topic BOM Sequential Numbers in Inventor Forum

BOM Sequential Numbers

Anonymous — Wed, 29 Mar 2017 15:29:33 GMT

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

Re: BOM Sequential Numbers

cbenner — Wed, 29 Mar 2017 17:37:36 GMT

@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

@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?

Re: BOM Sequential Numbers

mcgyvr — Wed, 29 Mar 2017 18:09:03 GMT

@Anonymous wrote:

Hello,

Is there a way of doing this?

Many Thanks

As you said.. add a custom iproperty..

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2016/ENU/Inventor-Help/files/GUID-9CD4A22C-7172-43BC-8AC8-A9CBB6AD6613-htm.html

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

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2016/ENU/Inventor-Help/files/GUID-5DE668D7-6288-477E-BFF8-941AC7B810DB-htm.html

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?

Re: BOM Sequential Numbers

johnsonshiue — Wed, 29 Mar 2017 21:14:51 GMT

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!

Re: BOM Sequential Numbers

salariua — Thu, 30 Mar 2017 06:17:36 GMT

Sounds like you're after this:

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

Re: BOM Sequential Numbers

john_s2 — Thu, 30 Mar 2017 08:16:59 GMT

"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.

Re: BOM Sequential Numbers

GORDONMABIYA — Tue, 27 Jun 2017 09:14:53 GMT

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.

Re: BOM Sequential Numbers

Anonymous — Tue, 27 Jun 2017 10:15:56 GMT

@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

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.

Re: BOM Sequential Numbers

GORDONMABIYA — Tue, 27 Jun 2017 12:40:22 GMT

"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.

Re: BOM Sequential Numbers

jtylerbc — Tue, 27 Jun 2017 13:33:25 GMT

@Anonymous wrote:

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

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:

Leader Text: The property value is pulled from the part that the leader touches.
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.

Re: BOM Sequential Numbers

Anonymous — Wed, 28 Jun 2017 10:26:26 GMT

@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.

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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