SETTING STOCK NUMBER VALUE BASED ON PARAMETERS

[Keith.Challinor3761]

The code below allows me to insert an ipt and set the parameters during insert, all works well 

in the code there is a portion to set the stock number based on the parameters , for some reason it sets the stock No to the ipt's original values not the ones stated during insert 

can some one assist please as i need it to use the values set during insert   



Dim oAsm As AssemblyDocument = ThisDoc.Document 
Dim oPath As String = ThisDoc.Path 
If oPath = "" 
	MessageBox.Show("Message", "Title", MessageBoxButtons.OK)
End If
Dim oCode As String = InputBox ("Code:W,S,OM,EX,", "Code","?") 
Dim oThickness As String = InputBox("Thickness:", "Thickness", "2") 
Dim oDia As String = InputBox("Diameter 80 - 400:", "Duct Diameter", "ENTER")  
Dim oLength As String = InputBox("Length:", "Length 500,1000,2000", "2000") 
Dim oFlange As String = InputBox("Flange:", "Flange", "6mm LIP")
If System.IO.File.Exists(oPath & "\"& " Ø"& oDia & " Straight Duct" & " x " & oLength & "mm x " & oThickness & " Thick, " & oFlange & ".ipt") Then
	ThisApplication.CommandManager.PostPrivateEvent(PrivateEventTypeEnum.kFileNameEvent, oPath & "\"& " Ø"& oDia & " Straight Duct" & " x " & oLength & "mm x " & oThickness & " Thick, " & oFlange & ".ipt") 
	ThisApplication.CommandManager.ControlDefinitions.Item("AssemblyPlaceComponentCmd").Execute 
Else 
	Dim oTemplate As String = "J:\Inventor Library\Ducting\JKF_DUCT.ipt" 
	Dim pDoc As PartDocument = ThisApplication.Documents.Add(DocumentTypeEnum.kPartDocumentObject, oTemplate, False)  
	pDoc.ComponentDefinition.Parameters.Item("DIA").Expression = oDia
	pDoc.ComponentDefinition.Parameters.Item("Length").Expression = oLength
	pDoc.ComponentDefinition.Parameters.Item("Thickness").Expression = oThickness 
	pDoc.Update 
	ThisApplication.UserInterfaceManager.DoEvents 
	iProperties.Value("Project", "Stock Number")= ("oCode" &"/"& "oDIA" & "/" &"oLength")
	pDoc.SaveAs(oPath & "\" & " Ø"& oDia & " Straight Duct" & " x " & oLength & "mm x " & oThickness & " Thick, " & oFlange & ".ipt", False) 
	pDoc.Close 
	ThisApplication.CommandManager.PostPrivateEvent(PrivateEventTypeEnum.kFileNameEvent,oPath & "\"& " Ø"& oDia & " Straight Duct" & " x " & oLength & "mm x " & oThickness & " Thick, " & oFlange & ".ipt")
    ThisApplication.CommandManager.ControlDefinitions.Item("AssemblyPlaceComponentCmd").Execute 
End If 
oAsm.Update 

[WCrihfield]

Are you wanting that "Stock Number" property's value to be based on your InputBox values directly, or are you trying to get it to contain live references to custom iProperties, which are linked to 'exposed' Parameters?

The location of your 'DoEvents' line doesn't seem right.  It seems that line should be right after each of the PostPrivateEvent lines.  Maybe try changing that around, and see if it fixes anything.  Which scenario is it happening in, the preexisting part file, or the 'new' part file?

[Ralf_Krieg]

Hello

Why do you set all of the input variables in double quotes?

iProperties.Value("Project", "Stock Number")= ("oCode" &"/"& "oDIA" & "/" &"oLength")

 The result should be the String "oCode/oDIA/oLength" which is surely not what you want. Could you try instead

iProperties.Value("Project", "Stock Number")= oCode & "/" & oDIA & "/" & oLength

[Keith.Challinor3761]

Thanks for the reply 

i have tried what has been suggested by all but to little  success

the part created in the assembly refuses to have the stock number set to the parameter values stated during its creation 

when i have got it to work it will update the dia and length but not the code the code stays set to what was stated in the original template ipt 

still open to suggestions before i through it all in the bin 😉

[Ralf_Krieg]

Hello

In addition to the hint I gave you above, in the same line the command did not write the iProperty to your part, but to the assembly the part is placed in.

iProperties.Value("Project", "Stock Number")= ("oCode" &"/"& "oDIA" & "/" &"oLength")

