macros and layers

Try these codes and use as needed

'Demonstrates how to open the layer and print windows

'Preconditions: Active file is a Drawing

 

Option Explicit

Dim swApp As SldWorks.SldWorks

Dim swModel As SldWorks.ModelDoc2

 

Sub main()

    Set swApp = Application.SldWorks

    Set swModel = swApp.ActiveDoc

 

    If (swModel Is Nothing) Then

        MsgBox " Please open a drawing document. "

        End

    End If

   

     If (swModel.GetType <> swDocDRAWING) Then

        MsgBox " Please open a drawing document. "

        End

    End If

   

    'Open SOLIDWORKS Layers Window

   swModel.Extension.RunCommand swCommands_LayerProperties, ""

 

    'Open SOLIDWORKS Print Window

    swModel.Extension.RunCommand swCommands_Print, ""

   

End Sub

Deepak's answer highlights the fact that the macro recorder can't record all actions, but that the API does have functions for most of the possibilities of SolidWorks. It seems that any sketching, modeling and drawing creation work can be recorded (albeit poorly) and any work regarding windows and screens cannot be recorded.

The macro recorder is not an effective way to create a macro in many instances, since it:

• Can't record certain actions
• Can't record logic
• Can't get user input

Other downsides:

• The resulting code is usually messy and might not use the best API calls or show you the ideal way to automate via API a certain task

In short, it isn't a tool that professional API developers like myself use very often. But in your case, I understand why you want to use it, since it gives the impression of being able to record the macro you need. The name "Macro Recorder", then is somewhat of a misnomer.

Here are some API calls that might be necessary in the macro you are looking for:

• IDrawingDoc::SetCurrentLayer
• IDrawingDoc::CreateLayer2
• IModelDocExtension::PrintOut4

The names should be self-explanatory. Needless to say, these API calls will perform the same actions you would normally do in GUI, but without the GUI. The options you set in the GUI are passed in as arguments to those API calls, roughly speaking.

If you need help writing this, please explain more thoroughly what you are trying to automate. Please see How to ask a good question in the API forum for reference.

Keith

SolidWorks API Training and Services

I came across this Sub (can't remember what post it came from on the Forum but thank you to whoever posted it!) that can be put into the standard Print and Convert tasks (though I am not sure of your final application):

Sub LayerVisibility()

    Dim Part As Object

    Dim swLayerMgr As Object

    Dim swLayer As Object

    Set swApp = CreateObject("SldWorks.Application")

    Set Part = swApp.ActiveDoc

    Set swLayerMgr = Part.GetLayerManager

    ' Selecting QC-Balloons Layer  (Layer name can be changed to whatever layer is desired)

    Set swLayer = swLayerMgr.GetLayer("QC-Balloons")

    ' Turn layer OFF (False) or ON (True)

    swLayer.Visible = False

    Set swLayer = Nothing

    Set swLayerMgr = Nothing

    Set Part = Nothing

End Sub

Paste this entire Sub into the script of the Task and call on it as needed.

For the Print Task I put it into the Open Document with an If statement - though not sure if the If this is required:

    ' Open document

    If docType = swDocNONE Then

        Set swModel = swApp.LoadFile4(docFileName, "", Nothing, errors)

    Else

        Set swDocSpecification = swApp.GetOpenDocSpec(docFileName)

        swDocSpecification.DocumentType = docType

        swDocSpecification.ReadOnly = True

        swDocSpecification.Silent = True

        swDocSpecification.ConfigurationName = ""

        swDocSpecification.DisplayState = ""

        Set swModel = swApp.OpenDoc7(swDocSpecification)

        errors = swDocSpecification.Error

        'Set swModel = swApp.OpenDoc6(docFileName, docType, swOpenDocOptions_Silent Or swOpenDocOptions_ReadOnly, "", errors, warnings)

        If docType = swDocDRAWING Then

                LayerVisibility

        End If

    End If

For the Convert Task it was a bit simpler:

    If docType = swDocDRAWING Then

        Dim vSheetNames As Variant

        Set swDrawing = swModel

        QCLayerVisibilityOn

....

Please note, Red Text is existing scripting in the Task, Green Text is what should be added.

Hope this helps!