Sketcher Workbench/ja

はじめに
スケッチャーワークベンチはパートデザインワークベンチやその他のワークベンチで使用するための2次元形状を作成するために使われます. ほとんどのCADモデルでは2次元形状が開始点となることが普通です・・まず簡単な2次元スケッチを'押し出して'3次元形状を作り、その形状の表面に穴を開けるための2次元スケッチを追加したり、スケッチで'突起'（押し出し形状）を定義したりします. スケッチャーはブーリアン演算と並んで3次元形状デザイン作成の中核を成す機能なのです.

スケッチャーワークベンチの特徴はなんといっても拘束です・・これによって2次元形状を厳密な幾何定義に従って拘束することが可能です. また拘束用ソルバーによって2次元形状の拘束範囲を計算したり、スケッチの自由度を対話的に検査したりすることが可能です.



スケッチ拘束の基本
スケッチャーがどのように動作するか説明するには"従来"の製図方法と比較するとわかりやすいでしょう.

従来の製図
"従来"のCAD製図方法は過去の製図板を用いた方法を受け継いでいます. （2次元）正射影図を手書きすることで製図（いわゆる青写真）を作成します. 物体は意図したサイズ、寸法に合わせて正確に描画されます. もし点(0, 0)から伸びる100mmの水平線を描きたければまずラインツールを選択し、画面をクリックするか座標(0, 0)と入力して始点を設定した後、終点をクリックするか座標を(100,0)を入力します. あるいは位置を気にせずに線を描き、後から位置を調整します. 形状を描き終わったらそれらに寸法を追加します.

拘束スケッチ
スケッチャーの方法は全く異なります. 物体を厳密に描く必要はありません. なぜなら物体は後で拘束をかけることによって定義されるからです. 物体はおおまかに描けばよく、拘束をかける前であれば変更も可能です. 実際の所、物体は"流動的"で動かしたり、伸ばしたり、回転させたり、拡大縮小させたりといったことが可能です. これによってデザイン作業がとても柔軟なものになります.

拘束とは何なのか？
拘束は物体の自由度を制限するために使用されます. 例えばラインは拘束がない場合は4つの自由度を持ちます. つまり水平方向、垂直方向への移動と拡大縮小と回転が可能です.

水平拘束、垂直拘束、あるいは（他のラインか座標軸の一つに対する）角度拘束を適用すると回転が制限され自由度は3つに減ります. 片方の短点を原点に対してロックすることでさらに2つの自由度が減ります. 最後にサイズ拘束を適用すれば最後の自由度が無くなります. こうしてラインは完全拘束状態になります.

複数のオブジェクトがある場合は相互に拘束が可能です. 二本のラインがあった場合、点一致拘束を使用することでそれぞれの端点をつなぎ合わせることができます. また二本のラインの間の角度を設定したり、二本のラインが垂直になるよう設定することも可能です. ラインに対しては円弧や円の接線となるように拘束することもできます.

拘束には二種類あります. 幾何拘束と寸法拘束です. これらについては下の'ツール'セクションで詳しく説明します.

スケッチャーに向かないもの
スケッチャーは2次元図面を作成するためのものではありません. ソリッド形状を作成するとスケッチは自動的に非表示になります. 寸法はスケッチ編集モード時のみ表示されます.

もし印刷用の2次元表示を作成するだけで3次元モデルが必要ないのであれば製図ワークベンチをチェックしてください（製図ワークベンチでも2次元形状が作れることを記憶に留めておいてください. 今のところスケッチャーでは使用できない機能、例えばB-スプラインなどを使うこともできます）.

Sketching Workflow
スケッチは常に2次元（2D）です. ソリッドを作成するには、囲まれた1つの領域の2Dスケッチを作成し、次にPaddedまたはRevolvedで3次元を追加して、2Dスケッチから3Dソリッドを作成します.

スケッチが互いに交差する線分、Pointが線分上に直接ない場所、または隣接する線分の端点間にギャップがある場所では、PadまたはRevolveはソリッドを作成しません. この規則の例外は、それがConstruction（blue）Geometryには適用されないことです.

