Custome Content Centre parts - Browser name?

[gerhick]

Hi all,

How do I control the appearance of Content Centre parts Browser Node name (i.e. the name that appears in the Model Browser)? I've checked the family tables, and family properties, but it just appears to be a random combination of fields.

Cheers

[pauldoubet]

If you read the help files you will find an explanation of where the browser name comes from. It is not a random name but a combination of specific data that is a part of the Content Center family info.

Paul

[gerhick]

Hi Paul,

Thanks for the reply, but it would be super helpful if you could post some specific information on the solution. I don't post in these forums without having a good look for the solution myself.

Thanks

[pauldoubet · Accepted solution]

Sorry, I thought the previous suggestion might point you in the right direction. I am assuming you are using Inventor 2011. The following is from the help file for Content Center, customizing file names (Note the bold type at the bottom):

Customize the file name for families in a category

You can create a file name scheme for families in a category. When you insert a part family member (part) in an assembly, the file name for the created part file corresponds to the file name scheme.

The File Name must be unique for all family members that use the same storage folder (specified by the Family Folder Name). When a file name is not unique, placement of the family member to an assembly can be disabled. This situation occurs if a standard part file with the same name but belonging to another family member exists in the storage folder.

File Names must include family-specific identifiers to be unique in Content Center. The File Name expression for custom families must include all custom columns to define unique file names for all custom family members.

To begin, display the Content Center dialog box. Click  Manage tab Content Center panel Editor . Then select a read/write library in the Library View list.

1. In the Content Center Editor dialog box, use the Category View mode or Search to locate the category you want to edit.
2. Right-click the category, and select File Naming.
3. In the File Naming Options dialog box, enter an expression in the File Name Expression text box:
   • Click next to the edit box to display the list of available parameters for the Category. Double-click a parameter to insert it in the file name scheme.
   • If appropriate, enter allowed characters (separators, and so on).
     NoteThe following characters cannot be used in the file name scheme: \ / : * ? " < > | & { } [ ] %
4. To add the File Name Expression as a prefix or suffix to the current file name, select Add to existing. Then select As prefix or As suffix.
5. Click OK to apply the file name schema to all families in the selected category.

Tip:To use the file name as occurrence name in the assembly browser, map the File Name to Member.DisplayName. Open the Family Table for a part family, right-click the File Name column, and then select Column Properties. Select the Member.DisplayName iProperty in the Map to Autodesk Inventor Properties list.

Hope this helps, Paul

[gerhick]

Paul,

You're a legend.

For the record, this bit is the nugget of info I've been looking for:

---

@pauldoubet wrote:

Open the Family Table for a part family, right-click the File Name column, and then select Column Properties. Select the Member.DisplayName iProperty in the Map to Autodesk Inventor Properties list.

Now..... Next problem is how to implement these changes to existing parts.

I know normally you just hit 'refresh standard components' but it's not working... I had to delete the local copy of the file, re-insert (re-create it) before it updated in existing drawings. Hope there's an easier way to do this...

[pauldoubet]

I would recommend you try a 'Rebuild All', if that does not work a 'Replace from Content Center' should cause the info to be reread/rewritten from the Family Table.....and if that does not work I would try a 'Replace Family Template' as a last resort. And if the problem is just in the idw or dwg file make sure you have the 'Associative' box checked when you edit/create the view.

Good Luck, Paul

[Brojefj]

---

@pauldoubet wrote:

Tip:To use the file name as occurrence name in the assembly browser, map the File Name to Member.DisplayName. Open the Family Table for a part family, right-click the File Name column, and then select Column Properties. Select the Member.DisplayName iProperty in the Map to Autodesk Inventor Properties list.

Hope this helps, Paul

---

I have used the above tip many times but I'm still running in to an issue with a few of my tables:

the tables in question have a key column with a unspecified length (for pipe, tubing, hose, etc.)

Is there a way you can map the member display name to a non-standard part? Currently when I place the file from content center my default prompts me to save the file as a custom file.(because of the unspecified length key column setting) is there any way to relay the initial "save as" file name back to the member display name?

Example: table filename shows "123456" for the part number for a specified size

however this one size could have hundreds of different lengths so when it prompts to save the file we add a dash number to the file name. Example 123456-0012.00 for a 12 inch length of the sock part 123456.

I'm wondering if there is any way to relay the "save as" file name back to the member display name?

Currently if I would save 123456-0012.00 the file name would read = 123456-0012.00 but the member display name still reads the original file name in the table = 123456 (no dash call out)

is there any way to link this?

P.S.. I am using 2010

[pauldoubet]

I will have to check on this problem you are seeing in 2010. I seem to remember there was a hotfix or service pack that addressed an issue similar to what you describe. However it seems that the browser would display the original template file part number in this case...I will see what I can come up with.

Paul

[Brojefj]

---

@pauldoubet wrote:

I will have to check on this problem you are seeing in 2010. I seem to remember there was a hotfix or service pack that addressed an issue similar to what you describe. However it seems that the browser would display the original template file part number in this case...I will see what I can come up with.

Paul

---

yes, you are correct. after I linked the member.display name to the file name and it didn't work the way had hoped I then un-linked it and that is exactly what happens, the original file name for the template appears for anything that I place from that table.

I'm using build 272, SP3. and thank you for all your help.

[PMeierENG]

Apologies if this appears naive (self taught).  My work flow for content centre parts is to place from content centre in an assembly.  I then open that bolt (lets say) and then save it in say a fasteners folder in my project. That way I can open the same folder from different workstations without the issue of Content Centre synching.  When you open the part, which is now renamed say F01-M24 Hex Bolt, you can paste that new name in the part header in the browser.  It will then appear as that new name in your assembly once you place it from the fasteners folder (not from content centre).  You can update the description in the iProperities in order to populate your Parts list correctly.  Perhaps a long winded way of doing it but it works for me.  I often have projects where I need to give fasteners a project specific number.