topic Re: Add or Remove Solid Bodies from Derived Part. in Inventor Programming Forum

Add or Remove Solid Bodies from Derived Part.

C_Haines_ENG — Wed, 04 Oct 2023 17:05:19 GMT

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?

Re: Add or Remove Solid Bodies from Derived Part.

bradeneuropeArthur — Thu, 05 Oct 2023 08:57:53 GMT

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?

Re: Add or Remove Solid Bodies from Derived Part.

C_Haines_ENG — Thu, 05 Oct 2023 13:09:50 GMT

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:

Re: Add or Remove Solid Bodies from Derived Part.

A.Acheson — Thu, 05 Oct 2023 14:39:35 GMT

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.

Re: Add or Remove Solid Bodies from Derived Part.

C_Haines_ENG — Tue, 17 Oct 2023 19:09:11 GMT

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

Re: Add or Remove Solid Bodies from Derived Part.

C_Haines_ENG — Wed, 25 Oct 2023 20:15:33 GMT

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