Global update model in Ilogic before going on with rest of script

[peterd123]

I am having trouble getting this to work. 

I have VBA running in Excel that cycles through many iterations of an assembly changing the parameters in each cycle.

Simplified, on the excel side it changes the parameters, saves the file and then waits for 30 sec before repeating.

Inventor is detecting the change via a trigger (set in excel with a NOW()).  Then it should update model, and then save as dwg and obj (with name brought in from excel).

PROBLEM:

What I am realizing is that it is not saving them with the current model, but rather the model of the previous iteration.

Below is the ilogic script, with ' comments of things I have tried to no avail.  Any suggestions on how to force update before proceeding with rest of script?

trigger = ExcelTrigger

brand = GoExcel.CellValue("dimensions.xlsm", "Sheet2", "B7")
family = GoExcel.CellValue("dimensions.xlsm", "Sheet2", "B8")
full_name = GoExcel.CellValue("dimensions.xlsm", "Sheet2", "B9")
part_num = GoExcel.CellValue("dimensions.xlsm", "Sheet2", "B10")
file_name = GoExcel.CellValue("dimensions.xlsm", "INPUT", "B2")
file_directory = GoExcel.CellValue("dimensions.xlsm", "INPUT", "G2")

'RuleParametersOutput()
'InventorVb.DocumentUpdate()

Call ThisApplication.CommandManager.ControlDefinitions.Item("AppLocalUpdateCmd").Execute
Call ThisApplication.CommandManager.ControlDefinitions.Item("AppGlobalUpdateWrapperCmd").Execute
System.Threading.Thread.CurrentThread.Sleep(15000)

'iLogicVb.UpdateWhenDone = True
'iLogicVb.UpdateWhenDone = True
'ThisApplication.DocumentUpdate = True
'iLogicVb.UpdateWhenDone = True
'Parameter.UpdateAfterChange = True
'ThisApplication.ActiveDocument.Update2
'Application.Wait (Now + TimeValue("0:00:12"))
' didnt work ThisApplication.ActiveView.Update()
' didnt work ThisApplication.ActiveDocument.Rebuild
' didnt work ThisApplication.ActiveDocument.Update() 
'Save .igs in new file path
ThisDoc.Document.SaveAs(ThisDoc.Path + file_directory + file_name + ".obj", True) 
ThisDoc.Document.SaveAs(ThisDoc.Path + file_directory + file_name + ".dwg", True) 
 
GoExcel.DisplayAlerts = False

GoExcel.Close
 
'iLogicVb.UpdateWhenDone = True

[gcoombridge]

How about a rebuild-all prior to the save? This may slow things down but might force an update..

ThisDoc.Document.Rebuild()

[bradeneuropeArthur]

Dim a As Inventor.Application = ThisApplication

Dim b As Inventor.Document = a.ActiveDocument

b.Rebuild2(True)
If b.RequiresUpdate = True Then
	
b.Update2(True)
b.Save2(True)

End If

With this it should work!

Regards,

[peterd123]

I tried this out.  I notice that the output files are being created about 5 sec before the model updates.

[greggeorgi · Accepted solution]

Your thread.sleep might not be helping anything. Worst case, it is actually pausing the command manager execution.

You can try using Execute2 and/or DoEvents.

Execute2(True) might be the same as regular Execute, not sure, I only use Execute2. (Executes synchronously if true, asynchronously if false)

DoEvents will essentially pause the iLogic thread, process inventor stuff, then return. Some might say its not good practice to use it, but the way Inventor is programmed, it is basically required in certain cases. This may be your best bet after running the commands. (maybe a DoEvents after each execute)

Call ThisApplication.CommandManager.ControlDefinitions.Item("CMD").Execute2(True)
Call ThisApplication.UserInterfaceManager.DoEvents

If there is some sort of flag that can be set, you can also use DoEvents to wait for the process to definitely finish

dim flag as boolean = false

While not flag

    'check if flag should be set to true, or use an event?

    Call ThisApplication.UserInterfaceManager.DoEvents

End While

[peterd123]

Adding this after the model update and before the saves seems to have done the trick:

Call ThisApplication.UserInterfaceManager.DoEvents

Thanks!

[maxim.teleguz]

ThisApplication.ScreenUpdating = True
iLogicVb.Automation.RulesOnEventsEnabled = True
ThisApplication.SilentOperation = False
UpdateRevBlockOnSyncProp = 1
'https://knowledge.autodesk.com/support/vault-products/learn-explore/caas/CloudHelp/cloudhelp/2015/ENU/Vault/files/GUID-DFE2BDB7-4A6D-49D7-9083-18DCB20B7505-htm.html

'activecmd = ThisApplication.CommandManager
'If activecmd.ActiveCommand = activecmd.ActiveCommand Then
'MsgBox(activecmd.ActiveCommand)
'End If
SendKeys.SendWait("{ESC}")
AppActivate(ThisApplication.Caption)

On Error Resume Next
Dim selectCmd As ControlDefinition
    selectCmd = ThisApplication.CommandManager.ControlDefinitions.Item("AppContextual_CancelCmd")
    selectCmd.Execute

ThisApplication.CommandManager.ControlDefinitions.Item("VaultRevisionBlockTableNode").Execute2(False)

a = iProperties.Value("Project", "Revision Number")
iProperties.Value("Custom", "REV") = a

InventorVb.DocumentUpdate()

here is code updating the revision block. This works really well in canceling out any commands that are running first.