Bit for HDPE?

[Terry Davis]

What kind of bit do I need for cutting parts out of 3/4 HDPE - High Density Polyethylene. These parts will have dados, dovetails, slots and line boring. They are foe outdoor cabinetry.

[Damon Nabors]

Terry,

We cut some 1" UHMW last night and found that we had to slow the bit down to 300ipm. Snapped a 1/2" Vortex Viper compression like butter (ouch!!!!!) Also only cut .25 depth at a time to clear out the shavings to prevent them from packing back down in the dado and melting back together.

I think HDPE is softer than UHMW so feed speed may not be as big an issue, but I would think the melting/heat would still be a factor. It is also pretty slick and wants to move on the table.

If I get much more request for cutting plastic, I am going to try an O'Flute router bit. I have read that they are the preferred bits for plastic.

Good Luck,
Damon

[Terry Davis]

We ended up calling a Tech at Vortex Corp. and he said to use a 4200 series 2 flute upspiral cutting at 350 ipm at 16,000 rpm spindle speed.

[Michael Kowalczyk]

Hey Terry,
We use a 1/2 Viper with mortise tip to cut our HDPE all the time. Now we do not go all the way through but cut 3/8" in a 1/2" board at 700ipm+- with out a problem other than the occasional birds nest that will free it self typically. You may want to use an upshear on your 1st pass and then use a down shear for you onion skin pass. I would also talk to Greg at Courmatt, Someone at Onsrud cutter, and any other bit vendor you may use. Now remember that the up spiral will tend to lift your material, so I hope you have good vac on this slipppuurrryyy material.

Damon,
I have never had a remelting issue with HDPE or UHMW. Acrylic and Sintra yes . That sounds like you are moving too slow or your RPM's are up to high for your feedrate. Get a scrap piece and draw a bunch of long skinny rectangles, ovals or even just a straight line. Program each of them in 25-50 IPM intervals and adjust rpm for your best chip load. See which one gives you the best finish. Another way is to make a long line down the side of a sheet and program it for say 700IPM but make several of them with different RPM's. Put magic marker lines every 2 feet. On your controller use the feedrate over ride to start at say 60% feedrate and move it up in 10-20% intervals at each of the magic marker lines. Keep good notes and you will see what works best for you. You can do this using a variety of bits also. You can also call Thermwood and ask what they would recommend.

Also are you using Climb or Conventional?

[Damon Nabors]

Michael,

You are correct in your findings, I had the feed rate and rpm's up too high. This being the first time we had cut 1" thick material, we were not sure how deep to cut and found out that anything more than maybe a 1/4" to 3/8" was too much. We found that cutting around 300 to 500 ipm was best for this material. When we shattered the bit, I think we were running at 18,000 rpm's and 750 ipm. It did ok on the outer edge, but when it came down the middle, it was too much. I was cutting the material into strips by using the manual panel input in CN and it tried to cut too deep too fast. We manually adjusted the z-axis each pass and made it through the material without any further mishaps.

[Terry Davis]

1/2 Viper with mortise tip

Thanks for your replies, where would I get such a bit?

[Michael Kowalczyk]

1/2 Viper with mortise tip

Thanks for your replies, where would I get such a bit?

Vortex has them. Talk to Linda and tell her Mike form houston said to call her.

Here is the link for the bit.

http://vortextool.com/index.cfm?fuseact ... uct_id=334


Look at this page as well

http://vortextool.com/index.cfm?fuseact ... egory_id=9

The prices are list and you get a discount for how much you buy. Last time I bought I got 30% and if you buy after IWF you can get upto 50% off.

[Michael Kowalczyk]

Michael,

You are correct in your findings, I had the feed rate and rpm's up too high. This being the first time we had cut 1" thick material, we were not sure how deep to cut and found out that anything more than maybe a 1/4" to 3/8" was too much. We found that cutting around 300 to 500 ipm was best for this material. When we shattered the bit, I think we were running at 18,000 rpm's and 750 ipm. It did ok on the outer edge, but when it came down the middle, it was too much. I was cutting the material into strips by using the manual panel input in CN and it tried to cut too deep too fast. We manually adjusted the z-axis each pass and made it through the material without any further mishaps.

Hey Damon,
if you were just cutting strips why not use a table saw or did you sell it to make room for your CNC thinking you'd never use it again. I still use mine occasionally because I do not have a roller hold system so it won't cut 6 sheets of 3mm at a time. But I have cut 3 sheets of 1/4" MDF sheets stacked with a 20 HP vac cutting 1000's of 9" x 12" blanks on my Thermwood. Only a few of them moved but at that rate it didn't matter.

[Damon Nabors]

No, I still have the table saw, but the customer did not want any saw marks on the edges, and that stuff is bad heavy in 4x8 sheets. The parts had to be exact width and I was not certain that I could slide it, keep it tight to the fence, and not hurt myself trying to slide that heavy sheet by my self late in the evening after my helper had gone home.