Autodesk Inventor

[#1]

Does anyone know a way or a code to physically change the sheet metal defaults using iLogic code, I want to change parts in my assembly without opening each individual part and changing it there. Please help!

[#2 · Accepted solution]

  Dim oAssyDoc As AssemblyDocument
  oAssyDoc = ThisApplication.ActiveDocument  
  Dim oDoc As Inventor.Document

'Add Input Box to retreive value here
  Dim oTargetTHK As Double
  oTargetTHK=25.4
  
  'Check all referenced docs 
  For Each oDoc In oAssyDoc.AllReferencedDocuments

    'verify document type (we are interested in metal sheets only)
    If oDoc.ComponentDefinition.Type = 150995200 Then
		Dim oSheetMetalCompDef As SheetMetalComponentDefinition
		oSheetMetalCompDef = oDoc.ComponentDefinition
		
		' Override the thickness for the document
		oSheetMetalCompDef.UseSheetMetalStyleThickness = False
	
		' Get a reference to the parameter controlling the thickness.
		Dim oThicknessParam As Parameter
		oThicknessParam = oSheetMetalCompDef.Thickness
		
		' Change the value of the parameter.
		oThicknessParam.Value = oTargetTHK
		
	Else
	End If
Next

I was able to put the above code together after reviewing the example titled 'Sheet Metal Thickness Editing API Sample' from the Help pull down menu > Community Resources > Programming Help. Seems to work on the few simple examples I've tested. 

Hope this helps.

[#3]

I get an error when i copy this code into it's own rule that says "Error on Line 10 : 'For' must end with a matching 'Next'.

Am I doing something wrong or do I need to change anything in the code to personalize it?

Thank you

[#4]

Hi rdiamond113,

Just a guess but did you happen to miss the last line when you copied the code?

The last line, Line 29,  contains the missing Next statement.

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

[#5]

I added it to my assembly and when I ran the rule I received a ton of errors. I'm using this to change the sheet metal type of a round column cover consisting of 4 quarter "skins". I'm not sure what type of parts you're using this code with but some of the errors I got had to do with basically rebuilding the skin and what not, like bend radius errors and sketch geometry errors

[#6]

Hi rdiamond113,

It worked for me using an assembly with 3 sheet metal parts and 2 non-sheetmetal parts.

I made a couple of modifications, by adding an update statement and adding an input list, but other than that it's the same.

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

Dim oAssyDoc As AssemblyDocument
oAssyDoc = ThisApplication.ActiveDocument  
Dim oDoc As Inventor.Document

'Add Input Box to retreive value here
Dim oTargetTHK As Double
'get user input
'oTargetTHK= InputBox("Enter Thickness", "iLogic", "0.2")

'create list of thicknesses
dList = new double(){0.1,0.2,0.3}
'get user input from list
oTargetTHK = InputListBox("Select a Thickness", dList, dList(0), "iLogic", "Thicknesses")

  
  'Check all referenced docs 
For Each oDoc In oAssyDoc.AllReferencedDocuments

	'verify document type (we are interested in metal sheets only)
	If oDoc.ComponentDefinition.Type = 150995200 Then
		Dim oSheetMetalCompDef As SheetMetalComponentDefinition
		oSheetMetalCompDef = oDoc.ComponentDefinition
		
		' Override the thickness for the document
		oSheetMetalCompDef.UseSheetMetalStyleThickness = False
	
		' Get a reference to the parameter controlling the thickness.
		Dim oThicknessParam As Parameter
		oThicknessParam = oSheetMetalCompDef.Thickness
		
		' Change the value of the parameter.
		oThicknessParam.Value = oTargetTHK
	Else
	End If
Next

InventorVb.DocumentUpdate()

[#7]

Okay I got it to work, the only issue I have now (LOL) is setting my specific sheet metal thickness, I changed where you had the thicknesses listed and found that it was setting the thickness to half what I ented in the list. how should I enter my standard sheet thicknesses?

[#8]

I just realized the output from the code is metric, how can i change it to Inches?

[#9 · Accepted solution]

Hi rdiamond113,

Internally Inventor works with centimeters as the default unit, to adjust your input to inches can multiply your input by 2.54 as shown in this example.

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

Dim oAssyDoc As AssemblyDocument
oAssyDoc = ThisApplication.ActiveDocument  
Dim oDoc As Inventor.Document

'Add Input Box to retreive value here
Dim oTargetTHK As Double
'get user input
oTargetTHK= InputBox("Enter Thickness", "iLogic", "0.2")*2.54

 
  'Check all referenced docs 
For Each oDoc In oAssyDoc.AllReferencedDocuments

	'verify document type (we are interested in metal sheets only)
	If oDoc.ComponentDefinition.Type = 150995200 Then
		Dim oSheetMetalCompDef As SheetMetalComponentDefinition
		oSheetMetalCompDef = oDoc.ComponentDefinition
		
		' Override the thickness for the document
		oSheetMetalCompDef.UseSheetMetalStyleThickness = False
	
		' Get a reference to the parameter controlling the thickness.
		Dim oThicknessParam As Parameter
		oThicknessParam = oSheetMetalCompDef.Thickness
		
		' Change the value of the parameter.
		oThicknessParam.Value = oTargetTHK
	Else
	End If
Next

InventorVb.DocumentUpdate()