How to Duplicate a Solid Body in Part File inplace.

[Anonymous]

I have one simple solid body in a part file, of coarse with its own 2D Sketch. I want to duplicate it (copy & paste or something???) in place right on top of the first one as a second solid body. I will then modify the second solibody sketch resulting in a second unique solid body. 

How do I do this simple operation???

Thanks!

[SBix26 · Accepted solution]

My first thought is that you simply need to copy the sketch from the first solid and create another solid that way.  That is, edit the sketch for your first solid, select everything and copy (Ctrl-C or RMB Copy).  Start a new sketch on the same plane, and Paste (Ctrl-V or RMB Paste).  The copied sketch will end up right where your first one is, but not constrained to the origin.  Offset it some distance if you wish, and then extrude, choosing New Solid.  Now you have two independent solids which are each editable however you wish.

Hope that helps,

Sam B

Inventor Professional 2015 SP1 Update 2
Windows 7 Enterprise 64-bit, SP1
HP EliteBook 8770w; 8 GB RAM; Core™ i7-3720QM 2.60 GHz; Quadro K4000M

[rdyson]

One Way:

[kjacquesE7SLR]

I know it's an old post but search engine lead me here and could lead others as well. I often like to preserve parametric function which the previous suggestions don't do. Instead, you may prefer to save the solid where you feel you want to preserve it as a source for later parts and the derive it in new part files (or derive twice into a single part).

[SBix26]

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@kjacquesE7SLR wrote:

...  I often like to preserve parametric function which the previous suggestions don't do.

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Can you explain how my suggestion (post #2) doesn't preserve parametric function?  If I copy all the elements of a sketch to a new sketch, from which a new solid is made, it's entirely parametric, and independent of the first one, which I believe is what the OP was asking for.

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Sam B
Inventor Pro 2022 | Windows 10 Home 2004
LinkedIn

[kjacquesE7SLR]

You're correct. I wasn't quite precise in my comment. It works for simple extrusions and such but when you have 10 or more operations that you want to duplicate, things could get tedious. In the screenshot I have here, I wanted the black and silver pieces to mate in a complicated way. They're both derived from the same base geometry in an original file that has 16 features. I can carve out one and use it to shape the other or in this case it was simple shell and offsets.

2021-04-21_15-37-34.png

[johnsonshiue]

Hi! If you want to create independent bodies, Copy Objects can help. But, if you want to replicate bodies and keep association, you can pattern the bodies and keep them as individual bodies.

Many thanks!

[Anonymous]

It would be handy if you could just duplicate a solid body and include all features independently.  It's likely not really needed because you can just do a better workflow with derived bodies as kjac said.

You can select all the features, copy and paste and then edit the new features to create a new body and reselect that new body as the target for all the features. This will copy a body and all the features as a new independent body that's exactly the same. 

[RAMONYIP]

I just figured this out a few weeks ago. If you use Rectangular Pattern and set your Count to 2, Spacing to 0, and select Create new bodies, it effectively acts as a Copy, but is actually Associative. I'm using Inventor 2023, but I don't know if that matters.

 Screenshot 2023-06-07 132729.png