Looking for suggestions on modeling this vase... WITHOUT creating each fin individually

john_lopez363

So this is the vase.


I can created the basic shape of the vase easily using a couple of Lofts and some Guides.  I can also create the fins using Sweeps... I was hoping to use a circular pattern of the Sweep feature... but that doesn't work correctly due to the angled middle plane.  Would need the pattern function to follow that angled plane (sketch) for this to work.

Looking for another way to complete the model WITHOUT having to create 48 individual Sweep features and their associate "paths".  Any ideas?




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romeograham

Here's one approach to consider.

Think about the body that defines the "bottom" of the ribs as a separate body that defines the outer profile of the ribs. You can see the gray "inner surface" body below is NOT cut by the ribs, while the blue "ribs" body is cut by the Extrude 1 feature that creates the space between the ribs. 

https://cad.onshape.com/documents/848622d119fd107c6b9dde45/w/52ed72574ec1872019c5ebd2/e/be793d5b2d65a8fd1efc4d98?renderMode=0&uiState=65837b256350524513a263d2

Cut away the ribs from the outer body (here, using a sketch that uses variables to make sure the ribs always have positive draft - depending on how many ribs there are):

Then, a Circular pattern that patterns Features (in this case, just Extrude 1) completes the ribs - and is very tolerant of changes. Make sure to select "Reapply features".

Then a couple more Boolean operations to create a shell feature, and you have a vase.

Using Variables and careful attention to design intent - you can build a robust model that is tolerant to different dimensions, rib counts etc.

Good luck!

S1mon

The photo is not very high resolution, so it's hard to understand some of the details.

Are the fins supposed to be a constant thickness or do they have any variation?

What are the thin edges of the fins supposed to look like? Are they normal to the sides of the fins or could they be the result of cutting away the not-fin part of the model you've started?

There should definitely be a way to do this with a pattern, but how you do it really depends on what the details are.

eric_pesty

Like @S1monsaid a bit hard to tell from that picture but it looks like the ribs are constant thickness, if that's the case, it's probably best to add the fins rather than try to cut them away, the easiest might to draw the fins "oversize" and pattern them then remove the material from them using similar technique to what you did for the base shape.

romeograham

Here's one approach to consider.

Think about the body that defines the "bottom" of the ribs as a separate body that defines the outer profile of the ribs. You can see the gray "inner surface" body below is NOT cut by the ribs, while the blue "ribs" body is cut by the Extrude 1 feature that creates the space between the ribs. 

https://cad.onshape.com/documents/848622d119fd107c6b9dde45/w/52ed72574ec1872019c5ebd2/e/be793d5b2d65a8fd1efc4d98?renderMode=0&uiState=65837b256350524513a263d2

Cut away the ribs from the outer body (here, using a sketch that uses variables to make sure the ribs always have positive draft - depending on how many ribs there are):

Then, a Circular pattern that patterns Features (in this case, just Extrude 1) completes the ribs - and is very tolerant of changes. Make sure to select "Reapply features".

Then a couple more Boolean operations to create a shell feature, and you have a vase.

Using Variables and careful attention to design intent - you can build a robust model that is tolerant to different dimensions, rib counts etc.

Good luck!

john_lopez363

romeograham ... Thanks... this approach works great....the "inner Surface" was the ticket!

_anton

The variable approach was surprisingly tricky to get fully right. :P After some fiddling: https://cad.onshape.com/documents/b68568f4a3a49a130f1824ea/w/e6aebb3dcb06f8dbf32c55a4/e/f3aab50099054ca99b49404f

The pattern is variable-driven - basically @romeograham's suggestion. This would also let you vary the angle of the fin with the vertical, though I didn't do that.

john_lopez363

@_anton   Absolute elegant solution!!!
Spectacular use of that "#interpolation_factor" variable and the value formula ((1 - cos(#i rad * PI / (#fin_count / 2))) / 2). As well as brilliant use of that variable in the circular pattern.  I'm definitely going to study this some more.

The interior or the model should follow the basic contour of the exterior.... I'm going to try your approach which seems more efficient that the way i came about it.   Many thanks!

john_lopez363

romeograham ... Thanks... this approach works great....the inner Surface "Enclose" was the ticket!

glen_dewsbury

Just some more thoughts.
https://cad.onshape.com/documents/d20a98aa13b2bd66eeced4c3/w/f9f32466bbd2c1f92f1493dc/e/c18c425faecdd25f4e51760f