COMBINE OPERATION IN INVENTOR OF TWO BODIES FAILED

[jihadfettah.9]

Hello everyone,

I can't combine two bodies (a blade :a surface body 1 and a hub:body2: please see the file attached)

If anyone had any ideas please help me.

Thanks in advance.

[SBix26 · Accepted solution]

It works if the two bodies overlap just a little.  I tried using Direct Edit to increase the diameter of the cone (shaft?) by 1mm, and then the Combine operation works. 

Not knowing your design, I can't say what the best approach is, but perhaps you could create an offset surface slightly smaller than the surface of the shaft and use this as the termination for Extend2 and Extend3.  Then the bodies overlap a little and Inventor will be able to trim the bodies properly.

Also, your Inventor 2021 is badly out of date; the current version is 2021.4, while I see you're working in 2021.1.

This works, too:

• Create a 0mm offset surface of the cone
• Use Replace Face tool to replace the inner face of the blade with the new conic surface
• Combine solid bodies

I believe the problem is the inner surface of the blade, which is a lofted surface and not at all precisely fit to the conic face of the shaft.  Using Replace Face with the shaft face makes a better-defined face for the subsequent combine operation.

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Sam B

Inventor Pro 2022.2.2 | Windows 10 Home 21H2