Many ways to skin... a surface?

tom_auger

Sorry for the not-so-catchy title. In fact, my question isn't even about surfaces.

I'm looking to see if there's a faster / easier way to accomplish what I want, in the interest of continuing to improve my OS skills.

In the image at left I have extruded a face to create a hollow tube with a circular outer profile and an elliptical inner profile.

My objective is to "cap" the top - adding a new solid to the existing part that closes the top. There are a few ways I can think of going about this, but I'm hoping for something simpler - ideally it would have been to select JUST the outer edge (the circular edge) and then create an additional extrusion from that edge upward - but you can't select edges of existing parts, only faces in the extrude dialog.

Other options that come to mind:

1. extrude the solid tube using the original sketch, and then subtract the inner ellipse from the resulting solid, making sure it's not quite as tall to leave a cap. The problem with this is: the original sketch is offset quite a bit below the bottom of the extrusion, requiring me to make some calculations of the offset, and making it more tedious when making adjustments to the other components of the part, requiring me to either create a series of variables or to manually adjust the offset every time I change the height of the features below it.
   
   2. Create a new sketch at the top of the part, project the outer curve onto it and then extrude that. I'll probably end up using this method, but I hate having to add the clutter of another plane and another sketch just to accomplish this.

I'm curious to learn whether there is an obvious feature or tool that I'm not thinking of - some way of filling in that top hole only up to a certain depth (thicken uses the entire inner face).

Anything I should be considering?

rick_randall

Create one angled plane first, then extrude "up to face" selecting the plane as the face. Or maybe use a mate connector as the face, if you don't like planes.

Matt_Shields

If I understand your question correctly:

• Create a sketch on the top of the orange extrusion
• Use the Use tool to grab the outer edge.
• Extrude downward (into the orange extrusion)

MDesign

https://forum.onshape.com/discussion/26451/many-ways-to-skin-a-surface

Extrude only the outer circle solid up to the height you want. then extrude cut the oval up to that height-offset dimension.

MDesign

Just realized I may have misunderstood the goal. which might of been to have a new part all together. prior suggestion was to not bother with a cap at all and it be a solid object inclusive of a cap.

To include a new part based on the existing part. I'd extrude your cap using the circle from the sketch you created the tube from and use a starting offset from the top of the tube and blind thickness from there. Then the tube and the cap are based on the same sketch circle.

tom_auger

Hi everyone, thanks so much for the quick answers! What a community!

It's always hard to explain these things, both the intent of the design and the intent of the question.

I was really looking to see whether there was a tool or feature I wasn't yet aware of to simplify the process - like some way to "fill" that empty surface and then thicken it or "cap" a solid with an inner loop somehow (like you can do with frames, for example).

@rick_randall I wasn't sure I understood your approach - what does the angled plane do in this situation?

@Matt_Shields totally love this upside-down thinking; hadn't considered it - I like that thought because then you can decide how "thick" the cap is based on the initial offset of the extrude and then extrude down to the bottom face of the solid (or down to "next" would probably do it just as well)

@MDesign no, you had it right the first time, I'm using the term "cap" but I didn't really want another part, just a way to close the inner "void" as it were. The problem is that I can't get a hold of the outer solid circle because it's actually the (already hollow) face of an extrusion below it, and there would be no way to select all the other faces that would 'fill' it in to make it a solid.

I"m still open to more suggestions, but I guess I was hoping there was a hidden feature (like the cap on frames for example) that would serve in this instance that I just hadn't learned about yet…

MDesign

Are you able to share your design link?

rick_randall

@tom_auger

The angled plane is where the extrude will end. Even if it is not "normal to" the original sketch.

jelte_steur814

I'd reuse the initial sketch as much as possible.

using 'starting offset' set to 'entity' smartly in the extrude dialog, this could be done.

tom_auger

https://forum.onshape.com/discussion/comment/112103#Comment_112103

Yes, this is awesome. I just discovered it a few moments ago and will definitely use this trick again!

I am curious however to see whether there is yet another approach - is there any way to "fill" the hole afterwards without using another sketch?

jelte_steur814

sure:

I'd use my custom Extract Surface Feature. this applies a 'offset surface of 0' with a delete original surface checkmark, it separates the top surface from the solid.

then use the fill feature, add it to the top face. because it's a planar edge creating a planar surface in a planar face it'll just shut the hole.

then thicken (add) can be applied to cap the solid:

(I'd still prefer the extrusion method, but here you go for learning purposes)

https://cad.onshape.com/documents/d4f0cb956901919d478760a1/w/c4ae125b4a602f38237f49a7/e/c023d1ecdfc48f9a2a815773?renderMode=0&uiState=67855bb270b1b216e525fc5c

jelte_steur814

you could fill the hole immediately as well (without the extract surface). But Thicken will respond to the new surface differently than the top face. In my try, it thickened in opposite directions. (see V1 in previous document)

MDesign

https://forum.onshape.com/discussion/comment/112144#Comment_112144

This is what I was trying to explain. using the original sketch. I failed to get that point across. my bad. if you want to fill the hole rather than cap the tube just pick the oval sketch line in the original sketch with appropriate starting offset, direction and blind thickness.