囲まれた領域の内側に、重ならない小さな領域を含めることができます. 3Dソリッドを作成すると、これらは無効になります.

Once a Sketch is fully constrained, the Sketch features will turn green; Construction Geometry will remain blue. It is usually "finished" at this point and suitable for use in creating a 3D solid. However, once the Sketch dialog is closed it may be worthwhile going to Part Workbench and running  to ensure there are no features in the Sketch which may cause later problems.

ツール
スケッチャーワークベンチのツールはスケッチャーワークベンチをロードすると表示されるSketcherメニューに配置されています.

General

 * [[Image:Sketcher_NewSketch.svg‎‎|32px]] New sketch: Creates‎ a new sketch on a selected face or plane. If no face is selected while this tool is executed the user is prompted to select a plane from a pop-up window.


 * [[Image:Sketcher_EditSketch.svg|32px]] Edit sketch: Edit the selected Sketch. This will open the Sketcher Dialog.


 * [[Image:Sketcher_LeaveSketch.svg|32px]] Leave sketch: Leave the Sketch editing mode.


 * [[Image:Sketcher_ViewSketch.svg|32px]] View sketch: Sets the model view perpendicular to the sketch plane.


 * [[Image:Sketcher_ViewSection.svg|32px]] View section: Creates a section plane that temporarily hides any matter in front of the sketch plane.


 * [[Image:Sketcher_MapSketch.svg|32px]] Map sketch to face: Maps a sketch to the previously selected face of a solid.


 * Sketcher_ReorientSketch.svg Reorient sketch: Allows you to attach the sketch to one of the main planes.


 * Sketcher_ValidateSketch.svg Validate sketch: Verify the tolerance of different points and adjust them.


 * [[Image:Sketcher_MergeSketches.svg|32px]] Merge sketches: Merge two or more sketches.


 * [[Image:Sketcher_MirrorSketch.svg|32px]] Mirror sketch: Mirror a sketch along the x-axis, the y-axis or the origin.


 * Sketcher_StopOperation.svg Stop operation: When in edit mode, stop the current operation, whether that is drawing, setting constraints, etc.

Sketcher geometries
These are tools for creating objects.


 * [[Image:Sketcher_CreatePoint.svg|32px]] Point: Draws a point.


 * [[Image:Sketcher_CreateLine.svg|32px]] Line: Draws a line segment between 2 points. Lines are infinite regarding certain constraints.


 * [[Image:Sketcher_CompCreateArc.png|48px]] Create an arc: This is an icon menu in the Sketcher toolbar that holds the following commands:


 * [[Image:Sketcher_CreateArc.svg|32px]] Arc: Draws an arc segment from center, radius, start angle and end angle.


 * [[Image:Sketcher_Create3PointArc.svg|32px]] Arc by 3 points: Draws an arc segment from two endpoints and another point on the circumference.


 * [[Image:Sketcher_CompCreateCircle.png|48px]] Create a circle: This is an icon menu in the Sketcher toolbar that holds the following commands:


 * [[Image:Sketcher_CreateCircle.svg|32px]] Circle: Draws a circle from center and radius.


 * [[Image:Sketcher_Create3PointCircle.svg|32px]] Circle by 3 points: Draws a circle from three points on the circumference.


 * [[Image:Sketcher_CompCreateConic.png|48px]] Create a conic: The sketcher provides the following conical sections. Unlike B-splines they can be used with all sorts of constraints such as Tangent, Point On Object, or Perpendicular.
 * [[Image:Sketcher_CreateEllipseByCenter.svg|32px]] Ellipse by center: Draws an ellipse by center point, major radius point and minor radius point.
 * [[Image:Sketcher_CreateEllipseBy3Points.svg|32px]] Ellipse by 3 points: Draws an ellipse by major diameter (2 points) and minor radius point.
 * [[Image:Sketcher_CreateArcOfEllipse.svg|32px]] Arc of ellipse: Draws an arc of ellipse by center point, major radius point, starting point and ending point.
 * [[Image:Sketcher_CreateArcOfHyperbola.svg|32px]] