Correct Order of Ops for Creating a New 3D swept part (tubing) in an assembly

[jmongi]

So, I know I've done this in other models but apparently I've forgotten the proper setup to create a new part within the assembly that is a 3D sweep from one fitting to another.

When I create a 3D sketch on its own and then go to Insert > New Part, then I can't select the 3D sketch for the sweep path because its not within the part I'm doing.

So, please help refresh my memory. What is the easiest way to create a tubing profile and then sweep on a 3D sketch path.

[SPerman]

I would create the sketch in the part, but in the context of the assembly. If you want the sketch at the assembly level, then you need to duplicate it in the part. Does "convert entities" work on a 3d sketch?

[Glenn Schroeder]

That's not working because you can't directly use an Assembly sketch for a Part feature. Create the new Part first, with nothing selected. Edit this Part within the Assembly, create the 3d sketch, and then you should be able to perform the Sweep function.

If re-creating the sketch is too much trouble you should be able to use the "Convert Entities" function to reproduce it in the Part, but unless the sketch is very complex I wouldn't recommend it. I'm afraid that would add another layer of complexity, and be more prone to errors, though it may work fine.

[jmongi]

Ok. So the part I was forgetting is that I have to start an empty part first. I don't need the sketch in the assembly, just getting caught out by doing things "normally" in preparing everything first then creating a part.

I appreciate the help. In a bit of time crunch and i could let you fine folks tell me instead of dorking around relearning this. Thanks!

[HerrTick]

NEVER use an external sketch/curve/edge/face to create a feature. ALWAYS copy entities into an internal sketch or feature.

There's exceptions for everything. There are also exceptions to "There are exceptions for everything." NO EXCEPTIONS!!!

[TooTallToby]

I know you're already at your solution but I just wanted to confirm what you came up with:
1. File, NEW, part
2. Save the part with a new name
3. (optionally) - insert a new 3D sketch and mock up a rough estimation of what you think the 3D sketch will look like
4. Flip to assembly
5. Insert > Component (existing part)
6. Select your new part
7. SINGLE CLICK ON THE ORIGIN of the assembly. this will "FIX" you new part, so that the XYZ of your new part is right on the XYZ of the assembly. - You do this because you don't want your new part to be "floating around" in the assembly. you want it locked, origin to origin.
8. go into EDIT PART mode
9. Make your 3D sketch so it starts and ends at the desired locations, using EXTERNAL REFERENCES to hook to the other parts, in the assembly.

I made a QUICK TIP video showing how to change your parts color settings, to make it a little easier to do an EDIT PART in the context of the assembly command:


I also made a longer livestream showing how I approach overall in context assembly modeling (skeleton sketch technique) - I know thats not exactly what you're doing, but I think some of the "setup" tips and tricks will be useful in your application.


Hope this helps,
Toby

[jmongi]

Interesting. I was doing...
In Assembly
Insert > New Part
Click in Empty Space
RMC on New Part and Select Edit Part
Create 3D Sketch
Create 2D Sketch
Feature > Sweep
Exit Part