Cut Knurling

[trirotor]

Hello all! I like to machine parts for a multitude of things. I would consider myself a hobbyist. I finally purchased a Quick cut knurling tool for diamond style knurling. I am using this on a manual Hardinge HLV-H. I need to knurl a 6061 aluminum tool / knob/ hand-grip thing. Its 2.5" diameter and about .750 wide. I'm using .8mm pitch cutter wheels. The problem I am having is that I get a near perfect pyramid for the first .250", and then I start to loose the peaks after that, all the way to the end. I did some practicing on different diameters and with multiple pitches, and got great consistent patterns. Why does the nice cut stop half way thru now?

 

[L Vanice]

I have a number of older Miller Quick three-wheel tailstock-mounted knurling tools that perform very well. I have some Quick wheels that came with some of the tools, but have always bought USA-made Accotrak metric wheels when I needed new ones. I think I have only used my Quick tools on steel, so I have no experience with knurling aluminum.

I made a set of new steel stop screws and lock nuts for an old Hardinge turret, to give you an idea of how my tools perform.

Larry

 

[William Payne]

I’m going to pay attention to this. Out of all the things a person can do on a lathe I never had much success knurling. It was such a rare thing to need to do that I never got much practice and when I had to do it I sucked.

 

[Cole2534]

The circumference needs to be an exact multiple of the wheels pitch.

2.5" diameter gives a 199.517mm circumference. 2.496 is the next multiple down, but probably won't clean up. 2.476 is what I'd probably shoot for.

 

[trirotor]

The circumference needs to be an exact multiple of the wheels pitch.

2.5" diameter gives a 199.517mm circumference. 2.496 is the next multiple down, but probably won't clean up. 2.476 is what I'd probably shoot for.

If so, how does the first part of the run turn out nice / perfect, and as it continues it degrades? Wouldn't it all be poor from one side to the other?

 

[machinistrrt]

The circumference needs to be an exact multiple of the wheels pitch.

2.5" diameter gives a 199.517mm circumference. 2.496 is the next multiple down, but probably won't clean up. 2.476 is what I'd probably shoot for.

It doesn't need to be a perfect multiple, there is some latitude but the closer the better. The OP should acquire a copy of Reed's book on the subject, and yes, google is your friend.

http://www.reed-machinery.com/wp-content/uploads/2019/04/knurls-and-knurling-tech-data-master.pdf

I've found better results using the two diagonal knurl method compared to a single diamond knurl.

 

[sfriedberg]

If so, how does the first part of the run turn out nice / perfect, and as it continues it degrades? Wouldn't it all be poor from one side to the other?

Inspect the cutters at the end of a cut, after they've started messing up. Are the teeth clean or have little chips accumulated?
Do you have a DRO? Does it read the same at the beginning and end of cut, or is the cross-slide pushing away?
Is the compound securely clamped, or is it pushing away?
Check for the obvious, too: measure your pre-knurl part at both ends to see if there's a taper.

 

[Billtodd]

With my homebrew version oof the hardinge cut knurler, I find i have to angle the tool into the job to give some clearance to the trailing part of the cutters.

Generally, it is a pita to get right.

 

[Cole2534]

If so, how does the first part of the run turn out nice / perfect, and as it continues it degrades? Wouldn't it all be poor from one side to the other?

Cumulative error, I think.

It doesn't need to be a perfect multiple, there is some latitude but the closer the better. The OP should acquire a copy of Reed's book on the subject, and yes, google is your friend.

http://www.reed-machinery.com/wp-content/uploads/2019/04/knurls-and-knurling-tech-data-master.pdf

I've found better results using the two diagonal knurl method compared to a single diamond knurl.

Discussing with Accutrak, they want to see the circumference/pitch relation accurate with a thousandth and really prefer a few tenths.

How do you select a feed for the tool?

Thanks for linking the Reed manual, I'd not seen that.

 

[machinistrrt]

Discussing with Accutrak, they want to see the circumference/pitch relation accurate with a thousandth and really prefer a few tenths.

