用默认模板新建零件，并修改用户偏爱：
let newPart (swApp: ISldWorks) =
// Get the file path of the default part template
let partTemplate = swApp.GetUserPreferenceStringValue(int swUserPreferenceStringValue_e.swDefaultTemplatePart)
let swModel =
swApp.NewDocument(partTemplate, 0, 0.0, 0.0)
|> unbox<ModelDoc2>
swModel.Extension.SetUserPreferenceInteger(
int swUserPreferenceIntegerValue_e.swUnitsLinear,
int swUserPreferenceOption_e.swDetailingNoOptionSpecified,
int swLengthUnit_e.swMM)
|> ignore
swApp.SetUserPreferenceToggle(int swUserPreferenceToggle_e.swInputDimValOnCreate, false)
swModel
修改零件的材质：
let testPartMat (swModel: ModelDoc2) (swApp: ISldWorks) =
let setPartMat (mat:string) =
let swPart = swModel :?> PartDoc
/// 设置零件，当前配置，当前材料数据库
swPart.SetMaterialPropertyName2("", "", mat)
let mat1,db1 = swPart.GetMaterialPropertyName2 ""
swApp.SendMsgToUser $"{mat1},{db1}"
setPartMat "1060 Alloy"
setPartMat "Brass"
绘制草图的基本框架：
let drawSketch draw (swModel: ModelDoc2) (swApp: ISldWorks) =
swModel.SketchManager.AddToDB <- true
//PROFILE
let boolstatus = swModel.Extension.SelectByID2("Front Plane", "PLANE", 0, 0, 0, false, 0, null, 0)
swModel.SketchManager.InsertSketch false
draw swModel
swModel.SketchManager.AddToDB <- false
绘制草图实体：
let drawRect height width (swModel: ModelDoc2) =
let SketchSegmentObj = swModel.SketchManager.CreateLine(0.05, 0.05, 0, 0.05, 0.05 + height, 0.0)
//Add a dimension to the selected entity
swModel.Extension.AddDimension(0.0, 0.05 + height / 2.0, 0.0, int swSmartDimensionDirection_e.swSmartDimensionDirection_Down)
|> ignore
swModel.SketchManager.CreateLine( 0.05, 0.05 + height, 0.0, 0.05 + width, 0.05 + height, 0.0)
|> ignore
swModel.SketchManager.CreateLine( 0.05 + width, 0.05 + height, 0, 0.05 + width, 0.05, 0.0)
|> ignore
swModel.SketchManager.CreateLine( 0.05 + width, 0.05, 0, 0.05, 0.05, 0.0)
|> ignore
swModel.Extension.AddDimension( 0.05 + width / 2.0, 0.0, 0.0, int swSmartDimensionDirection_e.swSmartDimensionDirection_Down)
|> ignore
swModel.ClearSelection2 true
//Select the origin
swModel.Extension.SelectByID2( "", "EXTSKETCHPOINT", 0, 0, 0, false, 0, null, 0)
|> ignore
//Select an end point on the profile
swModel.Extension.SelectByID2( "", "SKETCHPOINT", 0.05, 0.05, 0, true, 0, null, 0)
|> ignore
//Add a vertical dimension
swModel.AddVerticalDimension2( 0, 0.025, 0)
|> ignore
swModel.ClearSelection2 true
//Select the origin
swModel.Extension.SelectByID2( "", "EXTSKETCHPOINT", 0, 0, 0, false, 0, null, 0)
|> ignore
//Select an end point on the profile
swModel.Extension.SelectByID2( "", "SKETCHPOINT", 0.05, 0.05, 0, true, 0, null, 0)
|> ignore
//Add a horizontal dimension
//to fully constrain the sketch
swModel.AddHorizontalDimension2( 0.025, 0, 0)
|> ignore
swModel.ClearSelection2 true
//Select a profile edge
SketchSegmentObj.Select4( false, null)
|> ignore
//Create the offset sketch profile from the selected edge
//and its chain of sketch entities
swModel.SketchManager.SketchOffset2(0.002, false, true,
int swSkOffsetCapEndType_e.swSkOffsetArcCaps, int swSkOffsetMakeConstructionType_e.swSkOffsetDontMakeConstruction,
false)
|> ignore
画圆：
let drawCircle (radius:float) (swModel: ModelDoc2) =
swModel.SketchManager.CreateCircleByRadius(0.05 + radius, 0.05 + radius, 0, radius)
|> ignore
swModel.SketchManager.SketchOffset2(0.002, false, true,
int swSkOffsetCapEndType_e.swSkOffsetArcCaps, int swSkOffsetMakeConstructionType_e.swSkOffsetDontMakeConstruction,
false)
|> ignore
拉伸特征：
let featureExtrusion (depth:float) (swModel: ModelDoc2) =
swModel.FeatureManager.FeatureExtrusion2( true, false, true, 0, 0, depth, 0, false, false, false, false, 0, 0,
false, false, false, false, false, false, false,
int swStartConditions_e.swStartSketchPlane, 0.0, false)
|> ignore
旋转特征：
