2007, 03:34 AM
Brian at integra can help you with bit selection. Be sure to tell him what type of plastic your working with, the tools have specific grinds matched to the type of plastic(probably he'll recomend a "O-flute"). I prefer to use a single flute upcut, and the smallest diameter possible (something like 3/8" dia. or less if you can do it). And don't forget the air blast.

TcomGregg
06-30-2007, 10:03 AM
One of the DOPE manufacturers reccomends Spiral drill bits with a flute angle of 20-30 degrees and with a point angle of 110-120 degrees. For deep holes they also reccomend that you do several plunges to clear the swarf and allow the material to cool.

Buzz9075
07-01-2007, 07:45 PM
Thanks for all the input, been doing lots of testing primarily with machine cuts and not holes with end mills. While I can get a straight fluted end mill to get the plastic of the cutter with air, it does not do a very good job on the moving cuts.