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The dreaded knurling problem...

M

Markaj

Member
I seem to be getting asked for a knurled finish on parts quite a lot recently. I design & make custom made lights (luminaires), and customers do like to see a bit of knurling! - the industrial look is as popular as ever.
So as you can imagine rendering can get painfully slow. I was wondering how best to speed things up? Is it better to make a cut & pattern it, or make the pattern in the sketch & make one cut? Or would using a boolean subtract make a 'quicker' part? Is there some way of incorporating a step file? Or is it just something you have to put up with?
The same applies to perforated material - I had to do some Meccano type components a while back, - any timesaving tips?
 

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Lew_Merrick

Lew_Merrick

Guest
Markaj said:
I seem to be getting asked for a knurled finish on parts quite a lot recently. I design & make custom made lights (luminaires), and customers do like to see a bit of knurling! - the industrial look is as popular as ever.
So as you can imagine rendering can get painfully slow. I was wondering how best to speed things up? Is it better to make a cut & pattern it, or make the pattern in the sketch & make one cut? Or would using a boolean subtract make a 'quicker' part? Is there some way of incorporating a step file? Or is it just something you have to put up with?
The same applies to perforated material - I had to do some Meccano type components a while back, - any timesaving tips?
Click to expand...
What I do is have an Equation Editor controlled female knurl that I can adjust, use the Save As to my project folder such that I can use that to create a Boolean Subtract on my part. I actually have a couple of female knurl parts such that I can "break" the knurl into "edge 1" and "edge 2" with a "break" in between to merely show the limits of the knurled area. Basically, you will need to calculate the knurl size (more properly: knurl pitch) and adjust it to your part's diameter.

I am somewhat pressed for time, but I can dig them out and post them here later.
 
M

Markaj

Member
Thanks Lew, I was wondering about using a boolean subtract & I like the idea of using an equation to drive it. So once the boolean subtract part has been created, is it less of a headache for the software to generate? Or just the same.
 
Lew_Merrick

Lew_Merrick

Guest
Markaj said:
Thanks Lew, I was wondering about using a boolean subtract & I like the idea of using an equation to drive it. So once the boolean subtract part has been created, is it less of a headache for the software to generate? Or just the same.
Click to expand...
Most all knurling tools create a 90° included angle knurl. By using the OD to define things, I can leave a small "flat" on the knurl that is (shall we say) less damaging to the hands that have to grip it. The 90° included angle is actually "normal" (i.e. perpendicular) to the 45° spiral path. By using an integer Count as my variable for Pitch (i.e. number of knurl groove around the periphery) and can easily change the size of the knurl and not screw up the overall "fit."

The angular span of a full knurl is 360°/Pitch. The "trick" is then defining your inner polygon based on the OD and Pitch of the knurl. It takes a bit of "math" to make it work out (I use 95% of "actual" to be sure I get good coverage in my Boolean Basis part).

The thing is that adding this geometry does slow things down while you are working. This is why I (A) often only define the "ends" of the knurl and (B) suppress them until I am ready to display them.

The other thing is that few machinists have more than a couple of pitches available to their knurling heads. This is why real world knurled parts usually have a line of incomplete knurls when they are done.
 
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