Derive assembly to part and save as step, with ilogic.?

[LSA-skan]

Hi

I have been searching all over this forum, youtube, google, and what not, and i haven't found a solution for my problem.

When we send 3D models to customers, we always derive the assembly to make it 1 solid part, so the customer cannot disassemble it to copy our product, and then save it as a step file.

I want to Derive an assembly to a part and then save it as a *.step file with an ilogic rule.

I worked out the last part, but i cannot find the Derive assembly code anywhere.

Im not an experienced programmer, i can only Copy paste, so if the solution is already posted in a simular rule, i will not be able to pick what i need from the code 🙂

hope someone can help me !

/LSA-skan 

[Curtis_Waguespack]

Hi LSA-skan,

Here's an example that will derive the assembly to a single solid with seams and then save that as a STP file. This example discards the derived part without saving it.

Attached it the code in a *.txt file in case pasting from this forum directly causes formatting errors.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

'set a reference to the assembly component definintion.
'this assumes an assembly document is open.
Dim oAsmCompDef As AssemblyComponentDefinition
oAsmCompDef = ThisApplication.ActiveDocument.ComponentDefinition    

'define the path and file name
Dim sPathandName as String
sPathandName  = ThisDoc.PathAndFileName(False) 

' Create a new part file to derive the selected part into 
'note: kPartDocumentObject is the default template
'you could specifiy a path and file name for a custom template
Dim oPartDoc As PartDocument
oPartDoc = ThisApplication.Documents.Add(kPartDocumentObject, ThisApplication.FileManager.GetTemplateFile(kPartDocumentObject)) 

'create the derived assembly deffinition
Dim oDerivedAssemblyDef As DerivedAssemblyDefinition 
oDerivedAssemblyDef = oPartDoc.ComponentDefinition.ReferenceComponents.DerivedAssemblyComponents.CreateDefinition(sPathandName & ".iam")

'Set derive style options
oDerivedAssemblyDef.DeriveStyle = DerivedComponentStyleEnum.kDeriveAsSingleBodyWithSeams
'options:
	'kDeriveAsSingleBodyWithSeams 
	'kDeriveAsSingleBodyNoSeams 
	'kDeriveAsMultipleBodies 
	'kDeriveAsWorkSurface 

'Create the derived part
Dim oDerivedAssembly As DerivedAssemblyComponent 
oDerivedAssembly = oPartDoc.ComponentDefinition.ReferenceComponents.DerivedAssemblyComponents.Add(oDerivedAssemblyDef)

'- - - - - - - - - - - - - - - - save *.stp  file- - - - - - - - - - - - - - - - - - - - - - - - - - - 
' Get the STEP translator Add-In.
Dim oSTEPTranslator As TranslatorAddIn
oSTEPTranslator = ThisApplication.ApplicationAddIns.ItemById("{90AF7F40-0C01-11D5-8E83-0010B541CD80}")
Dim oContext As TranslationContext
oContext = ThisApplication.TransientObjects.CreateTranslationContext
Dim oOptions As NameValueMap
oOptions = ThisApplication.TransientObjects.CreateNameValueMap

If oSTEPTranslator.HasSaveCopyAsOptions(ThisApplication.ActiveDocument, oContext, oOptions) Then
    ' Set application protocol.
    ' 2 = AP 203 - Configuration Controlled Design
    ' 3 = AP 214 - Automotive Design
    oOptions.Value("ApplicationProtocolType") = 3
    ' Other options...
    'oOptions.Value("Author") = ""
    'oOptions.Value("Authorization") = ""
    'oOptions.Value("Description") = ""
    'oOptions.Value("Organization") = ""
    oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism
    Dim oData As DataMedium
    oData = ThisApplication.TransientObjects.CreateDataMedium
    oData.FileName = sPathandName  & ".stp"
oSTEPTranslator.SaveCopyAs(ThisApplication.ActiveDocument, oContext, oOptions, oData)
End If
'- - - - - - - - - - - - end of *.stp  file code - - - - - - - - - - - - - - - - - - - - - - - - - 

'close the derived part without saving
oPartDoc.Close(True) 'True set's the skipsave boolean variant
MessageBox.Show("STP file created: " & sPathandName & ".stp", "iLogic")

[LSA-skan]

Hi Curtis

First of all, im very impressed that you came up with this in such short time.!

This works on small assemblies (tested with an assembly with 10 parts), but a larger assembly with 258parts (1015 occurrences) the step file contains 93 solid bodies instead of just 1.?!

Do you have any idea why theres is this difference..?

It takes about 5 min for inventor to derive this assembly, is that somehow cut short by the rule, so it never finishes or something crazy like that?

Secondly: the big assemly have diffrent Position, and Views, that i would like to choose between, before it makes the derived part if that is possible..?

/LSA-Skan