Weld Configurations

[Arrush80_]

I have created a saddle which I control using excel for dimensions and several features that I control using a ilogic form. Depending on the load that saddle needs to support I need to adjust the number of ribs and their placement. 

Where I run into problems is with welds. I have found no way to supress a weld along with a part and from what I've read this can not be done. So my question is, what is the best approach? I do not want to recreate or have to delete weld features every time I remove or add a rib.

The only thing I can think of is to create a new assembly for each configuration of the saddle but that seems a little counter productive.

Any suggestions would be welcome.

[adam.nagy]

HI,

Do you know how to achieve what you want through the UI?

If so, then could you list the steps you do in the UI and now you want to automate?

If you do not know how to do this in the UI, then it would be worth asking in the Product Forum as well.

Cheers,

[Arrush80_]

Hi Adam

I can definetly do the work using the UI but the weld beads do not show up in the ilogic browser. If you look at the images below, I am trying to go from a single to a double rib configuration and I have that working easily with ilogic by supressing components but as I can not supress the welds using ilogic the weld bead will fail as soon as I change the configuration.

[adam.nagy · Accepted solution]

Thanks for the pictures, Arek.

It did not error out for me when I suppressed a part that had a welding - but still, I guess you would not want a welding hanging in the air.

This is the workaround I could come up with. I hope this helps.

http://adndevblog.typepad.com/manufacturing/2014/04/run-command-on-browser-item.html

Cheers,

[Arrush80_]

Adam,

This looks exactly like the sort of automation I am looking for. Unfortunately the code is a little over my current skill set. Would you be able to look at the attached assembly and perhaps plug in one weld to suppress and un-suppress using your ilogic script? I am currently changing the number of rib using an ilogic form from 1 to 5 but if you were able to do a single one it would help me out immensely. 

[adam.nagy]

Hi Arek,

A few files are missing, which makes it more difficult to test things. Could you provide those?

00-SEED-000000.xlsx, 00-SEED-000057.ipt, 00-SEED-000058.ipt.

Also, you don't seem to have welding added for all the plates.

You could name the weld beads the same as the part they belong to, that should make the code a bit clearer.

Cheers,

[Arrush80_]

My apologies I was trying to keep the file size down. I've added the welds for the single and double gusset configurations.

[adam.nagy]

Hi Arek,

I've done it for Ribs 1 and 2 - you should be able to set it up for the rest:

Sub Main
'Select number of ribs
If RIBS = "1" Then
Component.IsActive("Gusset Plate 1") = True
Component.IsActive("Gusset Plate 2") = False
Component.IsActive("Gusset Plate 2 Mirror") = False
Component.IsActive("Gusset Plate 3") = False
Component.IsActive("Gusset Plate 3 Mirror") = False
SuppressWeldBeads( _
  New List(Of String)(New String(){"Gusset Plate 2-A", "Gusset Plate 2-B", "Gusset Plate 2-C"}), _
  New List(Of String)(New String(){"Gusset Plate 1-A", "Gusset Plate 1-B", "Gusset Plate 1-C"}))
RIBS_ADJUSTMENT = False
Else If RIBS = "2" Then
Component.IsActive("Gusset Plate 1") = False
Component.IsActive("Gusset Plate 2") = True
Component.IsActive("Gusset Plate 2 Mirror") = True
Component.IsActive("Gusset Plate 3") = False
Component.IsActive("Gusset Plate 3 Mirror") = False
SuppressWeldBeads( _
  New List(Of String)(New String(){"Gusset Plate 1-A", "Gusset Plate 1-B", "Gusset Plate 1-C"}), _
  New List(Of String)(New String(){"Gusset Plate 2-A", "Gusset Plate 2-B", "Gusset Plate 2-C"}))
RIBS_ADJUSTMENT = False
Else If RIBS = "3" Then
Component.IsActive("Gusset Plate 1") = True
Component.IsActive("Gusset Plate 2") = True
Component.IsActive("Gusset Plate 2 Mirror") = True
Component.IsActive("Gusset Plate 3") = False
Component.IsActive("Gusset Plate 3 Mirror") = False
RIBS_ADJUSTMENT = False
Else If RIBS = "4" Then
Component.IsActive("Gusset Plate 1") = False
Component.IsActive("Gusset Plate 2") = True
Component.IsActive("Gusset Plate 2 Mirror") = True
Component.IsActive("Gusset Plate 3") = True
Component.IsActive("Gusset Plate 3 Mirror") = True
RIBS_ADJUSTMENT = True
Else If RIBS = "5" Then
Component.IsActive("Gusset Plate 1") = True
Component.IsActive("Gusset Plate 2") = True
Component.IsActive("Gusset Plate 2 Mirror") = True
Component.IsActive("Gusset Plate 3") = True
Component.IsActive("Gusset Plate 3 Mirror") = True
RIBS_ADJUSTMENT = True
End If

