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IF or then in BOM

Question asked by Marc Plensou on Mar 9, 2018
Latest reply on Mar 12, 2018 by Marc Plensou

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Hello

I would like to insert a column in my BOM, that would tell me whether my weldments are cut at an angle in one end, the other end or both ends, by inserting

a symbol that would look like I=/ or perhaps something else. The symbol is to tell the projectmanager, that they need to look at the drawing before ordering materials.

I have been trying out some IF OR equations with the custom properties angle1 and angle2, but I am at a loss. The angles are show in the drawings, but the BOM is also what we order materials from.

Any ideas?

This is what I have in mind.

Elmar Klammer Mar 9, 2018 9:32 AM

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Hi Marc,

Insert a BOM with indented cutlist shown. Select to show Angle 1 & Angle 2 in two columns. SW has it's own format for if statements that refer to custom properties or column headers. Look up equations, bom in the help file. You should be able to check if your angles are unequal to empty. That should work.

Simply hide the angle columns after.

You need a little patience. The SW Bom is awful to work with. The good news is after you have spent 2 hours to write a 10 second excel-like equations you can save out the template and start forgetting about the obnoxious experience you just went through.

No way around it, until SW coders themselves have to work with it and say "the hell with this, after a mere 2 seconds"

Elmar

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Deepak Gupta Mar 9, 2018 4:48 AM
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You can get the cut list properties to show in the BOM and can show the angle values for both side. And based on that, the person ordering the material can verify the required length.
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- Marc Plensou @ Deepak Gupta on Mar 9, 2018 5:04 AM
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  I am aware of that, but I don't want to show the angle values on the BOM. Just a column that would tell the person ordering materials, whether the weldment is cut at an angle or not with a symbol of a kind. This column is like a note that says "This weldment is cut at an angle, look at the drawing before ordering".
  
  What I am talking about might be an equation like this: IF("ANGLE1>0 OR "ANGLE2">0)THEN "insert symbol or maybe text".
  This equation obviously doesn't work, but it's an example of what I would like to do.
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  - Elmar Klammer @ Marc Plensou on Mar 9, 2018 9:32 AM
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    Hi Marc,
    
    Insert a BOM with indented cutlist shown. Select to show Angle 1 & Angle 2 in two columns. SW has it's own format for if statements that refer to custom properties or column headers. Look up equations, bom in the help file. You should be able to check if your angles are unequal to empty. That should work.
    Simply hide the angle columns after.
    
    You need a little patience. The SW Bom is awful to work with. The good news is after you have spent 2 hours to write a 10 second excel-like equations you can save out the template and start forgetting about the obnoxious experience you just went through.
    
    No way around it, until SW coders themselves have to work with it and say "the hell with this, after a mere 2 seconds"
    
    Elmar
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    - Marc Plensou @ Elmar Klammer on Mar 12, 2018 5:13 AM
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      Hello Elmar,
      
      I tried a simple angle1 + angle2 equation and then hid both columns, I still got the result, so that works fine.
      The equation I am after looks like this in Excel: =IF((OR(A2>0;B2>0));"Yes";"No").
      
      The help file shows a good example: IF(`Description`<>"";`Description`;"-")
      I tried writing mine based on the example, it seemed to work: IF(`ANGLE1`>0"Yes";"") so every row, where ANGLE1 is bigger than 0 says Yes, the rest are blank. Now I just need to incorporate ANGLE2 in the same equation.
      
      Still working on it.
      
      Edit:
      Got it, I think: IF('ANGLE1'>0;"Yes";IF('ANGLE2'>0;"Yes";""))
      
      I agree, the BOM is very limited and it should be at least as good as Excel.
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      - Elmar Klammer @ Marc Plensou on Mar 12, 2018 5:17 AM
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        Hi Marc,
        
        You are already there. Use the column where you add angle1 and angle2. If that is 0 then you have a straight cut on both ends. If that is > zero then you have an angled cut. That gives you a simple if statement. It is best to keep equations real simple. If statements can give different results depending on your sequential order of your check condition.
        Your approach works too and gives the added bonus if you want to indicate bevels on one or two ends. In structural we sometimes indicate B2E or B1E.
        
        Elmar
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        Marc Plensou @ Elmar Klammer on Mar 12, 2018 6:58 AM
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        Hello Elmar,
        
        I think it works.
        IF('ANGLE1'>0;"Yes";IF('ANGLE2'>0;"Yes";"")) Works well with weldments.
        
