ilogic

[dhaval3112]

Hello Sir,

I am trying to make vessel in Autodesk Inventor using iLogic but i get some trouble to suppress component.
When i suppress component inventor make LOD. I dont understand why they make LOD.
Can you please guide me further ?? or give me any other solution to suppress parts.

Thanks,

Dhaval

[JoyceZhou]

Hi

In one assembly, you could suppress component by context menu-Suppress command or from iLogic-suppress.

The suppress action will create LOD.

If you want to know more about LOD, you could find the help content of the LOD

http://help.autodesk.com/view/INVNTOR/2017/ENU/?guid=GUID-BB22DDCB-F370-4BF0-B438-EC1D0E91D49E

You could use Design View instead of LOD in your assembly. Select one component, right click, visibility. Uncheck the visibility will hide the component, and you could switch between different Design View for different intent.

Hope this helpful for you.

Thanks,

[CCarreiras]

Hi!

You must Create a LOD called  iLogic to be able to suppress parts usig iLogic rules.

[dhaval3112]

Hello,

Thanks for prompt replay.

If i choose visibility option then part will be shown bill of materil and for the same i have to mannualy correct as off from BOM.

Thanks

Dhaval

[JoyceZhou · Accepted solution]

May I know which version are you using?

If you are in R2017, you could get the correct component quantity in drawing Partlist by filter with Assembly Design View->select "Limit QTY to visible components only"

Hope this helpful for you.

Thanks,

[Anonymous · Accepted solution]

If you're not using inventor 2017 then there is a other way.

I've been struggling with the LOD for a long time and decided to make use of the visibility of parts.

Like you said, the BOM will not be influenced by the visibility of parts. Therefore I'm using the next Ilogic code.

It sets the parts that are invisible to reference in the BOM.

SyntaxEditor Code Snippet

Sub Main()
Question = MessageBox.Show("Wilt u de Bill Of Materials updaten? Dit kan enkele minuten duren.", "BOM",MessageBoxButtons.YesNo,MessageBoxIcon.Information)
If Question = vbYes Then

    Dim oAsmCompDef As AssemblyComponentDefinition
    oAsmCompDef = ThisApplication.ActiveDocument.ComponentDefinition
    Dim oOccurrence As ComponentOccurrence
    For Each oOccurrence In oAsmCompDef.Occurrences
        Call toggle(oOccurrence)
        If oOccurrence.DefinitionDocumentType = kAssemblyDocumentObject Then
        Call ListComp(oOccurrence)
        End If
        Next
    End If
End Sub

Sub ListComp(oOcc As ComponentOccurrence)
    Dim oOcc1 As ComponentOccurrence
    For Each oOcc1 In oOcc.SubOccurrences
        Call toggle(oOcc1 )
        If oOcc1.DefinitionDocumentType = kAssemblyDocumentObject Then
            Call ListComp(oOcc1)
        End If
    Next
End Sub

Sub toggle(oOcc As ComponentOccurrence)

If Not TypeOf oOcc.Definition Is VirtualComponentDefinition Then
    If Component.Visible(oOcc.Name) = True Then
        Component.InventorComponent(oOcc.Name).BOMStructure = _
        BOMStructureEnum.kDefaultBOMStructure
    ElseIf Component.Visible(oOcc.Name) = False Then
        Component.InventorComponent(oOcc.Name).BOMStructure = _
        BOMStructureEnum.kReferenceBOMStructure
    End If
End If


End Sub

In my assembly it takes up to 3-4 minutes to walk through the whole model 

[dhaval3112]

Solution is work. Thanks to all of you. 

[bionorica2015]

Please help me

Link: https://forums.autodesk.com/t5/inventor-forum/vba-ilogic-rule-to-rename-model-parameter-names/td-p/1...