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How to create a low-poly object in Onshape
vikram_koli595
Member Posts: 31 EDU
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!
0
Best Answers
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MichaelPascoe
Member Posts: 2,012 PRO
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
Learn more about the Gospel of Christ ( Here )
CADSharp - We make custom features and integrated Onshape apps! Learn How to FeatureScript Here 🔴0 -
MichaelPascoe
Member Posts: 2,012 PRO
Learn more about the Gospel of Christ ( Here )
CADSharp - We make custom features and integrated Onshape apps! Learn How to FeatureScript Here 🔴2 -
EvanReese
Member, Mentor Posts: 2,188 ✭✭✭✭✭
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).Evan Reese3
Answers
- 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.Learn more about the Gospel of Christ ( Here )
CADSharp - We make custom features and integrated Onshape apps! Learn How to FeatureScript Here 🔴
Learn more about the Gospel of Christ ( Here )
CADSharp - We make custom features and integrated Onshape apps! Learn How to FeatureScript Here 🔴
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).
Learn more about the Gospel of Christ ( Here )
CADSharp - We make custom features and integrated Onshape apps! Learn How to FeatureScript Here 🔴
You may follow this thread and related.
Learn more about the Gospel of Christ ( Here )
CADSharp - We make custom features and integrated Onshape apps! Learn How to FeatureScript Here 🔴
- 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