Single Point Knurling on CNC Lathe - Can it be done?

I've got a customer who orders some knurled rollers from me for use in the mfg of tires. (I have a NDA in place, therefore, NO pics or drawings can be shared with you - Sorry.) The knurl is a 16 TPI Diamond, sharp, done on a manual lathe with a two roll knurl holder. Just to keep things interesting these rollers are tapered, or conical. As you all know this is supposed to be impossible to do. Well, I do it and as you might imagine the results aren't exactly stellar. While the customer accepts this finish, I want to provide something better in order to further differentiate my shop from the other local shops. Not to mention get this knurling job OFF that manual lathe as I don't like the pressures involved. I think it's ruining the cross feed screw.

I have sitting here an Okuma & Howa ACT-20 lathe with a Fanuc 18T control. I also have limited experience with this machine, however, I have about eight years programming/operating experience on CNC mills. FWIW I have manuals on this lathe which aren't the greatest. The MTB manual points to the Fanuc control manual while the Fanuc control manual points to the MTB manual on so many things such as capabilities. This is where I'm hoping you all can help.

Okay - I heard you say, "just get on with it already!" So, my question is: Can this knurl pattern be cut with a single point tool onto the tapered surface of this roller? There is an encoder on the spindle. Does this mean the machine is capable of multi-start threads, or rigid tapping even? If so, what's the limit on the number of starts? It seems to me a single point tool similar to a threading tool, held normal to the tapered surface of the part (with custom holder, of course) could be used to cut the pattern. But, I have ran into a few things already with this lathe that seem simple, but require hidden parameter changes, etc.

I'm not sure you can single point a knurl easily. It might be doable if you have a lathe that can index and rotate with the movement of the tool. You will also probably need a specially ground tool that cuts more like a shaper tool than a threading tool. If you look at a knurl the helix angle is much shallower in relation to the centerline of the shaft than a thread is. The spindle would not be rotating in order to do this. You would have to move the tool and basically scratch the surface as the spindle turns to the proper angle over the length. It sounds like a far too difficult and time consuming operation to make money on. Maybe just invest in a better knurling tool and run them on the CNC that way. The CNC is much more ridgid than that manual lathe is. Good luck.

Bernard

Never thought of this... I feel like it definitely wouldn't look/feel the same because knurling relies on pushing material "up and over" instead of cutting in, creating semi-rounded peaks. In the machines I use, Q is the modifier for the thread start angle, for instance:

G76 X0.913 Z-1.0 K.004 D.011 F.0625 Q5000
G76 X0.913 Z-1.0 K.004 D.011 F.0625 Q10000
G76 X0.913 Z-1.0 K.004 D.011 F.0625 Q15000

... and so forth up to 360000 would give you thread leads staring 5 degrees off of each other.

That being said, I have a few parts I run regularly that we knurl in the CNC lathe with the standard double roller style tool. Just takes some experimentation and note taking and you will be able to get repeatable good results.

lpmagruder said:

... I have a few parts I run regularly that we knurl in the CNC lathe with the standard double roller style tool. Just takes some experimentation and note taking and you will be able to get repeatable good results.

Click to expand...

I must be losing my MIND!!! I click "Reply With Quote" and it REPLACES YOUR "CNC mill" with 'CNC lathe'!! WTH??? I did this three times with the same result!

Are the parts you knurl tapered?

lpmagruder said:

Never thought of this... I feel like it definitely wouldn't look/feel the same because knurling relies on pushing material "up and over" instead of cutting in, creating semi-rounded peaks....

Click to expand...

I agree the look will be different as the material won't be displaced but rather cut. While I've never used one, knurls are available that cut instead of displace...

WayneC369 said:

I must be losing my MIND!!! I click "Reply With Quote" and it REPLACES YOUR "CNC mill" with 'CNC lathe'!! WTH??? I did this three times with the same result!

Are the parts you knurl tapered?

Click to expand...

When you say tapered. Do you mean conical? Seems to me like you could angle a knurling tool to the right position and program the piss out of it.

Then again, you might be able to use round knurls, keep the tool oriented properly and just program it that way. I think there are lots of ways to skin this cat.

BR3 said:

When you say tapered. Do you mean conical? Seems to me like you could angle a knurling tool to the right position and program the piss out of it.

Click to expand...

Yes, indeed - conical...

This same method is what is being used on the manual lathe. Swing the compound around to the proper angle and shove it in. But, the knurl is fugly. As diameter changes the knurl can't track properly.

BR3 said:

Then again, you might be able to use round knurls, keep the tool oriented properly and just program it that way. I think there are lots of ways to skin this cat.

Click to expand...

The knurl rolls used currently are rounded. These provide a better finish than square, but it's still lacking....

WayneC369 said:

I must be losing my MIND!!! I click "Reply With Quote" and it REPLACES YOUR "CNC mill" with 'CNC lathe'!! WTH??? I did this three times with the same result!

Are the parts you knurl tapered?

Click to expand...

Ha, I realized my mistake and immediately edited, I should have left a note!

No, they are not tapered, but with the correct angled rollers and a little math it should be no problem getting the code to do it correctly.

lpmagruder said:

Ha, I realized my mistake and immediately edited, I should have left a note!

Click to expand...

