Modeling - Pipe on 45deg against pipe

[marius.andersen3RVB4]

Situation
Two pipes welded together at typ. 45deg.

I need to project this curve to center-plane

It is not possible to project this.

I also need a horizontal workplane tangent to lowest point of curve.

And most important thing... the features must update while changing dimensions and angle.

Believe me...
I have tried mostly everything i can come up with.
If we start thinking 3D-sketch...
I have a feeling that new projections are created when dimensions are changed.
The projection functions in 3D-sketch is faulty.

I have 20 years of expreience in Inventor, so believe this is a hard one to crack.
I can give more information on request.

[Sila0658]

I managed to do it this way, and the curve updates perfectly to changes.

[Sila0658]

Next you can create a line that's has a horizontal constraint and a tangent constraint to the bottom side of the curve. Then make a horizontal plane from the line.

[CCarreiras]

HI!

Here's an idea... exploring multisolid (you didn't refer if you are in assembly or part context).

[A.Acheson]

Are you using this projected geometry to cut the pipe end afterwards and need a paper flatpattern? If so I suggest a different approach. Use sheetmetal part, set diameter of run/branch. Use contour roll on branch. Split contour roll. Unfold branch pipe to flat pattern. 

[IgorMir]

Frankly - I don't see the problem. To create the model requires a small extra step, that's it. Unless I am missing something. Here is a file in IV2020 format.
Cheers,

Igor.

[cadman777]

The first question that comes to mind is:
What kind of parts are you making?
Are you using ContentCenter parts?

Are you making these from scratch using basic Inventor tools?

I ask that because you say this:

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@marius.andersen3RVB4 wrote:

And most important thing... the features must update while changing dimensions and angle.

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Which leads me to believe you want to make some kind of library you can reuse and change the sizes and angles.

So, depending on whether this is done in an Assembly or Part determines the method you will use.

[johnsonshiue · Accepted solution]

Hi! I think this is a bug or a limitation. The issue here is that Inventor has trouble projecting the 3D spline loop onto a plane, probably due to confusion at the start or the end. A simple workaround is to split the cylindrical face in half. More than likely the projection will work. If you don't want to modify the solid geometry, you may create a zero-offset surface (Thicken/Offset) and split the surface body in half.

Many thanks!

[marius.andersen3RVB4 · Accepted solution]

Attached you can see current solution.
Model will be fine-tuned.
Part run by user-parameters.
Own iLogic form for easy access.
Thanks for your attention.

Marius