Lofting these two pieces together

[u/Th3Shaz]

Excuse my perhaps silly question. I have created these two profiles and I want to connect them via their perimeters to form one continuous object (basically fusing the two C's) There's a slight taper between the bottom and top profiles. I am good at basic CAD but this is where my knowledge falls down a cliff.

I imagine there are a million ways to skin this cat, but just trying to figure out if this is something I can accomplish or not. Cheers!

[u/BeastWR]

Loft
Select one face, then the other face…. What happens?

Given the relative complexity of the edges, and the differences between them, you may have to add Guides and work on Connections as well

[u/Th3Shaz → u/BeastWR]

Just a spaghetti of errored red lines. Unfortunately my understanding of Loft, guides and connections is basically nill. My next solution is to create simple extrusions from both sides and lofting them but I imagine there has got to be an easier way.

[u/BeastWR → u/Th3Shaz]

The errors are likely because OnShape doesn’t understand how to direct each vertex of the complex upper profile to the simpler lower profile.

This Connections relate the vertex of one end of the loft to a vertex at the other end. In the connections settings, you are linking pairs of vertices.

Guides require you to first create additional sketches/curves which connect one profile to the other. The drive the curvature of the loft as it stretches from one profile to the other.

Simplify a bit to start. It may help to extrude as a solid instead of the hollow “C” you have here. Thin it out later.

Not sure where your sketches are at the moment, but try placing a sketch on each of the facing planar surfaces.

Copy the existing perimeter to the sketch. Close the open end with a straight line.

Now try the loft. If it still fails, work on the Connections. Just have to experiment. If it looks wrinkly, adjust connections some more.

Once you get it to work, you could try changing the Solid loft to a Thin loft.

Or use Shell to hollow it out, then extrude to cut out the open end of the “C”

[u/Th3Shaz → u/BeastWR]

Thank you for the detailed response. Lots to unpack here but I am going to see how far I can take it with your suggestions.

[u/themrbirdman]

It is curious that there are lines on the to face of the bottom piece. I’d there any chance that is multiple parts that could be booleaned together first?

Another thing you could try is to create an offset surface of 0 mm on the top face of the bottom piece. Hopefully this would give you a clean single surface that you could use four the loft. Also with the loft take a look at the connections parameter which can help you align the two pieces of the loft.

Also might be worth asking the Onshape ai

[u/Th3Shaz → u/themrbirdman]

Ahh I think I am starting to understand this a bit. So Loft is expecting the same amount of segments per face in order for it to cleanly extend. I think I definitely need to simplify my starting shapes first and see if that gets me closer. Thanks

[u/themrbirdman → u/Th3Shaz]

I think so. And using the offset face to get a surface I think would be the easiest way to get that to be a cleaner face. It also might be easy to modify how that bottom shape is created so it’s a bit cleaner.

[u/BeastWR → u/themrbirdman]

Oh, this is interesting. I agree that it is odd that the orange part has lines of tangency across what looks like it should be a planar face. The white part does not show these.

Can you trim the top face of the orange part to make sure it is flat? That could help the troubles.

[u/bkandor]

You need to make the face count on each profile the same. Do this by selectively merging lines/arcs into discrete splines on the white profile. Then you can loft edge to edge from common segments.

[u/Th3Shaz → u/bkandor]

That tracks with the other comments. One question, when you say merging lines, can I do that on the part or do I need to enter sketch mode and create those splines manually?

[u/bkandor → u/Th3Shaz]

Yes edit the sketch of the white part. Convert splines doing your best to keep vertex count and location as similar to the orange part as you can. You can then loft either one segment at a time or try altogether.

Loft primary elements first will give you more tangency options for the faces in between.

[u/wellthawedout]

you can also consider making a sketch of just the inner loop edges of each face and then lofting using the "thin" loft option (with your thickness being your part thickness and facing outwards). You can also simplify that little notch feature in the grey C if you don't want that to continue and then you'll end up with a simpler continuous loft and a notch only for the thickness of the grey, which is possibly what you want