If you wish to change a Property's value on a document having Model States, the workflow via API is the similar to the Inventor UI:
- Activate the required Model State using ModelState.Activate.
- Set the MemberEditScope to either kEditActiveMember or kEditAllMembers based on whether the updated value would be applied only to the active model state or all members.
- Get the property from Factory document (and not the Model State document), and change its value.
- To confirm whether the required Property has been correctly updated, activate the respective Model State and query the property from the Factory Document.
Here is a sample VBA code that exhibits a similar workflow:
Dim oPartDoc As PartDocument
Set oPartDoc = ThisDocument
Dim oCompDef As PartComponentDefinition
Set oCompDef = oPartDoc.ComponentDefinition
Dim oModelStates As ModelStates
Set oModelStates = oCompDef.ModelStates
‘Fetch the required Model State from the collection
Dim oModelState As ModelState
Set oModelState = oCompDef.ModelStates("Model State 1")
'Activate the model state
' Get the design tracking property set for our model state.
Dim oSummaryInfo As Inventor.PropertySet
Set oSummaryInfo = oPartDoc.PropertySets.Item("Inventor Summary Information")
' Get the Comments property.
Dim oCommentsProperty As Property
Set oCommentsProperty = oSummaryInfo.Item("Comments")
' Set the Member Edit Scope
oModelStates.MemberEditScope = kEditActiveMember 'kEditAllMembers for all members
'Set the value
oCommentsProperty.Value = "Updating comments via API!"
A couple of things to remember:
- It is recommended to edit in the Factory Document context and activate the Model State you wish to edit.
- It is not recommended to change the Model State Member Document directly. Also, the Member Document may not exist, if not already generated. Hence, your code would return a ‘Null’ in such cases, as shown below.