PDA

View Full Version : cutting data for Delrin and High Molecular Weight Polyethylene



jedioliver
09-01-2006, 06:11 AM
Hi guys,

It's the first time I come on this forum and I have already found some precious informations.
I thought that some of you could help me.

I have some Delrin and High Molecular Weight Polyethylene parts to mill, but I have no idea of the cutting datas to use.
I have done some test with Delrin and the finish was quite disappointing.
The Delrin get fluffy instead of being slick and bright.
Doas anyone already experienced this?

I think I use some wrong cutting datas, but I don't know wich one to use.
Do you have some cutting data that are good for these kind of plastics?
I would need usual VC, Vf, fz and N datas if you some.

I have personnaly used:
N: 9500 rpm
Vf: 3mm/s

What about datas for High Molecular Weight Polyethylene?


Please feel free to ask me any questions if needed.
I will answer on next monday. Sorry for the delay.

Thanks.

Olivier

jedioliver
09-01-2006, 07:52 AM
BTW, I forgot to mention that I am a hobbyist and do not have a lot of experience in milling.

Thanks.

Olivier

grapes
09-01-2006, 01:47 PM
Sounds like you've got a dull tool! The sharper the tool the better, brand new is best if you can. As for cutting data, you're gonna have to play with it. I've been machining all types of plastic for a long time and have yet to find any data worth using (even the data given in the catalogue where I work is junk!)
If I were milling a 1/2" slot in a piece of UHMW 1/2" deep I'd run it at 1000 rpm at 25 ipm. For the same cut in delrin I'd go about 1400 rpm and 15 ipm. If you have some extra material just play with it.

jedioliver
09-04-2006, 06:04 AM
Thank you for your answer.

Well, I have used a new tool so I do not think it came frome the tool. I have done some test and for the moment, the best result I found was 12ipm. Unfortunately, I can't go slower than 8000 rpm as I use a High Frequency spindle. I have done the test using a 3mm end mill, 4 flutes. I am quite afraid because I will have to use some micro end mills (0.3 mm) and I really do not want to break them.

Any advices?

Thank you once again.

Olivier

carlnpa
09-04-2006, 02:58 PM
I cut alot of UHMW and HDPE. What size mill are you trying to use? In general spiral upcut 1 or 2 flute will work best. To surface a part without fluffing the material the leading edge of the mill should have a radius. The photo shows the larger mill (with radius) used to cut the surface of the part to the needed thickness. This part is nylon 6/6 with moly but the color shows cut path and finish well.
The pockets in the part in photo were cut with 3.2mm 2 flute spiral upcut (for aluminum) at 3mm cut depth per pass at 12000rpm and 6.3mm/s.

Carl

grapes
09-04-2006, 09:29 PM
If it's not a dull cutter the fluffing is from the chips not being properly cleared from the endmill and melting to the finished part, the heavier the feed the better. That's why I tend to use a slower speed with a heavy feed on the manual. I also run a cnc router that does'nt perform well under 18,000, so I tend to run it at 300-400 ipm. Your biggest problem is going to be breaking those tiny endmills, even the 3mm are going to snap in plastic (especially nylon) if you feed them too fast! Also, I've never had any luck with four flute endmills in plastic, there is nowhere for the chip to go. Try a two flute if you can! Hope that helps, let me know how you make out!

jedioliver
09-05-2006, 02:41 AM
Hi guys,

Thank you very much for your message.

Well, I have done some test and the best result I got for the moment with a 3mm end mills, 4 flutes is 8000rpm (I can't go slower) and around 5mm/sec (12ipm). I really would like to try with slower rpm but I don't see how for the moment.

It's true I could use a radius mills for surfacing, but I will have some pockets to make, so I will still need some end mills. But I will try to use 2 flutes. It seems that you have better finishes than mine using 2 flutes mills.

Ok, let's keep in touch.

Thanks

Olivier

Paul_S
09-05-2006, 02:56 AM
For Delrin I use 400 SFPM for HSS end mills and 800 SFPM for carbide end mills. 150 SFPM for drilling. If you are using a CNC control, if it has G73 pecking cycle, use it to break the chips. Using a standard G81 cycle the chips can be stringy and stick to the drill.

I don't know about the High Molecular Weight Polyethylene, I would try the above though.