How do you select a feed for the tool?

I did my knurling on an engine lathe, the diamond knurls were for gripping by hand, and aesthetics mattered, or for cast in place bearing liners. Some experimentation was needed. Straight knurls were done on replaceable liners and were specified as to pitch and the amount the knurl was raised. Again, calculation of integral number of teeth was done, it's surprising how a minor change in the before knurl diameter affected end result. Lower speeds and hand feed was the rule. I think Accutrak is off base here, or are assuming mass production rather than small batches.
Knurling is a forming process, always seemed kinda brute force to me, best results were "by feel".

 

[technocrat]

touch the work with the knurl tool, just enough to leave an impression. Rotate the chuck by hand just over 1 turn and check the over/under lap. Take a light cut if necessary to adjust the diameter.

 

[swarfless]

Looks to me like the height adjustment on the tool shifted, notice the difference in the two cross helices. Another consideration might be that aluminium, being softer than steel has less 'drive' & the cutters are not equal in their demands on that score. Personally I use neat cutting oil when cut knurling out of consideration for lubrication of the cutter 'bearings' as much as for clearing the swarf. I think aluminium would be more sensitive to uneven friction too, but I lean mainly to shift in height.

 

[basalt]

Have you tried cutting oil or coolant and compressed air to blow away the chips?

 

[Cole2534]

Looks to me like the height adjustment on the tool shifted, notice the difference in the two cross helices. Another consideration might be that aluminium, being softer than steel has less 'drive' & the cutters are not equal in their demands on that score. Personally I use neat cutting oil when cut knurling out of consideration for lubrication of the cutter 'bearings' as much as for clearing the swarf. I think aluminium would be more sensitive to uneven friction too, but I lean mainly to shift in height.

If I'm using a 2 roller tool on a QD post I don't lock down the elevation, I let the tool float.

 

[Sam I]

I've got the same tool and use it fairly regularly with great success on both our CNC's and manual machines (although I tend to just leave it in the turret on the CNC now). These may not solve your problem but here are a few things I've found to help:

Ensure both wheels touch the workpiece at the same time. You can adjust the height of the tool with an adjustment screw on the head and lock it into place with two cams. I find that tightening the cams shifts it a bit so I usually have to go a little higher or lower to compensate. Takes a few minutes to get right.

The adjustment of the wheels to give the correct clearance is important and on mine at least the numbers on the dial are more of a guide. Touch off the workpiece and check the clearance by eye - it should be 1-2 degrees so only slight. If you adjust the clearance you'll need to go back and touch of the work piece to set your X diameter as it changes with the adjustment. Sometimes if the knurl isn't great I'll play around with this a little and the result improves.

Start the knurl in the correct place. These tools need to be started in the work piece. According to the manual it's about 1 mm from the end of the part. Feed in slowly then use the auto feed when you get to depth (which is about .8 mm dia / .4 mm radial for a .8 mm pitch). I'm not 100% why this is by my theory is that of you feed in Z into the part it'll push the material up and not cut which could explain this.

Sometimes on gummy materials you may need to adjust this. Maybe take a cut at half depth and see how that looks then go back for a second pass if required. The wheels should pick up the existing knurl.

Flush with coolant - the cut knurl creates a lot of tiny chips. If they're not cleared they'll get smushed in to the workpiece and this cumulation can cause irregular finishes on the knurl.

These tools shouldn't run off the end of a work piece - you should back away in X before reaching the end of a part. I usually allow a few mm extra material then machine this off later if required.

Cut knurling is great. I can stick in just about any size work piece within the range of the tool and as long as I've followed the above steps the knurl usually comes out great first time.

 

[animal12]

I've been able to get some pretty nice knurls on aluminum & even some steels with my South Bend 9A using a old Armstrong knurlier & even with teh one that came with my import QCTP . Fluid , lots of fluid is how I did it , ya gotta keep them wheels cleaned out .
animal