How to design 3D items with complex shapes?

[MichaelSGao]

I´m a newcomer of Fusion 360 and would like to design something similar to the item in the picture below.

How should I build the dome part? (Which is something that has curvy exterior with irregular shape and void space inside.)

From which 2D-shape should I extrude to obtain such an item? Or are there more steps to be done after extrusion? 

[davebYYPCU]

Similar to this, edit and dimension my sketches to pull into shape....

Might help...

[MichaelSGao]

Thank you so much for the answer!

Could you please also recommend some references about how to make this design? Or maybe which keyword should I look for in a reference? I had a look into the timeline of your editing history and could not understand all of the processes. Thanks again.

[TheCADWhisperer]

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@MichaelSGao wrote:

… and could not understand all of the processes. 

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What projects have you done in leading up to this project?

Can you Attach some examples?

[MichaelSGao]

Sorry for the misunderstanding. Not every process is clear to me, that was what I wanted to express.

A T pipe like the one in the attachment is what I could do/ have done till now.

[TheCADWhisperer]

Did you notice what happened to your pipe when you added the Thread feature?

[MichaelSGao]

Are you suggesting that the thickness of the pipe went unrealistically low after the thread feature was added? Well yes, I was aware of and didn´t mess with that, since this is a project I learned from an illustrative online tutorial and not a real-world scenario.

[davebYYPCU · Accepted solution]

My timeline - the tools used can be researched easy enough, 

3 sketches, one for the fat bulb on centre line, one on flat plane for bottom tube opening, 

and one on front top for the top piece.  Not dimensioned cause there is no size information from the question, you put the size dimensions you need in my sketches.

Extrude the the bottom tube.  (Two sides)

Change to Surface Area from Solid area.

Extrude surface the centre line sketch.

Hide the sketches.

make a Loft from the two bodies, and change / adjust the condition of the centre line profile, to tangent, and use the pulling handle to make the desired shape.

Show - sketch 3 and Revolve outside lines.

Mirror the Lofted body as Join.

Trim Cut the Revolve body with the bulb body. (is too deep)

Trim Cut the bulb body with the top body.(make the hole)

Stitch the two bodies.  

Fillet the sharp corner at the intersection.

Thicken the body.

Remove the 3 bodies, used to make the part, but not needed now.

Might help.....

[MichaelSGao]

Thank you very much, I appreciate your explaining the whole designing process in detail. Now I have a clue.
Best regards.

[MichaelSGao]

My problem is now solved.

Solution: Instead of revolving an entirely enclosed sketch to form the top part, only the outer edges should be revolved. 

Original post: 

While reproducing your work, I´ve noticed that after your second "surface trim", there´s a white circle which I assume it is projected onto the shadow at the bottom of the 3D-design. However, there isn´t one in my work. Did I miss any step or procedure?

ps, I am not sure whether the top part of my work is open, according to its appearance. (I tried to examine this with multiple material textures, but the top part from my work seems to be enclosed).

[TheCADWhisperer]

Your Sketch7 is not fully defined?

Add a Horizontal constraint between the Origin and the center point of the circle.

Sketch8 the Construction line is not needed...

The 90° could be replaced with a Vertical constraint (assuming this angle won't be edited).

Lock symbols indicate that the sketches are now fully defined.

You have two unstitched surface bodies rather than Solid body and Top is closed while two Bottom holes are not closed.

[MichaelSGao]

Thanks for pointing out these aspects.

However, the main issue is that I´ve revolved the whole enclosed sketch. I´ve solved this on my own (my last post was updated).