I-Logic with Derived Parts

[cwilliamson232RQ]

Is there a way to Turn on and off my Derived Part thru I-logic? 

[johnsonshiue]

Hi! I am sorry that I don't understand the request. You want to turn on/off a derived part in an assembly? Or, you want to turn on/off derived feature within the derived part? Or, you want to drive derive or not from the source part?

Many thanks!

[cwilliamson232RQ]

So I have a part and inside that Part I have a Derived Part called "BOLT". I created a Parameter called "HARDWARE" and it is a multi-value text with the values "ON" and "OFF". I can I make the I-Logic be able to Turn the Derived Part 'BOLT" to be ON and OFF. 

[johnsonshiue]

Hi! I think it is doable. You want to suppress, right? Are you trying to make Text parameter in an iPart?

Many thanks!

[cwilliamson232RQ]

Yes Suppress and Yes an IPart.

[A.Acheson]

Can you attach an a simple part showing your workflow. There are a few ways to derive so we would need to target the way you are manually deriving at the moment in order to replicate. Controlling an iPart through the factory can be tricky due to the members needing to update. Derive should be easier. Here is some reading on derived parameters. 
https://help.autodesk.com/view/INVNTOR/2021/ENU/?caas=caas/discussion/t5/Inventor-Customization/iLog...

[cwilliamson232RQ]

Here is a simple I-part with a Derived Part in it that I broke the Link. 

[cwilliamson232RQ]

Here is a better Example

[cwilliamson232RQ]

Can you try the derived part with my test part i sent? 

[cwilliamson232RQ]

How?

[A.Acheson]

@cwilliamson232RQ 

I will try this if I get a chance, hopefully other users have experience with this also. Is it a inv 2020 or earlier file? Otherwise I am out unfortunately. 

[cwilliamson232RQ]

It is in Inventor 2020

[A.Acheson]

I was able to turn off the derived part in this derived part you have attached.  Below is how this is achieved and I have included this in the attached part. Depending on how you are going to use this, it will need to be adapted, have you a larger end goal? 

'https://forums.autodesk.com/t5/inventor-customization/ilogic-rule-to-include-exclude-derived-parameter-in-all-parts/td-p/8691196

If ThisApplication.ActiveDocument.DocumentType <> kPartDocumentObject Then
	MessageBox.Show("Make a Part Document the active document,Exiting", "iLogic") 
Else
	
	Dim oDerSolidBodyList As New ArrayList
	
	Dim oDerPart As PartDocument
	oDerPart = ThisApplication.ActiveDocument

	'Look for Derived part components
	If oDerPart.ComponentDefinition.ReferenceComponents.DerivedPartComponents.Count < 1 Then
		MessageBox.Show("No Derived Part Components in this part", "iLogic")   

	Else
		' Set a reference to the part component definition
		Dim oDerPartCompDef As PartComponentDefinition
		oDerPartCompDef = oDerPart.ComponentDefinition
		
		'Get a reference to derived part components in this part
		Dim oDerPartComps As DerivedPartComponents
		oDerPartComps = oDerPartCompDef.ReferenceComponents.DerivedPartComponents
		
		'Get a reference to derived part component
		Dim oDerPartComp As DerivedPartComponent
		oDerPartComp = oDerPartComps(1)'1st component
		
		' Derived part component by name
		'MessageBox.Show(oDerPartComp.Name, "iLogic")
		
		'ReferenceFeature objects 'Found in API Help searching solidbody
		Dim oDerSolidBodies As ReferenceFeaturesEnumerator
		oDerSolidBodies = oDerPartComp.SolidBodies
		
		Dim oDerSolidBody As ReferenceFeature
		
		For Each oDerSolidBody In oDerSolidBodies
			'Add each solid body to array list
			oDerSolidBodyList.Add(oDerSolidBody.Name)
			'MessageBox.Show(oDerSolidBody.Name, "iLogic")
			
			If HARDWARE = "OFF" Then
				oDerSolidBody.Suppressed = True
			ElseIf HARDWARE = "ON" Then
				oDerSolidBody.Suppressed = False
			End If	
			
		Next
		'oDerSolidBodyName = InputListBox("Select one", oDerSolidBodyList, oDerSolidBodyName, Title := "Title", ListName := "Solid Body List")
	End If
End If

[cwilliamson232RQ]

So seems this Suppresses ALL of my Derived parts. Is there a way to specify specific Derived Parts Only? 

[A.Acheson]

This snippet targets the first derived component in your part, in your case the derived assembly by number but you could also type an occurence name.  

'Get a reference to derived part component
		Dim oDerPartComp As DerivedPartComponent
		oDerPartComp = oDerPartComps(1)'1st component
		
		' Derived part component by name
		'MessageBox.Show(oDerPartComp.Name, "iLogic")

In your case you have multiple parts in a derived assembly so you would need to target the solid body by name or number with this snippet.

oDerSolidBody.Name

So is it parts (solid body) in the derived assembly you need to target or just the main derived part? You could put the list of derived components and solid bodies in an array list box and deselect one by one what you don’t want/add what you do want.  This filtering will really depend how frequent you will use this rule and what you may need to filter. 

[cwilliamson232RQ]

The array list might work best. So say I have 15 Derived parts but only 5 of those are going to be considered "HARDWARE" so I can turn those 5 on and off. 

So in that I-logic code you posted. Which lines are supposed to be COMMENTED out? 

So replace this name with ASSY_Bolt_Carraige_0.375x1.ipt  

[cwilliamson232RQ]

Here is a updated part with a few more derived parts in it. 

[A.Acheson]

If the derived assembly components are not going to change name  run a filter like the below based on the occurrence name. I haven't tested this so hopefully there isn't any issues. There maybe other easiers ways. 

'Get a reference to derived part component
Dim oDerPartComp As DerivedPartComponent
Dim ExcludeList As New ArrayList
'add the exclusion occurance names here
ExcludeList.add ("ASSY_Bolt_Carraige_0.375x1.ipt")
'ExcludeList.add ("...............")
Dim oExcludePart As String
For Each oDerPartComp in oDerPartComps
   For Each oExcludePart in Excludelist
           'Remove this derived part from the search
            If Not oDerPartComp.Name Then
             ...... Turn off solid bodies here
            End IF
    Next
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