Please try

Dim oAsm As AssemblyDocument = ThisDoc.Document 
Dim oPath As String = ThisDoc.Path 
If oPath = "" 
	MessageBox.Show("Message", "Title", MessageBoxButtons.OK)
End If
Dim oCode As String = InputBox ("Code:W,S,OM,EX,", "Code","?") 
Dim oThickness As String = InputBox("Thickness:", "Thickness", "2") 
Dim oDia As String = InputBox("Diameter 80 - 400:", "Duct Diameter", "ENTER")  
Dim oLength As String = InputBox("Length:", "Length 500,1000,2000", "2000") 
Dim oFlange As String = InputBox("Flange:", "Flange", "6mm LIP")
If System.IO.File.Exists(oPath & "\" & " Ø" & oDia & " Straight Duct" & " x " & oLength & "mm x " & oThickness & " Thick, " & oFlange & ".ipt") Then
	ThisApplication.CommandManager.PostPrivateEvent(PrivateEventTypeEnum.kFileNameEvent, oPath & "\"& " Ø"& oDia & " Straight Duct" & " x " & oLength & "mm x " & oThickness & " Thick, " & oFlange & ".ipt") 
	ThisApplication.CommandManager.ControlDefinitions.Item("AssemblyPlaceComponentCmd").Execute 
Else 
	Dim oTemplate As String = "J:\Inventor Library\Ducting\JKF_DUCT.ipt" 
	Dim pDoc As PartDocument = ThisApplication.Documents.Add(DocumentTypeEnum.kPartDocumentObject, oTemplate, False)  
	pDoc.ComponentDefinition.Parameters.Item("DIA").Expression = oDia
	pDoc.ComponentDefinition.Parameters.Item("Length").Expression = oLength
	pDoc.ComponentDefinition.Parameters.Item("Thickness").Expression = oThickness 
	pDoc.Update 
	pDoc.PropertySets("{32853F0F-3444-11D1-9E93-0060B03C1CA6}").Item("Stock Number").Value  = (oCode & "/" & oDia & "/" & oLength)
	pDoc.SaveAs(oPath & "\" & " Ø"& oDia & " Straight Duct" & " x " & oLength & "mm x " & oThickness & " Thick, " & oFlange & ".ipt", False) 
	pDoc.Close 
	ThisApplication.CommandManager.PostPrivateEvent(PrivateEventTypeEnum.kFileNameEvent,oPath & "\"& " Ø"& oDia & " Straight Duct" & " x " & oLength & "mm x " & oThickness & " Thick, " & oFlange & ".ipt")
    ThisApplication.CommandManager.ControlDefinitions.Item("AssemblyPlaceComponentCmd").Execute 
End If 
oAsm.Update 

[WCrihfield · Accepted solution]

I got thinking about this later while I was working on something else, and the thought came up that the iProperties.Value() call may not be working for you, because that part that you just created 'invisibly' may not be the 'active' document at that moment, and that call works with the 'active' document.  So you would have to write that iProperty to that part using the longer route.  So I revisited this post with this update, and moved a couple other things around too.  Here's what I came up with.  See if this works any better.

Dim oAsm As AssemblyDocument = ThisDoc.Document
Dim oPath As String = ThisDoc.Path 
If oPath = "" 
	MsgBox("The 'Path' of the assembly is empty. Exiting.", , "")
	Exit Sub
End If

Dim oCode As String = InputBox ("Code:W,S,OM,EX,", "Code","?") 
Dim oThickness As String = InputBox("Thickness:", "Thickness", "2") 
Dim oDia As String = InputBox("Diameter 80 - 400:", "Duct Diameter", "ENTER")  
Dim oLength As String = InputBox("Length:", "Length 500,1000,2000", "2000") 
Dim oFlange As String = InputBox("Flange:", "Flange", "6mm LIP")
Dim oFName As String = oPath & "\" & " Ø"& oDia & " Straight Duct" & " x " & oLength & "mm x " & oThickness & " Thick, " & oFlange & ".ipt"

Dim oCM As CommandManager = ThisApplication.CommandManager

If Not System.IO.File.Exists(oFName) Then
	Dim oTemplate As String = "J:\Inventor Library\Ducting\JKF_DUCT.ipt" 
	Dim pDoc As PartDocument = ThisApplication.Documents.Add(DocumentTypeEnum.kPartDocumentObject, oTemplate, False)
	Dim oParams As Parameters = pDoc.ComponentDefinition.Parameters
	oParams.Item("DIA").Expression = oDia
	oParams.Item("Length").Expression = oLength
	oParams.Item("Thickness").Expression = oThickness 
	pDoc.Update
	'since you created the Part invisibly, it might not be the 'active' document, and the iProperties.Value() call acts on the 'active' document
	'so we'll set this parts iProperty this way, instead, to be sure
	pDoc.PropertySets.Item("Design Tracking Properties").Item("Stock Number").Value = oCode & "/" & oDia & "/" & oLength
	pDoc.SaveAs(oFName, False) 
	pDoc.Close 
End If 
oCM.PostPrivateEvent(PrivateEventTypeEnum.kFileNameEvent, oFName)
ThisApplication.UserInterfaceManager.DoEvents
oCM.ControlDefinitions.Item("AssemblyPlaceComponentCmd").Execute 
oAsm.Update

Oops. Looks like we were both working on this at the same time and @Ralf_Krieg posted something similar first.

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[Keith.Challinor3761]

Krieg

I appreciate the efforts unfortunately the latest didn't work , the Ø value and the length updated and were entered into the stock number but the code fails to update the letter stays as stated in the template IPT

[Keith.Challinor3761]

WCrihfield
Sorry to report this doesn't work either , I truly appreciate all the efforts being put into this but am beginning to feel it isn't possible ( deep down the must be a way )
Is it because the code is text ?
As the numeric inputs for dia and length work OK
Keith

[WCrihfield]

Well, setting a parameters 'Expression' definitely works differently than setting its 'Value', but can sometimes be more stable that way.  When setting the expression (as a simple value, not an equation), it is understood as literal, and doesn't attempt to convert its units, but when you set the value of a numeric parameter with a simple numeric value, it will by default get converted (understood as 'database' units), which causes a lot of folks problems.

[Ralf_Krieg · Accepted solution]

Hello

You're right, the text parameter needs extra quotes. I forgot, sorry. Edit the line to

pDoc.ComponentDefinition.Parameters.Item("Code").Expression = Chr(34) & oCode & Chr(34)