Reply with QuoteBTW, I forgot to mention that I am a hobbyist and do not have a lot of experience in milling.
Thanks.
Olivier
cutting data for Delrin and High Molecular Weight Polyethylene
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
Similar Threads:
BTW, I forgot to mention that I am a hobbyist and do not have a lot of experience in milling.
Thanks.
Olivier
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.
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
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
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!
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
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.
Last edited by Paul_S; 09-05-2006 at 03:02 AM. Reason: add feeds.
Safety - Quality - Production.
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.
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
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.
Safety - Quality - Production.
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
G90 is normaly the Absolute Coordinate code. Usually best to use this. (not G91 incremental as inaccuracies build up)
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
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.
Safety - Quality - Production.
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.
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
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
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.
Last edited by Paul_S; 09-12-2006 at 05:53 AM. Reason: Add note regarding shear mills.
Safety - Quality - Production.
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
Posting Permissions