As for chip loads I use the same as I would for aluminum. Without the concern for horsepower or breaking tools. For end mills .010 x the dia x number of flutes x the RPM. For finish .016 x sqr(dia) x RPM (minimum finish feed.) For end cuts .0095 x RPM. For drills .020 x dia x RPM.

chipproducer
09-05-2006, 11:03 AM
are you using coolant?
I find that it often helps even in plastics. Just make sure to clean them good after, as they tend to absorb water and swell over time.
Two flutes are a must. If you don't use coolant, blow air on the cutter to move the chips out of the way.

jedioliver
09-05-2006, 11:13 AM
Dear guys,

Thank you very much for your answers.

Well, I do not use coolant as my machine do not offer such perfection...lol...
I have done an other try still with a 4 flutes mill (I do not have 2 flutes for the moment) and the result seems much better. The spec are 8000 rpm and 3mm/s.

It's true I have problems with chips so I make the milling process in 2 or 3 steps in order to clean the part between each stage.

Paul s, I really do not know what are G73 or G81 cycle. Could you please explain this.

Thanks a lot. guys.

Olivier

Paul_S
09-06-2006, 03:46 AM
G73 and G81 are drilling cycles, preparatory "g" codes used in CNC (Computer Numerical Control).

My notes on the feeds were in inches, sorry. The same in mm would be as follows:

As for chip loads I use the same as I would for aluminum. Without the concern for horsepower or breaking tools. For end mills .010 x the dia x number of flutes x the RPM. For finish .4064 x sqr(dia/25.4) x RPM (minimum finish feed.) For end cuts .2413 x RPM. For drills .020 x dia x RPM.

And yes, I used coolant. If you have the material melting, reduce the RPM if cutting dry.

And the SFPM was in Feet Per Minute. Meters Per Minute becomes 122 SMPM for HSS end mills, and 244 SMPM for carbide end mills and 45 SMPM for drilling.

jedioliver
09-06-2006, 03:58 AM
Paul, thank you very much for your answer.
That's what I thought about the G73 and G81. That it was dealling with the G code. I am not wrong...lol...
I have done some searches, and the only type of info I have is "G90".
I have opened mu *.iso file and it is written "G90". Is this a good or a bad news?...lol...

Thank you for your translation in mm.

In fact, I am now milling the part with the cutting datas written above, and the finish seems good now: slick and bright.

I will try to send pictures to show this part and to have your opinions guys.

Thank you once again.

Olivier

chipproducer
09-06-2006, 08:57 AM
G90 is normaly the Absolute Coordinate code. Usually best to use this. (not G91 incremental as inaccuracies build up)

jedioliver
09-10-2006, 02:34 AM
Well, I must admit I gave up. I can't find the finish I would like. Plastic is too complicated for me.

I plan to use wax modeling boards instead. Do you know such type of materials?

Thanks for your help.

Olivier

Paul_S
09-11-2006, 01:27 AM
Finish is a function of peeks and valleys on the surface of the part. Different things can affect this. For example a zig zag cut will have no better finish typically than a one way cut with double the step over. While that may not be always true. It is mostly.

Typically cutting a feed rate in half will improve the finish by 4. That is true of any radius on the cutting edge. The exception being sharp edges on the cutter leaving sharp steps.

The limiting factor being the finish on the cutter edge itself. So a finish may not be better than the finish on the cutter. True in turning and mostly true with end mills, side cutting.

chipproducer
09-11-2006, 08:39 AM
sorry to hear that you will give up. You must be very frustrated.

I have been doing this for over 15 years now, and always come across these kind of problems. Even as we speek, a lathe job we are doing right now ran the first 12 pieces perfect, but now the boring bar decided to chatter and give a horrible finish no matter what we try.

You are not alone. But if you keep trying, you would learn a heck-of-alot once you figure it out.

:cheers:

jedioliver
09-12-2006, 04:47 AM
Thank you very much for your help.

I have decided to try again today. I want to make these parts!...nothing else!!...lol...

thanks...

Olivier

jedioliver
09-12-2006, 04:57 AM
BTw, I have decided to buy some new end mills as mine are not intended for plastic materials.
It seems that 1 or 2 flutes mills are the best to use, but is true for square end mills and for ball nose end mills?
What about the helix? Is 30° better than 45° helix?
What's the best tool to use?...

Thanks.

