What's new
What's new

knurling 101, never done it

viper

Titanium
Joined
May 18, 2007
Location
nowhereville
We have a couple part numbers we are quoting that require knurls. I am curious what I need to know to knurl a part? I have always wondered if the diameter of the knurl wheel needs to be of a certain size compared to the part? I am just wondering about the knurls of one rev not lining up with the next and they get all smooshed together.

Is there a certain way to feed a thinner knurl over a longer Z length and make it all look uniform? What kind of feeds/speeds are we looking at for this?

One part is Al and one part is SS which kind of worries me.
 
Best advice I can offer is to get your hands on one of Dorian's knurling catalogs. It has someof the best descriptions I have seen and they work because I have had good success using it.

Charles
 
I knurl a part in 17-4 and I feed into at about .01- .015ipr about 300-400 rpm. and there is a formula, like the previous post said look in their catalog. And one thing I read and learned was you may need to change your o.d. by a few thousands to make the roller track correctly. and are you doing straigt or diamond and is it a male or female knurl? I've read there's diffrent tricks depending on which one you are going to be doing.
 
Just program a multi-lead thread with a 45 degree helix angle and number of starts to equal the teeth per inch of the knurl you want to create. Then machine a left hand thread overlapping. Voila, diamond knurl, 4 hours of macro programming fundamentals and tool grinding and 45 minute cycle time later, you're DONE!

hahaha just kidding. I have wanted to figure out the formula for a long time now. If you get it before I do, please post it to this thread! I would 'prech.

;)
 
We have a couple part numbers we are quoting that require knurls. I am curious what I need to know to knurl a part? I have always wondered if the diameter of the knurl wheel needs to be of a certain size compared to the part? I am just wondering about the knurls of one rev not lining up with the next and they get all smooshed together.

Is there a certain way to feed a thinner knurl over a longer Z length and make it all look uniform? What kind of feeds/speeds are we looking at for this?

One part is Al and one part is SS which kind of worries me.

Smooshed?? Now there is a technical term for ya! ;)

Light pressure, with no feed, until both knurls have established a proper 'track', then feed across. If it starts wrong, skin the diameter to get rid of the bad track and try again. It only takes a depth of .002"-.005" to see if the knurls are tracking correctly. It can be a bitch to get them started correctly especially if it happens that the knurl diameter/part diameter ratio is exactly wrong.

If this is the case, hopefully you can play with the starting diameter/circumference to something that is closer to an even multiple of whatever knurl you are using.

This is the procedure I have used on manual machines, don't know how this translates into use on cnc.
:D Dave
 
Correct me if I'm wrong.
If I remember correctly, The pitch of the knurl and the feed should be the same.

Slow speed and rapid feed.

You have to play with the height of the knurling tool to get equal pressure on both wheels or the wheel with less pressure might double cut.
 
Ditto on slow speeds & fast feeds. Make sure the coolant is blasting your knurl(s) to keep down shavings. If you have to feed in Z, use a brisk feed rate. Especially with straight knurls, it's been my experience that using cylindrical knurls with sharp corners leaves a visibly slight border between the surface of the initial plunge & the rest of the length. Form Rol (and probably others) have radiused knurls which are supposed to help with that, but I've never tried one.
http://www.formrolldie.com/prod03.htm
You may have to play around with X offset & pre-knurling diameter a tiny bit to find a "sweet spot", but don't agonize over it. We use a single knurl bump-type (OR BH-OU).
(general knurling info)
http://www.formrolldie.com/new_page_1.htm
 
I can''t offer anything new here as I'm a relative novice when it comes to knurling too. but I just finished knurling a run of .375 stainless pins and can tell you stainless isn't too bad to knurl.
 
We knurl A LOT of parts, and have for years. There are some pretty good resources out there to gain the knowledge you need to get started. Its really more of an art than a science. We use a company called Accu-Trak for most of our stuff. They have tooling small enough to fit in our Swiss machines, and their staff has a lot of experience.

Knurling diameter is going to depend on the TPI of the knurl. A 30 TPI knurl will grow the diameter about .010"-.011", but that is still just a rule of thumb. I start the set-up with the knurl barely touchine the material, and then slowly increase the depth of the knurl and the diameter until I get the results I need. Once you get the hang of it, the material really doesn't matter, you just need to adjust the speeds and feeds, like any other tool. Do not make the mistake of dwelling at the bottom of the stroke, get in and get back out.

I hope some of that helps, there is a lot more info that could be put down on paper. Just take your time and be patient.
 
The aluminum part is the one to worry about. Especially if it gets color anodized. Because of the softness of aluminum you'll get a lot of flecking of the material. The flecks get beaten back into the material. During anodizing some flecks break loose leaving bare spots.

