solidworks api ch02

使用ISldWorks

open SolidWorks.Interop.sldworks

let cmdConnect (swApp: ISldWorks) =
    swApp.SendMsgToUser $"RevisionNumber:{swApp.RevisionNumber}"
    
    swApp.DisplayStatusBar true
    swApp.SendMsgToUser $"DisplayStatusBar Ok!"
    
    let lang = swApp.GetCurrentLanguage()
    swApp.SendMsgToUser $"SOLIDWORKS is currently using the {lang} language."

新建零件：

let cmdNewModel_Part (swApp: ISldWorks) =
    
    let swModel = 
        swApp.NewDocument(Path.Combine(TEMPLATEDIR, "gb_part.prtdot"), 0, 0.0, 0.0)
        |> unbox<IModelDoc2>
       
    swModel.InsertFamilyTableNew()

    swApp.SendMsgToUser "InsertFamilyTableNew"
            
    let text = "Sample Note"
    let swNote = 
        swModel.InsertNote(text)
        |> unbox<INote>
    let swAnnotation = 
        swNote.GetAnnotation()
        |> unbox<IAnnotation>

    swAnnotation.SetPosition(0.01, 0.01, 0.0）
    |> ignore

    swApp.SendMsgToUser "Note"

新建装配体

let cmdNewModel_ASM (swApp: ISldWorks) =
    
    let swModel = 
        swApp.NewDocument(Path.Combine(TEMPLATEDIR, "gb_assembly.asmdot"), 0, 0.0, 0.0)
        |> unbox<IModelDoc2>
       
    swModel.InsertFamilyTableNew()

    swApp.SendMsgToUser "InsertFamilyTableNew"
            
    let text = "Sample Note"
    let swNote = 
        swModel.InsertNote(text)
        |> unbox<INote>
    let swAnnotation = 
        swNote.GetAnnotation()
        |> unbox<IAnnotation>

    swAnnotation.SetPosition(0.01, 0.01, 0.0)
    |> ignore

    swApp.SendMsgToUser text

新建工程图：

let cmdNewModel_DRW (swApp: ISldWorks) =    
    let swModel = 
        swApp.NewDocument(Path.Combine(TEMPLATEDIR, "gb_a1.drwdot"), 0, 0.0, 0.0)
        |> unbox<IModelDoc2>
    let drawname = swModel.GetTitle()
    let partpath = @"C:\Users\cuisl\Documents\cstick.SLDPRT"
       
    let _ =
        let mutable errors = 0
        let mutable warnings = 0    
        swApp.OpenDoc6(partpath, 1, 0, "", &errors, &warnings)

    let swDrw = 
        let mutable errors = 0
        swApp.ActivateDoc3(drawname, false,int swRebuildOnActivation_e.swRebuildActiveDoc, &errors)
        |> unbox<IDrawingDoc>

    swDrw.EditSheet()

    let preparedrawingView() =
        swDrw.CreateDrawViewFromModelView3(partpath,"*Isometric", 0.1, 0.1, 0.0)
    
    let swView = preparedrawingView()

    swView.FocusLocked <- true

    swModel.Extension.SelectByID2(swView.GetName2(), "DRAWINGVIEW", 0, 0, 0, false, 0, null, int swSelectOption_e.swSelectOptionDefault)
    |> ignore

    swModel.InsertFamilyTableNew()
    swApp.SendMsgToUser "InsertFamilyTableNew"
        
    let text = "Sample Note"
    let swNote = 
        swModel.InsertNote(text)
        |> unbox<INote>
    let swAnnotation = 
        swNote.GetAnnotation()
        |> unbox<IAnnotation>
    swAnnotation.SetPosition(0.01, 0.01, 0.0)
    |> ignore

    swApp.SendMsgToUser text

步骤 23

let cmdPart_Click (swApp: ISldWorks) =    
    let swModel = 
        swApp.NewDocument(Path.Combine(TEMPLATEDIR, "gb_part.prtdot"), 0, 0.0, 0.0)
        |> unbox<IModelDoc2>

    let swPart = swModel :?> IPartDoc

    swModel.SketchManager.InsertSketch true
    let _ = swModel.SketchManager.CreateCornerRectangle(0, 0, 0, 0.1, 0.1, 0)
    let _ = swModel.FeatureManager.FeatureExtrusion2( true, false, 
        false, 0, 0, 0.1, 0.01, false, false, false, false, 
        0.01745329251994, 0.01745329251994, false, false, 
        false, false, true, true, true, 0, 0, false)
        
    swPart.EditRollback()

步骤 24

let cmdAssy_Click (swApp: ISldWorks) =   
    let mutable fileerror = 0
    let mutable filewarning = 0
    let _ =
        swApp.OpenDoc6(partpath, int swDocumentTypes_e.swDocPART, int swOpenDocOptions_e.swOpenDocOptions_Silent, "", &fileerror, &filewarning)
    
    let swModel= 
        swApp.NewDocument(Path.Combine(TEMPLATEDIR, "gb_assembly.asmdot"), 0, 0.0, 0.0)
        |> unbox<IModelDoc2>
    let swAssy = swModel :?> IAssemblyDoc
    let _ =
        swAssy.AddComponent5(partpath,int swAddComponentConfigOptions_e.swAddComponentConfigOptions_CurrentSelectedConfig, "", false, "", 0.0, 0.0, 0.0)
    ()

