Ascending numbering in the component from 1-300

[infoXFJXM]

I need 300 sheets with ascending numbering in the component from 1-300.
Is there a possibility that Inventor 2023 will be able to generate the components automatically?

Via macro or iLogic?

I am an absolute layman in this field

[tdant]

Stuff like this is very doable in Inventor through a few different channels. If you're able to provide the part file, I can work something up and talk you through how I did it.

[C_Haines_ENG]

Do you mean that it would create a new part? This code will do that. You enter what number you'd like to start at, and what number you'd like to end at. You can try and use it in the attached part file.

Sub Main

	Dim oDoc As PartDocument = ThisDoc.Document

	Dim oPath As String = ThisDoc.Path & "\"

	Dim oEmboss As EmbossFeature = oDoc.ComponentDefinition.Features.EmbossFeatures(1)

	Dim oStart As Integer = Int(InputBox("Enter Starting #", "Plate Duplicator", "1"))
	If oStart < 1 Then Exit Sub
		
	Dim oEnd As Integer = Int(InputBox("Enter End #", "Plate Duplicator", "2"))
	If oEnd < 2 Then Exit Sub

	Dim oSketch As Sketch = oEmboss.Profile.Parent
	Dim oTextBox As Inventor.TextBox = oSketch.TextBoxes(1)
	Dim oFontSize As Double = Split(Split(oTextBox.FormattedText, "'>")(0), "<StyleOverride FontSize='")(1)

	For i = oStart To oEnd

		Dim oText As String = i & "-"
		oTextBox.FormattedText = "<StyleOverride FontSize = '" & oFontSize & "'>" & oText & "</StyleOverride>"
		oDoc.Update
		
		Dim oDocName As String = "PLATE #" & i
		oDoc.SaveAs(oPath & oDocName & ".ipt", True)
		Logger.Info("Ran Once!")

	Next

End Sub

[J-Camper · Accepted solution]

Depending on what you want to do with these parts, you might not even need iLogic.  ModelStates might be able to do what you want pretty quickly:

[infoXFJXM]

Thank you for the help. It worked very well. If you know how to do it, it's really easy.
Can you help me how I can convert the individual model states to DXF files?

[J-Camper]

Are looking for an export of the cut face as a 2D sketch?  Or do you need a 3D Object in AutoCAD?

[infoXFJXM]

That's right. I need the component as a 2D sketch for further processing.

[J-Camper · Accepted solution]

Create a Sketch on the same plane as the first one and project the cut geometry.  Name the sketch "ExportThisSketch" and run this rule:

Dim pDoc As PartDocument = TryCast(ThisApplication.ActiveDocument, PartDocument)
If pDoc Is Nothing Then Logger.Debug("Not Run In Part Document") : Exit Sub

If pDoc.FullFileName Is Nothing Then MessageBox.Show("Please save this file before running rule.")

Dim ExportSketch As PlanarSketch
Try
	ExportSketch = TryCast(pDoc.ComponentDefinition.Sketches.Item("ExportThisSketch"), PlanarSketch)
Catch
	MessageBox.Show("Please Create a 2D sketch that you want to export and name it: ""ExportThisSketch"".")
	Exit Sub
End Try

Dim DXFfilename As String 

Dim sysPath As System.IO.Path
DXFfilename = sysPath.GetDirectoryName(pDoc.FullFileName)
DXFfilename = sysPath.Combine(DXFfilename, sysPath.GetFileNameWithoutExtension(pDoc.FullFileName) & "_DXF_Exports")

If Not System.IO.Directory.Exists(DXFfilename) Then System.IO.Directory.CreateDirectory(DXFfilename)

Dim AllModelStates As ModelStates = pDoc.ComponentDefinition.ModelStates
For Each ms As ModelState In AllModelStates
	If ms.Name = String.Empty Then Continue For
	If ms IsNot AllModelStates.ActiveModelState Then ms.Activate

	Call ExportSketch.DataIO.WriteDataToFile("DXF", System.IO.Path.Combine(DXFfilename, ms.Name & ".dxf"))
Next

Here is an example of me setting it up:

You should end up with a folder in the same location as your part file with all the exported sketches.  It may take a while for all 300.

Let me know if you have any questions, or run into any issues.

[infoXFJXM]

The rule works, but the numbers are not displayed correctly. saving the individual disks as DXF works, but unfortunately not with the rule. I have uploaded the components and a picture of the plate 179.
Alternatively, you could also store the individual model states in a DWG and then save them. 
Or is that not possible?

[bradeneuropeArthur]

Actually there is no code needed. 

You can use Inventor I-part features to do this.

See attachment

[J-Camper · Accepted solution]

It looks like you chose to project the face instead of choosing the "Project Cut Edges" option.  This led to bad updates as the face geometry changes.  Please remake the sketch using an origin plan and the "Project Cut Edges" option:

[infoXFJXM]

Now everything has worked out. Thank you for the help and support.