BOM Sequential Numbers

[Anonymous]

Hello,

I need to add custom properties that will sequential number the parts in my BOM the same way that the item columns does (i.e. 1 then 1.1, 1.2 etc for parts) but so that the number is fixed with the part. I wish to add this column to the drawings so when I produce a drawing they can as for item 5.. and it will work in the BOM, also i can say item 4 has been replaced with item 40 and this will tie in completely with the model.

Is there a way of doing this?

Many Thanks

[cbenner]

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@Anonymous wrote:

Hello,

I need to add custom properties that will sequential number the parts in my BOM the same way that the item columns does (i.e. 1 then 1.1, 1.2 etc for parts) but so that the number is fixed with the part. I wish to add this column to the drawings so when I produce a drawing they can as for item 5.. and it will work in the BOM, also i can say item 4 has been replaced with item 40 and this will tie in completely with the model.

Is there a way of doing this?

Many Thanks

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@Anonymous

Can you give us an illustration of what you are trying to achieve?  Are you sure this isn't something that can be done out of the box?

[mcgyvr]

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@Anonymous wrote:

Hello,

Is there a way of doing this?

Many Thanks

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As you said.. add a custom iproperty.. 

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2016...

Here is how to modify your BOM to show that..

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2016...

Of course I don't know why you would ever want to do that..

Why not just use the part number to achieve the same exact functionality?

Why do you need another number to identify parts by?

[johnsonshiue]

Hi! It sounds like you want a unique integer number for each part and the number would be stored in the iProperties if the part, right?

Many thanks!

[salariua]

Sounds like you're after this:

http://cadsetterout.com/inventor-tutorials/autodesk-inventor-creating-coordinated-bom-for-large-asse...

[john_s2]

"Why do you need another number to identify parts by? "

It makes a lot of sense. Many use names not part numbers for parts, or the part numbers are two long to be easily identifiable.

Also, if you are creating a suite of unrelated drawings, you may want a consistent small number reference across all the drawings.  I appreciate you could use "views" of a sub assembly, or part, from the main assembly to maintain the main assembly BOM structure, and referencing, but this can become cumbersome. It is also just plain irritating, when when adding further parts to the main assembly after you have configured your "view" defined sub group.

Here's a thing, why can't "view" be defined by adding parts rather than hiding parts? That way, when you add more parts to an assembly subsequently they wont contaminate your predefined  "view".  If this were the case using views to subdivide an assembly would be a more practical proposition.  

[GORDONMABIYA]

I was hoping that you would provide an efficient method of using the very integer used in the Item column of the BOM as a non-customizable field which is based on sequence but is also available to appended in other fields i.e. part number, description.

[Anonymous]

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@Anonymous wrote:

Hello,

I need to add custom properties that will sequential number the parts in my BOM the same way that the item columns does (i.e. 1 then 1.1, 1.2 etc for parts) but so that the number is fixed with the part. I wish to add this column to the drawings so when I produce a drawing they can as for item 5.. and it will work in the BOM, also i can say item 4 has been replaced with item 40 and this will tie in completely with the model.

Is there a way of doing this?

Many Thanks

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WE do that, we use the authority property but a custom property would be as simple.

But we copy the item # from the BOM to the authority property, done with I-logic so would be easy enough to set a property.

I finish an assembly, then organize my bOm the way I want it, renumber the Item property the way I want and run the I-logic. I can then set and other BOM or balloon to the authority property and it will display across any IDW file.

We create 2 idw files, a set for the waterjet and bending part of the plant and then a fabrication drawing. 2 different formats. Balloon numbers are common to both drawings.

[GORDONMABIYA]

"But we copy the item # from the BOM to the authority property, done with I-logic so would be easy enough to set a property."

Hi Mario428

How do you copy with iLogic. Can you please provide the steps.

I am bit of a novice when it comes to Inventor programming.

[jtylerbc]

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@Anonymous wrote:

also i can say item 4 has been replaced with item 40 and this will tie in completely with the model.

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What you want to do with the item numbers is possible with some iLogic programming - I've seen posts here on these forums where it has been done.  However, I'm not sure your note itself is possible.

When you include iProperties in drawing text, you have two basic scenarios:

1. Leader Text:  The property value is pulled from the part that the leader touches.
2. Regular Text:  The property value is pulled from the first model that a drawing view was placed for.  Typically, in an assembly drawing like what you are describing, that means it will be pulling from the assembly, and not a part at all.

There is a way to do so for Parameters, but I am not aware of a way to insert iProperties from multiple parts into the same piece of text. 

[Anonymous]

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@GORDONMABIYA wrote:

"But we copy the item # from the BOM to the authority property, done with I-logic so would be easy enough to set a property."

Hi Mario428

How do you copy with iLogic. Can you please provide the steps.

I am bit of a novice when it comes to Inventor programming.

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Hello Gordon

See the I-logic below, was incorrect in my first post

Item is copied to the Engineer property but easy enough to change it.

Since we use frame generator the property Item Qty is copied to authority

There is also a "NUM_OF_ASSYS" property added to your parameters, we use this if there is multiple assemblies, multiplies item qty so authority property reflects how many parts required to do all the assemblies

Hope it helps

doc = ThisDoc.Document
Dim oAssyDef As AssemblyComponentDefinition = doc.ComponentDefinition
Dim oBOM As BOM = oAssyDef.BOM

oBOM.PartsOnlyViewEnabled = True

Dim oBOMView As BOMView = oBOM.BOMViews.Item("Parts Only")

Dim oBOMRow As BOMRow

For Each oBOMRow In oBOMView.BOMRows
    'Set a reference to the primary ComponentDefinition of the row
    
    Dim oCompDef As ComponentDefinition
    oCompDef = oBOMRow.ComponentDefinitions.Item(1)
    
    Dim CompFullDocumentName As String = oCompDef.Document.FullDocumentName
    Dim CompFileNameOnly As String
    Dim index As Integer = CompFullDocumentName.lastindexof("\")
    
    CompFileNameOnly = CompFullDocumentName.substring(index+1)
    
    Dim Itm As Integer
    Itm = oBOMRow.ItemNumber ()
        If iProperties.Value(CompFileNameOnly, "Project", "Engineer") = "" Then
        
        iProperties.Value(CompFileNameOnly, "Project", "Engineer") = Itm
        End If
        
        If iProperties.Value(CompFileNameOnly, "Project", "Engineer") <> Itm Then
        
        iProperties.Value(CompFileNameOnly, "Project", "Engineer") = Itm
        End If
   
    Dim Qty As Integer
    Qty = oBOMRow.ItemQuantity
    
        If iProperties.Value(CompFileNameOnly, "Project", "Authority") = "" Then
        
        iProperties.Value(CompFileNameOnly, "Project", "Authority") = NUM_OF_ASSYS*Qty
        End If
    
        If iProperties.Value(CompFileNameOnly, "Project", "Authority") <> NUM_OF_ASSYS*Qty Then
        
        iProperties.Value(CompFileNameOnly, "Project", "Authority") = NUM_OF_ASSYS*Qty
        End If

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