Wheeeww... Nothing on you, but I run into this constantly it seems. I see something on screen and later it turns out it wasn't there. Just yesterday I edited a drill cycle. I knew I changed the G83 to G81, but to my dismay I left it as G8 - a non-modal rapid. Snapped the 1/2" shank off flush with the body of a 1" single flute countersink on it's very FIRST use - straight out of the box. $50 down the drain. But, I digress...

Sometimes it helps to think about what the finished parts has to look like. I'm trying to imagine how the knurl progresses as the diameter changes, and it's not working for me. I wonder if you called Eagle Rock or some other place that makes rolls and tools, if they'd have some trick for this situation, maybe even a special knurl.

Conrad Hoffman said:

Sometimes it helps to think about what the finished parts has to look like. I'm trying to imagine how the knurl progresses as the diameter changes, and it's not working for me. I wonder if you called Eagle Rock or some other place that makes rolls and tools, if they'd have some trick for this situation, maybe even a special knurl.

Click to expand...

Agreed. The taper or cone shape IS the problem. I contacted both Eagle Rock Tech. and Dorian with no joy. Both reps pointed me to a tutorial on how it's done on straight shafts. I don't recall which but one of them suggested the sintering process IIRC of which neither I or my customer are interested in due to cost.

WayneC369 said:

Agreed. The taper or cone shape IS the problem. I contacted both Eagle Rock Tech. and Dorian with no joy. Both reps pointed me to a tutorial on how it's done on straight shafts. I don't recall which but one of them suggested the sintering process IIRC of which neither I or my customer are interested in due to cost.

Click to expand...

You need a do the knurling with a conical knurl as well. It needs to work like two bevel gears. See this discussion:

How To Knurl Prop Drivers

Can you change the knurl pattern to be a square grid vs a diamond pattern? What I am thinking is the end result would be a square pattern vs the diamond. Each island would be like a pyramid. You would cut the grooves around the cone on the lathe then use a mill with an indexer or a live tool on the lathe to cut parallel to the axis to get the other groove to finish out the pattern.

Not sure if that made sense at all, but what I am picturing would be a straight forward task and you wouldn't be relying on knurling tools. I am guessing that they are being used as some sort of feed roll, so the pattern may not matter as long as it works and doesn't tear up whatever it is feeding?

Chris Lesiak said:

You need a do the knurling with a conical knurl as well. It needs to work like two bevel gears. See this discussion:

How To Knurl Prop Drivers

Click to expand...

Thanks, but I don't need a straight knurl pattern, it must be a diamond pattern.

Hello Wayne,
Knurling with a single point tool is quite doable. Basically you cut a multi-start, left and right hand thread on the feature where the knurl is required. If you can only start at one end of the feature, you need to use two tool, one upside down and one right way up and reverse the spindle. Alternatively, start the left hand threads from the chuck end of the feature. Depending on the helix angle of the grooves being cut, the tool may have to be cranked over to accommodate

The problem is with the taper. Because the circumference at the large end of the taper is greater than that of the small end, the spacing between each thread groove will be greater at the large end; same number of divisions at each end, but the circumferences are different.

Regards,

Bill

macgyver said:

Can you change the knurl pattern to be a square grid vs a diamond pattern? What I am thinking is the end result would be a square pattern vs the diamond. Each island would be like a pyramid. You would cut the grooves around the cone on the lathe then use a mill with an indexer or a live tool on the lathe to cut parallel to the axis to get the other groove to finish out the pattern.

Not sure if that made sense at all, but what I am picturing would be a straight forward task and you wouldn't be relying on knurling tools. I am guessing that they are being used as some sort of feed roll, so the pattern may not matter as long as it works and doesn't tear up whatever it is feeding?

Click to expand...

I understand what you're getting at and that just might work. I think I would use a threading tool in the lathe, then thread mill on the milling machine. You are correct in your feed roll assumption.

If I could only figure out if this Okuma can allow multiple thread starts (as in 22)...

AND allow a high enough Z axis feed rate with this wonky "threading" move...

I would then figure out how to take a stand up threading tool and roll it over 90° so that it's facing the chuck in an axial direction and figure out how to center it...

Then figure out how to mount the part in the chuck (on a mandrel perhaps) with plenty of clearance in case something went awry to avoid a chuck/turret collision...

I suppose before all that I should determine whether I can write the code to make it work....

Ooops I think I visualize an issue... The OC distance between the grooves will get wider on the fat end than whats on the skinny end...

WayneC369 said:

Thanks, but I don't need a straight knurl pattern, it must be a diamond pattern.

Click to expand...

OK, so you need two conical knurls: one with a right hand helix and another with a left hand helix.

But the most important thing from the "knurling a prop driver" article is the explanation of why your cylindrical knurls can't work -- the pitch needs to change with changing part diameter. But your cylindrical knurls have a fixed pitch.

If you single point the knurl pattern, you can achieve the variable pitch required. But be aware that the variable pitch can mess with the resulting taper. You probably want the pitch diameter (not the minor diameter) to match the taper.

angelw said:

Hello Wayne,

The problem is with the taper. Because the circumference at the large end of the taper is greater than that of the small end, the spacing between each thread groove will be greater at the large end; same number of divisions at each end, but the circumferences are different.

Regards,

Bill

Click to expand...

I wouldn't begin to know how to do the math or if the machine will do both at the same time but couldn't you cut a multi-start thread with a increasing and decreasing variable lead to keep the spacing uniform the whole length of the taper?

Brent