topic Re: How to link Excel VBA with parameterization to Inventor VBA? in Inventor Forum

How to link Excel VBA with parameterization to Inventor VBA?

ThyagoVicent — Fri, 09 Jun 2023 15:48:15 GMT

Is it possible to link a parameterization made in Excel with Inventor's VBA?

I have performed parameterization of a machine in Inventor using Excel, in which when a measurement is changed in Excel, the machine adjusts its dimensions accordingly. However, I would like to implement this in VBA so that when Excel is opened, only the dimension fields that need to be changed are visible, and then the changes can be saved, the VBA closed, and the designer can open the Inventor file to see the changes in the project. Alternatively, if it is possible to incorporate this into Inventor's VBA, a VBA window could appear upon opening the project to modify the dimensions.

Thank you in advance.

Re: How to link Excel VBA with parameterization to Inventor VBA?

Crstiano — Fri, 09 Jun 2023 16:27:04 GMT

You can use the Parameters command to link with excel file.

After just use the variables where you desire.

Re: How to link Excel VBA with parameterization to Inventor VBA?

A.Acheson — Sat, 10 Jun 2023 00:25:32 GMT

Hi @ThyagoVicent

As @Crstiano suggest using the built in parameter linking with excel is one route. It can be a little inflexible depending on where your data is stored, the units etc.

Another method is using ilogic editor and ilogic API and go excel you can point to a cell and import the data.

Parameter("d5") = GoExcel.CellValue("filename.xlsx", "SheetName", "Cell")
iLogicVb.UpdateWhenDone = True

The hardest method is using inventor VBA. The reason being it uses Inventor API. Open Excel and reference excel workbook and point to a cell and import parameters.

Getting data from excel sample here.

Setting a parameter value from Inventor API Help here.

You can ask programming questions on the dedicated forum here

Re: How to link Excel VBA with parameterization to Inventor VBA?

tonythm — Mon, 12 Jun 2023 00:36:46 GMT

Hello @ThyagoVicent

I think, you should use function available in Inventor.
Or you can use below VBA code, I'm really not good at VBA but I can only write what I know.
You can create a VBA that can run multiple .*ipt updates in .*iam.

Sub CreateParam() Dim oWkbk As Workbook Set oWkbk = ThisWorkbook Dim oSheet As Worksheet Set oSheet = oWkbk.ActiveSheet Dim oCell As Range oLastRow = oSheet.Cells(oSheet.Rows.Count, 1).End(XlDirection.xlUp).Row Dim oInv As Inventor.Application Set oInv = GetObject(, "Inventor.Application") Dim oDoc As Document Set oDoc = oInv.ActiveDocument Dim partDoc As PartDocument Set partDoc = oInv.ActiveDocument Dim userParams As UserParameters Set userParams = partDoc.ComponentDefinition.Parameters.UserParameters a = "A" i = 0 For Each oCell In Range(a & i + 3, a & oLastRow) Dim param As Parameter On Error Resume Next Set param = userParams.AddByExpression(oCell, oCell.Offset(0, 1).Value, oCell.Offset(0, 2).Value) If Err.Number <> 0 Then On Error Resume Next End If Dim oUserParam As UserParameter For Each oUserParam In userParams Dim oLen As Variant oLen = Len(oUserParam.name) 'If oLen <> 5 Then 'oUserParam.Delete 'End If If oUserParam.name = oCell.Value Then oUserParam.Comment = oCell.Offset(, 3) End If Next Next oCell MsgBox "Done!" End Sub

Sub UpdateParam() Dim oWkbk As Workbook Set oWkbk = ThisWorkbook Dim oSheet As Worksheet Set oSheet = oWkbk.ActiveSheet Dim oCell As Range oLastRow = oSheet.Cells(oSheet.Rows.Count, 1).End(XlDirection.xlUp).Row Dim oInv As Inventor.Application Set oInv = GetObject(, "Inventor.Application") Dim oDoc As Document Set oDoc = oInv.ActiveDocument Dim partDoc As PartDocument Set partDoc = oInv.ActiveDocument a = "A" i = 0 For Each oCell In Range(a & i + 3, a & oLastRow) Dim userParams As UserParameters Set userParams = partDoc.ComponentDefinition.Parameters.UserParameters Dim oUserParam As UserParameter For Each oUserParam In userParams If oUserParam.name = oCell.Value Then oUserParam.Expression = oCell.Offset(0, 1).Value End If Next Next MsgBox "Done!" End Sub