How To Placing Multiple Base Views at a time ???

[sguan1212]

Anyone who can help please.

Let's say I have a weldment made up of 10 parts. I would detail this weldment on sheet 1, and sheet 2 is left for placing the 10 flat patterns which will be used for laser profile cutting.

To produce flat patterns, i would have to place base view 10 times to drop part into the sheet 1 by 1. If this weldment was to consist of more than upwards of 10 parts, this process can be very repetitive and tedious. Does anyone know a way to place multiple base views at 1 time to reduce receptive work and increase productivity ?? Is there an ilogic rule that can do this ???

[bradeneuropeArthur]

You could create a sheet format. This is out of the box inventor, and no coding required!

[MechMachineMan]

@sguan1212 There are many samples and resources out there regarding similar operations.

https://forums.autodesk.com/t5/inventor-customization/ilogic-coding-to-create-automated-drawing/m-p/...

[sguan1212]

That doesn't seem to be what I want to do. I'm not trying to automate the drawings.

I just want to place multiple base views on the drawing at a time. Is there anyone that can help ?

[sguan1212]

hi Bradeneurope, 

Can you please elaborate on how exactly this is done

[MechMachineMan]

But aren't you trying to take a process (placing 10 views, 1 at a time) that is currently done manually, and have it done.... automatically?

That's what automation is.

You'll have a very hard time finding something that does the drawing completely automatically because it's a very complicated process with a lot of nuances.

[bradeneuropeArthur]

@sguan1212

I wrote this:

"You could create a sheet format. This is out of the box inventor, and no coding required!"

This seems to be working for only 1 view and not multiple, sorry for my misunderstanding..

[sguan1212]

Hi Mechmachineman,

Sorry I haven't made myself clear.

What I really want is instead of only been able select 1 component to drop into the drawing at a time, I would like to be able to select a bunch of components and drop it into the drawing  

Please see attached file for a snapshot

[MechMachineMan]

Ahhh. Makes sense. Something could be programmed to do that through an alternate dialog box. Seems like a good Idea for the IdeaStation if it's not available by the program already!

[yooko1987]

Hi,

Do we have anything that can make this though happen? I'm also looking for this type of solution that can automate placing multiple base views of opened parts.

Hope there is some good news 🙂

Best

Yang

[Anonymous]

Sorry to open this topic again, but there is no answer yet. Can somebody help? Im trying to put all frame members from the frame generator onto a sheet at once.

Thanks in advance.

[marcin_otręba]

Hi,

run it when you are in drawing:

   Dim oFileDlg As Inventor.FileDialog
   Call ThisApplication.CreateFileDialog(oFileDlg)

   Dim sInitialDirectory As String
   oFileDlg.MultiSelectEnabled = True
   oFileDlg.ShowOpen
   
   Debug.Print (oFileDlg.FileName)
   Dim files() As String = Split(oFileDlg.FileName, "|")
   MessageBox.Show(files(0), "Title")
   Dim draw As DrawingDocument = ThisDoc.Document
   For i=0 To files.Length
If files(i)<>"" Then
Dim oBaseViewOptions As NameValueMap
        oBaseViewOptions = ThisApplication.TransientObjects.CreateNameValueMap
        ' Create the placement point object.
        Dim oPoint As Point2d
        oPoint = ThisApplication.TransientGeometry.CreatePoint2d(25, 25)
Dim oModel As Document
        oModel = ThisApplication.Documents.Open(files(i),False)
        ' Create a base view.
        Dim oBaseView As DrawingView
        oBaseView = draw.ActiveSheet.DrawingViews.AddBaseView(oModel, oPoint, 2,
  ViewOrientationTypeEnum.kIsoTopLeftViewOrientation, DrawingViewStyleEnum.kHiddenLineRemovedDrawingViewStyle,
, , oBaseViewOptions)
End If
Next

[DRoam]

@sguan1212, there's a free add-in called QuickViews that I think would work great for you. The way it works is it shows a list of each assembly in your drawing. You can expand an assembly and see its sub-components, and whether or not each one has been detailed yet. If it hasn't, you can just double-click it or click "Add View' to add a view of it. The QuickViews window stays open while you do this, so after you place a view you can move straight on to the next part. It's about as streamlined as it gets. Not quite as streamlined as moving straight from one component to the next, but almost.

