Issue with loft and matching verticies

steven_abiuso

It seems no matter which verticie I pick to mate to, the right side face coming from the body tries to connect to the top of the circle. I have no manually placed vert there, nor could I select one at that location. My ideal situation would be that it follows my sketch as a guide, but I realized you cannot select more than one pair of verts to assist the loft in creation. Is there something I am missing here, or is this an intended feature?

I am most concerned about the geometry being symetrical as this is a functional part and will be 3d printed. Any suggstions or help here would be appreciated!

mahir

You're right, you can only select one vertex per profile. Don't think of Match Vertices as a vertex-to-vertex map. It's more of a clocking feature that sets "vertex 0" for each profile. The best way to force correct vertex mapping is to make sure each profile has the same number of line segments. It looks like your blue body has 8 segments (4 sides, 2 chamfers, 2 fillets). Instead of using the end of your shaft as the profile, start a sketch on that surface, Use/Convert the circular edge, and use the Split command to segment that circle into 8 pieces. Now when you use the Match Vertices option, the rest of the loft should fall in line.

Here's an example.
https://cad.onshape.com/documents/57acdfaae4b005c413ed9b6f/w/3fd585a46d3af1b3ba413c53/e/d83a0ad59f9f6a2a297dc6e7

konstantin_shiriazdanov

maybe worth to try to select edges instead of faces, or make several surface lofts with Enclose

mahir

You're right, you can only select one vertex per profile. Don't think of Match Vertices as a vertex-to-vertex map. It's more of a clocking feature that sets "vertex 0" for each profile. The best way to force correct vertex mapping is to make sure each profile has the same number of line segments. It looks like your blue body has 8 segments (4 sides, 2 chamfers, 2 fillets). Instead of using the end of your shaft as the profile, start a sketch on that surface, Use/Convert the circular edge, and use the Split command to segment that circle into 8 pieces. Now when you use the Match Vertices option, the rest of the loft should fall in line.

Here's an example.
https://cad.onshape.com/documents/57acdfaae4b005c413ed9b6f/w/3fd585a46d3af1b3ba413c53/e/d83a0ad59f9f6a2a297dc6e7

steven_abiuso

mahir said:

You're right, you can only select one vertex per profile. Don't think of Match Vertices as a vertex-to-vertex map. It's more of a clocking feature that sets "vertex 0" for each profile. The best way to force correct vertex mapping is to make sure each profile has the same number of line segments. It looks like your blue body has 8 segments (4 sides, 2 chamfers, 2 fillets). Instead of using the end of your shaft as the profile, start a sketch on that surface, Use/Convert the circular edge, and use the Split command to segment that circle into 8 pieces. Now when you use the Match Vertices option, the rest of the loft should fall in line.

Here's an example.
https://cad.onshape.com/documents/57acdfaae4b005c413ed9b6f/w/3fd585a46d3af1b3ba413c53/e/d83a0ad59f9f6a2a297dc6e7

Worked like a charm! thanks for teachine me a neat trick