How to fill solid of the inside suction cup's bellow?

ismat_jahan

Hello,

I am trying make inside solid-mold of the suction cup's bellow part like the reference. For this I need to fill up the inside of the bellow to get the solid inside-curves.

My plan is after getting the inside curve solid model, 3D print it & use it inside of the silicone mold. I just can't fill the hole accurately to get the inside's solid curves.

How do I do it? Suggestion please, I am struggling on this...

Also attaching the Onshape document I am working on https://cad.onshape.com/documents/dbca8efe127f123f23de7f2e/w/ab863033ff5c445898d1b3dc/e/5f07cb0ab04fc4577eb1947a?renderMode=0&uiState=6290ec095abc44465af34b23

 

eric_pesty

I think the "enclose" feature should work for this...
Or you might have to do a "zero offset" surface out of the external faces and cap the open end(s) with the "fill" feature

EvanReese

Here's one way: https://cad.onshape.com/documents/6a8c57e1984ede436963960c/w/711cd9e35e2ccb6e745f3f68/e/82616a56f77e60981828b474

mahir

One lazy way would be to just model a new block around the bellows, perform a boolean subtract, and then delete the external body to leave the internal volume. It's not necessary the most elegant method, but it requires few selections and is robust to changing geometry. The block would just need to have the same flat top and bottom surfaces as the bellows.

https://cad.onshape.com/documents/9274ff6f8d6ef85343d41bc3/w/1e2f935958fd3d24ad19de38/e/debefeb8fb0d2e985eb8bee2

S1mon

Another quick way:

Create top and bottom surfaces with Fill (just pick the circular edge). Then Enclose (pick the fill surfaces and the bellows). Then you can Boolean Union. This doesn't require any sketches, and the selections are very simple.

ismat_jahan

I did the zero offset of the external surface but I can't fill with solid by capping the open ends

ismat_jahan

Evan_Reese said:

Here's one way: https://cad.onshape.com/documents/6a8c57e1984ede436963960c/w/711cd9e35e2ccb6e745f3f68/e/82616a56f77e60981828b474
   Thanks a LOT!!!! I'm overwhelmed with joy!  

eric_pesty

ismat_jahan said:

I did the zero offset of the external surface but I can't fill with solid by capping the open ends

The fill can only do one opening at a time, you just need to use 2 separate fill features.

EvanReese

eric_pesty said:

ismat_jahan said:

I did the zero offset of the external surface but I can't fill with solid by capping the open ends

The fill can only do one opening at a time, you just need to use 2 separate fill features.

This is the exact kind of thing I wrote that Cap feature for. It just finds open edge loops and does a fill with positional continuity. Nothing groundbreaking but it's convenient.

ismat_jahan

S1mon said:

Another quick way:

Create top and bottom surfaces with Fill (just pick the circular edge). Then Enclose (pick the fill surfaces and the bellows). Then you can Boolean Union. This doesn't require any sketches, and the selections are very simple.

It's the most easiest way I found! worked like magic! THANK U.

ismat_jahan

Evan_Reese said:

eric_pesty said:

ismat_jahan said:

I did the zero offset of the external surface but I can't fill with solid by capping the open ends

The fill can only do one opening at a time, you just need to use 2 separate fill features.

This is the exact kind of thing I wrote that Cap feature for. It just finds open edge loops and does a fill with positional continuity. Nothing groundbreaking but it's convenient.

Yes, the cap feature is new to me! from u I learned this method. Appreciated.

ismat_jahan

eric_pesty said:

ismat_jahan said:

I did the zero offset of the external surface but I can't fill with solid by capping the open ends

The fill can only do one opening at a time, you just need to use 2 separate fill features.

Got it!

ismat_jahan

S1mon said:

Another quick way:

Create top and bottom surfaces with Fill (just pick the circular edge). Then Enclose (pick the fill surfaces and the bellows). Then you can Boolean Union. This doesn't require any sketches, and the selections are very simple.

   Thanks a LOT!!!! I'm overwhelmed with joy!  

ismat_jahan

mahir said:

One lazy way would be to just model a new block around the bellows, perform a boolean subtract, and then delete the external body to leave the internal volume. It's not necessary the most elegant method, but it requires few selections and is robust to changing geometry. The block would just need to have the same flat top and bottom surfaces as the bellows.

https://cad.onshape.com/documents/9274ff6f8d6ef85343d41bc3/w/1e2f935958fd3d24ad19de38/e/debefeb8fb0d2e985eb8bee2

Thanks a LOT!!!! I'm overwhelmed with joy!