Round shapes on a rounded surface

[t_smith5]

Hi

This is closely tied to this forum thread I posted about getting flat shapes on a cylindrical body. Emboss worked perfectly for that job. However, for one of my current issues, it's not possible. I'm trying to extrude a bolt from the back's design so it's the right kind of roundness, but also so it lies on the surface correctly. Extruding it and using the Project Profile, Object and Offset options don't give me the desired look I'm after. Extruding it to the face just makes it look skewed. 😕

And sadly, Emboss doesn't work in this instance. Not quite sure why. The jetpack was cylindral and that worked perfectly. This isn't cylindrical, but is merely a rounded surface. Essentially, I'm not able to select the necessary face; it only gives me the option to select the flat side and bottom faces.

What would be the best approach for something like this? Thanks.

Latest file is attached.

[davebYYPCU]

There are no inbuilt tools to do what you want, but you can construct your way to the end game.

Create a section sketch, with Plane on Angle at the centre line. (Highlighted)

Project intersect the face involved, (x) sketch the centre line / profile, 

Pipe > Cut on the centre line of the sketch or 

Construct a revolve profile for the bolt / or bolt hole.

More than one was not mentioned, but circular pattern comes to mind.

Might help....

[t_smith5]

Yeah, I'll be using the circular pattern for the rest of them. 🙂

I'm just struggling to see where one thing starts and one ends in your image based on the angle. Is there any chance of doing your workflow in the file I've attached and then upload that? That way, I can scrub through the timeline to see exactly what you've done. 🙂

[davebYYPCU]

Yes and no, I can send a file tomorrow.

In the file as it arrived, there was that visible sketch on the Origin Plane.

I used the vertical line, to put a Plane at Angle, (+/- 45 deg) in the pic, can’t remember which way the 45 goes.  Can be the vertical Origin Axis.

Sketch on that plane.  Project > Intersect the body face, because I am near the top corner, the short purple curve is supplied.

I constructed the centre line, normal to the purple arc, (with a construction chord line) from the arc towards the centre of the body.  That’s all you need for a pipe > cut.

(Centre Line can be used for Plane on Path to sketch the circle profile but that’s more work)

If you have a specialised Profile, to revolve, (Rivet Head?) make it suit the centre line axis.

If your inserting a bolt - Joint to the end of the centre line.

Might help....

[t_smith5]

I'm a little unclear where your placing the Construction Line - the starting point and the end point on the curve...? I can't seem to get it right without the line going off elsewhere.

[davebYYPCU]

Your purple curves should be Arcs, (and not Splines,)

for the position of the height of bolt along the arc,

draw the centre line from the arc centre point to ( where it is needed)....

If it is a Spline, ( would be if the plane is to be parallel to the cut line) 

Draw a short chord line connected to the spline,

@ the mid point of this line (will be close enough - ) draw the line perpendicular to the chord line.  Extend to the spline.  Slide (click drag) the line end point to (bolt position).....

Might help.....

[t_smith5]

Sorry, but I'm confused with your explanation still. I'm not very good with text explanations when using software like this. 😓 I definitely need visualized explanations/breakdowns. I mean, this is definitely all done on a separate sketch, right? So there's the original Back Panel sketch and the new one via the angled Sketch Plane that was projected? Because if I'm working in one Sketch I'm not able to connect any lines to the other.

[davebYYPCU]

Correct, the new sketch, Hide the back one it is not needed.

In the new sketch you Project just the face the bolt goes on.  The rest could be deleted.

Use my steps on the purple curve.  You are constructing a side view of the bolt centre line.

when you get that far, you can Joint a bolt, Revolve a profile to cut the body, or Pipe Cut a drilled hole, and / or Pipe New body for a cylinder to fit the drilled hole.

To use the Hole Tool, (counterbore, countersink, threads) you need a New Plane on Path of the centre line.

What size hole, bolt, rivet, and where is it needed?  Similar to the canvas?

Can do a model in the morning.

[t_smith5]

I'll have to wait for the model demonstration. 😔

[davebYYPCU]

Plane at Angle is aligned from the origin, at a position that suits.  (You had that)

Project > Intersect the face this plane intersects with (you had that)

Draw one (or many) centre lines (- construction for this pic make one line normal for next steps)

from centre point to arc, for the Rivet Head, change the purple line to construction.

Draw the 10cm line - make the midpoint of this line coincident to the centre line,

make both end points coincident to the arc. 

Draw the 2 point circle from each line end point. Trim the circle if you wish.

Revolve the Head profile, Set to Join.

Might help....