fusion 360 knurling

[steve918]

 I have a curved surface (spiral) that I want to apply a knurled texture to, but I'm not really sure where to start.  Anyone done something similar? 

[steve918]

Also, this is going to be designed to be 3D printed so it needs to be an actual texture, not just visual effect.

[SallyYang]

Hi Steve,

If you want to 3D print the knurled textured surface, you have to create features on the face, such as sweep or pattern along the spiral edge. I've seen your other post in the forum asking for sweep issues for the similar model, and I am very happy to heard that you have finally got your expected result. Hope you enjoy designing in Fusion 360.

[steve918]

I know how to sweep a 2D sketch around a profile, but can you take a 3D body and make it repeat around a curve using sweep?

[carl_bass]

This one was done by projecting a line to the surface of the cylinder to make a 3D curve -- then a profile was swept along the curve to make the cut. The cut was then arranged in a circular pattern to make all the "cuts" one way and then mirrored to get the crisscross pattern. You can make it look good but it's painfully slow.

[steve918]

This took me a while to grasp and get working like I expected, but your reply was extremely helpful.  Even though what I have now is not exactly what I'm trying to accomplish, it's pretty close and I know what I need to do to get it right.

Thanks!

[Pildammarna]

Hi, 

I am trying to project a knurling like this to a concave cylinder. But I cannot figure out how to do it, I only get different error messages about the sketch when using projecting to surface. 

Is there a tutorial on how to do this somewhere?

[colin.smith]

Hi Pildammarna

Can you share a screen shot of what you are trying to do?

Thanks

Colin

[jeff_strater]

I'm not sure exactly what error messages you are seeing using Project To Surface, but I can make a guess:  Is it:  "Not support projecting sketch geometry into same sketch, please change the target sketch or geometry"?  If so, this is because you need two sketches for this command - one as a source, and the other as a destination.  See:  project-to-surface-what-do-we-do-wrong for more information.

Jeff Strater (Fusion development)

[Pildammarna]

Hello,

I did not get any notifications of new posts in this thread so I have not continued to explore it (I have subscribed now). For the time I have used a bitmap to visualise the look I want. 

I will try it out more if/when 3d-printing it. 

I did get the skech error message you are talking about, but I did solve that problem on my own. It was the next step that I did not work for me. I will post a screenshot when I get back to it, perhaps it works now with the lates update. 

[EDuffner]

Hi, I've just started using Fusion 360, it's amazing!. Carl, how did you twist your profile curve so that it stays perpendicular to the cylinder surface and sweep curve? Thank you.

I've been wondering if you could do this another way but is it possible to multi select points of a body in the "Model" workspace and move, rotate them relative to the same body?

So let's say you require a knurled part approximately 22mm diameter, plus knurl depth and 14mm high; my thinking is:

1. Sketch a circle 22mm dia'.

2. Sketch a profile of one knurl point onto the edge of the circle, 0.6mm. (a bit like a one-tooth gear)

3. Extrude the circle and the point to the required length, 14mm.

4. Create a circular pattern of the two long faces of the knurl to however many will fit around the circumference of the created cylinder, around 40 knurls. (This makes a straight knurled part).

---- Here's where I'm not sure if the following is possible...

5. Construct an axis through the cylinder.

6. Multi select all the points at one end of the of the cylinder and rotate them around the axis, causing the knurls to twist or tip at an angle around the cylinder.

7. Select all the angled knurl patterns and mirror them the other way around the cylinder.

     

 

So I'm thinking somehow grab a hold of just one end of this cylinder shape and twist it.

If this is possible there is one catch. The resultant pattern will be an internal or 'female' knurl, so the method would have to be performed on a tool and used to make a boolean subtract on a blank cylinder.

Regards,

Ed.

[Anonymous]

Hi there, just started with Fusion last Saturday and came up with this problem myself, while trying to recreate the Schaller M6 locking machine-head.

So this is what I did:

1. Create the cylinder, sketch the diagonal at a 3o degree angle, midpoint constrained to cylinder axis, and projected to cylinder surface:

 

2. Created two triangles at each projected endpoint of the projected curve with necessary constraints (this sounds funky):

3. Loft feature, with projected curve as the centerline, set to cut:

4. Pattern the Loft, mine took 32 copies to fill the circumference:

5. Mirror using a plane that contains the revolution axis:

6. Combine-intersect the two bodies and all done:

I don't know if this is an approved method, but this is the best I could do at the time without searching too much in the net.

BTW this is as far as I got in my recreation:

I hope that was usefull.

Cheers!

PS: Sorry for the discrepancy in images sizes...

[brianrepp]

Very nice @Anonymous!  Curious what you're designing/building?  Assuming a guitar of some sort based off the tuner?

If so, there have been a few great threads related to guitar building you might want to check out:

http://forums.autodesk.com/t5/design-validate-document/beginner-question-arch-top-guitar-model/m-p/5564290/highlight/true#M11145

http://forums.autodesk.com/t5/design-validate-document/guitar-body-help/m-p/5792319/highlight/true#M31634

http://forums.autodesk.com/t5/design-validate-document/guitar-fretboard-help/m-p/5796834/highlight/true#M31865

http://forums.autodesk.com/t5/design-validate-document/finished-guitar/m-p/5839643/highlight/true#M34321

[Anonymous]

Thanks Brian!

I'll definetly take a look.

I've been thinking of designing a guitar for quite some time, and after finding out about Fusion I decided to make it a training project.

The next item on my list is a bridge, haven't decided on which one yet...

Hopefully I'll learn a lot through this.

🙂

[brianrepp]

@Anonymous Love the idea... don't hesitate to start a thread at some point to talk about your progress, seek advice, etc.  There are a surprising number of luthiers here on the forums, myself included!

[zenkustumz]

I'm very new to Fusion and have tried to replicate this knurling and have not even come close. i'm wondering is somone could assist me in step by step maybe?

I am looking for only doing the single diagonal cut not the knurling look as in this post.

Thanks in advance.

John

[Anonymous]

Well, the single diagonal cut is half the knurl, since the latter is created by combining two such steps. All you need is the path of the cut, as path on surface (projected maybe), and the start-end sections for the sweep.

Hope this makes sense to you.

[Anonymous]

brilliiant work!

[EDuffner]

Fantastic work nnatsios !!!

I'll have to try again with your method. I wonder if you can rotate your triangle shapes 180° so that the knurl is in the correct orientation and save having to do the combine/intersect step?

Kind regards,

Ed.

[Anonymous]

Hi Ed,

I think it has more to do with the direction of the sweep path, than with
the orientation of the profile.
If you try it, let us know how it worked.

N.