In SolidWorks, I would simply add a concentric mate of the curved surface on the Part 2 grey tube to the curved surface of part 1. I would then align a plane on both parts to ensure it was vertical and then create a distance mate between a plane on Part 2 and some feature – perhaps the face with a dot on it – to another plane on Part 2.

I'd do the same as Nigel in Alibre to assemble the two

Though if it was going to be 3D printed as a single part I would have drawn it as one to start with

Looking again at your firs part, the half round. If that had been extruded equally about plane 1 rather than all to one side you should then have been able to use that plane to line up the two parts provided the circular part was central to two axis.

The added bonus would be that you could also have mirrored the tabs about the central axis too.

Extruded centrally and tabs mirrored

Then align the two vertical axis and then the horizontal planes and they all sit in the correct position but it does need some thought at the sketching stage to make assembly this easy.

Assembly screen showing half round lined up in XY&Z (green) and the geometry of the tube in brown

Edited By JasonB on 06/05/2022 18:13:52

Fusion360 and SE both work like that. FreeCAD is still primitive in this department, but getting better.

This example is Solid Edge. I designed a door bolt, which although based on the domestic item, is original : my dimensions, not a copy.

First part is the bolt body:

Created separately is the bolt. It has to fit into the body, correct diameter, length, handle to fit the slots etc.

SE (and similar CAD packages) allow two or more parts to be combined as an Assembly, which achieved by drag and drop plus intents – axial, rotation allowed or not etc. The result is two parts working together.

The software understands the bolt slides in the body, and detects collisions and interferences. When the design is correct, the bolt can be moved realistically on screen to prove all is well:

Mildly useful for designing a simple door bolt, but highly valuable when developing a multi-part object like an engine, where pistons must fit into cylinders without smacking into the head or valves, whilst the conrods turn the crankshaft without jambing. At the same time, the valve gear is driven from the crankshaft by a chain, and valve events delivered with cams. Saves an enormous amount of time when fits of all these different parts can be confirmed in a model, rather than painfully made for real, only to find they crunch expensively together inside the prototype!

Challenging enough to build an engine from someone else's plan, but much harder to reverse engineer an old engine from pictures or to develop a working engine from scratch. These tools are primarily for creating original work, not copying what went before.

Dave

Did I mention that I don't watch "Coronation Street" No? Well it's on TV now, so while my wife gets her Friday fix, I thought I'd do it my way.

I sort of combined some of the previous ideas but latched onto Jason's idea to do it all in one drawing. So, I thought, how about treating it as if it were a solid casting and "machining away the unwanted bits?

First, sketch the basic profile and extrude from a mid-plane, With lugs drawn once in a separate sketch and mirrored around two planes:

Then add the side extension as a solid :

Followed by removing the semi-circular section :

Then "hollow out" the side pipe section:

Just one 3D drawing in Alibre and for export to a STEP or STL file for printing.

John

You can then use the Section Analysis tool to show the interior.