Modelling a Knurl

ShepRCS

HI All

Did anyone manage to make a Knurl work? I'm trying to find the best way. 

My normal method (solidworks) would be to do the following

1. Draw Helix on the surface to be Knurled
2. Sketch a triangle at end of Helix
3. Sweep a cut with the sketch along the Helix
4. Circular pattern the the sweep
5. Mirror the circular pattern
   

With Onshape I finally managed to get the following to work

1. Draw Helix on surface Clockwise
2. Draw Helix on surface Anti-Clockwise
3. Sketch Triangle at end of helix
4. Sweep a New part on first Helix
5. Sweep a New part on second Helix
6. Circular pattern both of the new parts
7. Boolean Add all of the sweeps together
8. Boolean Subtract Sweep mesh from part I want to Knurl

It works but is a bit long winded mainly because you can't pattern or mirror the feature you have to do the faces, but faces patterning does not work when the resultant geometry intersects.

Anyone any thoughts on how to do this more efficiently?

Screenshot of my end result attached


Shep

burhop

I gave it a shot but my variations were dead ends.  I ended up with the same solution as you  

lougallo

Currently we cannot pattern a pattern or mirror a mirror etc but those will come.  As far as approach, I did:

1. Helix/triangle/sweep
2. circular pattern body around center axis (n times)
3. Mirror all bodies about a plane located at the knurled circular body center.
4. Boolean subtract.

I could also do a face pattern for the first circular pattern then just mirror the single seed part then copy the faces and do another face pattern but face patterns are much more efficient but less robust to change.

ShepRCS

@LouGallo Looks good.  I tried mine with that few steps but had problems with spinning circle of death.  I'm on slow internet at the moment though so that is probably something to do with it!

Looking forward to pattern a pattern etc!

nathaniel_zaharia

How can you modify this to add a knurl to only a portion of a cylinder?  For example, I am modeling a maglite flashlight and the battery tube has a knurl about 4 inches long in the center of the tube.  

Here's what I tried to do:
-I made a separate cylindrical surface
-I made a helix on that surface and swept a cutting tool with it
-I moved that cutting tool to the maglite tube and made a circular array to have multiple tools
-I tried to Boolean those cutting tools to make half the knurling... and the boolean tool fails at that step

I suspect that I might be having an issue with trying to cut too many things at once, but I don't want to cut each piece of the knurling one at a time...

Any ideas?

traveler_hauptman

Can you share the model public?

nav

Hi @nathaniel_zaharia here is an approach, instead of having a surface separately why don't you draw it in your existing cylinder and extrude it the 4 inches you need, then you can create in that surface the two helix you need. One sweep to remove material and the second one to create new material then you use the boolean subtract to obtain the desired results.

nathaniel_zaharia

Awesome!  Thanks for the advice.  I thought I would get an email or something when people commented on this, sorry it took me so long to check back.

viru

@nathaniel_zaharia , Onshape already had given provision for getting notifications if anybody commented on your Initiated discussion or you tagged in any post.

Narayan_K

Yes. also you can set the notification preference such that you get the mail notification also.
1.click on account option in the right top corner and click on Preference.


2. You can set the following settings.


then save the preferences.Now you can get the mail for the notification.

nathaniel_zaharia

You guys rock my world.  

Thanks so much for the help.

nathaniel_zaharia

@nav can you explain this a little more?  I didn't quite understand.

nav

Hi @nathaniel_zaharia below the steps with images if still have doubts please let me know.

1. Extrusion of the maglite body

2. Extrude a surface using the external cylinder (Use the USE command to include the geometry)







3. Draw a plane where the extruded surface starts
4. Draw the sketch you need to sweep 

5. Sweep cut the sketch from last step using the helix as sweep path

6. Use Circular array command (Select face pattern) make sure you select all faces of the sweep 
7. Create another helix in the extruded surface this time change direction to counterclockwise
8. Sweep the same sketch from step four using the new helix and instead of cutting select the option NEW

9. Circular array of the new part.

10. Now a boolean subtract operation (Tools the 40 + parts you created in the last step, Target Part 1 in my case) 

 11. Final Result

andrew_troup

@nav
Could you alternatively use only the second part  of your procedure, then mirror the resulting 40 tools (about your "Top" Plane) to provide the opposite handed array of a further 40, prior to doing the Boolean subtraction?

nav

Hi @andrew_troup could you please send me some screenshots of your proposed method I couldn`t replicate it, thanks

nathaniel_zaharia

@andrew_troup :
I think the issue with your idea is that the tools disappear after the boolean subtract operation.

nathaniel_zaharia

@nav
Thanks so much, man!

andrew_troup

nathaniel_zaharia said:

@andrew_troup :
I think the issue with your idea is that the tools disappear after the boolean subtract operation.

Hmm... the way I visualised it, the Boolean Subtract would not happen until last thing, at which point, I would actually want the tools to disappear.

