# Machining Delrin Round Stock?



## RVJimD (Jun 18, 2015)

I am turning some 1/4" delrin round stock and find it gta smaller toward the headstock.  I don't notice this problem with metals.  Any hints or method I can use to reduce the problem?  I am loosing almost .001" per inch.  I am trying to make little axels for my idler tumblers on my crawler undercarriage project.

Thanks,

Jim


----------



## aeroHAWK (Jun 18, 2015)

You haven't noticed with metals because they don't deflect as much, since they are stiffer. It still happens but it is so small, you haven't seen it.

The solution is not easily defined given the lack of information about what the part looks like. If you can use a center in the tailstock, it would help. But if the part is too long and skinny, it will bow in the middle. You can also look at the tool geometry. High speed steel sharpened and stoned razor sharp is important. Carbide inserts are not a good idea here.


----------



## Wreck™Wreck (Jun 18, 2015)

Buy a Swiss type lathe this will solve all of your flexy stock problems.


----------



## brino (Jun 18, 2015)

I believe one problem could be tool bit shape. Plastic can be sticky and the bit digs in if there's and backlash in the lead screw.

I think that a tool more like a brass one, larger rounded tip and little or no top rake.
Some say really sharp, but always flat topped.

-brino


----------



## aeroHAWK (Jun 18, 2015)

brino,

I have to disagree here. I machine delrin all the time - today as a matter of fact. Delrin won't do what you suggest, especially small diameter like here. But I do agree the tool geometry can have an affect.


----------



## RVJimD (Jun 18, 2015)

I tried a different tool without a radius and it was a bit better.  I will have to keep working at this...

If I didn't say, I'm trying to make a few shafts from 1/4".  They need to be 3/16" in the center 75% and each end a bit smaller to fit into wheel collars.

Thanks for the ideas...

Jim


----------



## Bill C. (Jun 18, 2015)

aeroHAWK said:


> You haven't noticed with metals because they don't deflect as much, since they are stiffer. It still happens but it is so small, you haven't seen it.
> 
> The solution is not easily defined given the lack of information about what the part looks like. If you can use a center in the tailstock, it would help. But if the part is too long and skinny, it will bow in the middle. You can also look at the tool geometry. High speed steel sharpened and stoned razor sharp is important. Carbide inserts are not a good idea here.




Plastic material cuts better with HHS bits.  I know Nylon shavings will either melt or ball up on the part if it gets to hot.  The shavings will not break so no chip breaker is needed.  Good luck


----------



## RJSakowski (Jun 18, 2015)

One way to get around the flexing issue is to start with larger diameter stock.  If you use 1/2" diameter and finish as you go, the flexing will be minimal.  Delrin cuts easily so you can cut in a single pass if you have the right tool.  Use sharp tools and +1 on the HSS.  The cost differential between 1/4" and 1/2" is minimal.


----------



## mikey (Jun 18, 2015)

Delrin likes very sharp edges with large relief angles and large side and back rake on the HSS turning tool. This reduces cutting forces and cutting temperatures so less melting occurs. Finishes get better with a larger nose radius, too; somewhere around 1/32" nose radius works well. Delrin also likes slower speeds and faster feeds than metals. Watch your depth of cut. Delrin cuts easily but the lubricity can cause the part to slip in the chuck if it doesn't have tailstock support. For trimming the ends of the shaft a knife tool works well; just put a radius on the tool and it will cut fine. 

I am curious if this isn't a lathe alignment or leveling issue, though. I cut Delrin all the time and do not have taper issues so you may want to check these possibilities out.


----------



## aeroHAWK (Jun 18, 2015)

Mikey has good suggestions. With the small diameter you are working with, I would keep the nose radius pretty small. That will keep the cutting forces more axial than radial, therefore less likely to push the material away from the tool. Another thing you may try is to raise the tool slightly above the centerline. This will help in case the part is raising up due to cutting forces.


----------



## RVJimD (Jun 19, 2015)

I think I will try using a larger bore on the wheel and start with 1/2" stock on the delrin.  It might be a better design, probably keep the wheel more square with a larger D.

