How to add a raised edge to a curved surface to align 2 parts(solids)

[_KevinH_]

Hi All,

My first post but I'm really scratching my head on this one... I'm designing a fuselage for a model airplane which is supposed to be 3D printed. For this reason I've split the fuselage into 2 solids so I can print them separately and glue them together afterwards. Now, I would like to add an extended edge to one of the parts in order for the second part to "slide over" and be aligned with the first one. On the included part file I've turned on the visibility of the 2 sketches that contain the lines where that "raised edge" should be. I've tried with sweep but since the fuselage is constantly changing shape I'm unable to get it to stick to the surface. Then there is also the problem of the second part which is a separate solid and seems to be ignored whenever I want to extrude, cut, etc...

I'm really curious how something like this can be solved.

Thanks for helping me out!

Regards,

Kevin

[Xun.Zhang]

How about the Plastic - Lip command? It should be helpful for you!

[IgorMir]

Hi Xun;

Do you really believe - one tool you have mentioned will fix the OP's design issues? You must be very optimistic if you do. 

Cheers,

Igor.

---

@Xun.Zhang wrote:

How about the Plastic - Lip command? It should be helpful for you!

---

[JDMather]

I would have done a simple Revolve on one sketch (and no extra workplanes) instead of Loft1.

Is there a logical reason that Sketch7 is off-centered rather than symmetrical?

[_KevinH_]

Yes indeed, a revolve would even have been better. I started originally with a different design and this one required the work planes, I guess I didn't consider using the revolve tool on this design afterwards.

Thanks for spotting that mistake, it indeed needs to be symmetrical!

I'm still trying to find out how I should do the "edge" I was talking about. I'm now thinking to do the split of the fuselage at a later stage and first draw the "edge" with the sweep tool and make it a separate solid, then do the fuselage split and then combine the edge with one of the 2 halves.

Let you know if it succeeds... Still open for different approaches though

[andrewdroth · Accepted solution]

This is kind of a clunky way to do it, but hopefully it makes sense.

Split one of the bodies by the amount you want to overlap. Then copy the overlap section so you have two identical bodies (there's no easy way to do this, so you have to copy object and then do a stitch on the new surface). 

After that you just need to modify the height and width to suit your overlap, use offset or direct edit. I added more material to the inside, but you could split the difference of the part thickness to save weight.

Then it's just a matter of using combine/cut to trim away the interference material and join the two haves to the interface solids. 

Hopefully that makes some sense...

[JDMather]

When I get a chance - I will show my way.

It will be 1000.4 times easier.

[SBix26]

Here's a pretty easy solution, using @Xun.Zhang 's suggested Lip tool.  As others have suggested, there are a lot of problems with this model, but once you get those resolved (probably start over with what you've learned so far), the Lip feature should make it pretty easy to get the alignment features you want.

Edit: I used Delete Face with Heal to get rid of the small end slivers left after placing the groove.  You may think of other ways to design that joint so that the alignment feature isn't so visible.

---

Sam B
Inventor Pro 2020.2 | Windows 7 SP1
LinkedIn

[johnsonshiue]

Hi! On top of what experts already mentioned, I would use Guide Rail Sweep to create the first body instead of Loft.

Many thanks!

[andrewdroth]

@SBix26 I think there's an issue with the lip technique, Unless you can get the pull direction to work.
See section image below.

@JDMather How'd you make out with yours?

[SBix26]

Good catch, @andrewdroth .  It was a pretty quick and dirty effort, obviously.  Using the Y axis as the pull direction gives somewhat better results with a pretty consistent minor protrusion into the interior all around:

---

Sam B
Inventor Pro 2020.2 | Windows 7 SP1
LinkedIn

[_KevinH_]

Your result is exactly what I was looking for, thank you!

I'm still curious to see the 1000.4 times easier solution as well 😉

[andrewdroth]

No Problem

---

@_KevinH_ wrote:

I'm still curious to see the 1000.4 times easier solution as well 😉

---

Me Too!

@JDMather, don't leave us hanging like this!

[JDMather]

I have 1000.3 other things I need to get done first.

Could be a while...  ...I need some help here.

[_KevinH_]

So... I don't know if this is a 1000.4 times easier solution but I had another look at it and came up with this way to do it. The end result is the same but it doesn't require any stitching and copying of objects. Again, thank you very much andrewdroth for helping me out! I'll post a picture once I have the model printed.

Happy new year everybody!