How do I change the document Units?

[karthur1]

I have imported a large .sat assembly file that has its units set to "feet". When I imported this assembly, I had to use feet in order to get the parts to come in correctly. Now all the parts in this assembly also have the document units set to feet. I would like to now change all the parts to have the document units set to inch. There are over 1,300 parts that I have to change, so I don't want to have to open each part up and change it. Looking for a macro or some way to go thru the parts and set this quickly.

Thanks

[alewer]

On a small test assembly, this macro seems to do the trick.

Public Sub SetActiveDocUnits()
'(Run this macro)
Dim oActiveDocument As Inventor.Document
Set oActiveDocument = ThisApplication.ActiveDocument

SetLengthUnitsToInch oActiveDocument
End Sub

Private Sub SetLengthUnitsToInch(Document As Inventor.Document)
'Get Units of Measure
Dim oUOM As Inventor.UnitsOfMeasure
Set oUOM = Document.UnitsOfMeasure

'Set lenght units to inch and save
oUOM.LengthUnits = kInchLengthUnits
Document.Save

'Run recursively for assembly
If TypeOf Document Is Inventor.AssemblyDocument Then
Dim oAssemblyDocument As Inventor.AssemblyDocument
Set oAssemblyDocument = Document
Dim oOccurrence As Inventor.ComponentOccurrence
For Each oOccurrence In oAssemblyDocument.ComponentDefinition.Occurrences
SetLengthUnitsToInch oOccurrence.Definition.Document
Next oOccurrence
End If
End Sub

[karthur1]

It changes the units, but I can't get it to save the change to the parts. After I run this macro, I can open the parts individually and the units are changed. But, if I close the assembly and open the part itself, it is back to the old units.
When I have the assembly open and run the macro, I saved the assembly. I thought that the parts were also getting saved, but they are not.

If I open a part and manually change the document settings, it will dirty the part and it shows that it needs to be saved. If I run this macro it changes the document settings, but it does not dirty the part. Edited by: karthur1 on Sep 25, 2009 8:52 AM

[karthur1 · Accepted solution]

Here is a corrected version alewer sent me that dirty's the file so it will be saved. Thanks.

Public Sub SetActiveDocUnits()

Dim oActiveDocument As Inventor.Document
Set oActiveDocument = ThisApplication.ActiveDocument
SetLengthUnitsToInch oActiveDocument
End Sub

Private Sub SetLengthUnitsToInch(Document As Inventor.Document)

'Get Units of Measure
Dim oUOM As Inventor.UnitsOfMeasure
Set oUOM = Document.UnitsOfMeasure
'Set length units to inch and save
oUOM.LengthUnits = kInchLengthUnits
document.Dirty = True
Document.Update
Document.Save

'Run recursively for assembly
If TypeOf Document Is Inventor.AssemblyDocument Then
Dim oAssemblyDocument As Inventor.AssemblyDocument
Set oAssemblyDocument = Document
Dim oOccurrence As Inventor.ComponentOccurrence
For Each oOccurrence In oAssemblyDocument.ComponentDefinition.Occurrences
SetLengthUnitsToInch oOccurrence.Definition.Document
Next oOccurrence
End If
End Sub

Edited by: karthur1 on Sep 25, 2009 4:13 PM

[scottmoyse · Accepted solution]

Just to contribute to this beauty. I've tweaked this to correct the units for the rest of the world 😉

Also changed it from only modifying Length units, but also mass & angle.

Thanks to all in this thread for posting this in the first place. I'll be using this to convert all of the Inventor HSM CAM datasets to metric from imperial.

Public Sub SetActiveDocUnits()
Dim oActiveDocument As Inventor.Document
Set oActiveDocument = ThisApplication.ActiveDocument
SetUnitsToMetric oActiveDocument
End Sub

Private Sub SetUnitsToMetric(Document As Inventor.Document)
'Get Units of Measure
Dim oUOM As Inventor.UnitsOfMeasure
Set oUOM = Document.UnitsOfMeasure
'Set length units to Metric and save
oUOM.LengthUnits = kMillimeterLengthUnits
oUOM.MassUnits = kGramMassUnits
oUOM.AngleUnits = kDegreeAngleUnits
Document.Dirty = True
Document.Update
Document.Save

'Run recursively for assembly
If TypeOf Document Is Inventor.AssemblyDocument Then
Dim oAssemblyDocument As Inventor.AssemblyDocument
Set oAssemblyDocument = Document
Dim oOccurrence As Inventor.ComponentOccurrence
For Each oOccurrence In oAssemblyDocument.ComponentDefinition.Occurrences
SetUnitsToMetric oOccurrence.Definition.Document
Next oOccurrence
End If
End Sub

[WHolzwarth]

Good stuff, Scott.

I think, that can be used with imported STEPs or other types for changing angles from radians to degrees, too.

I'll try it instantly.