Jim


----------



## brino (Jun 19, 2015)

aeroHAWK said:


> I have to disagree here. I machine delrin all the time - today as a matter of fact. Delrin won't do what you suggest, especially small diameter like here. But I do agree the tool geometry can have an affect.



Hi areoHAWK,

I probably should have said "some plastics" in my original post.
My plastic working is usually on unknown scraps from the bin. (I barely know my ABS from a hole in the ground  )

So I will happily defer to someone who cuts delrin regularly.
Teach me! What tool shape(s) are you using successfully?
Pictures would be fantastic!

Do you reccommend what mikey says:


mikey said:


> Delrin likes very sharp edges with large relief angles and large side and back rake on the HSS turning tool........For trimming the ends of the shaft a knife tool works well; just put a radius on the tool and it will cut fine.



What's considered a "large relief angle" and "large side and back rake"?

Thanks,
-brino


----------



## mikey (Jun 19, 2015)

Hey Brino,
I would use about 15 degrees of both side and end relief, boost side rake to about 20 degrees and back rake to 35 degrees. This is similar to but more aggressive than angles for aluminum. The larger relief and side rake angles will create a narrower included angle at the cutting edge so penetration is enhanced and reduces cutting forces that can push the material away from the cutting edge; this aids in holding tighter tolerances. The increased side rake greatly improves chip flow out of the cut, which reduces cutting temperatures. The increased back rake focuses the cutting forces at the very tip of the tool to enhance the finish on the easily gouged Delrin while helping to flow the chips out of the cut. Anything that improves chip clearance will improve results with Delrin because much of the heat of the cut is ejected with the chip. I prefer a 1/32" nose radius. While this may seem large for thin work, the geometry of the tool above will negate much of the effect of the radius on cutting forces and will produce a cleaner finish. 

Most materials will allow us to increase speed and reduce feed to get a nicer finish. Do that with Delrin and it tends to leave tiny spirals in the material and dulls the finish due to increased heat at the point of the cut. Better, and more accurate, to keep speeds on the low side and feed smoothly and fairly fast. I normally turn Delrin at about 500 RPM and feed manually to get the finish I want. You also do not want to take too light a depth of cut, even when finishing, as this increases cutting forces at the tip. I normally rough until I'm about 0.02" away from final size and dial in the final finishing cut from there.

Hope that clarifies my earlier remarks.


----------



## aeroHAWK (Jun 19, 2015)

As I said in my other post, Mikey has good suggestions. I was going to say to start with geometry similar to aluminum, but more aggressive - but Mikey already did. Delrin cuts very freely and because of its lubricity, doesn't wear the tool, so you can get even more aggressive if you want.

I generally don't use tool radii as large as Mikey suggests, but I see no reason for it to be a problem.


----------



## chips&more (Jun 19, 2015)

With no pics and or drawings you are going to get a gamut of responses. In general, the plastic material family is rather flexible. So, if given the chance, it’s going to flex rather than be machined under tool pressure. Support the work/material. Use the tail stock, follower rest or similar. Try and machine all your steps as close the chuck/collet as possible. If you can, move the work out of the chuck as you machine your progress. This keeps the machining close to the chuck but run out could be a problem…Dave.


----------



## mikey (Jun 19, 2015)

I agree with chips&more - support is important. I suggest you start with a larger OD stock than needed and use tailstock support to machine it to the large OD of the axle in one or two passes, then chuck that OD close to the chuck and machine the ends. This gives you as much support as possible and a deeper depth of roughing cut will reduce deflection potential.

Or you can use a Swiss lathe ...


----------



## mikey (Jun 19, 2015)

I totally forgot to expand on one more thing, Brino. Since Jim probably has to cut a fairly sharp shoulder to get the wheel to fit up close to the axle I suggested a knife tool for that. This is a facing and finishing tool with a tiny nose radius to cut cleaner shoulders. It faces nicely but it tends to leave tiny spirals in the work. While that would be hidden by the wheel in this case it is still not good workmanship. A knife tool with a small flat at the very tip, about 1/32 across, will finish nicely and still allows you to cut to a very clean shoulder. This one isn't my idea; Ian Bradley of the UK uses this flat thing and I stole the idea from him. Surprisingly, it works really well on Delrin.