步骤 25

let cmdDraw_Click (swApp: ISldWorks) =   
    let swDrw = 
        swApp.NewDocument(Path.Combine(TEMPLATEDIR, "gb_a1.drwdot"), 0, 0.0, 0.0)
        |> unbox<IDrawingDoc>
    let msg =
        if swDrw.GetEditSheet() then
            "sheet"
        else "template"
    swApp.SendMsgToUser msg
    //swDrw.EditTemplate()
    //swDrw.EditSheet()
    ()

2.4 实例学习，连接到现有文件

training2_frmExistingDocs

步骤 29

let cmdConnect_Click  (swApp: ISldWorks) =
  
    //If chkOpen.Value = True Then
    let mutable fileerror = 0
    let mutable filewarning = 0
    let _ =
        swApp.OpenDoc6(partpath, int swDocumentTypes_e.swDocPART, int swOpenDocOptions_e.swOpenDocOptions_Silent, "", &fileerror, &filewarning)
          
    //If chkLoad.Value = True Then
    let mutable errors = 0
    let ImportedModelDoc = 
        swApp.LoadFile4(Path.Combine(TRAININGDIR, "cstick.igs"), "", null, &errors)
  
    //If chkNewWindow.Value = True Then
    swApp.CreateNewWindow()
    swApp.ArrangeWindows 1

步骤 33

let cmdNewModel_Click(swApp: ISldWorks) =
    let swModel = swApp.ActiveDoc |> unbox<IModelDoc2>
    let toolbars = 
        [
            swToolbar_e.swFeatureToolbar      
            swToolbar_e.swMacroToolbar        
            swToolbar_e.swMainToolbar         
            swToolbar_e.swSketchToolbar       
            swToolbar_e.swSketchToolsToolbar  
            swToolbar_e.swStandardToolbar     
            swToolbar_e.swStandardViewsToolbar
            swToolbar_e.swViewToolbar         
        ]

    toolbars
    |> Seq.iter(fun tb -> 
        swModel.SetToolbarVisibility(int tb,false)
    )
      
    let custPropMan = swModel.Extension.CustomPropertyManager("")
    let _ = custPropMan.Add3("MyInfo", int swCustomInfoType_e.swCustomInfoText, "MyData", int swCustomPropertyAddOption_e.swCustomPropertyDeleteAndAdd)
    ()

步骤 36

//注意：源零件不能只有焊件
let cmdPart_Click(swApp: ISldWorks) =
    let swModel = swApp.ActiveDoc |> unbox<IModelDoc2>
    let swPart = swModel :?> IPartDoc

    //执行之前保存原文件名
    let partname = swModel.GetTitle()


    let _ = swModel.Extension.SelectByID2("Top", "PLANE", 0, 0, 0, false, 0, null, 0)

    let mirFeat,mirModel =
        swPart.MirrorPart2(false,int swMirrorPartOptions_e.swMirrorPartOptions_ImportSolids)

    mirModel.ShowNamedView2("*Isometric", 7)
    mirModel.ViewZoomtofit2()

    swApp.ArrangeWindows 1

    // 重新选中源文件
    let swModel =
        let mutable errors = 0
        swApp.ActivateDoc3(partname, false,int swRebuildOnActivation_e.swRebuildActiveDoc, &errors)
        |> unbox<ModelDoc2>

    let _ = swModel.DeSelectByID("Top", "PLANE", 0.0, 0.0, 0.0)
    ()

整数与布尔型的转化：

System.Convert.ToBoolean(1);;
val it: bool = true

步骤 39

let cmdAssy_Click(swApp: ISldWorks) =
    let swModel = swApp.ActiveDoc |> unbox<ModelDoc2>
    let swAssy = swModel :?> AssemblyDoc

    let assyname = Path.GetFileNameWithoutExtension(swModel.GetTitle())
    
    // EditPart2 sheetmetalsample-1
    let boolstatus =
        swModel.Extension.SelectByID2(
        $"sheetmetalsample-1@{assyname}", "COMPONENT", 0, 0, 0, 
        false, 0, null, 0)

    let mutable info = 0
    let _ = swAssy.EditPart2(true, false, &info)

    // InsertCavity4 plug-1
    swModel.ClearSelection2 true

    let boolstatus =
        swModel.Extension.SelectByID2(
        $"plug-1@{assyname}", "COMPONENT", 0, 0, 0, 
        true, 0, null, 0)

    swAssy.InsertCavity4(10, 10, 10, true, 1, -1)

    // EditSuppress2 plug-1
    swAssy.EditAssembly()
    let _ =
        swModel.Extension.SelectByID2(
        "plug-1@sheetmetalsample", "COMPONENT", 0, 0, 0, 
        true, 0, null, 0)

    swModel.EditSuppress2()
    |> ignore

步骤 42

open System.Drawing

let cmdDraw_Click (swApp: ISldWorks) =
    let swModel = swApp.ActiveDoc |> unbox<ModelDoc2>
    let swDraw = swModel :?> DrawingDoc

    swModel.ClearSelection2 true
    let retval = 
        swDraw.CreateLayer2("MyRedLayer", "Red", Color.FromArgb(255, 0, 0).ToArgb(),
        int swLineStyles_e.swLineSTITCH, int swLineWeights_e .swLW_THICK, true, true)
    ()