What's new
What's new
By:
Advanced search…

How do you make machined delrin not look like poop?

R

rk9268vc

Aluminum
Joined
Dec 2, 2021
Location
Minnesota
How do you make machined delrin not look like poop? <SOLVED: Use new cutters>

I'm trying to machine some delrin and am struggling to get a nice surface finish. Side-milling works fine, but I cant figure out how to face it well.
It leaves little fuzzies and isnt nice and smooth like aluminum. It also seems like the chips dont really want to break.

Here is what Ive tried

1: Tormach Super fly - 3in fly cutter
9in/min, 10thou DOC, 3thou feed/tooth (ignore right side, didnt cut deep enough to get rid of saw marks)
IMG_20211202_193434877.jpgIMG_20211202_193434877.jpg

HSS 4flute 1/2in endmill
36in/min, 20thou DOC, 3thou feed/tooth
You can see the sides turned out fine with side-milling, just not the face
IMG_20211202_175245114.jpg IMG_20211202_175245114.jpg
IMG_20211202_175400174.jpg IMG_20211202_175400174.jpg

Also I am not using any kind of coolant/ fluid, should I be? my thought was no since its plastic, but what do i know

Thoughts?
 
Last edited:
You need brand new razor sharp tools, and you need a corner rad too, doesnt need to be very big at all, but try and avoid flat endmills, they dont do well.

Aluminum specific endmills/inserts with ground sharp inserts work well. Once you use a tool on metal it will never cut plastic like a brand new tool. Tormach sells a polished aluminum insert for their superfly. Try these, Im guessing by the pics your using the steel inserts.
 
I don't want to be that guy, but it aint the plastic, its the machine

Delrin is the most amazing plastic to machine.

Comes out perfect every time

It is sometimes in many areas hard to explain the difference a 'real' machine makes.


On a 60 year old bridgeport that surface would look like glass
 
If you're using a flycutter find a LH insert tool that uses either TCMT or CNMG inserts. Run a super sharp,
uncoated insert designed for aluminum--make sure it has a large nose radius. I think your feed rate and
DOC could both be higher. Experiment a little and you should be able to get a really nice finish...

Edit,,,it appears that I'm old and type really slow...we're all saying essentially the same thing, though...
 
thanks for the tips

Unfortunately I have to make some slots in the part as well with square corners, so I cant just use bullnose endmills

I am using the polished cutter meant for aluminum, but I could try rotating it to a new side. I did a test running at only 3in/min on the superfly and it did leave a somewhat nicer finish.

Is it fine to use 4 flute endmills, or do only 2 flute ones work? I am assuming I can only use 2 flutes in the smaller sizes like 1/8in diam.
 
IMG_20211202_211720964.jpg
Put a new insert in the super fly and ran it at only 3in/min
Thing feels like my dam surface plate

Unfortunately I have a hair of nod in the head, so you can see a whiff of recutting, but it is niiiice
 
IMG_20211202_212422437.jpg

OK new insert was the key, its like glass now

Thanks for the help yall. I didnt realize having a brand new cutter was so important, I was just using the ones I ran on aluminum.
 
rk9268vc said:
View attachment 335956

OK new insert was the key, its like glass now

Thanks for the help yall. I didnt realize having a brand new cutter was so important, I was just using the ones I ran on aluminum.
Click to expand...

Plastic likes brand new tools like we said :) Wait till you try a used tool on UHMW, WAY less forgiving then delrin.

Unfortunately I have to make some slots in the part as well with square corners, so I cant just use bullnose endmills
Click to expand...

If you want a good finish use a small rad anyway. Im not talking a large radius bull nose, just order your square endmill with a 0.010 or 0.020" corner radius. Will make a world of difference to the finish and a small rad like that wont make any difference to the function of the part 99% of the time.
 
rk9268vc said:
thanks for the tips

Unfortunately I have to make some slots in the part as well with square corners, so I cant just use bullnose endmills

I am using the polished cutter meant for aluminum, but I could try rotating it to a new side. I did a test running at only 3in/min on the superfly and it did leave a somewhat nicer finish.

Is it fine to use 4 flute endmills, or do only 2 flute ones work? I am assuming I can only use 2 flutes in the smaller sizes like 1/8in diam.
Click to expand...