There is no easy solution to the problem. We've dealt with it for years. Some parts are sent to a sheltered work shop where they have the guys brush the knurled areas with brass wire brushes prior to anodize. On black parts we touch up the white spots with felt markers.

I just had that very problem on some parts i just made. i ended up using a touch up pen from birchwood casey and it worked awesome. i tried the black felt markers but the color looked funny compared to the anodize. here's a link to the markers:

http://www.birchwoodcasey.com/sport/

click on gun blueing the super black touch up pens are near the bottom of the page.
 
I think it was summed up pretty well with the statement it is more of an art then a science.

That said there are general rules of thumb and if your are close you get satisfactory results. Then you get jobs where you just want to pull your hair out as the tool don't track right, knurls look horrible, size won't grow anymore or grows too much. You fix one issue only to have another pop up. I had a job recently that i could get to run in my manual with zero issue, put it in the CNC and crap, just crap came out. I adjusted the diameter,angles speeds feeds and just crap. Put it back in the manual and I could do not wrong, feed crooked, straight, fast slow by hand it all looked great, back in the CNC with same tooling and crap.

Anyway 90% of the time just follow the rules of thumb mentioned and it is a piece of cake.
 
Why hasn't anyone mentioned cut knurls? I've always understood they were better than 'smoosh' knurls. Do high production guys not use cut knurls?
 
I used a Eagle Rock scissors type in a cnc lathe all the time with good results.

If you're using a "bump" type...abandon hope.

David
 
Just one word of advice. If the parts are less than 3/4 diameter or so (more or less), and the knurl has to be 3 inches long (more or less) you will need to program a taper. (Ask me how I know...) I had a job that repeated several times.. 303 ss, 5/8 diameter, called for medium knurl 3 inches long, in the 300-400 quantity range. I saved the program because it was tweeked perfectly. Then the customer started importing them from China. (Oh well.... that's life in the world of manufacturing, I guess.)
 
I recently looked in a book called Machine Shop Secrets, or something like that, for advice on knurls. The idea was to find the pitch of the knurl grooves on your knurler and divide by PI. The diameter you are to knurl must be a multiple of that number. The error here is measuring that pitch with your calipers, so preferrably you can verify that pitch some other way.

For instance: a .050 knurl pitch divided by PI = .0159155
So if your diameter to be knurled is one inch, the nearest preferred diameters are: 1.0027 and .9867
 
That is precisely what I was pondering. That the knurl wheel diameter must match the diameter of the part in an even ratio like 2:1, 3:1, etc so the hatching will line up and not "smoosh" (note, engineering term) things together. I think I may try to call Dorian and see if they can send me some info.


Sounds like this will become a deep subject but one that will have to be covered at some point.
 
That is precisely what I was pondering. That the knurl wheel diameter must match the diameter of the part in an even ratio like 2:1, 3:1, etc so the hatching will line up and not "smoosh" (note, engineering term) things together. I think I may try to call Dorian and see if they can send me some info.

You should compare circumference, not diameter.

However even this would not account for different pitches of knurls, depending on what coarseness or fineness (more engineering lingo ;) ) is specified.

Ideally, using this logic, the CIRCULAR PITCH of the knurls should divide evenly into the CIRCUMFERENCE of the blank.

But there is an amount of leeway in this relationship. The crests of the knurls will tend to 'seek' a previously made track.
:D Dave
 
I seem to have the opposite experience as everyone else, which is kind of typical for me. Knurling is definately an art. I dread it on a manual lathe like going to the dentist. I find it slow and have never had consistent results, even with being taught by a few wise toolmakers.

I did get some work for the CNC lathe and bought one of Dorian's cut knurling heads, and was knurling stainless parts by the hundreds. It was so much better! Took a couple of hours to set up the first time, then it was off to the races. Pumped the daylights out of coolant onto the wheels and it made beautiful knurls, after a little tweaking of the diameters. I have had good luck with aluminum as well.

The tool is pricey, but you can buy different heads for it if you have to do different diameters that are a lot different in size. Good luck!
 
Hy,
calculate the diameter of the part so it´s a multitude of the knurls pitch. You can´t use enough coolant here, go slow. If possible, start the knurl on a piece of the part that will get machined anyhow, so you get rid of the knurls start. Use a tool with opposite knurlwheels if possible.

Greetings,
Johann
 
Knurling

While on the subject, have a face knurl in the stack comming up, last one I did was on a turret lathe back in 1958!! Any pointers on CNC face knurling?

Cheers, Les H.
 








 
Back
Top