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Hi @jeslinakoruth. It is difficult to diagnose problems with your code without being familiar with what all the custom terms being used within it represent. Since the code is just black & white text in a code window (the way we usually like to see it) we can not tell if some of them may be blue, unquoted names of parameters, and directly recognized as representing local parameters...or just terms being used as local variables within the code, and do not actually directly represent parameters. We also do not know what types of parameters they are, or what types of values they may have. At first, working with parameters can be a bit tricky, due to the differences in units and automatic (or not) unit conversions that happen.
Is 'partOD' only a local variable, as it looks like, or is it also the exact spelling and capitalization of a parameter in the same model that the iLogic rule is saved within? Same for 'size', 'sizec', 'sizeb', 'sizet', 'zdiameter', zdiameterc' , 'zdiameterb', 'zdiametert', and so on. If any of those terms are just local variables, then they should be 'declared' (using the Dim keyword), and should have their Type specified where they are declared, such as:
Dim size As Double...if that is just a local variable, and not a blue, unquoted parameter name. Also, keep in mind that when working with blue, unquoted parameter names, or when working with the Parameter("ParamName") type iLogic snippets, the 'value' will be in 'document units' (the value specified within the Document Settings as the default length/distance unit), not necessarily in the parameter's own units (if they are different units). However, when working accessing the actual Parameter object by Inventor API code (such as what you are doing in the last 12 or so lines of code), then the value will always be in 'database units' (always centimeters for length/distance, no matter what the document units or parameter units are).
Wesley Crihfield
(Not an Autodesk Employee)
Hi @jeslinakoruth. This is just a slightly modified version of your original code. I added some additional feedback into it, and enclosed some areas of the code within a few Try...Catch...End Try statements, to help narrow down where errors are happening, and potentially avoid them. I do not know if this will actually eliminate any errors you are currently seeing, but it may help you narrow down where the error is happening or further develop your code in a way to avoid the errors.
' Prompt the user for the part OD
Dim sPartOD As String = InputBox("Enter the Part OD:", "Part OD Input", "")
If sPartOD = "" Then Return 'exit rule if no value entered
Dim dPartOD As Double
If Double.TryParse(sPartOD, dPartOD) = False Then
MsgBox("Could not convert input value to a Double!", vbCritical, "iLogic")
Return
End If
'if you expect that an error could happen, but can not avoid it
'then you can enclose the code within a Try...Catch...End Try statement
'that will 'catch / handle' the error, allowing your code to continue, if needed
'the Catch side can be used for feedback, and/or to try an alternate code
Try
' Set dimensions based on part OD
If dPartOD > 0 And dPartOD <= 2.25 Then
size = 3.5
sizec = 3.5
sizeb = 3.5
sizet = 3.5
ElseIf dPartOD > 2.25 And dPartOD <= 3.5 Then
size = 4.75
sizec = 4.75
sizeb = 4.75
sizet = 4.75
ElseIf dPartOD > 3.5 And dPartOD <= 4.5 Then
size = 6.0
sizec = 6.0
sizeb = 6.0
sizet = 6.0
ElseIf dPartOD > 4.5 And dPartOD <= 6.25 Then
size = 7.75
sizec = 7.75
sizeb = 7.75
sizet = 7.75
ElseIf dPartOD > 6.25 And dPartOD <= 8.0 Then
size = 9.75
sizec = 9.75
sizeb = 9.75
sizet = 9.75
ElseIf dPartOD > 10 And dPartOD <= 12 Then
size = 14.0
sizec = 14.0
sizeb = 14.0
sizet = 14.0
End If
Logger.Info("Checked 'PartOD' and set 'size' param value OK.")
