Merge 2 Parts Together

[Anonymous]

I have 2 different parts that I created as separate ipt files. I then bring them into an assembly and place them how I want, but they have overlapping material. Is it possible to turn these 2 parts into one part? If yes, how? Please keep it relatively simple if possible, im not an expert with Inventor.

Thank You!

[Curtis_Waguespack]

Hi wilson12,

Do you need to be able to modify the parts independantly, or is it okay if you loose some of the sketches and inputs?

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Anonymous]

Thanks for the quick reply! Well the part is actually 4 parts that form a sort of rectangle. Both opposite sides are the same part. The trouble I'm having is the corners where they meet overlap. Therefore, on the mechanical drawings, a line is visible where there is an overlap. So, I think it is okay if i loose the sketches, I don;t believe I'll have to do much more modifying of the parts, and if I do I can just make new sketches.

Thanks!

[Curtis_Waguespack · Accepted solution]

Hi wilson12,

Here is one method:

• Open your assembly file with both parts constrained in the orientation that you want them to be together.
• Then edit one part from within the assembly (rather than opening it up independently).
•   Then use the Copy Object tool to copy the other part into the part your editing, choose to bring it in as a new solid body.
• And then finally, use the Combine tool to merge the two solids together in the part file you're editing.

The result will be that the copied part will be a dumb solid in your edited part file.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Anonymous]

Thank You!

That was the solution I needed.

I appreciate your fast responses!

Kudos to you, sir.

[Anonymous]

Sir,

i am fresher to INVENTOR the method n explanation by u was easy n catchy sir,

i had tried this method and it was the same as expected thank you for that

but my doubt is

can we show two level of details 

1) one level of detail should show the single part.

2) the second level of detail should shoe the two solid boddies.

when i am trying to develop the idw means it being a bit problem for me because it is giving weight of two bodies.

[Curtis_Waguespack]

Hi prasannamech,

Unfortunately you can not show a level of detail for the part in the IDW.

The think the only way to do what you are attempting to do is to use the Make Components tool to write out the solid bodies as seperate files:

https://www.youtube.com/watch?v=iDRotf2Is2g

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[TyRusley85]

I know I'm a little late to this party, but here's an alternative way.

When you have an assembly and want to merge two or more parts, you can click on the Simplify Tab and click the "Create Simplified Part"

By doing this, you will be merging any visible parts in your assembly into one derived part. Any parts that you hid the visibility on, will not be merged into this part, only the parts that were visible in the original assembly will merge. Make sure that you save the part to a specific folder that will be easily found and to change the name of your part. Also, if the original parts that are now merged get modified and you update the new part, since they are derived from the original parts, any new changes will update to your new part as well. For example, if you added a hole to one original part, open the new merged part and click on local update (Orange Lightning Bolt by Home Icon).

[Anonymous]

it doesnt work? i cant copy as a solid it will only do Group,Repaired Geometory,Surface or composite. So the combine tool errors everytime. Am i missing something. Invenotr 2018.2

[Curtis_Waguespack]

Hi @Anonymous,

Are you editing a part file from the context of an assembly? If not that is likely the issue. The instructions in the solution above start with taking 2 part files and constraining them in relation to one another in an assembly. This can just be a temporary "throw away" assembly that you do not end up saving. 

Once the 2 parts are in the assembly, edit one of the parts, and then use the Copy Object tool as described to copy the other.

If you're doing all of that and seeing the same results still, you might take some screen captures and attach them here for others to look at, in order to determine what's going on.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Anonymous]

yep ok got it now thanks!

[Anonymous]

I had add some parts (.ipt) to an assembled part individually. 

How can I extract these individual parts and save them to a new assembled one (.iam)

[TheCADWhisperer]

Component>Demote.

Attach your files here if you can't figure it out.

[johnsonshiue]

Hi! I have re-read your posting a few times to understand your request. I suspect you are talking about Demoting. Select the components and right-click -> Components -> Demote. Is this what you were after?

Many thanks!

[Anonymous]

Thanks, it is solved. 

[sschneiderXHH8R]

I know this is hella old, but this still applies, and it was just what I needed. Thanks!