Add or Remove Solid Bodies from Derived Part.

[C_Haines_ENG]

Good afternoon,

I need some help figuring out how to add or remove solidparts from an extracted "Derived Part".

I can use the "make components" tool to extract my solid bodies but I need to be able to add / remove parts from the derived part and I need to be able to switch model states of the derived part aswell.

Could anyone help with this?

[bradeneuropeArthur]

Could you explain a bit more in detail?

Maybe you can make some screenshots to explain what you try to do.

Your question is based on i-logic or via VBA or via an add-in?

[C_Haines_ENG]

My question is a iLogic questions, here is what I mean by derived part:

Its a single solid body extracted from a larger part file containing all the solid bodies, and im trying to select whatever solid body I want within this menu:

In iLogic, however I cant seem to figure out how exactly this works, and on top of that id like to be able to select what model state it wants as shown below:

[A.Acheson]

Hi @C_Haines_ENG 

There is a post on this forum for adjusting the solidy body shown here There is also a DerivedPartDefinition help page here where you can start adjusting the outcome of the derive. Attach your attempted sample if you get stuck implementing. 

[C_Haines_ENG]

Is there anyway to simplify this? Seems like I have a couple things here that do not need to be there.

Edit: This code can only be run on an already extracted derived part.

Dim ODDoc As Document = ThisDoc.Document
Dim oDPComp As DerivedPartComponent
Dim oDPComps As DerivedPartComponents
oDPComps = ODDoc.ComponentDefinition.ReferenceComponents.DerivedPartComponents

	For x = 1 To oDPComps.Count
		oDPComp = oDPComps.Item(x)
		Dim oDPDef As DerivedPartUniformScaleDef = oDPComp.Definition
		Dim oDPEnts As DerivedPartEntities = oDPDef.Solids
		Dim oDPEnt As DerivedPartEntity
		
			For Each oDPEnt In oDPEnts
				
				'CHANGE MODEL STATE
				oDPDef.ActiveModelState = "MODEL STATE NAME"
			
                                'ADD PART YOU WANT BY SOLID NAME
				If oDPEnt.ReferencedEntity.Name = "YOUR SOLID BODY NAME" Then
					oDPEnt.IncludeEntity = True
					Exit For
				End If
				
			Next
			
	oDPComp.Definition = oDPDef
	
	Next

[C_Haines_ENG · Accepted solution]

For anyone who comes by this in the future, this code will extract all solid bodies from your part file, allowing you to select the model state.

Dim doc As PartDocument = ThisApplication.ActiveDocument

For Each sb In doc.ComponentDefinition.SurfaceBodies
				
    'Create Part With A Derived Part Component
    Dim prt As PartDocument
    prt = ThisApplication.Documents.Add(kPartDocumentObject, "PART TEMPLATE DIRECTORY")
    
    Dim oDPComps As DerivedPartComponents = prt.ComponentDefinition.ReferenceComponents.DerivedPartComponents
    Dim oDPDef As DerivedPartUniformScaleDef = oDPComps.CreateUniformScaleDef(doc.FullDocumentName)
	
	'Select Model States
	oDPDef.ActiveModelState = "MODEL STATE NAME"	
	
    'Hide All Other Solid Bodies
    Dim oDPEnt As DerivedPartEntity
   	For Each oDPEnt In oDPDef.Solids
	
        oDPEnt.IncludeEntity = oDPEnt.ReferencedEntity Is sb
		
    Next
	
	oDPComps.Add(oDPDef)
	
	        prt.SaveAs("DRIVE PATH" & sb.Name & ".ipt", False)
		
		prt.Close
		
Next