let featureRevolve (angle) (swModel: ModelDoc2) (swApp: ISldWorks) =
let Angle = angle * Math.PI / 180.0
let swFeatMgr = swModel.FeatureManager
swFeatMgr.FeatureRevolve2( true, true, false, false, false, false,
int swEndConditions_e.swEndCondBlind, int swEndConditions_e.swEndCondBlind, Angle, 0.0, false, false, 0.0, 0.0,
int swThinWallType_e.swThinWallOneDirection, 0.0, 0.0, true, false, true)
|> ignore
基于草图的特征运行：
let testRectExtrusionUsingSketch (swApp: ISldWorks) =
let swModel = newPart swApp
drawSketch (drawRect 0.2 0.1) swModel swApp
featureExtrusion 0.3 swModel
let testCircleExtrusionUsingSketch (swApp: ISldWorks) =
let swModel = newPart swApp
drawSketch (drawCircle 0.2) swModel swApp
featureExtrusion 0.3 swModel
let testRectRevolveUsingSketch (swApp: ISldWorks) =
let swModel = newPart swApp
let draw (swModel) =
drawRect 0.2 0.1 swModel
//if Revolve was chosen, an axis of revolution is needed
swModel.SketchManager.CreateCenterLine (0, 0, 0, 0, 0.05, 0)
|> ignore
drawSketch draw swModel swApp
featureRevolve 90 swModel swApp
let testCircleRevolveUsingSketch (swApp: ISldWorks) =
let swModel = newPart swApp
let draw (swModel) =
drawCircle 0.2 swModel
//if Revolve was chosen, an axis of revolution is needed
swModel.SketchManager.CreateCenterLine (0, 0, 0, 0, 0.05, 0)
|> ignore
drawSketch draw swModel swApp
featureRevolve 90 swModel swApp
选择草图实体作为轮廓：
let procContourSelection select (swModel: ModelDoc2) (swApp: ISldWorks) =
let smgr = swModel.SelectionManager:?>SelectionMgr
smgr.EnableContourSelection <- true
select swModel swApp
smgr.EnableContourSelection <- false
let rectContour1 width (swModel: ModelDoc2) (swApp: ISldWorks) =
swModel.Extension.SelectByID2("", "SKETCHCONTOUR", 0.05, 0.05 + width / 2.0, 0, true, 0, null, 0)
|> ignore
let rectContour2 width (swModel: ModelDoc2) (swApp: ISldWorks) =
swModel.Extension.SelectByID2("", "SKETCHCONTOUR", 0.05 - 0.002, 0.05 + width / 2.0, 0, true, 0, null, 0)
|> ignore
let circleContour1 (radius:float) (swModel: ModelDoc2) (swApp: ISldWorks) =
swModel.Extension.SelectByID2( "", "SKETCHCONTOUR", 0.05 + radius, 0.05, 0, true, 0, null, 0)
|> ignore
let circleContour2 (radius:float) (swModel: ModelDoc2) (swApp: ISldWorks) =
swModel.Extension.SelectByID2( "", "SKETCHCONTOUR", 0.05 - 0.002, 0.05 + radius, 0, true, 0, null, 0)
|> ignore
用草图轮廓生成特征：
let testRectContourExtrusion (swApp: ISldWorks) =
let swModel = newPart swApp
drawSketch (drawRect 0.2 0.1) swModel swApp
procContourSelection (rectContour1 0.1) swModel swApp
procContourSelection (rectContour2 0.1) swModel swApp
featureExtrusion 0.3 swModel
let testCircleContourExtrusion (swApp: ISldWorks) =
let swModel = newPart swApp
drawSketch (drawCircle 0.1) swModel swApp
let contour swModel swApp =
circleContour1 0.1 swModel swApp
circleContour2 0.1 swModel swApp
procContourSelection contour swModel swApp
featureExtrusion 0.3 swModel
let testRectContourRevolve (swApp: ISldWorks) =
let swModel = newPart swApp
let draw (swModel) =
drawRect 0.2 0.1 swModel
//if Revolve was chosen, an axis of revolution is needed
swModel.SketchManager.CreateCenterLine (0, 0, 0, 0, 0.05, 0)
|> ignore
drawSketch draw swModel swApp
let contour swModel swApp =
rectContour1 0.1 swModel swApp
rectContour2 0.1 swModel swApp
procContourSelection contour swModel swApp
featureRevolve 90 swModel swApp
let testCircleContourRevolve (swApp: ISldWorks) =
let swModel = newPart swApp
let draw (swModel) =
drawCircle 0.1 swModel
//if Revolve was chosen, an axis of revolution is needed
swModel.SketchManager.CreateCenterLine (0, 0, 0, 0, 0.05, 0)
|> ignore
drawSketch draw swModel swApp
let contour swModel swApp =
circleContour2 0.1 swModel swApp
circleContour1 0.1 swModel swApp
procContourSelection contour swModel swApp
featureRevolve 90 swModel swApp
