Offset path on cylinder

[u7120482]

Following on from my recent post Raise a section of a curved face, I realised I also have no idea how to do the next stage of my design.

In this design, I am creating a rivet-like effect by using path-pattern to repeat a series of small bumps around a path based off of a face.

On a flat surface this is pretty easy: Sketch -> Project face onto sketch -> Offset the path described by the face by -3 mm. It creates a path like the inner construction line in this screengrab. This sketch is just a generic example, to show the point that I have irregularly shaped faces.

How could I achieve something similar on a cylindrical or conical surface? I'm only recently familiarised with the surface tools: Could something like 'trim' be useful here? Or perhaps a 3d sketch could project the curved profile?

Here's a rough sketch of what I'm aiming for. Unfortunately I can't just use circular path, as it's not a rectangular surface. The blue circle is an example of just an initial bump that would be patterned along that path.

I do need the path to be a fixed offset from the edge of the face, 3 mm in my case, to create the effect I'm looking for.

Anyone who knows a good general process for this kind of thing, I would be very appreciative. I'm learning a lot with this design and it's good!

[davebYYPCU · Accepted solution]

From that previous example, you can modify the surface body used in the loft, by trimming the Offset amount away.

Boundary of this modified surface body is the path for the pattern.  You may have trouble with  rivet orientation, so use a sphere.  Cut screwdriver slots with face orientation way more difficult.

Might help....

[u7120482]

Hi Davey!

You're really saving my bacon today. I just gave that method a whirl and it works a treat! Good point on the spheres, I think I'll go back and replace my other rivets with full spheres too for consistency. I haven't tried with the screwdriver cuts yet, but worst comes to worst they can be done manually.

The only thing is that it's a jot tedious to have to go and create four offset planes/surfaces (I use the ruled surface tool and then the offset surface tool on my curved edges to create the trimming tool) and then do four whole trims. Is there a way similar to the extend surface tool to trim a surface?

[davebYYPCU]

Well, if I am following properly,  Kidney shape aside, will work for them too, 

We have a base cylinder surface, you want an offset surface 3mm above that.  

You were going to chamfer the draft faces, after lofting.  

Before you do the chamfer, take offset faces from the faces you are adding draft to.

Without the solid body you get this

These surfaces offset to the sphere path.  Some need trimming to the top surface, Use top of these surfaces edges for the Pattern.

Hide / Remove surface bodies and chamfer the sides.

That said, I am not following for the 4 x planes and trimming... your mentioning.

Might help.....

[u7120482]

Ahh I see what you mean now. That's a good way to go about it.

I was taking the offset face that I used for the loft, and created a number of planes and surfaces to using as "Trim Tools" with Trim, that were all 3mm offset. Then I had a version of my surface that I used for the loft that was now shrunk by 3mm.

[davebYYPCU]

Yep, but can't do planes for your kidney shape.  (Been thinking,  helps when you have to demo what your saying,  

When you Split face for whatever shape, thicken it by the lift amount.  No need to Loft.

Might help.

[u7120482]

For the kidney shape, I just used a ruled surface which I then offset from, and then used that surface to cut my original surface.

I did a bit of messing around with your method, but unfortunately it wont't quite work, as clean as it is. The -3 mm is from the edge of the fillet that I have on the chamfer that I forgot to mention. I'm happy for now with my method, as it gets the job done.