Export flat pattern with iProperty as filename

[Anonymous]

Hi all,

Is there a way to export a dxf with a custom iProperty as filename? It would be great if i can click on a face of a part and select the face to export it as a dxf.  Something like "Export face as" but then with the right name.

Many thanks

[mcgyvr]

Are you familiar with ilogic?

There is no "out of the box" solution but some ilogic code can handle the request for you..

If you need help please indicate the specific name of the custom iproperty and we can help modify the code posted here..

https://forums.autodesk.com/t5/inventor-customization/help-code-for-quot-export-face-as-quot-have-tr...

Specifically the code in post 9 in that thread

[Anonymous]

Thanks for the reply, I'm not that good with iLogic but I know how to make and use rules.

The Custom iProperty is POS.

Regards, Wim

[Sergio.D.Suárez · Accepted solution]

		
Dim doc As PartDocument= ThisDoc.Document
Dim oPath As String = ThisDoc.Path & "\"
Dim My_Prop As String = doc.PropertySets.Item("Inventor User Defined Properties").Item("POS").Value
		
Dim oFilename As String =  oPath & My_Prop  &  ".dxf"

Dim oCommand As CommandManager
oCommand = ThisApplication.CommandManager

oCommand.PostPrivateEvent(PrivateEventTypeEnum.kFileNameEvent,oFilename) 
oCommand.ControlDefinitions.Item("GeomToDXFCommand").Execute2(True)

Hi, click on a flat face and then try to execute this ilogic code. I think it could be useful. save a dxf in the path of your active file. It will take the name of the custom property "POS"
I hope this helps. regards 

[Anonymous]

This will do it.  Thank you very much!!!

[Anonymous]

Hi Sergio,

I think there's something wrong with the rule.  When I open multiple parts to save them as a DXF, the rule pick properties from another part.  So the 'POS' fields doesn't match with geometry.  Is this solvable?

Many thanks,

Wim Webers

[Sergio.D.Suárez]

I think maybe you're trying to run the rule from an assembly that contains the parts. The rule refers to the active document, and if it is an assembly it will return data from an assembly. If this is so, I'll see if I can modify it so that the actions from an assembly. regards

[Sergio.D.Suárez]

If you are working from a master assembly try this rule, I have not tried it, but I think it should work.
Keep in mind that it will return error if there is no "POS" property in the part.

Dim oFace As FaceProxy = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFacePlanarFilter, "Select Face")
	If oFace Is Nothing Then Exit Sub
		
Dim oOcc As ComponentOccurrence = oFace.ContainingOccurrence

oOcc.Edit
		
Dim doc As PartDocument = oFace.NativeObject.Parent.Parent.document

Dim oPath As String = Left(doc.FullFileName, (InStrRev(doc.FullFileName, "\", -1, vbTextCompare)))

Dim My_Prop As String = doc.PropertySets.Item("Inventor User Defined Properties").Item("POS").Value
		
Dim oFilename As String = oPath & My_Prop & ".dxf"

Dim oCommand As CommandManager
oCommand = ThisApplication.CommandManager

oCommand.DoSelect(oFace)'Select face
oCommand.PostPrivateEvent(PrivateEventTypeEnum.kFileNameEvent,oFilename) 
oCommand.ControlDefinitions.Item("GeomToDXFCommand").Execute2(True)

oOcc.ExitEdit(63747)

I hope I help you with your problem. regards

[Anonymous]

I'm exporting from a part and not from an assembly, but I opened them from the BOM in an assembly.  Now I opened them again, closed the assembly and start to export and it works now.  I'm not sure if there was the problem is but is working now.

Thanks for your time.

Regards, Wim

[jimmydieck]

Does the .dxf file default to a certain file type and version (i.e. AutoCAD 2013 DXF vs. 2018 )? If not, is there a way this can be controlled using code or properties in Inventor?

Thank you,

Jimmy