Olivier

Paul_S
09-12-2006, 05:48 AM
A 0 deg cutter is straight up and down, a 30 deg cutter spreads the same cut over a longer cutting edge, a 45 deg even more cutting edge is removing the same amount of material. In other words, reduced cutting force with the higher helix. A higher helix should have less deflection of the material or tool. Above 45 degs like 60 deg the load goes up, but the deflection is still less. The cutting forces are more up than to the side.

jedioliver
09-12-2006, 06:18 AM
Thank you Paul for your answer.

So a 45 deg should be better if we need a clean and easy work?
So why are most of mills sold in 30 deg?

Please give me a little bit more info.

I was planning to buy some 2 flutes, 45 deg, center cut mills for my acetal parts. Do you think it would be ok?

Thank you once again.

Olivier

carlnpa
09-12-2006, 02:07 PM
Try these Onsrud 40 series for small mills <6mm, they work very well in plastics, are low cost.
https://www.onsrud.com/xpost


Look under catalog, they are under wood bits.

Paul_S
09-12-2006, 03:21 PM
Here is a page which explains helix angles on end mills:
http://www.manufacturingcenter.com/tooling/archives/1105/1105tooling_around.asp

Paul_S
09-12-2006, 03:31 PM
Here is a pdf file on machining plastics:
http://www.connecticutplastics.com/understanding.pdf

jedioliver
09-12-2006, 04:42 PM
thanks guys for your help...I really appreciate...
I think I have many things to learn...;-)))...

I will keep you updated...

Olivier...

carlnpa
09-12-2006, 09:16 PM
Jedi-
I'll try to help with specific mill selection.
What size parts are you tring to make?
What is your spindle rpm(range)?
What size collets do you have?
What milling operations, surfacing, pockets (need corner radius), cut out?
What is the maximum depth of cut?
Can you change tools during the process?
How will you hold the part?
In general cutting plastics is all about the cutting tool, specific cutting tools.
The good ones will have a sweet spot but tend to work over a wide range of rpm and feed speeds.
You must always be moving while in contact with the part, no movement will instantly cause the material to melt and gum up the cutting edge.

In inches small mills
Onsrud 40-101 and 40-101L 1/4 shank by 1/8 about $7
Onsrud 40-103 1/4 shank by 3/16 - excellent for plastics $7

jedioliver
09-13-2006, 06:57 AM
Hi guys,

Thank you once again for your help.

Paul, it seems that a 45&#176; helix is better than a 30&#176;. I think I will try them as it seems to be more efficient.
Did you already use such mills? What is your opinion?

BTW, I also red that some helixes are going downside. It seems that the chip goes donwside with such mills. Does it really offer an advantage?

Carl, here are the answers to your questions:

- parts are going to be from 10x10x12 mm to 150x100x35 mm.
- spindle rpm: from 8000 to 24000
- size collet: from 3mm to 6 mm (from 0.11" to 0.23")
- milling operations: all you can imagine...unfortunately...lol...
- depth of cut max: 40mm (+/-1.6")
- I can change the tools, no problems
- the parts is on the 4th axis wich can be indexed or continuous


From your comments, I think I will choose the following end mills:

- 1 flutes, 30&#176; helix, center-cut, upside helix
- 2 flutes, 45&#176; helix, center-cut, upside helix

I am waiting your comments on downside helix. I planed to buy 1 flute and 2 flutes mills with such helix in 30&#176;.

Feel free to contact me if needed.

Thanks ones again.

Olivier

pced
11-13-2006, 10:26 AM
If anybody needs help with machining plastics, please check out my website www.cncplastics.com Lots of great technical info. Physical properties and machining information. You can also call us at 1-800-265-7351 for small and large quantities of plastic rods, plate and cut to size blocks.

Paul_S
11-14-2006, 05:01 AM
Paul, it seems that a 45&#176; helix is better than a 30&#176;. I think I will try them as it seems to be more efficient.
Did you already use such mills? What is your opinion?

I have typically used 2 flute 30&#176; helix HSS or carbide cutters cutting delrin.

[I have used 60&#176; helix 3 flute for roughing and finishing a 1/4 dia post in 17-4 steel. Using a RobJack tuffy brand 3/16, 3/4 flute cut length. Other brand cutters would just shatter. It would cut nice and straight with little or no taper. If this works this well in steel, plastic should be like butter. Also in plastic that brand would not be required.]

pced
11-14-2006, 08:23 AM
Go here http://www.cncplastics.com/PDFs/Machining%20Acetal%20Delrin.pdf for detailed info on machining Delrin. Other great info available at www.cncplastics.com (http://www.cncplastics.com) in the physical properties section.