Catch ex As Exception
MsgBox("Error while checking 'PartOD' or setting value of 'size' parameter." _
& vbCrLf & ex.Message, vbExclamation, "iLogic")
Return
End Try
'apply any changes made to local variables representing parameters
'to the model document at this point
RuleParametersOutput()
Try
' Set other dimensions based on the sizes
If size = 3.5 Then
zdiameter = 3.245
zdiameterc = 3.245
zdiameterb = 3.245
zdiametert = 3.245
maxpindiameter = 1.125
maxpindiameterc = 1.125
maxpindiameterb = 1.125
maxpindiametert = 1.125
ElseIf size = 4.75 Then
zdiameter = 4.495
zdiameterc = 4.495
zdiameterb = 4.495
zdiametert = 4.495
maxpindiameter = 1.125
maxpindiameterc = 1.125
maxpindiameterb = 1.125
maxpindiametert = 1.125
ElseIf size = 6.0 Then
zdiameter = 5.745
zdiameterc = 5.745
zdiameterb = 5.745
zdiametert = 5.745
maxpindiameter = 1.5
maxpindiameterc = 1.5
maxpindiameterb = 1.5
maxpindiametert = 1.5
ElseIf size = 7.75 Then
zdiameter = 7.495
zdiameterc = 7.495
zdiameterb = 7.495
zdiametert = 7.495
maxpindiameter = 1.75
maxpindiameterc = 1.75
maxpindiameterb = 1.75
maxpindiametert = 1.75
ElseIf size = 9.75 Then
zdiameter = 9.495
zdiameterc = 9.495
zdiameterb = 9.495
zdiametert = 9.495
maxpindiameter = 1.875
maxpindiameterc = 1.875
maxpindiameterb = 1.875
maxpindiametert = 1.875
ElseIf size = 14.0 Then
zdiameter = 13.745
zdiameterc = 13.745
zdiameterb = 13.745
zdiametert = 13.745
maxpindiameter = 2.75
maxpindiameterc = 2.75
maxpindiameterb = 2.75
maxpindiametert = 2.75
End If
Logger.Info("Checked 'size' and set value of 'zdiameter'/'maxpindiameter' params OK.")
Catch ex As Exception
MsgBox("Error checking 'size' or setting value of 'zdiameter'/'maxpindiameter'." _
& vbCrLf & ex.Message, vbExclamation, "iLogic")
Return
End Try
'apply any changes made to local variables representing parameters
'to the model document at this point
RuleParametersOutput()
'get access to the document
Dim oDoc As Inventor.Document = ThisDoc.Document
'get access to its parameters
Dim oParams As Inventor.Parameters = Nothing
If (TypeOf oDoc Is AssemblyDocument) OrElse (TypeOf oDoc Is PartDocument) Then
oParams = oDoc.ComponentDefinition.Parameters
ElseIf (TypeOf oDoc Is DrawingDocument) Then
oParams = oDoc.Parameters
End If
If oParams Is Nothing Then Return 'exit rule, parameters collection could not be obtained
'if any of these parameters are not found, it will throw an error
'if the document is ReadOnly for some reason, then trying to change parameter values will throw error
'if the file is in the Content Center or a library folder, it will act like ReadOnly
Try
oParams.Item("size").Value = size
oParams.Item("sizec").Value = sizec
oParams.Item("sizeb").Value = sizeb
oParams.Item("sizet").Value = sizet
oParams.Item("zdiameter").Value = zdiameter
oParams.Item("zdiameterc").Value = zdiameterc
oParams.Item("zdiameterb").Value = zdiameterb
oParams.Item("zdiametert").Value = zdiametert
oParams.Item("maxindiameter").Value = maxpindiameter
oParams.Item("maxpindiameterc").Value = maxpindiameterc
oParams.Item("maxpindiameterb").Value = maxpindiameterb
oParams.Item("maxpinDiametert").Value = maxpindiametert
Logger.Info("Set param values OK.")
Catch ex As Exception
MsgBox("Error setting parameter values." & vbCrLf & _
ex.Message, vbExclamation, "iLogic")
Return
End Try
Wesley Crihfield
(Not an Autodesk Employee)
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