'Sets rib thickness
Parameter("Gusset Plate 1", "RIB_THK") = RIB_THK
Parameter("Gusset Plate 2", "RIB_THK") = RIB_THK
Parameter("Gusset Plate 3", "RIB_THK") = RIB_THK
End Sub

Sub SuppressBead( _
  wcd As WeldmentComponentDefinition, _
  wbn As BrowserNode, _
  unsuppress As Boolean)
  Dim name As String
  name = wbn.BrowserNodeDefinition.Label

  ' If the bead is already suppressed then its BeadFaces will be 0
  If (wcd.Welds.WeldBeads(name).BeadFaces.count = 0) <> unsuppress Then Exit Sub
  
  ' Get the CommandManager object
  Dim cm As CommandManager
  cm = ThisApplication.CommandManager
  
  ' Get the collection of control definitions
  Dim cds As ControlDefinitions
  cds = cm.ControlDefinitions
      
  ' Run the "Suppress" command
  ThisApplication.SilentOperation = True
  Call wbn.DoSelect
  'MsgBox(name)
  Call cds("AssemblySuppressFeatureCtxCmd").Execute2(True)
  ThisApplication.SilentOperation = False
End Sub

' weldNamesS - to suppress
' weldNamesU - to unsuppress
Sub SuppressWeldBeads(weldNamesS As List(Of String), weldNamesU As List(Of String))
  ' Get document
  Dim doc As AssemblyDocument
  doc = ThisApplication.ActiveDocument
  
  Dim wcd As WeldmentComponentDefinition
  wcd = doc.ComponentDefinition
  
  ' Get "Model" browser
  Dim bp As BrowserPane
  bp = doc.BrowserPanes("AmBrowserArrangement")
  
  ' Get "Welds" node
  Dim wbn As BrowserNode
  For Each wbn In bp.TopNode.BrowserNodes
    If wbn.BrowserNodeDefinition.Label = "Welds" Then
      Exit For
    End If
  Next
  
  ' Get "Beads" node
  Dim bbn As BrowserNode
  For Each bbn In wbn.BrowserNodes
    If bbn.BrowserNodeDefinition.Label = "Beads" Then
      Exit For
    End If
  Next
  
  ' Get the Beads we want to suppress/unsuppress
  For Each wbn In bbn.BrowserNodes
    If weldNamesS.Contains(wbn.BrowserNodeDefinition.Label) Then
      Call SuppressBead(wcd, wbn, False)
	ElseIf weldNamesU.Contains(wbn.BrowserNodeDefinition.Label) Then
      Call SuppressBead(wcd, wbn, True)
    End If
  Next
End Sub

Attached is the modified assembly.

Cheers,

[Arrush80_]

Adam thank you very much for your help, could not have done this without your help!

[mlkuselan]

Sorry for posting the same question once again. Since i did not received any reply on this question.

Iam posting the same question in this subject.

The following code works and suppress the weldbead when it is placed in module and run from module

BUT WHEN WE PLACE THE SAME CODE IN USERFORM AND RUN IT THE WELDBEAD GETS SELECTED BUT IT IS NOT GETTING SUPPRESSED I DON'T KNOW WHY

Please give some suggestion on this.

Enum SuppressOption
    kSuppress
    kUnsuppress
    kToggle
End Enum

Private Sub SuppressWeldBeads_Click()
    
    Call SuppressWeldBead("Fillet Weld 1")

End Sub

Sub SuppressBead(wcd As WeldmentComponentDefinition, wbn As BrowserNode, _
                    so As SuppressOption)
    Dim name As String
    name = wbn.BrowserNodeDefinition.Label
    'We only need to check the current state of the bead if
    'We are not just toggling its state but want a specific one
    If so <> kToggle Then
        'If the bead is already suppressed then its
        'BeadFaces.Count will be 0
        Dim bfs As Faces
        Set bfs = wcd.Welds.WeldBeads(name).BeadFaces
        If bfs.Count = 0 Xor so = kUnsuppress Then Exit Sub
    End If
    'Get the commandManager object
    Dim cm As CommandManager
    Set cm = ThisApplication.CommandManager
    'Get the collection of control definitions
    Dim cds As ControlDefinitions
    Set cds = cm.ControlDefinitions
    
    'Run the "Suppress" command
    ThisApplication.SilentOperation = True
    
    Call wbn.DoSelect
    Dim oSuppControlDef As ControlDefinition
    Set oSuppControlDef = ThisApplication.CommandManager.ControlDefinitions.Item("AssemblySuppressFeatureCtxCmd")
    oSuppControlDef.Execute2 (True)
    'Call cds("AssemblySuppressFeatureCtxCmd").Execute
    ThisApplication.SilentOperation = False
End Sub

Sub SuppressWeldBead(WeldName As String)
    'MsgBox (WeldName)
    'Dim WeldName As String
    'WeldName = "Fillet Weld 1"
    
