Inventor General Discussion

Inventor General Discussion

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Registered: ‎05-08-2012
Post 1 of 5

Bolt assembly descriptions in a parts list

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07-25-2012 08:50 AM

At my workplace it has been standard practice in Autocad to call out bolt assemblies in a parts list as: 1/2-13 unc hex hd. bolt w/flat washer & nut.  Has anyone figured out how to do this in Inventor?  I know I can enter this info on the assembly iProps for the bolt assembly, I was hoping someone came up with an automated format, maybe pulling info from the bolt itself to populate the assembly iProps?  Any info/suggestions greatly welcomed!

James Winkler

Product Design Suite Ultimate 2014
Vault Professional 2014
Windows 7 Pro


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Registered: ‎05-18-2011
Post 2 of 5

Re: Bolt assembly descriptions in a parts list

07-25-2012 08:59 AM in reply to: Winks87

you can use ilogic to do this easy. as long as it is set up from the get go. Do you use content center hardware or do you have a lybary?

 

When you insert a bolt nut wash ect.. is it an assembly or parts brought in?

 

Are they ipart hardware?

 


Please mark this response as "Accept as Solution" if it answers your question.

James Letcher
2012 Factory Design Suite ( will not load 2013)
What happen to my Inventor :-(
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Post 3 of 5

Re: Bolt assembly descriptions in a parts list

07-25-2012 09:17 AM in reply to: Winks87

We have built standard bolted assemblies for our most commonly used configurations and placed them in our library.

 

This way everyone is using the same assebmlies, and the descriptions come in the same way everytime for everyone.

Mike Patchus

Inventor 2012 SP3 ~ Vault Pro 2013
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Mentor
189 Posts
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Registered: ‎05-08-2012
Post 4 of 5

Re: Bolt assembly descriptions in a parts list

07-26-2012 05:03 AM in reply to: Winks87

Currently, we bring in standard content center parts with bolted assembly.  I have no experience with iLogic yet, but  I am willing to experiment as long as it is not complicated for the users.  We have multiple users and would like an easy solution for the end users.  I would be open to iParts or iLogic.  We will be upgrading to 2012 soon and would be a good time if I need to modify content center or create new libraries if needed.  What is involved in the iLogic route?

James Winkler

Product Design Suite Ultimate 2014
Vault Professional 2014
Windows 7 Pro


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Registered: ‎11-23-2005
Post 5 of 5

Re: Bolt assembly descriptions in a parts list

08-07-2012 01:54 PM in reply to: Winks87

Not sure if iLogic will help you at all because we disable iLogic rules inside Bolted connection assemblies.

 

Here is a another thought. If you place below macro in your VBA Application project , select a bolted connection first and then run the macro, you will get a string similar to what you want in the Description property of the bolted connection subassembly. Of course this is far from being automatic (only works on one bolted connection at a time and has to be repeated if the composition of the bolted connection changes)

 

By using the "-" string as separator between each individual component's description, I was able to come up with overall description strings like:

ANSI B18.2.2 - 1 1/2 - 6-Lock Washers (Inch Series)Extra-Duty Helical Spring Lock Washer-Heavy Hex Bolt-Washer A-Hex Nuts (Inch Series) Slotted Hex Nut

 

or:


DIN 6924 - M4-Hexagon Socket Countersunk Head Screw-Spring Washer-Hex Nut

 

Option Explicit
Sub boltnaming()
Dim assydoc As AssemblyDocument
Set assydoc = ThisApplication.ActiveDocument
Dim partdoc As ComponentOccurrence
Dim lastdoc As ComponentOccurrence
Dim enhanceddesc As String
enhanceddesc = ""

' Check to make sure a sub-ssembly is selected.
If assydoc.SelectSet.count > 0 Then
If (assydoc.DocumentType <> kAssemblyDocumentObject) Then
   MsgBox "A bolted connection must be selected first."
   Exit Sub
End If
Else
  MsgBox "A bolted connection must be selected first."
  Exit Sub
End If

Dim subassydoc As ComponentOccurrence
Set subassydoc = assydoc.SelectSet.Item(1)

Set partdoc = assydoc.SelectSet.Item(1).Definition.Occurrences.Item(1)

For Each partdoc In subassydoc.Definition.Occurrences

Dim partdesc As Property
Set partdesc = partdoc.Definition.Document.PropertySets.Item("Design Tracking Properties").Item("Description")
enhanceddesc = enhanceddesc + "-" + partdesc.Value
Set lastdoc = partdoc
Next partdoc

Dim partnumber As String
partnumber = lastdoc.Definition.Document.PropertySets.Item("Design Tracking Properties").Item("Part Number").Value
subassydoc.Definition.Document.PropertySets.Item("Design Tracking Properties").Item("Description").Value = partnumber + "-" + enhanceddesc

End Sub

 

 

Cheers

Bob

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