What type of hardware do you have?
I have a knurling job and all I here is what a pain it is .I can't even get info on it from the tool house that specializes in knurling.The son is now the owner and aparently didn't learn any thing from his dad before he died.
What type of hardware do you have?
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Check Out My Build-Log: http://www.cnczone.com/forums/showthread.php?t=6452
There are a couple of things that can make knurling go better....
1) Some form of coolant or oil to keep the knurls from loading
2) Quality knurls - they need to be "sharp" and more importantly, the correct diameter / pitch
3) Rigid machinery, if your machine isn't up to the task, don't over do it. Knurling requires a good amount of side force against the part.
4) Watch your speed. More often than not, the maximum speed is controled by the knurling tool and how fast the knurling wheels can spin on their axels.
5) Perhaps one of the most overlooked, but perhaps most critical aspects - The part must be the correct diameter for the pitch of the knurl being used. Think of a knurl as a gear. In order for a gear to have 'X' number of teeth, the diameter of the gear must be the correct size. So, the diameter of the part and the pitch of the knurl MUST BE MATCHED to work good.
Hope that helps you a bit!
like Java says, more details including lathe, type of knurl (straight, diamond, cut), size and type of material being knurled etc.
just for fun, here are some great shots of a rope knurl done with a home made knurl by Frank Ford. http://www.frets.com/FRETSPages/Mach...ropeknurl.html
Oh Jeez Chris, now you've done it. Don't you know that your point 5 is 100x more controversial than religeon & politics combined for a metalworking forum! wars have broken out over the subject. there are some really accomplished metal workers on either site of that debate, for formed knurls, i'm more of school it doesn't matter, esp for a diamond knurl, although experiments by John Stevenson suggest it doesn't matter for straight formed knurls either. cut knurls are another matter
Last edited by Mcgyver; 09-09-2005 at 06:08 PM.
I guess some info would help huh?
The part is 4.75'' dia. 6061-T6.The knurl is a medium diamond female.
The machine is new Doosan cnc lathe w/ 3/4 tooling plenty ridgid.It's Equivilent to a Mori Sieki SL2.
My experience is manual not cnc so others here are better able to address this for cnc - I could describe the manual process but it would be a waste of time given your equipment.
AL is soft and easy to form knurl and that lathe is plenty big enough - i could do a good job of it with my 40 year old lathe in the garage so I think your lathe will handle it . It takes pressure to deform the work (unless you are doing cut knurls) so a light bench top lathe would need scissor knurls but it doesn't sound likes that going to be an issue.
Here is my advice. Use a manual machine. Take a skim cut on the od to "true it up". Use a "scissors type knurling tool". Use oil and blow the loose "flake's" of metal off the knurling wheels....
Knurling aluminum is pretty easy on a cnc lathe, once you get everything set up, it usually runs smoothly. Set your geometry offsets as you would any other od turning tool use the edge of the knurling tool as z 0...When I set the x geometry offset I skim cut the od with another tool first, then measure OD, then touch off the knurling wheels just untill both wheels leave witness marks then set the x offset at the diameter measured previously. Be sure to start your knurl with at least half of the wheels on the workpiece (in the Z axis) and plenty of x clearance. What I do is feed in to the cut diameter, then go 10 thou more, then feed z the desired distance, I get best results with .006/.008 per rev feed, after that use the x wear offset to tweek in the knurl, most of the time, it will take a couple trys to get it just right!
Oh, forgot-lots of coolant too!
Last edited by Chuck Pressure; 09-11-2005 at 12:53 PM.
I don't know how dead this thread may be but maybe someone's watching.
I'm making some small knobs with a hole into which I'm pressing allen head screws. The material is 303 stainless, .375" dia.
I've never done knurling with CNC, so I've never paid any attention to how deep I was going, I just pressed in until I had a good knurl and most of the time it worked.
So Now I want to do this CNC and the first results look like poop. I've set the knurl at first touch to .375, set the depth in the code to .345 fed straight in at 10 ipm delayed for 10 seconds and pulled out at G0. Crap!
Now I have a piece I did before without CNC, same material, same diameter, same knurl, and it's beautiful. What should I try?
your lathe feeds in IPM?... dont dwell. and dont feed at IPM,, feed per revolution. look up the specs for your knurling tool,and feed accordingly. Hope this helps.(I G92 it)
Okay, but it seems I might not get it knurled evenly all the way around. I'll try.
Feeds either way, Mach3
wait! what RPM What feedrate?