I don't grind this tiny flat on the tool; I create it with a hand-held diamond stone. If the tool is sharp it works really well on Delrin and most metals.


----------



## higgite (Jun 19, 2015)

mikey said:


> .....I normally turn Delrin at about 500 RPM and feed manually to get the finish I want. You also do not want to take too light a depth of cut, even when finishing, as this increases cutting forces at the tip. I normally rough until I'm about 0.02" away from final size and dial in the final finishing cut from there.
> .............



mikey,

I haven't turned much Delrin at all, but I take it that spring passes don't work well with Delrin. Is that right? Thanks.

Tom


----------



## mikey (Jun 19, 2015)

Hi Tom. In general, Delrin seems to like a fairly firm hand and it is better to take a decent cut to get the heat out of the cut fast. I rough as aggressively as the work holding situation allows and then take a finishing cut that is at least close to 1/2 the nose radius of my tool. Delrin likes to melt and this causes a hard crust to develop in the surface of the work; this makes it harder to take what you call spring passes and wind up with an accurate OD. For my personal tool, I know a finishing pass of at least 0.01-0.02"  or so deep will give a fairly good finish so I rough until I can dial that cut in. I don't try to get the finishing depth of cut exact, just close enough so when that pass is done I'm at final OD. 

Bear in mind that I'm not a Delrin turning expert. I've probably messed up more work pieces than the rest of the forum combined. I'm just reporting what I've found to finally work for me - hope it helps.


----------



## chips&more (Jun 19, 2015)

I have machined a bit of Delrin in my life time. One thing that stands out from other plastics. It’s rather difficult to polish. I have found that the best surface finish is going to be with the tooled finish from machining. So if you are trying to make it pretty, then get it correct the first time, when machining it. And I’m reading that a Swiss lathe is better at machining Derlin? Maybe yes, maybe no. IMHO this is one time that the operator must be more knowledgeable/skilled and with finesse than the machine being used.


----------



## mikey (Jun 19, 2015)

It was a joke, playing off of what Wreckwreck posted. I agree - cut it nice or live with it.


----------



## mikey (Jun 20, 2015)

Thinking that some of our guys may not wish to mess with grinding a tool to cut Delrin, I decided to try using a carbide tool to compare results. I used one of the most popular turning tools in existence, a SCLCR tool with a CCGT 22.51 Aluminum cutting insert. This insert is very sharp, has an aggressive positive rake at the tip and it cuts very well, indeed. I didn't have a 22.52 (1/32" nose radius) insert handy to compare but even the 22.51 (1/64" nose radius) left a nice finish when fed a bit slowly. It will also rough as aggressively as your work holding situation allows.

An SCLCR tool normally takes CCMT inserts but will fit the CCGT inserts as well. The aluminum cutting inserts work a treat for aluminum but I can confirm they also do Delrin quite nicely. The 1/64" nose radius cuts fine but finishes a bit spirally for my taste; for finishing, a 1/32" nose radius would be better in my opinion.

Is it better than HSS? No, it is not better than the tool I would normally use but then again, I had to grind it. This took me all of 30 seconds to put an insert in the tool. For the guy who doesn't turn Delrin often, this would probably work just fine. If you must cut tight to a shoulder a smaller radius works but for general work and finishing, the 1/32" nose radius insert would be better. Just be sure to get the insert intended for aluminum.


----------



## kingmt01 (Jun 20, 2015)

I don't turn the stuff but just wanted to say thanks for the question being asked & everyone giving the advice. I've found this thread to be very interesting.

I've only turned PVC tubing after heating to form close to the size needed. I consider that a big pain in the butt & this stuff sounds worse.