        It doesn't work with extrudes etc. I usually model beams and columns as weldments, but plates as extrudet sketches.
        Extrudes don't have any custom properties. Would there be any way to give them any?
        I know about the bounding boxes, but they won't let me alter the description and they don't have any angles even if they are cut in an angle.
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        Elmar Klammer @ Marc Plensou on Mar 12, 2018 7:42 AM
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        Courtesy Matt Martens
        
        '-----------------------------------------------------------------
        ' Creates the 3D bounding box around all items in the cut-list feature of a weldment.
        '
        ' Written By Matt Martens 9/19/13
        '
        ' Preconditions: The active document is a part file.
        '
        ' Postconditions: -Creates the SW 3D bounding box sketch for all cut-list folders. .
        '                   -If a cut-list feature is not found, will prompt the user before inserting
        '                    a weldment feature and then reruns.
        '                   -Any cut-list items that were created by extrude features and have the default
        '                    "PLATE, SW-Thickness x SW-Width x SW-Length" description will have the description
        '                    changed to be "SW-Thickness x SW-Width Bar Stock" and a "Length" property will be
        '                    added to all cut-list items with the value being "SW-Length"
        '------------------------------------------------------------------
        Dim swApp As SldWorks.SldWorks
        Dim swPart As SldWorks.ModelDoc2
        Function createBoundingBox() As Boolean
        Dim swPartExt As SldWorks.ModelDocExtension
        Dim swFeat As SldWorks.Feature
        Dim swSubFeat As SldWorks.Feature
        Dim boxCount As Integer
        Dim cutListDesc As String
        Set swPartExt = swPart.Extension
        'loop through all features and update the cut list feature and create
        'SW 3D bounding boxes for all cut-list folders
        boxCount = 0
        Set swFeat = swPart.FeatureByName("Solid Bodies")
        swFeat.GetSpecificFeature2.UpdateCutList
        Set swFeat = swFeat.GetFirstSubFeature
        While Not swFeat Is Nothing
        boxCount = boxCount + 1
        
        'check for existing bounding and skip if present
        Set swSubFeat = swFeat.GetFirstSubFeature
        Do While Not swSubFeat Is Nothing
            Debug.Print swSubFeat.GetTypeName2
            'If swSubFeat.GetTypeName2 = "3DProfileFeature" Then GoTo nextFeature
            Set swSubFeat = swSubFeat.GetNextSubFeature
        Loop
        
        'add 3D bounding box and alter cutlist properties to cut list folders
        swFeat.Select2 False, Empty
        swPartExt.Create3DBoundingBox
        Stop
        swFeat.CustomPropertyManager.Get4 "Description", True, cutListDesc, 0
        If UCase(Left(cutListDesc, 5)) = "PLATE" Then
            'Alter the system created description of non-weldment created bodies
            cutListDesc = Replace(cutListDesc, "Plate", "PL")
        
        '    cutListDesc = Left(cutListDesc, Len(cutListDesc) - 11) & "Bar Stock"
            swFeat.CustomPropertyManager.Add3 "Description", swCustomInfoText, cutListDesc, swCustomPropertyDeleteAndAdd
        End If
        'add length property as "SW-Length"
        swFeat.CustomPropertyManager.Add3 "Length", swCustomInfoText, "SW-Length", swCustomPropertyDeleteAndAdd
        nextFeature:
        Set swFeat = swFeat.GetNextSubFeature
        Wend
        'drop contents of objects
        Set swPartExt = Nothing
        Set swFeat = Nothing
        Set cutList = Nothing
        'set function to true if any bounding boxes were created
        If boxCount = 0 Then createBoundingBox = False: Exit Function
        
        createBoundingBox = True
        End Function
        Sub main()
        'Set the application and open document
        Set swApp = Application.SldWorks
        Set swPart = swApp.ActiveDoc
        'check for an open document
        If swPart Is Nothing Then
        swApp.SendMsgToUser2 "Please open a part file and try again.", swMbInformation, swMbOk
        Exit Sub
        End If
        'check if the open document is a part file
        If Not swPart.GextType = 1 Then
        swApp.SendMsgToUser2 "This command only works in .sldprt files.", swMbInformation, swMbOk
        Exit Sub
        End If
        'send message prompt if no bounding boxes were created
        If Not createBoundingBox Then
        'prompt user for creation of weldment feature and rerun subroutine if yes is selected
        If swApp.SendMsgToUser2("There is no weldment feature in this model." & Chr(13) & _
                                  "Would you like to insert one and continue?", _
                                  swMbQuestion, swMbYesNoCancel) = 6 Then
            swPart.FeatureManager.InsertWeldmentFeature
            createBoundingBox
        End If
        End If
        'Drop contents of all objects
        swPart.ClearSelection2 True
        Set swApp = Nothing
        Set swPart = Nothing
        End Sub
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        Marc Plensou @ Elmar Klammer on Mar 12, 2018 9:11 AM
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        That was something.
        I don't even know where to begin
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        Elmar Klammer @ Marc Plensou on Mar 12, 2018 9:15 AM
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        I am sure Matt Martens won't mind a thank you...
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        Marc Plensou @ Elmar Klammer on Mar 12, 2018 9:21 AM
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        I mean, I don't even how or where to use any of it
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IF or then in BOM

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