Hi.
Turning question.
I would like to get to know if anyone have solved the problem with chipbreaking when working with POM (maybe a tradename, but the same as Delrin)?
I have found that roughing can be done good, with a Sumitomo NS-U insert, 800m/min and feed about 1mm/rev.
However, finishing is a problem.
I use Aluminumtype inserts (like Sandvik Coromant Al-type), to make the shining finish with a low Ra-value, but chips are not breaking, and making a lot of problem further on in the production.
Have anyone found an untraditional solution?
Regrds
Kai

I have not done a whole lot of work with delrin itself, but I have machined a ton of nylon. One thing I do on my lathe is run and endmill down the diameter I am turning creating a flat side to the piece. That way when I turn it I have an interupted cut that has no choice but to break.

Oh yes, forgot to mention that trick.
It works, in any material, but its not possible to use that feature all the time, and mill can pickup a bush of chips.

.... anyone have solved the problem with chipbreaking when working with POM (maybe a tradename, but the same as Delrin)?....Have anyone found an untraditional solution?
Regrds
Kai

What do you consider untraditional :D ?

I suppose stopping the machine every ten parts when machining from bar stock does not qualify.

We do quite a lot of Delrin parts on both lathe and mill and have never solved the chip problem. We do use coolant which helps a bit because at least the chips don't melt and fuse up into a big mess but we have to clear them by hand most times.

It's excactly that problem, with stopping the machine I was hoping that someone had solved :(

Has anyone tried an extractor (shop vac)? I’ve been thinking about trying it next time I have Delrin on the lathe. Only problem I can see is the hose clogging; anyone tried it?

John

Untraditional method you say?

Place the material in dry ice prior to machining it. This changes the materials characteristics. So, you will need to work through a couple of test runs to determine the optimal bar length:chill time to X number of parts required.

Let us know the results if you give it a try...

Good luck,

Has anyone tried an extractor (shop vac)? I’ve been thinking about trying it next time I have Delrin on the lathe. Only problem I can see is the hose clogging; anyone tried it?

John

I had an opposite idea to this: Mounting an air nozzle in one of the tool positions and indexing to this to blow chips off the part. Also mounting one somewhere inside the machine so the tools could be moved in front of it to get the chips blown off.

But it sounded too complicated to try in case it didn't work :) .

I had an opposite idea to this: Mounting an air nozzle in one of the tool positions and indexing to this to blow chips off the part. Also mounting one somewhere inside the machine so the tools could be moved in front of it to get the chips blown off.

But it sounded too complicated to try in case it didn't work :) .

Not a bad idea but then think of the mess there would be to clean up. :)

Geof just out of interest why aren’t you a moderator?

John

Not a bad idea but then think of the mess there would be to clean up. :)

Geof just out of interest why aren’t you a moderator?

John

When you are machining Delrin or Polycarbonate there is one ***** of a mess to clean up anyway.

Why am I not a moderator? Because sometimes I like being totally immoderate :D .

Has anyone tried an extractor (shop vac)? I’ve been thinking about trying it next time I have Delrin on the lathe. Only problem I can see is the hose clogging; anyone tried it?



One of the shops that we do business with has a system setup like that, but he is taking long cuts on big diameters so he has something like a 1/2 wide ribbon be sucked into the tube. It works well he even stopped the cut to show me how it picks the chip right back up. His tube was about 2" in diameter so there was no clogging issues. I would think a smaller shop vac might clog but the bigger ones with the bigger hose would probably be alright.

One of the shops that we do business with has a system setup like that, but he is taking long cuts on big diameters so he has something like a 1/2 wide ribbon be sucked into the tube. It works well he even stopped the cut to show me how it picks the chip right back up. His tube was about 2" in diameter so there was no clogging issues. I would think a smaller shop vac might clog but the bigger ones with the bigger hose would probably be alright.

Thanks for that I'll give it a go :)

John

I do a fair bit of delrin production work - just program your CNC to "peck turn" and you're done.

It also works to take a few radial plunges every 1/2" or so down the length first and then do a regular roughing pass across them, but it's slower than the pecking method. If you're on a manual lathe though, that's the way to go.

DKOWALCZ what in the heck is peck-turn on a CNC lathe? I've never even heard of a term like that before... :D I like the idea, but unless there is a relevant modal G code for that, I don't even want to try manually inputting that code in my machine, good lord that'd add XXX amount of lines to every program I've ever written.

I'll admit having been a manual machinist as well as a CNC machinist for only 3 years, that's not a lot of code compared to some people, but more than most people with my time in the field. And I do mean CNC machinist, not operator, as I can diagnose & field repair machines, program, edit, set-up and tool-up machines. At least all the ones I have seat time on. :D

I used to turn HDPE for a company that makes plastic fusable fittings for water/gas lines (the big ones) on a manual lathe, and I just used a boxcutter to score the profile before I made a pass. It really helped keep the mess manageable, as having 20-30 feet of ribbon wrap around the spinning chuck and whipping the hell out of you before you can stop the spindle is a real experience...like when the 18" diameter (45 lbs.) part you are working on comes unchucked and bounces into your face because the flapping ribbon grabbed the toolpost and forced the tool deep into the part. You will never forget an experience like that. Makes taking the time to stop the spindle and score the workpiece every pass a necessity...unless you don't mind having a broken nose and a few missing teeth because of an occupational hazard that you could prevent.

I did notice, at least with HDPE, that when we brought stock in from the yard during the colder months, that it cut much "nicer"...the liquid nitrogen trick would definitely work, but man, what a PITA.

Personally, I have always thought that there should be an insert made specifically for plastic that has the cutting edge and then an edge that just makes contact with the part when the cutting edge is at depth, sort of a lobster claw arrangement with the longer edge above center line, that has a serrated element to it, or is heated, similar to a wire foam-cutter, just to help break the chip. If the plastic part was a big-ticket item, or constant production, it would really help and also justify such a specialty tool.

Or, on a CNC machine or manual lathe, just cut an appropriate left-hand thread to depth the length and profile of your piece, so when you take a normal cut, there are automatic chip breaks.

I know, not much help...but maybe it'll jog the brain of some tooling engineer to take up this issue. Especially since there are a lot of specialty plastic parts that don't justify molding or require the safety factor of machining from stock, ie. no voids in the material or excessively thin areas due to cooling shuts...

DKOWALCZ what in the heck is peck-turn on a CNC lathe? I've never even heard of a term like that before... :D I like the idea, but unless there is a relevant modal G code for that,......

Going from memory here.....peck turn is G74 Peck Face Grooving Cycle; peck face is G75 Peck Grooving Cycle. I use them I am just not sure if I have the correct G number. You set how far the tool advances per peck and at least on my machines (Haas) you define how far it retracts in a Setting.

Really useful canned cycles, I use them a lot for roughing large amounts off6061 to avoid big chip tangles.

G78 for peck arbitrary axis on TurboCNC - but it's more powerful to write a loop macro to do it as the g-code does a full retract which isn't necessary.

Most CNC's will take loop input of the form ... Ln where L is "repeat this line n times" so:

G91
G01 Z-0.100 F10.0 G04 P0.25 L9

gives you an inch of peck with dwell rather than retract, which should be good enough most of the time. If not, there's always "copy/paste programming".