ilogic parameter help

[dclunie]

Hi

I am after help to change some code that was supplied by Curtis Waguespack that adds description to all parts with a certain type of material,(ie finds all material that is plywood and adds a description formula to the parts within an assembly)

what i am after is a input box to change all part thicknesses of all parts that are found to new user value

User value that we use to hold thickness values in all .ipts is G_T

1. find all .ipts within an assembly
2. input to ask user thickness
3. change all .ipt parameters ("G_L") that control thickness to newly inputted value

below is code used to alter descriptions on all .ipts found with material = to (plywood)

''kUnknownDocumentObject = 12289

'kPartDocumentObject = 12290

'kAssemblyDocumentObject = 12291

'kDrawingDocumentObject = 12292

'kPresentationDocumentObject = 12293

'kDesignElementDocumentObject = 12294

'kForeignModelDocumentObject = 12295

'kSATFileDocumentObject = 12296

'kNoDocument = 12297

Dim openDoc As Document

openDoc = ThisDoc.Document

Dim mywidth As Integer

Dim docFile As Document

If openDoc.DocumentType = 12291 Then

      For Each docFile In openDoc.AllReferencedDocuments

            If docFile.DocumentType = 12290 Then

            Dim FNamePos As Long

                  FNamePos = InStrRev(docFile.FullFileName, "\", -1)   

                  Dim docFName As String

                  docFName = Right(docFile.FullFileName, Len(docFile.FullFileName) - FNamePos)                    

                  'select for part files with specified material

                  If iProperties.Material(docFName) = "PLYWOOD"  Then

                  'set description

                  iProperties.Value(docFName, "Project", "Description")= "=<Material> <G_L>"

                  iProperties.Value(docFName, "Project", "Part Number")  = Left(docFName, InStrRev(docFName, ".") - 1)

                  End If

            End If

      Next

      Else

      MessageBox.Show("You must have a valid Assembly document open before using this code!", "File Type Mismatch!")

End If

[Curtis_Waguespack · Accepted solution]

Hi dclunie, 

Here is some code that will set the Thickness parameter (if it is present) in each part file. You can use it as an example to modify your code.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Dim openDoc As Document
openDoc = ThisDoc.Document
Dim docFile As Document

'get input from user
myThickness = InputBox("Enter Thickness", "iLogic", "0.75")

'look at all of the parts in the assembly
For Each docFile In openDoc.AllReferencedDocuments
If docFile.DocumentType = 12290 Then
'get the part file names
Dim FNamePos As Long
FNamePos = InStrRev(docFile.FullFileName, "\", -1)   
Dim docFName As String
docFName = Right(docFile.FullFileName, Len(docFile.FullFileName) - FNamePos)                    
'select for part files with specified material
if iProperties.Material(docFName) = "PLYWOOD"  Then
'set description
iProperties.Value(docFName, "Project", "Description")= "=<Material> <G_L>"
iProperties.Value(docFName, "Project", "Part Number")  = Left(docFName, InStrRev(docFName, ".") - 1)
'ignore error if parameter is not in the part
Parameter.Quiet=True
'set parameter value
Parameter(docFName, "Thickness") = myThickness
End If
End If
Next

iLogicVb.UpdateWhenDone = True

[dclunie]

HI Curtis

Excellent piece of work you just saved me hours of manual work

Many Thanks

Dave

[Rich.O.3d]

I was under the impression that cc / ifeatures used, for eg:

100x10 Flat Bar x 500 Lg

would have:

G_W = 100

G_H = 10

G_L = 500

I was planning on using these parram names for ease of coord with existing Inventor Nomenclature

If im mistaken could you enlighten me a bit further on what parts of inventor use what parrams

Cheers