Shelling and tips

sam_sailor

Hi!
I'm quite new to onshape, and I'm working on an RC sailboat model that you can find here (Everything is in french, sorry...).
I have this shape for a keel balast that I need do hollow, with a 0.4mm wall thickness.  Sadly, I get this error: "Cannot shell parts with selections".

According to this thread, I should cut the model to try and find what part causes this. I thought that the pointy end would be the problem, but surprisingly, when I separate the model in half, I can hollow both parts! I'm a bit confused...
So sure, I could hollow the two parts and then join them back, but I still would like to know if someone has another idea.

To see what I tried, you can just unsuppress this:

S1mon

It does seem to be the pointy end of the ballast which is causing the issue. Somehow when you split the part, it's doing some internal workarounds differently than it does when the part is whole, but here's another fix which doesn't require splitting it into two parts and booleaning them back together:



I cut off the very tip, shelled it, and then delete face (with heal) to get back the point on the outside.

Here's my copy of the document.

glen_dewsbury

S1mon. I think your idea is slick and I have run into similar problems in the past. So I tried to quickly replicate the error but could not on my current sample unless shell is thick enough to close the object. In which case a shell is mute.
Used the hollow option with shell and it's working fine and holding steady no matter the dimensional changes. I'll have to go further back to see if I can find my previous problem when I have some time.

eric_pesty

Not sure why the shell if failing without a split, clearly it changes something internally... Might be worth submitting a ticket as they might have a bit of a bug in there.
I would add though that you wouldn't build it with a perfectly sharp point anyway so if you cut it off a short distance away you don't need to "restore" the point afterwards, even 0.5mm away is enough for the shell to work as shown below.

Note that @S1mon's method can be simplified if you use the split directly with a mate connector (eliminates the sketch and extrude features):

S1mon

@eric_pesty
I sometimes forget that mate connectors can be used to split things. I also really still think that split part should take a sketch and not need an extrude to create a surface. Coming from Pro/E and Solidworks where you can extrude a non-closed sketch to create a cut, I still really miss that way of thinking.

eric_pesty

@S1mon
I agree splitting directly with a line would make a lot of sense (it works for surfaces so why not for parts!)
I really like splitting directly with a mate connector as it's "even better" in many cases!

Evan_Reese

S1mon said:

@eric_pesty
I sometimes forget that mate connectors can be used to split things. I also really still think that split part should take a sketch and not need an extrude to create a surface. Coming from Pro/E and Solidworks where you can extrude a non-closed sketch to create a cut, I still really miss that way of thinking.

It's been the better part of a decade since my Solidworks days and I still keep trying to do this. It should absolutely work, and I'd love to see this update.