Saving an assembly as a part

[ToddPig]

In Solidworks, there is an option to save an assembly as a part.  This is very helpful when for example, dealing with printed circuit board assemblies.  You can save the assembly as a part, and then it's much easy to deal with in your assembly.  In Solidworks this is done by File, Save As, then change the extension to a part file.  I'm Inventor has a similar feature.  (I already tried all 'Save As', 'Save Copy As', Export', etc... options)

As usual, thanks in advance!!

Todd

[ToddPig]

More info ....

I'm starting with a STEP file (from a vendor).  When I open it in Inventor, all the parts in the assembly are solids.  When I use the Shrinkwrap feature, it turns everything into surfaces.  In Solidworks, when I open it, all the parts are solids, when I save it as a part, it remains a solid?

[Curtis_W · Accepted solution]

Hi ToddPig,

If you're starting with a STEP file then you should be able import it as a part file rather than an assembly.

Start a new part file, then go to the Manage tab and click the Import button. Select the options to bring it in as  Solids and as a multi-body part or a composite, as needed.

If you can't get the result you expect, attach the STEP file here for others to have a look at... if that's allowable.

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

[swalton]

I know Curtis answered your main question about importing stp files....

If you ever need to convert an assembly file to a part file, use the Derive workflow.

1. Create and save your assembly
2. Open a new part file
3. Select the Derive tool in the Create section of the 3D Model ribbon
4. Navigate to your saved assembly file on disk
5. Follow the dialog window to set various options depending on your downstream needs.
6. Click OK.
7. You now have a part file that is a dependent copy of an assembly file.

RMB on the derive node in the model browser and select "Suppress Link" to temporally break the part's dependency on the assembly file.  Or select "Break Link" to permanently break the dependency.

As a side note, the derive functionality is also used for mirrored parts, substitute Level of Detail parts and simplified parts.  You can also use it as a way to link parameters, sketches, or scale geometry from part or assembly files.

[ydagan]

Hi All, 
i have the same issue,but i don't understand way it need to be so complicated, 
is solidworks you do it in one "click"  
this is so useful when you need to convert assembly to simple part 

[JDMather]

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@ydagan wrote:

i have the same issue, but i don't understand way it need to be so complicated, 

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Inventor has far more functionality.

Did you figure it out?

[BDCollett · Accepted solution]

You can do it in two clicks with Simplify. 

[danielGW92Q]

Hey, yes and no. Lets say you have found a cad file on google somewhere that you want to be using in your modell, lets say it is an assembly, and you want it to save as a file without connection to anyfiles, if you save it as step or as simplyfy parts even with braket link you still need the whole assembly to drag arround in order to open a single part, and if you want to move it to another map you need to drag all the assemblies part, what i do now i make simple part and then save as STL file in order to completely delite link to the assembly out of this world

[SBix26]

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@danielGW92Q wrote:

... if you save it as step or as simplyfy parts even with braket link you still need the whole assembly to drag arround in order to open a single part, and if you want to move it to another map you need to drag all the assemblies part...

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This is not correct.  A STEP file has no links to any of its origin files, and if you create a simplified part from an assembly and break the link, there is no longer any tie to the assembly and components.  Try it for yourself-- I just did.

While it is true that a STL file has no connection to the model that produced it (as with STEP), a STL file is no longer usable geometry in Inventor or many other modeling systems.  A STEP file maintains the BREP geometry of the original.  A STL file approximates the original model using mesh geometry.

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Sam B

Inventor Pro 2022.2.1 | Windows 10 Home 21H2

[danielGW92Q]

Hey, yeah and MLT file have some more edit possibilities to edit but stil not perfect, any suggestions what kind of file best to be using if you dont beed any connectivity to assembly and at the same time very good to edit?

[danielGW92Q]

Mine steps has connectivity i dont know why, my step files some times need whole assebly in order to resolve the components, i an not using vault though

[SBix26]

If you want to edit with Inventor, then use a simplified assembly (=.ipt) file with the link to assembly broken.  If it's another solid modeling software (SW, for instance), then STEP.

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Sam B

Inventor Pro 2022.2.1 | Windows 10 Home 21H2

[danielGW92Q]

i have found why my steps had connectivity to assembly, because when i imported them i kept reference model on. Now it works just fine

[paul.hadleyEBN96]

A simple save as part would be great for what's needed! 

There's little point in having lots of functionality if it doesn't give value