Cnc Knurling help

Rogue_Machinist · Feb 18, 2020

Ok I used to knurl when i worked in a production shop but that was years ago. I have since forgotten how to set up and program a knurling job.

I need to program a knurl in D2 tool steel using a HSS 25tpi knurling tool. I dont even know if thats gonna be possible. Second we got a brand new Dorian Tool knurling tool.
How to cut knurl and is it a single pass and how do I set the tool. Its been probably 10 years since I did any knurling.

Sent from my HD1925 using Tapatalk

Nerdlinger · Feb 18, 2020

Is it a diamond shape pattern you’re going after? Is the “pre-knurled” diameter a section of material all by itself with relief on both sides? Is it a double wheel knurl?

Rogue_Machinist · Feb 18, 2020

Nerdlinger said:
Is it a diamond shape pattern you’re going after? Is the “pre-knurled” diameter a section of material all by itself with relief on both sides? Is it a double wheel knurl?

Double wheel knurl tool.
The knurled area will be slight larger than other diameters.diamon shaped pattern.

Sent from my HD1925 using Tapatalk

Nerdlinger · Feb 19, 2020

in short: make sure both wheels spin at the exact same time when hand-jogging up to the material, make sure the material diameter is proper for the pitch of the wheels you are using, feed in, over, and rapid out. I have tangled with my Dorian knurl over the years and found this guide to be darn good:

https://www.doriantool.com/wp-content/uploads/Knurling-Technical-Support-Final-Final.pdf

The only “trick” I discovered is for my application where we “form” knurl: ”in-feeding” did not work well for me. I made sure the part was the proper diameter, changed feed rates, etc but never got it to work. The instant I changed it to “end-feeding” (Without changing anything else) it worked beautifully.

Good luck!

Rogue_Machinist · Feb 19, 2020

Nerdlinger said:
in short: make sure both wheels spin at the exact same time when hand-jogging up to the material, make sure the material diameter is proper for the pitch of the wheels you are using, feed in, over, and rapid out. I have tangled with my Dorian knurl over the years and found this guide to be darn good:

https://www.doriantool.com/wp-content/uploads/Knurling-Technical-Support-Final-Final.pdf

The only “trick” I discovered is for my application where we “form” knurl: ”in-feeding” did not work well for me. I made sure the part was the proper diameter, changed feed rates, etc but never got it to work. The instant I changed it to “end-feeding” (Without changing anything else) it worked beautifully.

Good luck!

So the other question I have is do I set my workshift from the side of the tool or attempt to touch off the wheels. And that form you sent me is a PDF is there a place on the dorian tool website where that form is available to fill in the numbers for what I need. Like I said Ive done knurling before but it was years ago. And as we all know, if you dont do something often, sometimes we forget. And in this case Ive forgotten pretty much everything except how to set the diameter workshift. Hand wheel until both wheels spin and set to diameter.

Thanks very much.

FredC · Feb 19, 2020

I am going to ask a question I hope I do not confuse things for you. On my double wheel cut knurler I have to adjust the distance between the knurls for proper clearance for each diameter of work. Yours seem to be fixed as to the distance between the knurls.
Does your tool have a limited working range of diameters? If so is the work you intend to do have an OD within that range? The increments are 3,5,8,12,15,20,30,50mm on my tool.

Rogue_Machinist · Feb 19, 2020

FredC said:
I am going to ask a question I hope I do not confuse things for you. On my double wheel cut knurler I have to adjust the distance between the knurls for proper clearance for each diameter of work. Yours seem to be fixed as to the distance between the knurls.
Does your tool have a limited working range of diameters? If so is the work you intend to do have an OD within that range? The increments are 3,5,8,12,15,20,30,50mm on my tool.

Mine does have a working range. From 1" to 5" ideal size is 3" So for my work piece im fine.
Im just so forgetful when I dont do a job all the time. And all my old machining notebooks are long gone on how to set up a knurling tool. Hence why im asking how to set the face distance. LOL

Dan from Oakland · Feb 19, 2020

Dorian Tool has a very nice knurling calculator that runs in Excel. Call their tech service number and ask them to e-mail it to you. I just did a job that was a 25TPI straight knurl and the calculator was a big help in fine tuning the cut depth etc. Also, the Roll Form web site has a bunch of info and the formulas but its not as straightforward as using the spread sheet from Dorian. One thing that helped me was limiting the knurling time to about 20 revolutions. There are a few tricks to prevent double tracking that is addressed both at Dorian and Roll Form web sites.

Nerdlinger · Feb 19, 2020

nissan300ztt said:
So the other question I have is do I set my workshift from the side of the tool or attempt to touch off the wheels.

