Part Description in Assembly Browser

[Cadmanto]

I swear I have done this before in Inventor (unless I am having a relapse back to my old software days), but isn't there a way to show the part descriptions next to the file name shown in an assembly browser?  Nothing in the filter drop down is what I am looking for and I didn't see anything in the applications options under assembly either.

[SteveMDennis]

Scott, there is a way to display component names after constraints (Assembly tab of app options) and there is a way to display more info after features (part tab of app options). Are those what you are remembering?

[Cadmanto]

Steven,

The assembly tab in the applications options is what I tried.

Both in part and assembly.

I am not seeing any difference in the browser as you can see above with the above setting.

What I thought I remembered was some view setting that brought up a selection dialog that allowed you to show the part description (defined in the parts iproperties under the project tab) and that showing up in the assembly browser. 

[mcgyvr]

I think thats in the SDK or whatever it is where you have the "Inventor color scheme editor" and "Speeel Checker" 🙂

Or it was an Autodesk labs thing.. Can't remember exactly..

[karthur1]

The setting on the assembly tab shows this in the browser.  In your screen shot, expand the part node so you can see the constraints (if you have any).

As far as showing the description like you were saying... I dont know of a way to do that, but it would be sweet if you could do that and maybe even choose what extended information gets displayed (Title, Desc, Subject....etc)

Kirk

[Cadmanto · Accepted solution]

Kirk,

Yeah, I have done that.   I also installed the User Tools SDK and that didn't do anything either.  I must be recalling softwares of systems past.

Sounds like this would make a good idea.

Check out this idea and cast your kudo vote.

 http://forums.autodesk.com/t5/inventor-ideastation/part-description-in-inventor-assembly-browser/idi...

[SteveMDennis]

Scott, Just so I'm clear on what you want... (the IdeaStation post didn't clear it up for me). You want the ability to put iProperties into the display name of the components in the browser? Like part number, description, etc.? If I've got that right, if you rename the part those values are still there? i.e. they are not part of the name itself they are just a decoration to the default name or user override name? To do this right we would have to actually give you a "Component Naming scheme" that allowed you to pick iProperties, put delimiters in between them etc. Just trying to make sure we understand your request in a bit more detail.

[Cadmanto]

Steven,

What I have highlighted in your statement is exactly what I am trying to accomplish.

Functionality to add such properties picking them to add similar to the selections under the filter drop down.  I don't want to have to rename any files to see this type of information.  I want to see our part number (as the file name) showing up in the assembly browser, then the ability as we have described, to choose the descitpion and custom iproperties to displat after the file name in the browser.  With each property being seperated by ( ) .

Hope this makes sense.

[Anonymous]

While working on big assemblies, I often find it difficult to sift through 50 different 4 digit part numbers in the tree to find what I am looking for. This functionality would make working with similarly named parts much easier!

[swalton]

PTC Creo lets you add columns of parameters (Iprop equivalent) to the assembly browser.  Its like what IV can do in the BOM editor, but you don't have to open a separate window. 

I would expect that if IV implemented something like this, I would be able to edit values of the component iprops that I displayed in the assembly browser, just like I can do now in the BOM editor.

edit: ran spell check

[Mark.Lancaster]

Cadmanto

Here's something that I've done in the past for different plate stock configurations we had using iLogic:

oDoc=ThisApplication.ActiveDocument

Lgth=RoundtoFraction(length,1/16,RoundingMethod.Round)

Width=RoundtoFraction(width,1/16,RoundingMethod.Round)

Thk=RoundToFraction(thk,1/16,RoundingMethod.Round)

oDoc.DisplayName="Plate, Stock"+Lgth+"x"+Width+"x"+Thk+"in THK"

Everytime the part changed, its display name changes at the part and assembly level.  So you could adapt the code for your required needs if you know iLogic.

[Cadmanto]

Mark,

That's awesome.  I will try it out and let you know.

Thank you.

[Anonymous]

Mark,

Thanks for posting that snippet of code. The DisplayName method did exactly what we were looking for. Here's the code that we're putting in our assembly template to change the DisplayName of all parts contained within the assembly.

openDoc = ThisApplication.ActiveDocument

Dim docFile As Document
 
 'iterate through all components in ****'y
 For Each docFile In openDoc.AllReferencedDocuments
               
         'format file name                   
         Dim FNamePos As Long
         FNamePos = InStrRev(docFile.FullFileName, "\", -1)                        
         Dim docFName As String 
         docFName = Right(docFile.FullFileName, Len(docFile.FullFileName) - FNamePos)      

         'set display name
         docFile.DisplayName = iProperties.Value(docFName, "Project", "Part Number") & " <" & iProperties.Value(docFName, "Project", "Description") & ">"

         'rebuild to update the display
         docFile.Rebuild

        Next    

'update all
iLogicVb.UpdateWhenDone = True

[Anonymous]

And here's the code that changes the display name from a part level:

'create reference to part
openDoc = ThisApplication.ActiveDocument

'format display name
openDoc.DisplayName = iProperties.Value("Project", "Part Number") & " <" & iProperties.Value("Project", "Description") & ">"

openDoc.Rebuild

'update
iLogicVb.UpdateWhenDone = True

[Cadmanto]

It should be noted that the rule for the assembly as posted by "foxrid3r" should not be used.  Reason being is if there are standard CC parts in the assermbly, this rule actually changes the display of the CC parts in the assembly browser.  Thus really causing change to the standard CC parts.  Which can't happen.  I know this because I ran the rule, and it currupted my assembly.  Especially when Vault is involved. I actually got this error message when trying to open the assembly after closing it and reopening it, once the rule has been run.

 

I will be testing the part rule in the morning to see if there are any issues with that rule.  I will report back my findings.

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

[Cadmanto]

Nice job "foxrid3r".  The part rule works perfectly!!!  Ran in the parts and when the parts were inserted into the assembly, the description showed up not only in the part, but also the assembly as well.  The rule, unlike the unlike the original assembly rule you created, can run in an assembly, just showing the assembly description without effecting the standard CC parts.

This is a good work around until my idea gets implemented into a future version.

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

[Cadmanto · Accepted solution]

Slight modification to this rule.

'create reference to part
openDoc = ThisApplication.ActiveDocument

'format display name
openDoc.DisplayName = iProperties.Value("Project", "Part Number") & " (" & iProperties.Value("Project", "Description") & ")"
openDoc.Rebuild

'update
iLogicVb.UpdateWhenDone = True

Removed the angle brackets and replaced with parenthesis.

Reason was when the angle brackets were used, when creating a new file using the template with this rule in it, it would not save.

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

[jt]

Hi.
Thank's for sharing your solutions.

When do you run the rule?

 

[shawnme]

I see the original question was asked 6 years ago... Has Autodesk created a way to do this without writing code?? I have a need for this (that's why this popped up during a search) and was hoping there would be an easy solution, possibly within a menu pick... Please let me know.  Thanks!!

[SER4]

If you have Vault, you can show any iProperties in the Vault browser:

https://knowledge.autodesk.com/support/vault-products/learn-explore/caas/CloudHelp/cloudhelp/2018/EN...

Configure Which Vault Properties Show

You can configure which Vault Properties are displayed in the Vault Browser.

1. Click the Choose Properties icon  in the Vault Browser.
2. On the Choose Properties dialog, select the properties that you want to display after the file name and click Add->.

   You can re-order how properties display by moving them up and down in the Show these fields in this order list.

   Select a property in the Show these fields in this order list and click <-Remove to hide that property.

3. Click OK to save your changes.

The file properties are appended to the file name in the browser.