Machining Delrin Round Stock?

[RVJimD]

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]

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:

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]

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]

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]

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]

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]

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]

.....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]

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]

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.