----------



## aeroHAWK (Jun 21, 2015)

kingmt01 said:


> I've only turned PVC tubing after heating to form close to the size needed. I consider that a big pain in the butt & this stuff sounds worse.



Of all the plastics I've machined (pvc, uhmw, hdpe, nylon, acryic, ABS, polycarbonate, etc.), *Delrin is the BEST!* It cuts very freely (I equate it to free machining brass), and leaves a very nice surface finish. If you got the impression it is worse than PVC, I haven't made myself clear.  It is nowhere close to being a pain!


----------



## mikey (Jun 21, 2015)

I agree with aeroHAWK - Delrin is like machining firm butter, while Polyurethane is like machining the 1018 of the plastic family. Delrin can make me look like I actually know what I'm doing!


----------



## RJSakowski (Jun 21, 2015)

+1  with Aerohawk.  I have machined a lot of Delrin over the past decade, including parts as small as 1/8" diameter and have never found it to be particularly picky about tool grind.  I used HSS tools and kept them sharp.  Even with a zero radius tool, I would have nice finishes.  I don't ever recall having a problem with melting.


----------



## cazclocker (Jun 21, 2015)

I have found this thread very interesting too. I have a small project coming up that will require me to create a small push-handle for the end of a small shaft, out of Delrin. One question as another of the beginners here, is what is a Swiss-type lathe?  What are the defining characteristics of it?


----------



## mikey (Jun 21, 2015)

Swiss lathes are ultra-precision, very high-dollar CNC lathes. They are used for precision manufacturing of complex parts for many industries from almost any material, including plastics. I don't presume to know what Wreckwreck was referring to but this is what I was joking about:

http://www.3dmedicalmfg.com/capability/swiss-style-lathe/

Check the video at the bottom of the page. Probably won't score one of these on Craigslist anytime soon.


----------



## higgite (Jun 21, 2015)

mikey said:


> Swiss lathes are ultra-precision, very high-dollar CNC lathes. They are used for precision manufacturing of complex parts for many industries from almost any material, including plastics. I don't presume to know what Wreckwreck was referring to but this is what I was joking about:
> 
> http://www.3dmedicalmfg.com/capability/swiss-style-lathe/
> 
> Check the video at the bottom of the page. Probably won't score one of these on Craigslist anytime soon.



I'll bet a guy could make some nice brass kitchen drawer pulls with one of those in his garage. 

I turned and threaded some Delrin yesterday just for grins. (Not on a Swiss lathe, though.) Used HSS inserts and they worked well. I did discover that if you cut an unsupported 1" long 1/4-20 thread in Delrin, the outboard end threads will be a lot shallower than the inboard end. Go figure. 

Tom


----------



## Bill Gruby (Jun 21, 2015)

Let's bring the Swiss Machine to reality, then get back to the task at hand, helping the OP with his turning problem. We are straying from that. Here is a used Swiss 4 axis Swiss Machining Center for sale.

 "Billy G"

http://www.ebay.com/itm/HAAS-EC-400...635?pt=LH_DefaultDomain_0&hash=item1c4e2a4643


----------



## Ulma Doctor (Jun 21, 2015)

I have machined many projects from delrin rod.
It's one of the best machining materials i have run across. 
It's very easy to work, and is very useful for low speed/moderate load bushings and thrust washers.
It's very forgiving for first timers and is a great practice medium due to it's relatively low cost and ease of access 

Steps should be taken to avoid overheating delrin as it has a relatively low melting point .

I have used carbide , HSS, and carbon steel tooling to work it with great success, it may just be my favorite material to machine!


----------



## mikey (Jun 21, 2015)

Sorry Bill, you're right.

Tom, you raised a good point, one that was alluded to earlier in this thread. Proper work support is critical when working with Delrin because it will push away from the cutter as diameters drop off. Working with thin stuff caused me to look hard at tool geometry and it helps but we should always work close to the chuck when possible or use a live center or follow rest when we can't. In Jim's original post, his work was larger at the tail end and this is likely due to the part deflecting away from the cutter at the unsupported end; a live center or follow rest would help reduce that tendency. 

