Project sketch line onto curved surface

[psych_uk]

Hi Guys,

I've been trying to project a sketch line onto a cylinder (or a sphere) body in order to use that line as a path, curved objects cant be used as sketch planes so I was wondering how this is best achieved?

Right now I am splitting body (using the sketch line) and use the cut as the path reference, is there no easier way?

I am also concerned that the geometry isn't being calculated correctly using that method.

[davebYYPCU]

isn't being calculated correctly using that method.

Why?  

I prefer model edges over sketch projections.

Might help….

[psych_uk]

It seems to me that a project would take into account the curve, whereas the cut simply goes 90 degrees, maybe I am wrong about this, and project would do the same thing, in either case cutting involves having 2 bodies after the operation, and that pokes at my OCD.

[jhackney1972]

Take a look at the timeline on the attached model.  Change the Surface Sweep Twist Angle to experiment.  The same method can be used on a cylinder.  If you do not want a twist in the path, do not add it.   Model attached.

Edit:  Please ask if you have questions.

[psych_uk]

That's certainly a better way to get a repeating swirl around a cylinder or a sphere, however I couldn't get it to work with a spline, the profile and the path seemed to combine for some reason.

I guess what I was looking for is a method similar to the emboss, where your sketch geometry is projected onto the surface instead of a profile so you can use it as a path.

As you can see yourself, the method to achieve a quite simple task is very convoluted. I was hoping there would be an easier way.

[jhackney1972]

You can use a Spline for the path using the same method.  If you would attach your model, including the path you want, I would like to experiment with it.  Model attached.

[psych_uk]

I can see what you've done there, you've used the line and extruded it outwards to form the basis of the path, that's the same method I have been using (yours might be more elegant, I always forget about the surface tools).

The problem is there is no accounting for the curve, what you have is a curved plane protruding from the sphere flat (which is why you have to trim) By the way, if you extrude 'to object' instead of 'distance' you can omit the trim.

I'll give you an example, how did we get text to wrap before emboss? We had to flatten a wrapper and use it as the tool, just when we all got used to this, they gave us emboss, lol. I'd like the same mechanics to sketch lines, like you could take that spline and simply say 'give me a line on the surface I choose which will wrap the surface'.

[davebYYPCU]

What would you like us to say?  I have no trouble with a chine on a hull, using body edges.

Project to Surface, does what I think you want, but it is old school, 

As you can see yourself, yeah right!  My crystal ball is on an RDO.

even @jhackney1972 has provided his own model, 

You can only say Ah, but....

Might help....

[jhackney1972 · Accepted solution]

My last try to give you a pleasing solution.  Project to Surface is not perfect as it can get distorted as you reach the poles of the sphere but..  You can ignore one of the projected lines in the result.

By the way, I used a Trim Surface command in my last model to be sure you "understood" what I did.  I normally would do it the way you mentioned.  I never know the level of expertise of the user I am speaking to.

[psych_uk]

@davebYYPCU Little bit aggressive there dude, all I did was ask a question, and now we were having a civilized discussion.

[psych_uk]

Well now I feel stupid, 'project to surface' is what I wanted. Why did I not see that, I was sure I scoured all the menus.

Thanks @jhackney1972 

[psych_uk]

I've tried this myself and I cannot get the spline to project, I have included my attempt. It's saying projecting geometry onto the same sketch is not supported in the error dialog.

What I do is select the sketch on the offset plane (where the spline is) then I select project to surface, then I choose the sphere as the 'face' and the spline as the 'curves'. Is this right?

[davebYYPCU]

Project has always required the source to be in a previous sketch.

projecting geometry onto the same sketch is not supported

normal process,

Same for your example, you need a new sketch (editing) to put the result into.

I have done the same source with both options, Along Vector and Closest Point. 

Along Vector is your Extrude to Object, and 

Closest Point is effectively a Loft to Point.

Might help...

[psych_uk]

Thanks for the reply,

What was messing me up was the 3rd sketch (the 2nd of the pair), I couldn't figure out where it was coming from, but it's from the object face (it goes against my instincts to open a sketch on a curved surface). It didn't occur to me.

I have managed to reproduce the results, so thank you all.

[davebYYPCU]

Well that is not quite accurate. 

it goes against my instincts to open a sketch on a curved surface - which is not possible.

You still create the last sketch on a plane (or planar face n/a in this file)

Tick 3d sketch in the sketch palette, because your projection/s will be / are 3d,

and the rest takes care of itself.

Might help....

[psych_uk]

Ah, I see, must of been a fluke then that it chose the right plane, haha.

I just drew a rectangle on the sketch and now I can see it's on the same plane as the circle.

Makes sense I guess.

Thanks