Organising a Company Library (parts and assemnlies)

[jdg072]

We have a lot of own created or downloaded parts that we want to store somewhere in a library for later use. The parts are mostly valves & pumps with a Custom iProperty "TAG" which should be modified each time the valve or pump is inserted in assembly. Sometimes we need 3 valves of the same type, but with 3 different TAG's

My opinion is to make a copy of the library part in your project folder, modify the TAG there.

If we need the same valve again, we need to make a 2nd copy of that valve with a different filename.

How do we best organise this? Create a Custom Content Center library...?

[CflowAutodeskAdmin]

AutoCAD P&ID is the perfect program for you 😃 

Schematic drawings and it keeps track of all the tag numbers for you.

Give kudos if this comment helped you.

[jhackney1972]

I would suggest, if you want these components in Inventor, the creation of a Standard Parts Library and declare it in your Inventor Project file.  It can be a "Frequently Used Folder" or you can make it a "Write Once - Read only" declared library.  I would open each component assembly and add your TAG information either to a custom iProperty or an existing standard iProperty and then name the assembly with a - TAG 3 in the name such as Valve - TAG 1, Valve - TAG 2 etc.

[jdg072]

A" Standard Parts Library" is something different than Content Center?

[jhackney1972]

• Yes, a Standard Parts Library is just my name given to a folder declared in the Inventor project file under the Library section.  When you place a part in this folder, Inventor will warn you that the part will become read only.  This is normally good because a library part should remain constant.  There are easy ways to edit it if need but this should be restricted to managers.  A library contains descreat parts,  a Content Center library contains parametric parts built from table values.  To save a unique valve or other part as a CC library part would be very time consuming as well as being difficult to build.

[Mark.Lancaster]

@jdg072

Having tag information built into models has been requested for many years now.  Its not possible.  One thing that I've done is to replace the browser/occurrence name as the TAG #.  Others have done other things (paging @cbenner for ideas).  With Inventor 2018.1 you could use the MDB (3d annotations) and point them out in the model.

Also attached is a 60 min class I did on Content Center and your own library.  May help..   Also here's some links on content center since I notice you have been asking numerous questions about CC..

Part 1: https://synergiscadblog.com/2014/02/28/working-with-inventor-content-center-part-1-of-3/

Part 2: https://synergiscadblog.com/2014/03/17/working-with-autodesk-inventor-content-center-part-2-of-3/

Part 3: https://synergiscadblog.com/2014/03/28/working-with-autodesk-inventor-content-center-part-3-of-3/

Chris who I have tagged about has numerous information about CC as well.

[jdg072]

i am planning to have my valves (and other - to be tagged - parts) in a custom library in the CC. When I insert them, I choose to do it custom , and save them inside my project to a unique filename (maybe include tag in the filename?). That way i can use the custom iproperty of the part to have a TAG number in my drawings partlist.

[jhackney1972]

Since you have to author Content Center parts, I believe you will find the process much to time consuming for one off parts.  If I am guessing how the parts are being used, you will probably change your mind and use standard parts either in a library or a custom editable folder.  

[jdg072]

What do you mean by " you have to author Content Center parts"? I just have to publish an iPart and I have all the variants in CC. A part in CC I can copy to my project folder by selecting "custom", how do I do that with a standard library folder?

[jhackney1972]

I was not aware you already had iParts of your components, you are correct all you have to do is publish iParts.  

[Mark.Lancaster]

@jdg072

Update:  Clarification and added item #4.

But adding to @jhackney1972 statement..   Not there's no recommendations here..  But if you a purchase  a component that would only have a single member iPart configuration, putting it into CC may be a waste of time..  Here are some other things to consider..

1.  You don't need to fully configure an entire iPart member table to publish to the content center.  You can create one member in your iPart table and finish the rest of the members in your content center family.  In fact I prefer this method because I can start implementing column formals and expressions to automate my cells under the family table and thus end up with less work over filling in the info at the iPart level

2.  When publishing to CC, only purchased components (IPTs) should reside there..  Many times users will publish standard parts they actually manufacture (to CC) and when it comes time to modifications of those standard components, well then they realize how much pain it is to change that standard.

3.  Also think about your future..  Right now you say your piping components are not being used under routed system but could you in the future..  Publishing stuff to CC is like writing in stone.  Its hard to change it later down the road.. So think about your future and plans you may be taking down the road.

4.  Although one you publish the iPart to the CC the iPart factory is not longer needed and has no relationship to the family in CC..  However I always recommend to maintain that info for the future just in case something changes and you need to fall back on that original info.

[jdg072]

Could you tell me what to change on the valve parts to have them ready for routed systems?

[Mark.Lancaster]

@jdg072

I've miss-placed my routed system training manual that I wrote years ago but I would start here https://cadtipstricks.wordpress.com/category/inventor-tube-pipe/ with the information that @cbenner has created.  Most likely the stuff you'll need will be older blog articles that he wrote.

[cbenner]

@jdg072

>>Here is the link to my first Autodesk University class<< on Tube & Pipe basics.  The handout has a lot of information about setting up your Read/Write Content Center library, and then all about Authoring and Publishing fittings, valves etc for use with Tube & Pipe.  This should be a good starting point.

[jdg072]

@cbenner

@Mark.Lancaster

As you have guessed, finally I want my content center parts to be in my project folder after I insert them in an assembly. We made them small, so disk space won't be a problem. The advantages I see are:

- When Cc parts needs to be modified, we sure don't want old projects to inherent that modification, so the cc parts in the project folder won't be bothered, right?

- When I rename my CC parts with extensions -0001.itp, -0002.ipt, -0003.ipt, etc, I can add a TAG custom property.

- Designers opening projects made by other, will never have an issue finding cc parts.

I can place my cc parts "custom" so I can choose where in the project folder they are saved and by what filename. Or I can place them "as standard", so they are placed in the "Content Center files" folder, in my case, a folder relative to the project folder ".\Content Center Files"

The only thing I am looking for now is that when a cc part is placed "as standard", Inventor will checks if it already exists, and if so increment the extension by 1, so it becomes -0004.ipt, instead of it's current behaviour (using the same part).

Hoping you can see what I mean 🙂

BR, Johan

[cbenner]

@jdg072

If you place Content Center parts "As Custom", you may put them anywhere you want, and name them anything you want.  You may also independently modify those parts without affecting any others.

If you place them "As Standard", they will go under you default Content Center path, as defined in your Application Options.  You will NOT be able to rename them of modify them.

[jdg072]

Correction:

Could Ilogic (or programming inside Inventor?) do something like that?

The only thing I am looking for now is that when a cc part is placed "custom", Inventor will check if it already exists, and if so propose a filename with the extention incremented by 1, so it becomes valvex-0004.ipt.