Making big, short stuff with Delrin - a joy! Making small, thin stuff with a consistent diameter and nice finishes - not so easy! Delrin is a good teacher.


----------



## Lucky 13 (Jun 21, 2015)

Bill Gruby said:


> Let's bring the Swiss Machine to reality, then get back to the task at hand, helping the OP with his turning problem. We are straying from that. Here is a used Swiss 4 axis Swiss Machining Center for sale.
> 
> "Billy G"
> 
> http://www.ebay.com/itm/HAAS-EC-400...635?pt=LH_DefaultDomain_0&hash=item1c4e2a4643


That is a horizontal CNC milling machine, not a swiss lathe.


----------



## Garththomas (Apr 3, 2016)

What about using a travel rest?


----------



## gheumann (Apr 9, 2016)

I machine a lot of Delrin. The work is flexing, further and further the further it is from the chuck. As said metal will do this too. Without knowing diameter and length it is hard to recommend a solution - but you CAN make very light cuts on Delrin. I have had no trouble with melting, from extremely heavy roughing cuts to very light spring passes for .001". Unless you're up at 4" diameter or more, use the highest speed you have. I use the triangular replaceable (CCMT? i forget) carbide bits for this and almost everything else. Stop. Measure. Cut. Remeasure. If the part has high length to diameter you may have to use some other method to "even out" the diameter along the length. But make sure you plan to approach finished diameter with at least 3 light cuts (under .010) to minimize the effect of deflection.

A follow rest may help too.


----------



## CraigB1960 (Apr 9, 2016)

I machine Acetal/Delrin rod all the time, both using lathe and bridgeport.  One of my cases is made from acetal that I pot my electronics in.   I get excellent dimensional stability using HSS tooling.  I always take a very light final cut to achieve an excellent finish.

I typically turn it around 280 RPM and have no issues with melting, even when hogging out with a boring bar with carbon inserts.  Not knowing your complete specs.  (I turn 1.75" Acetal rod at .7" length), but at 1/4" rod, I would use a 5C collet to hold the work.   At that diameter, you can hardly go any length out of the chuck without tailstock, follower, and/or steadiest without flexing become a major issue.  Need sharp tool and take light cuts.

Since I have a slow spindle (700 RPM max) old lathe, I use a lot of HSS tooling.  I stopped grinding HSS unless I need a special form.  Instead I use Arthur Warner Co. tooling/inserts.  Once there is any wear on the insert, you just simply hone the top side and you are good to go.   A whole lot cheaper than carbon insets and cuts better on my lathe.  Puts a nice finish on the acetal.


----------



## Wreck™Wreck (Apr 9, 2016)

cazclocker said:


> I have found this thread very interesting too. I have a small project coming up that will require me to create a small push-handle for the end of a small shaft, out of Delrin. One question as another of the beginners here, is what is a Swiss-type lathe?  What are the defining characteristics of it?


A Swiss lathe has a moving head stock that does the work of a conventional lathe carriage, the work is held in the head stock by what ever method available, chuck, collet, etc. 
The work passes through a bushing that rotates at the same speed as the spindle, the turning tools are located at the bushing nose where they move in the X axis, the moving head stock moves the stock in the Z axis when being turned. Such lathes require accurate stock to begin with and are often very limited in the length of cut. They are not however strictly CNC machines, Swiss style lathes have been used for precision work for a very long time, they are also not very versatile for general lathe work.


----------



## Wreck™Wreck (Apr 9, 2016)

chips&more said:


> I’m reading that a Swiss lathe is better at machining Derlin? Maybe yes, maybe no.



A Swiss style lathe is a different method of doing the same thing that any other lathe does, the method employed is simply well suited to long L/D ratios. They have many requirements and limitations that make them unsuitable for general lathe work and most old manual Swiss lathes are very small indeed.


----------



## cascao (Apr 9, 2016)

High side rake and relief angle HSS tool very sharp finished in a oil stone.
Big round tip to good finish.

But, for 1/4" material, you can't go far from chuck even with everything right.


----------

