Results 1 to 11 of 11
Thread: Knurling 6061 speed and feed?
01-31-2008, 03:25 PM #1
Knurling 6061 speed and feed?
I have an upcoming job that needs a small amount of knurling for finger tighting a threaded pin. I have never had the occasion to do this before on a CNC so some recommendations would helpful.
The pin is 6061 and the body to knurl is .600” and I’ll be using a .750” straight 14TPI wheel. No specs on the knurl just clean and functional.
Reconditions for spindle speed, federate and dwell would be helpful
01-31-2008, 07:15 PM #2
I would look at one of those tools that "cut" a knurl rather than displace the metal.The ones that cut the knurl don't require as much force.
01-31-2008, 07:22 PM #3
I have found knurling on cnc is more of a pain in the a$$ than an art. the best thing you could do is call the tool manufacturer up and get a begening spec from them. more than likely it wont be right so try it on a test piece first. the trick is to come onto the part fast. i usualy feed on at 100 IPM. spindle rpm for this should start at 750rpm then g1 your z-axis at about 20 IPM. then rapid off the part. this is just a starting "SWAG" but it usualy gets me where i need to be. Best of luck....
01-31-2008, 08:06 PM #4
g-coder does it about the way I do. The key is to get onto the part and off asap, don't run the knurl over a previously knurled area.
If these parts are getting a dark color anodize you're up a creek no matter how you do it. Aluminum generates little flecks which pound back into the material when you knurl. During the anodizing process some of these invariably break off leaving little white specks (bare spots) on your work piece. No easy way around it.
01-31-2008, 08:29 PM #5
Just finished ('bout a month ago) a knurl in 6061 on 1.5" of stock material for a "functional" knurl knob. Took a .023 diametric cut (1.477 on X) at 1000 rpm (roughly 387 sfm). I fed in on Z at F.006 for about 2.5" an then back out on Z at same feed with no dwell. Left a beautiful knurl. I was using a double wheel tool locked on the medium wheels. Very little dust or specks left on the knurl. The other end was drilled and tapped. One dude took my "set-up" piece home to use it as a shifter knob. I have found that knurling on CNC is not much of a pain and can be tweaked just as any other operation. There's a job here now that is a .516 wide full radius 316 ss knob that needs a functional cross-hatch knurl along the whole raduis. That's gonna be done on a tool post lathe because the post has to angled 'bout 4 different ways to get the whole big radius knurled. That one won't come out pretty, but very grabby.
01-31-2008, 10:34 PM #6
With all the adjustments and movements at your beck and call - I Shirely don't know why knurling on CNC would be more daffycult than any other method?
I have had loose material in 1200 series steel knurls too. But alum's gotta be much werster! I know that I've done it - but not recently enough that I can remember. LOL!
I am Ox and I approve this here post!
02-01-2008, 02:18 AM #7
I don't have alot of machining experience but I have knurled alot of aluminum. On pc's that are long I use a straddle knurling tool with convex wheels. I set them up loose at first and adjust the pressure to get the look I want. Spindle speed is important also. 1000 rpm's or slower to 750 works good. I change my feeds until my part has almost no chipping at all. As was said in other threads get on and off fast so as not to over knurl. Sometimes hitting the material to fast can cause some chipping. Don't try to knurl to a sharp peak. That can create over knurling. Just create a slight valcano looking knurl and you will have less chipping. I use all 6061 for aluminum I have knurled. Good luck. Oh, all my parts get anodized by companies and they seem pleased.
02-01-2008, 02:50 AM #8
Go to the Dorian tool website. They have all the info you want. on cut knurls or formed. It's all in the numbers, bring a calculator.
02-01-2008, 04:35 AM #9
What GDgambler said.
accutrak is a very good source for knurling needs.
I would have to give them an A+++ on service and quality.
They mean it where they say ""questions? call us"" you will be talking to people that make this stuff and test it everyway possible.
02-02-2008, 10:53 PM #10
Tell ya somthing that will make you bite your nails when knurnling is Tungsten. I used to make some marine parts that started out at 3" dia X 4" long. the stock was $430.00 a pop. and just machining it was a nightmare. it kind of makes me think i would rather machine sandpaper. anyway, when it came to knurling i only had one shot. i whould wach the x axis load meter jump to 70-80% then here came the pucker factor. and axis foldback alarm whould have been detremental...
As far as the aluminum. the flaking from form knurling is a real PITA. i suggest vibratory the heck out of your parts befor anno. If you cant have a tummbled finnish you can use corn cobb or wallnut shells to beat the flakes off.
02-02-2008, 11:20 PM #11
If you can put a carbide shaft in the knurling tool it will not gall to the wheel, I prefer the scissor type knurling tools, but we found the secret to speed is the carbide pins and we used broken endmill shanks.