Creating ribs in a surfboard

bart_v_a

Hi there,

I am trying to design a printable surfboard, however I cannot figure out how to create ribs within my part. Does anyone know how to do this and what is the best way to go about it.

https://cad.onshape.com/documents/5f956327a9202bd9f1357623/w/2f820f0d0e71f32d5b0ea3bf/e/31cc2eb124199cd2f8271e32?renderMode=0&uiState=66c83dd857dcdd1765b21e5f

GregBrown

Something like this is really nice with a feature pattern:
https://cad.onshape.com/documents/2cb3df44323d9511195e427b/w/b2f5ece893e0e0c20302448f/e/5fe69308200186c9de80761f

Note the original BooleanInside feature needed to be edited to Keep tools as well. I added a couple more features in the Ribs folder in order to merge the ribs to the main board part…

bart_v_a

Thank you, that helps! I didnt know the feature pattern could be applied as a sort of function so the features differ each time, thats great to know

GregBrown

https://forum.onshape.com/discussion/comment/106239#Comment_106239

Great to hear! Yes, feature patterns are incredibly powerful and useful when you realize what you can do!

PS the Bottom surface of your surfboard is a bit ugly (check the curvature combs…) The edges in your guide curves for the Fill feature are not tangent continuous. This may or may not be something you'd want to control a bit more…

bart_v_a

Yes I saw that, but is the problem the tangent edges? I'd expect onshape to find the near smoothest way to follow curves but that is not whats happening, what would your solution be make the surface more smooth? Also I'm trying to fit a second part into the board, but making the surface "flat" is quite difficult using the guides, should I use another function for this or change my guides?

The past feedback has been incredibly useful!

GregBrown

If you really want to produce sharp edges/non-tangent edges along that bottom surface then Fill is not the right tool. You would have to set it up so that a loft (for example) could be your reference surface. But then you'll also have to use a the standard surface modeling approach where you over-build these big/block/slab surfaces then trim them to create the profile looking down on the board. The smoothing of the sides would then follow.

The Fill feature is working (hard) to create a single surface constrained by both the boundaries AND the guides that you give it. So yes, it is doing smoothing so that it gets rid of the discontinuities. Note you have left the parameter in the Fill feature set to Precise, which is you telling the system you want to fit really, really close to those guides! If you switched that to Sampled instead and use a really low number, e.g. 2 you'll get a much smoother result, whilst bringing in a certain amount of uncertainty in the shape.

The ultimate answer is - it depends. It depends on what your intent is. Perhaps the Sampled =2 approach in Fill is good enough? Perhaps you could replace the entities in ForwardPlaneSketch with an arc or Bezier sketch, making sure whatever you do remains tangent to the other entities. That's what I did here in a private copy of the doc - the arc I added is in orange here.

After fixing up the Fill (to reference the new edges) the result is very smooth (even with Fill set to Precise):

… compared to the original Fill/Precise

and Fill/Sampled = 2:

bart_v_a

Hi @GregBrown since your last advice I have changed quite a few things. Using a loft instead of fill helped massively with the curves, I realised a fill wasnt the best so I fully switched to lofts.

I got another question, I have this fin cutout I want to test before spending a lot of material. https://cad.onshape.com/documents/5f956327a9202bd9f1357623/w/2f820f0d0e71f32d5b0ea3bf/e/510ba06fb28df18a1f994cc7?renderMode=0&uiState=6744b6ad33986a65a001f115

How can I use a part to cut another part, is this possible? Now I have made a separate box in the main model, but could I use an assembly for that instead?