Here's a link to the add-in and a video demo.

Hope it helps you!

[Cris_Davis]

Has anyone found a solution to this problem?

[A.Acheson]

Hi @Cris_Davis, Message 12 by marcin_otręba  is the answer. I have tested it but it simply allows multiple files to be selected and it dumps the base view on the drawing. Have you tried this? 

[srinivasanyl]

Hi, many thanks for the code. But i want to place multiple flatpattern views at a time. Is it possible through ilogic code.

[marcin_otręba]

Hi,

Try this rule, it will allow you to click mouse where you want to place each view or it will place in the middle of active sheet.

Class thisrule
    Dim responce As MsgBoxResult
    Dim posx, posy As Double
    Dim bstillselecting As Boolean = True
	Dim oInteraction As InteractionEvents
   	Dim oMouse As MouseEvents
            
    Sub Main()
		Dim oFileDlg As Inventor.FileDialog
		Call ThisApplication.CreateFileDialog(oFileDlg)
        oFileDlg.Filter = "Inventor Files (*.ipt)|*.ipt|All Files (*.*)|*.*"
        oFileDlg.FilterIndex = 1
        Dim sInitialDirectory As String
        oFileDlg.MultiSelectEnabled = True
        oFileDlg.ShowOpen()
        Dim files() As String = Split(oFileDlg.FileName, "|")
        responce = MessageBox.Show("Do you want to choose views locations by mouse click?", "Views", MessageBoxButtons.YesNoCancel)
        If responce = vbYes Then
            oInteraction = ThisApplication.CommandManager.CreateInteractionEvents
            oMouse = oInteraction.MouseEvents
            AddHandler oMouse.OnMouseDown, AddressOf oMouse_OnMouseDown
            oInteraction.Start()
        End If
        Dim draw As DrawingDocument = ThisDoc.Document
        For i = 0 To files.Length - 1
            If files(i) <> "" Then
                bstillselecting = True
                Dim oBaseViewOptions As NameValueMap
                oBaseViewOptions = ThisApplication.TransientObjects.CreateNameValueMap
                Call oBaseViewOptions.Add("SheetMetalFoldedModel", False)
                ' Create the placement point object.
                Dim oPoint As Point2d
                If responce = vbYes Then
                    Do While bstillselecting
                        ThisApplication.UserInterfaceManager.DoEvents
                    Loop
                End If
				If responce = vbYes Then
                	oPoint = ThisApplication.TransientGeometry.CreatePoint2d(posx, posy)
				Else
					oPoint = ThisApplication.TransientGeometry.CreatePoint2d(draw.ActiveSheet.Width/2, draw.ActiveSheet.Height/2)
				End If
                Dim oModel As Document
                oModel = ThisApplication.Documents.Open(files(i), False)
                ' Create a base view.
                Dim oBaseView As DrawingView
                oBaseView = draw.ActiveSheet.DrawingViews.AddBaseView(oModel, oPoint, 1,
              ViewOrientationTypeEnum.kDefaultViewOrientation, DrawingViewStyleEnum.kHiddenLineRemovedDrawingViewStyle,
            , , oBaseViewOptions)
            End If
        Next
        oInteraction.Stop
        oInteraction = Nothing
        oMouse = Nothing
    End Sub

    Sub oMouse_OnMouseDown(Button As MouseButtonEnum, ShiftKeys As ShiftStateEnum, ModelPosition As Point, ViewPosition As Point2d, View As Inventor.View)
        posx = ModelPosition.X
        posy = ModelPosition.Y
        bstillselecting = False
    End Sub
End Class