knurling 101, never done it
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.
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.
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.
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)
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.
Originally Posted by viper
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 use B&S opposed wheel knurling tools originally designed for screw machine usage. Cheap and effective tools. Experiment with blank diameters to get the correct finished diameter . Piece of cake with a bit of practice, but don't under estimate the problems an inexperienced operator can have.
DEFINITELY DO NOT bid on the parts until you've played with knurling a bit or you are guaranteed to lose your shirt on the job. Be 100% sure you understand exactly what the customer expects in knurl appearance and function.
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.
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:
Originally Posted by Doug
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.
Originally Posted by imported_chip_maker
Old time anodizers tell me they used to dip black parts in India ink to cover the bare spots.
Since I first starting making a black aluminum part with diamond knurling 20 years ago I've been noticing how few products use diamond knurling on aluminum.
You look at knobs on high end electronics, instead of knurling they use extruded stock with straight serrations.
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?
My experience with cut knurls has been bad, not to mention expensive. Flecks of material beat back into the part.
Originally Posted by rklopp
The opposed forming knurls work so much better. Even the hundred buck scissor type tools for engine lathes do a better job.
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.
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.
I understand the theory...........But, I've been making good knurling for a lot of years and never considered this stuff.
Originally Posted by viper
Get yourself some type of opposed knurling tool. Opposed means having two wheels opposed from each other, the work is squeezed between them. Once I stated using that type tool all my knurling problems were over.
The only consideration for blank diameter is that the finished knurl comes to the proper diameter. In this respect it takes a few trials to establish blank diameter.
A good portion of the time we take a very light skim cut over the finished knurling to improve the appearance and bring it to exactly print spec. Yes, I once had a customer who dimensioned a knurled surface to .002"+/-.