Convex part by intersection of pipes

[FilipeMais]

Hi everyone,

I'm looking to the best and faster solution to get the parts in the photo. See the photo and the zip file bellow.

I'm using the intersection of two pipes perpendicular + an angle.

To do what you see I used two model states for both parts, created surfaces  and used sculpt option.

But, have you a better and more professional solution?

Thanks for your help

Desired part in orange

[Gabriel_Watson · Accepted solution]

I am not sure if this is the most professional, but certainly made the easiest workflow for me...

The key is that boolean cuts are best performed in Inventor when you derive/simplify (boil down) every component into a single part. There, you can use Combine, or maybe split and sculpt easily.

I set up the pipes in an assembly (see attached all files), then used "Create Simplified Part" (same as opening a new part and using Derive) to bring both parts as distinct solids in a new part/IPT. There, the fun happens.

As an alternative to this, I also tested using the Split tool instead of Combine, which worked well in a simple case like this (not attached, but here's a pic):

[blandb · Accepted solution]

You can do it with copy object as well. See if the attached video helps. I show 2 different ways you could cut the tube in the video. Just some food for thought.

[johnsonshiue · Accepted solution]

Hi! Slightly different approach than Gabriel's solution. I would not use Boundary Patch in this case. The base face is a cylinder. There is no need to recreate it. Just restore it. Use Delete Face -> check Heal option -> select the inner faces. The cylindrical faces from the pipe will be recovered.

Many thanks!

[FilipeMais]

Hi Gabriel! 

Thanks for your reply and all your care showing how to do it better. 

Unfortunately, I am using 2022 version and I cannot open your file. 

During the next days I will study it using your guidelines 

Once again, thank you for sharing. 

All the best,

FM

[FilipeMais]

Hi Blandb! 

Thanks for your reply & for your video. 

During the next days, I will study it using your guidelines 

Once again, thank you for sharing. 

All the best,

[FilipeMais]

Hi Johnsonshiue,

 Thanks for your extra information!

Best regards,

FM

[SBix26 · Accepted solution]

Here are files in Inventor 2022 format.  If I were doing this myself from scratch, I would start with the tubes modeled as two solid bodies in the same master part file, then derive them into separate parts for material and property assignments and sheet metal flat pattern, then assemble them.  This would only require four files instead of six.

Hope this helps.

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Sam B

Inventor Pro 2024.1.1 | Windows 10 Home 22H2

[FilipeMais]

Hi SBix26,

Many thanks! 

Best regards,

FM