Walter 

[aveen.design]

[WHolzwarth]

It's VBA, not iLogic

iLogic needs a minor change

[aveen.design]

dear sir I need illogic I don't know how VBA works

[WHolzwarth]

Look here. I think it's the same issue:

https://forums.autodesk.com/t5/inventor-customization/find-and-replace-code-inside-i-logic-rule/m-p/...

[eng.co]

Hello Scott,

Please, can you make a short screencast video which shows how to insert this code in inventor and how this code is used.

I know nothing about this things.

Thank you!

[Manuelcamposcosta]

Hi!

Could you please convert this code to ilogic?

Thanks in advance.

[johnsonshiue]

Hi Manuel,

The 2023 iLogic debug tool helps quite a bit. I can follow the error message and correct the syntax to VB.Net. Here you go. Just copy the following and paste it to a rule.

Many thanks!

Johnson

Public Sub Main()
Dim oActiveDocument As Inventor.Document
oActiveDocument = ThisApplication.ActiveDocument
SetUnitsToMetric(oActiveDocument)
End Sub

Private Sub SetUnitsToMetric(Document As Inventor.Document)
'Get Units of Measure
Dim oUOM As Inventor.UnitsOfMeasure
oUOM = Document.UnitsOfMeasure
'Set length units to Metric and save
oUOM.LengthUnits = kMillimeterLengthUnits
oUOM.MassUnits = kGramMassUnits
oUOM.AngleUnits = kDegreeAngleUnits
Document.Dirty = True
Document.Update
Document.Save

'Run recursively for assembly
If TypeOf Document Is Inventor.AssemblyDocument Then
Dim oAssemblyDocument As Inventor.AssemblyDocument
oAssemblyDocument = Document
Dim oOccurrence As Inventor.ComponentOccurrence
For Each oOccurrence In oAssemblyDocument.ComponentDefinition.Occurrences
SetUnitsToMetric(oOccurrence.Definition.Document)
Next oOccurrence
End If
End Sub

[Manuelcamposcosta]

@johnsonshiue Thanks a lot!

I know it was probably easy to solve, it's my fault not knowing how to program.

Also we aren't yet on 2023.

[Manuelcamposcosta]

@johnsonshiue 

I'm getting an error when I run it on assemblies, and also in parts when I run it with trigger before save.

[johnsonshiue]

Hi Manuel,

No, it is not your fault that you don't program. You don't need to. I am not a developer either. I am just a user happening to know the product relatively well.

If possible, please share the files and the rule with me directly johnson.shiue@autodesk.com. I would like to take a closer look. It is possible the rule has issues that I did not see.

Many thanks!

[johnsonshiue]

Hi Folks,

Manuel sent me his files and the rule. I think it was a bit over-complicated. Here is a simpler rule to change the document units. It should work.

Dim oAssy As Document = ThisApplication.ActiveDocument

Dim allDocs As DocumentsEnumerator = oAssy.AllReferencedDocuments

Dim oDoc As Document

For Each oDoc In allDocs

    oDoc.UnitsOfMeasure.AngleUnits = UnitsTypeEnum.kDegreeAngleUnits

              oDoc.UnitsOfMeasure.LengthUnits = UnitsTypeEnum.kMillimeterLengthUnits

              oDoc.UnitsOfMeasure.MassUnits = UnitsTypeEnum.kKilogramMassUnits

Next

Many thanks!

[Manuelcamposcosta]

@johnsonshiue Perfect!

Is there any possibility to have for example grams in parts and kilograms in assemblies?

Just to note for other people this rule doesn't change the values in the assembly we are running the ilogic, but that's easy to solve.

Thanks a lot Johnson!

[johnsonshiue]

Hi Manuel,

Here you go! You need to change the unit enums accordingly. This rule just shows how to change Doc Units per doc type within an assembly.

Dim oAssy As Document = ThisApplication.ActiveDocument
Dim allDocs As DocumentsEnumerator = oAssy.AllReferencedDocuments
Dim oDoc As Document
For Each oDoc In allDocs

If oDoc.DocumentType=Inventor.DocumentTypeEnum.kPartDocumentObject Then

oDoc.UnitsOfMeasure.AngleUnits = UnitsTypeEnum.kDegreeAngleUnits
oDoc.UnitsOfMeasure.LengthUnits = UnitsTypeEnum.kMillimeterLengthUnits
oDoc.UnitsOfMeasure.MassUnits = UnitsTypeEnum.kGramMassUnits

Else If oDoc.DocumentType = Inventor.DocumentTypeEnum.kAssemblyDocumentObject
oDoc.UnitsOfMeasure.AngleUnits = UnitsTypeEnum.kRadianAngleUnits
oDoc.UnitsOfMeasure.LengthUnits = UnitsTypeEnum.kMeterLengthUnits
oDoc.UnitsOfMeasure.MassUnits = UnitsTypeEnum.kKilogramMassUnits
End If

Next

Many thanks!