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Publishing family from different part files

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Message 1 of 5
hector.andres
452 Views, 4 Replies

Publishing family from different part files

Hi everyone,
It's my first time on the autodesk forum, so I'm sorry if I'm not making this question on the right place or maybe there is already a solution out there that I didn't find.
I work in a hydraulic company where we do assemblies with parts of different manufactures. Therefore, I am trying to create my first library on the Content Center, something I have no experience on. My question is: is there a way of publishing a family composed of different part files?
I know I can publish a part or an ipart (which will generate several parts). Most parts of my library are downloaded from the manufacturers. For example, for a check valve component, I have a part for each size model. The best will be to create an ipart of this component with the sizes modifications. But I can't take time for modeling iparts for each component. That's why I downloaded them from the manufacture, who gives you an independent part file for each size of the component, not a single ipart.
Can I then publish a family composed of this part files, selecting them, or is this only available for iparts? Must then I publish each part separately?

Hope someone can understand my question! Thanks in advance to everyone.

4 REPLIES 4
Message 2 of 5
CCarreiras
in reply to: hector.andres

Hi!

 

If you dont have the iParts, why you doesnt use instead a library folder?

 

You can place all these parts in a proper folder, "Library Folder",  and point this folder location on every project as your library content, this folder as a similar behavior as the Content Center, parts are only "Read Only".

 

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Regards.
CCarreiras
Message 3 of 5
cbenner
in reply to: hector.andres

Welcome Hector!

 

I'm afraid the answer in your situation is no.  Different part models cannot be published into one single family in the Content Center.  I am in the same situation as you, I download a lot of pipe fittings from the manufacturer's web site and publish to the CC.  Generally what I do is set up a unique sub folder under the appropriate fitting folder for these so that can be published as individual parts without over crowding the main folder.  For example, I recently downloaded a library of fittings from Durcor ™, they are all individual parts.  So, under my Elbows folder in the CC, I created a new folder called Durcor™, and put all of the sizes of Durcor™ elbows in there. Same with Tees, Flanges, etc.

 

Hope this helps!

Message 4 of 5
wimann
in reply to: hector.andres

Hi there Hector,

 

The post previous to mine is correct. You cannot publish an assembly nor can you publish a collection of different parts to the same family. However, I found a work-a-round besides the library folder that I've used for several months now. I made a part file that contains all the variations of one type part (provided by client) and was able to publish it to CC. I did this by:

 

1. Create new .ipt and new .iam

2. Place new .ipt at orgin of new .iam

3. Place 1 variant of client supplied model at origin of .iam (in desired orientation)

4. Edit-In-Place new.ipt

5. Copy Object and select client provided part as a solid

6. Return to Assembly

7. Delete Client.ipt from New.iam

8. Edit-In-Place New.ipt

9. Rename solid(s) for reference

10. Suppress solids

11. Repeat steps 3-10 for all client supplied parts

 

This will bring all of the client supplied parts into a multi-body part file. The trick is to set up a parameter that determines the size that is selected, then set up suppression conditions to determine which solid(s) is present based on the parameter.

 

It's also important to note that constraints to the geometry of the part file will fail during a Change Size and/or Replace From Content Center. To avoid this, you'd want to set up user work features (planes/axis/points) for the end user to constrain to. You will then also, however, have to make the work features reposition based on the selected size without reference to the actual model geometry. In other words, a plane's location would need to be determined by an offset from the origin and not by the geometry of the part.

 

Sorry for the long post. I hope this makes sense.

-Will Mann

Inventor Professional 2020
Vault Professional 2020
AutoCAD Mechanical 2020
Message 5 of 5

Thanks everyone, I'm impressed how quickly you answer!
The folder library solution is what I'm currently doing, probably I will stay with it or do as says, as I'm hoping that publishing parts in the CC will make the search more easy and also will help me with the Tube & Pipe utilities. Thanks also  answer giving a possible way of doing it, also I found it a bit tricky.

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