Thanks very much.

Ass-u-ming you have a Fanuc control, yes - hand wheel with the spindle on at a low RPM until the wheels just begin to track. When one begins to spin make sure the other begins spinning within another .001" click or two of the hand wheel. If not, you'll have to adjust the height of the tool until they BOTH begin to spin within .001" or .002" of each other. After you get them even jog the tool in X once again until they just touch the workpiece, type in the diameter in the offset page with the appropriate X Geometry offset highlighted and hit "measure" (i.e. "X3.000" + Measure). Then in your program you call up the tool and offset, say T0101 and feed .005" or whatever into the workpiece (i.e. T0101, G00 X3.1, G01 X2.995 F.010, etc.)

Good luck!

Rogue_Machinist · Feb 19, 2020

Nerdlinger said:
Ass-u-ming you have a Fanuc control, yes - hand wheel with the spindle on at a low RPM until the wheels just begin to track. When one begins to spin make sure the other begins spinning within another .001" click or two of the hand wheel. If not, you'll have to adjust the height of the tool until they BOTH begin to spin within .001" or .002" of each other. After you get them even jog the tool in X once again until they just touch the workpiece, type in the diameter in the offset page with the appropriate X Geometry offset highlighted and hit "measure" (i.e. "X3.000" + Measure). Then in your program you call up the tool and offset, say T0101 and feed .005" or whatever into the workpiece (i.e. T0101, G00 X3.1, G01 X2.995 F.010, etc.)

Good luck!

What about z?

Sent from my HD1925 using Tapatalk

FredC · Feb 19, 2020

After you have x set back off so your clear in Z, set your X in a few thousands and wheel in till you hear the knurls touch the end of your part and measure as usual. I would do this with a blank that is full stock diameter so I know where the where Z is in relation to the working diameter of knurls. If the surface that gets knurled is further back program your rapid approach accordingly.

Rogue_Machinist · Feb 19, 2020

Yeah ill write the program accord.

Sent from my HD1925 using Tapatalk

Rogue_Machinist · Feb 20, 2020

So todays the moment of truth. This is what ive calculated so far.
126RPM @.007"/rev for the knurl
my knurl calculator shows me for a 3.5" blank turn OD to 3.4887 and for a 25tpi knurl its going to be .014" per side.
So the knurl depth is going to be 3.461.

So hopefully it runs ok.
Got a piece of scrap in the machine and gonna go from there.

Nerdlinger · Feb 20, 2020

nissan300ztt said:
So todays the moment of truth. This is what ive calculated so far.
126RPM @.007"/rev for the knurl
my knurl calculator shows me for a 3.5" blank turn OD to 3.4887 and for a 25tpi knurl its going to be .014" per side.
So the knurl depth is going to be 3.461.

So hopefully it runs ok.
Got a piece of scrap in the machine and gonna go from there.

Good luck! Feel free to offset your tool out in X to start light and then move in to reduce the risk of blowing up your wheels!

Rogue_Machinist · Feb 20, 2020

Not quite right. But close

Sent from my HD1925 using Tapatalk

TeachMePlease · Feb 20, 2020

Infeed a little more, and get more coolant in there to get chips out.

Rogue_Machinist · Feb 20, 2020

TeachMePlease said:
Infeed a little more, and get more coolant in there to get chips out.

Feed was at .011 a rev.

Sent from my HD1925 using Tapatalk

Rogue_Machinist · Feb 20, 2020

Nerdlinger said:
Good luck! Feel free to offset your tool out in X to start light and then move in to reduce the risk of blowing up your wheels!

So yeah the wheels werent perfectly level. Re-leveled with a second pair of eyes. And did the feed at .011/rev and it did the wave and was inconsistent. So im gonna bump the feed up to f.012/rev and send it.

TeachMePlease · Feb 20, 2020

nissan300ztt said:
Feed was at .011 a rev.

Sent from my HD1925 using Tapatalk

I meant feed in deeper in X.

FredC · Feb 20, 2020

I do not have too many knurling programs, but the one I checked I use a feed in Z of .002 per rev. Your .011 seems to high to me, looks like 1/2 with of the diamond per rev.
I do agree with the others a little deeper in X and level out the tool so both cutters go to the same depth.

Cnc Knurling help

Hot Rolled

Stainless

Hot Rolled

Stainless

Hot Rolled

Diamond

Hot Rolled

Titanium

Stainless

Hot Rolled

Diamond

Hot Rolled

Hot Rolled

Stainless

Hot Rolled

Diamond

Hot Rolled

Hot Rolled

Diamond

Diamond

Similar threads