And even if I didn't, there's an option under BS to "keep tools" ... but perhaps I misunderstand what you're saying

@nav: for some reason I cannot currently connect to Onshape CAD, and it may be a while till I get a chance to try the method out.

imagineered

Not sure how this goes in Onshape, but in other packages, we'd normally just reference a knurl or texture it otherwise file size goes up 1000% & program speed goes down 500%. Can understand if it is a plastic part to be moulded but otherwise, times short  

nav

Hi @imagineered indeed this feature as well as others you'll see posted in the forums are just a note in a mechanical dtrawing (onshape currently lacks a drawing module but its coming soon), I believe by doing this we are pushing the limits of what OS can do online; in more complex assemblies these features probably won't be modeled. There are already some post in the forums talking about performance issues in large assemblies.

In my particular case that I'm part of this krurl post doing it even though I know its just a note in a drawing thought me some tricks from OS that I can use when modeling a different part.

Bobsico

Hey, I was looking at making a knurl on a curved surface and only found this

So I made it by splitting the curved surface with the extruded surface of the helix, then I just used a remove sweep along that surface's edges (and mirrored it for the other direction).

But my knurls point up, so something is going on here, the knurls are not uniform. I did click the keep orientation as the start and end orientation of the cut should be the parallel.

Anyone spot my mistake?

here's the workspace. BTW: it's a flywheel for a dart shooter, the intersecting cylinder is the soft dart.

https://cad.onshape.com/documents/f5df3b96c9aa9df4547fe789/w/7b122de7c5bf478aa0f7cecb/e/580b64043b172f4d71237eba

@imagineered : I'm designing to 3d print so I need all the final geometry in there.

Bobsico

I've found that my sketch profile did not rotate to keep aligned to the center of my helix to fix this I have now changed to using a loft and 2 profiles, this seems to work fine.

matthew_taylor783

It stills seems that Boolean Subtract does not actually subtract, infact it seems to duplicate parts instead of negating. I am having a very rough time with it currently. Video a guy posted on youtube shows it straight forward and on Onshape but after many thorough attempts I just cannot get it to properly knurl...very frustrating. Help please

SethF

@matthew_taylor783

matthew_taylor783 said:

It stills seems that Boolean Subtract does not actually subtract, infact it seems to duplicate parts instead of negating.

This part sounds to me like you need to deselect the "Keep tools" option within the boolean feature.

glen_dewsbury

This one was not hard to make with one sweep,  a mirror and circular pattern. The more items in the pattern the more time to drink coffee while the Boolean tool works!
https://cad.onshape.com/documents/12b0679a712bc6f544f72c07/w/67e973d9c8c7d9393a467fa0/e/7c9a41383482a51b93b58302

S_Regula

nav said:

Hi @nathaniel_zaharia below the steps with images if still have doubts please let me know.

1. Extrusion of the maglite body

2. Extrude a surface using the external cylinder (Use the USE command to include the geometry)







3. Draw a plane where the extruded surface starts
4. Draw the sketch you need to sweep 

5. Sweep cut the sketch from last step using the helix as sweep path

6. Use Circular array command (Select face pattern) make sure you select all faces of the sweep 
7. Create another helix in the extruded surface this time change direction to counterclockwise
8. Sweep the same sketch from step four using the new helix and instead of cutting select the option NEW

9. Circular array of the new part.

10. Now a boolean subtract operation (Tools the 40 + parts you created in the last step, Target Part 1 in my case) 

 11. Final Result

This is pretty slick, and easy to boot! I was looking for a simple way to model knurling on a cylindrical part, and I think this will suffice. Thanks for sharing!

EvanReese

Since this comment bumped the thread to the top I had to do my version. Here are some of my tricks:

• sweep the helix as a separate body
• use thicken on both ends of the helix to extend it out tangent to it so the knurl terminates more realistically
• mirror the swept part
• circular pattern set to PART, and REMOVE, so you don't need to boolean after. This also means if you add more grooves you don't have to edit the boolean feature to add them.

shaun_singh

Evan_Reese said:

Since this comment bumped the thread to the top I had to do my version. Here are some of my tricks:

• sweep the helix as a separate body
• use thicken on both ends of the helix to extend it out tangent to it so the knurl terminates more realistically
• mirror the swept part
• circular pattern set to PART, and REMOVE, so you don't need to boolean after. This also means if you add more grooves you don't have to edit the boolean feature to add them.

Works a treat!

gediminas_jurgaitis

lougallo said:

Currently we cannot pattern a pattern or mirror a mirror etc but those will come.  As far as approach, I did:

1. Helix/triangle/sweep
2. circular pattern body around center axis (n times)
3. Mirror all bodies about a plane located at the knurled circular body center.
4. Boolean subtract.

I could also do a face pattern for the first circular pattern then just mirror the single seed part then copy the faces and do another face pattern but face patterns are much more efficient but less robust to change.

2023 and we still can't pattern a pattern or mirror... unacceptable.

S1mon

That post was from 2015. You can pattern a pattern just fine now, and I’m pretty sure you can pattern a mirror.