How to create a low-poly object in Onshape

vikram_koli595

I would like to create these types of low poly shape in Onshape. It seems difficult to model because all of the faces point in random directions. Any help would be accepted. Thanks!

MichaelPascoe

Here is one approach you might try:

• Sketch the base
• Sketch front plane points (or another custom plane)
• Sketch side plane points (or another custom plane)
• Fit spline one line at a time
• Fill each triangle
• Fill the base
• Shell the faces that you want to be left open

If you do these kinds of parts a lot, consider having a custom feature made for this.

MichaelPascoe

EvanReese

check out the Convex Polyhedron feature by @konstantin_shiriazdanov.

Also, a note for the workflow above: you can loft a straight line to a point, and skip the splines, since you can use the edge of the loft before. (pro tip: Usually, this would make your UV curves all converge at the point, but since it's planar, Onshape recognizes that builds it as a trimmed rectangle).

MichaelPascoe

Here is one approach you might try:

• Sketch the base
• Sketch front plane points (or another custom plane)
• Sketch side plane points (or another custom plane)
• Fit spline one line at a time
• Fill each triangle
• Fill the base
• Shell the faces that you want to be left open

If you do these kinds of parts a lot, consider having a custom feature made for this.

MichaelPascoe

EvanReese

check out the Convex Polyhedron feature by @konstantin_shiriazdanov.

Also, a note for the workflow above: you can loft a straight line to a point, and skip the splines, since you can use the edge of the loft before. (pro tip: Usually, this would make your UV curves all converge at the point, but since it's planar, Onshape recognizes that builds it as a trimmed rectangle).

vikram_koli595

Thanks for the help! This is a great solution. I will model one of these shapes and will post the end result in the chat! Thanks again!

MichaelPascoe

That's pretty sweet.

Evan_Reese said:

check out the Convex Polyhedron feature by @konstantin_shiriazdanov.

Also, a note for the workflow above: you can loft a straight line to a point, and skip the splines, since you can use the edge of the loft before. (pro tip: Usually, this would make your UV curves all converge at the point, but since it's planar, Onshape recognizes that builds it as a trimmed rectangle).

vikram_koli595

One question, When you say Loft a line to a point, do you mean this?

EvanReese

yep! that's exactly what I mean. I also realized that I could pretty easily modify my Freeform Spline feature to be a 3D points feature, which I've wanted from time to time, so I just converted it real quick. You can add it here to make your points. I'll make an icon and tidy it up sometime soon and post in the main group, but it seems to work as-is.

vikram_koli595

Thanks for the resources! I will first finish the model and then take a glimpse into computer-generated models. Thanks

vikram_koli595

Another question. It keeps giving me an error once I have made a full rotation of bottom lofts. I'll include a gif.

vikram_koli595

Oh Fixed The problem. Here is how. 

bruce_williams

I believe that is from 'non-manifold' geometry. The surface cannot be joined at a single point. Once you create a new surface and then 'add' final it creates a full edge joint.

You may follow this thread and related.

vikram_koli595

Thanks for all of the help! I have finished the model. Here are some pics and a gif

MichaelPascoe

Nice work!

vikram_koli595

Thanks!

EvanReese

Nice! looks good.

vikram_koli595

Thanks!

roman_jurt190

Just used a Variant of this workflow and thought I'd share it:  

- Make a base-sketch with lines (as a start for the lofts)
- Make 3D-Points by using @Evan_Reese  3D Points FS 
- Use lofts "line to point" (ending each feature with [shift]+[return] opens a new loft-feature immediately!)
- Make a paper-thick sheetmetal

This process gives you free, fast and live 3d-manipulation of all points at the same time.
Adding new points to the "mesh" is still a huste, though.

This is potentially a fast process for prototyping and packaging:)

Have a look:
https://cad.onshape.com/documents/bbec0b3d977212a847973244/w/fcc4f6d8f58fe6b605d9e91e/e/4d91b54655dd25f7b6a89c92