When you get to the slotting try some of Harvey Tools plastic specific endmills. Plastics

I use the 3/8" 3 flute reverse spiral endmills for cutting delrin and they work amazing.
 
CAMasochism said:
When you get to the slotting try some of Harvey Tools plastic specific endmills. Plastics

I use the 3/8" 3 flute reverse spiral endmills for cutting delrin and they work amazing.
Click to expand...

I have used 1 and 2 flute downcut bits in wood on a shopbot cnc router before, how does wood compare to plastic? (This is literally my first time working with plastic/ delrin) I'm assuming it doesnt work well to spiral plunge? I know with wood it just turns to dust so it isnt as big of a deal. How does plastic behave?

I do have a 1/4in 4 flute compression cutter I pulled out of the garbage at work, it has a chip in the corner of one of the flutes though. Do you think this would work for delrin? Its a harvey 993716-C4 Harvey Tool

I have heard good things about harvey tools from youtube, but I like to stick to cheaper HSS because all my tools die to crashing, not to wearing out. The $5 endmills from shars hurt the bank way less than the 50$ ones from places like harvey tool.
I am eyeing up their 1/8 in high helix 2 flute for plastic, you think this is what I want? I need to make 3/16" slots 1/4" deep
Harvey Tool
Thanks!
 
rk9268vc said:
I have used 1 and 2 flute downcut bits in wood on a shopbot cnc router before, how does wood compare to plastic? (This is literally my first time working with plastic/ delrin) I'm assuming it doesnt work well to spiral plunge? I know with wood it just turns to dust so it isnt as big of a deal. How does plastic behave?

I do have a 1/4in 4 flute compression cutter I pulled out of the garbage at work, it has a chip in the corner of one of the flutes though. Do you think this would work for delrin? Its a harvey 993716-C4 Harvey Tool

I have heard good things about harvey tools from youtube, but I like to stick to cheaper HSS because all my tools die to crashing, not to wearing out. The $5 endmills from shars hurt the bank way less than the 50$ ones from places like harvey tool.
I am eyeing up their 1/8 in high helix 2 flute for plastic, you think this is what I want? I need to make 3/16" slots 1/4" deep
Harvey Tool
Thanks!
Click to expand...

Onsrud O flute single flute down spiral work very well for thinner materials that you want to stay on a vacuum spoil board, and splintery materials as well. I cut loads of canvas phenolic 3/8 with a 5 mm single flute down spiral. Nested small parts and after 4) 4 x 8 sheets the bit gets tossed.
 
I used to work at a plastics company and i've machined a ton of delrin. The key is to make sure you're not letting the part or cutter get too hot. reduce your RPM, increase your depth of cut significantly, increase chipload. Bigger chips cary the heat away from the workpiece faster. When delrin gets hot it doesn't cut as nicely. use air blast if you can.

You can get fancy with plastic specific end mills but you can easily get away with any cutter geared towards aluminum as well. make sure your cutter is sharp.

Seriously just try reducing your RPM first, I've had apprentices getting a similar surface finish from a facing operation, made them reduce RPM and the surface came out silky smooth
 
That looks more like UHMW than Delrin to me. In other words are you sure it's Delrin? As hard as I try and f'up some things up I've never had Delrin machine and give a finish like that.

Even a Tormach will get a good finish on Delrin.
 
DevinJB said:
Seriously just try reducing your RPM first, I've had apprentices getting a similar surface finish from a facing operation, made them reduce RPM and the surface came out silky smooth
Click to expand...

My mill only runs up to 3000 rpm, and thats what I have been running everything at. How much slower would you go?
 
triumph406 said:
That looks more like UHMW than Delrin to me. In other words are you sure it's Delrin? As hard as I try and f'up some things up I've never had Delrin machine and give a finish like that.

Even a Tormach will get a good finish on Delrin.
Click to expand...

Yeah it is delrin, got it from McMaster, sticker on it says delrin too. And it is the only plastic in my shop :P
My mill is quite similar to the tormach 1100, so good to hear lol
 
You must log in or register to reply here.

Similar threads

G
Meet Bertha! U.S. Machine Tool Co. Model VT vertical mill restoration
2
Replies
37
Views
24K
John Christopher
J








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top