    'Get Document
    Dim doc As AssemblyDocument
    Set doc = ThisApplication.ActiveDocument
    
    Dim wcd As WeldmentComponentDefinition
    Set wcd = doc.ComponentDefinition
    
    'Get "Model" browser
    Dim bp As BrowserPane
    Set bp = doc.BrowserPanes("AmBrowserArrangement")
    
    'Get "Welds" node
    Dim wbn As BrowserNode
    For Each wbn In bp.TopNode.BrowserNodes
        If wbn.BrowserNodeDefinition.Label = "Welds" Then
            Exit For
        End If
    Next
    
    'Get "Beads" node
    Dim bbn As BrowserNode
    For Each bbn In wbn.BrowserNodes
        If bbn.BrowserNodeDefinition.Label = "Beads" Then
            Exit For
        End If
    Next
    
    'Get the Beads we want to suppress
    For Each wbn In bbn.BrowserNodes
    
        If wbn.BrowserNodeDefinition.Label = WeldName Then
        
            Call SuppressBead(wcd, wbn, kSuppress)
        End If
    Next
End Sub

Thanks in Advance

M.L.Kuselan

[adam.nagy]

I answered on the other thread:

http://forums.autodesk.com/t5/inventor-customization/weld-bead-suppress-not-working-when-called-from...

[SitandGo]

First, many thanks for the code.

It is possible to suppress the welds in a sub assembly? Because i start severals configuration in the top level assembly.

Sub Main
If Drum_Tube_Divided= True Then

Component.Visible("Drum tube") = False
Component.Visible("Drum tube L1") = True
Component.Visible("Drum tube L2") = True

SuppressWeldBeads( _
  New List(Of String)(New String(){"Groove Weld undivided", "Fillet Weld undivided"}), _
  New List(Of String)(New String(){"Groove Weld divided L1", "Groove Weld divided L2", "Fillet Weld divided"}))

Else If Drum_Tube_Divided= False Then
Component.Visible("Drum tube") = True
Component.Visible("Drum tube L1") = False
Component.Visible("Drum tube L2") = False

SuppressWeldBeads( _
  New List(Of String)(New String(){"Groove Weld divided L1", "Groove Weld divided L2", "Fillet Weld divided"}), _
  New List(Of String)(New String(){"Groove Weld undivided", "Fillet Weld undivided"}))
  
End If


End Sub
Sub SuppressBead( _
  wcd As WeldmentComponentDefinition, _
  wbn As BrowserNode, _
  unsuppress As Boolean)
  Dim name As String
  name = wbn.BrowserNodeDefinition.Label

  ' If the bead is already suppressed then its BeadFaces will be 0
  If (wcd.Welds.WeldBeads(name).BeadFaces.count = 0) <> unsuppress Then Exit Sub
  
  ' Get the CommandManager object
  Dim cm As CommandManager
  cm = ThisApplication.CommandManager
'  
  ' Get the collection of control definitions
  Dim cds As ControlDefinitions
  cds = cm.ControlDefinitions
      
  ' Run the "Suppress" command
  ThisApplication.SilentOperation = True
  Call wbn.DoSelect
  'MsgBox(name)
  Call cds("AssemblySuppressFeatureCtxCmd").Execute2(True)
  ThisApplication.SilentOperation = False
End Sub

' weldNamesS - to suppress
' weldNamesU - to unsuppress
Sub SuppressWeldBeads(weldNamesS As List(Of String), weldNamesU As List(Of String))
  ' Get document
  Dim doc As AssemblyDocument
   doc = ThisApplication.ActiveEditDocument
'  doc = ThisApplication.ActiveDocument
  
  Dim wcd As WeldmentComponentDefinition
  wcd = doc.ComponentDefinition
  
  ' Get "Model" browser
  Dim bp As BrowserPane
  bp = doc.BrowserPanes("AmBrowserArrangement")
  
  ' Get "Welds" node
  Dim wbn As BrowserNode
  For Each wbn In bp.TopNode.BrowserNodes
    If wbn.BrowserNodeDefinition.Label = "Welds" Then
      Exit For
    End If
  Next
  
  ' Get "Beads" node
  Dim bbn As BrowserNode
  For Each bbn In wbn.BrowserNodes
    If bbn.BrowserNodeDefinition.Label = "Beads" Then
      Exit For
    End If
  Next
  
  ' Get the Beads we want to suppress/unsuppress
  For Each wbn In bbn.BrowserNodes
    If weldNamesS.Contains(wbn.BrowserNodeDefinition.Label) Then
      Call SuppressBead(wcd, wbn, False)
	ElseIf weldNamesU.Contains(wbn.BrowserNodeDefinition.Label) Then
      Call SuppressBead(wcd, wbn, True)
    End If
  Next
End Sub