Replace a part in multiple assemblies

[Anonymous]

Hello,

I have always worked with Solidworks, but 6 months ago our company switched to Inventor.

Everything is going well, but there is one thing i cant get done.

I have a lot of parts that occur in multiple assemblies. 

Sometime i want to replace a part for another part (look al like) in all the assemblies.

For example: a plate with 4 holes replace for the same plate with 5 holes.

In Solidworks you can use the Solidworks Explorer, and replace the part for the other part and it is applied in all the assemblies.

But in Inventor you only replace the part in 1 assembly, so you have to replace them all by yourself. (with design assistent or in the assembly by replace component).

My question:

Is it possible to replace a part in all of the assemblies?

Hope you can help me.

Gerwin.

[SharkDesign]

I think it can be done in vault, but would need to check. Do you have vault?

[SharkDesign]

You can definitely do it with iLogic and the code wouldn't be too hard. 

[Anonymous]

No we don't have Vault.

[Gabriel_Watson]

We typically leverage operations like that using Vault Professional's "Copy Design" tool, and "Replace":
https://knowledge.autodesk.com/support/vault-products/learn-explore/caas/CloudHelp/cloudhelp/2021/EN...

[SharkDesign]

I can write some code a bit later, just going to the supermarket now. 

[Anonymous]

haha thats okay

[johnsonshiue]

Hi! This can be done within Inventor via Replace Component workflow. Or, use the standalone Design Assistant. Right-click on the assembly in File Explorer -> Design Assistant -> Manage -> select the part -> Action = Replace -> select the new part.

Many thanks!

[Anonymous]

I know,  but i want to replace the part in all assemblies where the part occurs.

[SharkDesign · Accepted solution]

This won't go through your entire hard drive, just the sub assemblies within the one you have open. 

Also, I'm not an iLogic expert and I've only very basically tested this so try it on something you don't mind making a mess of, or at least do an iLogic design Copy on an assembly first to try it out.

You just need to copy and paste the code into a new rule in your iLogic pallet.

Then change these two lines. The first is just the file name of the part you want to remove, the second is the full path and file name of the part you want to put in. N.B. your new part, you say has a different number of holes, you have to have modelled this from the old part and changed the number of holes or your constraints are going to break.

These are the lines you need to change:

Good luck!!!

Class this rule
	
	Dim oOld As String = "xxx.ipt" 'Replace xxxxxx with the file name of part to replace
	Dim oNew As String = "C:\xxxxxxx.ipt" 'replace xxx with full path, name and .ipt on the end of the file you want to use instead
	
	
	Dim oOcname As String
	
Sub Main
	
	If ThisApplication.ActiveDocumentType <> kAssemblyDocumentObject Then MessageBox.Show("This rule is designed to only work in assembly documents.", "Wrong Document Type") : Exit Sub
	
	Dim parentDoc As AssemblyDocument = ThisApplication.ActiveDocument
	
	'Do anything unique to main assembly
	
	Call AssemblyRunner(parentDoc)
	
End Sub

Sub AssemblyRunner(aDoc As AssemblyDocument)
	
	'Do things to the assembly file if any
	'MessageBox.Show(aDoc.DisplayName, "Assembly:")
	
        'Start Looping
	For Each oOcc As ComponentOccurrence In aDoc.ComponentDefinition.Occurrences
		If oOcc.DefinitionDocumentType = kAssemblyDocumentObject
			Call AssemblyRunner(oOcc.Definition.Document)
		Else If oOcc.DefinitionDocumentType = kPartDocumentObject
			oOcname = oOcc.Name
			
			Call PartRunner(oOcc.Definition.Document, aDoc)
			
		End If
	Next
	
End Sub

Sub PartRunner(pDoc As PartDocument, parent As AssemblyDocument)
	
If pDoc.DisplayName = oOld
Component.Replace(oOcname, oNew, True)
End If

End Sub
End Class
'loop code borrowed from JCamper

[swalton]

That Solidworks tool sounds useful.  I am not aware of a direct equivalent in Inventor.

I'd try the following:

1. Make a temporary container assembly and name it George.iam.
2. Place a copy of each assembly you plan to modify in George.iam.
3. Save George.

At this point I'd have two choices.  I could use the Replace All command in George.iam to replace all the parts at once, or run Design Assistant on George to replace every instance.  I'm not sure that Replace All penetrates into sub-assemblies.  Testing is required.

I'm not aware of a workflow in Vault that lets me replace plate1.ipt with plate2.ipt in every assembly that uses plate1.ipt.

[Anonymous]

Good morning,

I tried this.

This works only in de assembly you have open, but i think it should be like this.

Or do i have to run this rule every time before open an assembly?

I can search in design assistant wich assembly uses my part, and then open all the assemblies and run in every assembly the rule. But that's still a lot of work.

Is it possible with ilogic, to make a rule who search in all the assemblies without open te concerned assembly?

thanks in advance.

[SharkDesign]

You can create a blank assembly, drop a load of assemblies in it and let it
run. Then just save afterwards.
You cave it in external rules and then have it run every time you open an
assembly but this is a bit dangerous and also would take ages to open an
assembly.

[Anonymous]

Thank you james.

I think the best way for me is, search in Desgin assistant wich assembly uses the part.

Then run the rule with event trigger after open all of the assemblies.

Save.

And then delete the rule.

I can work with it, thanks.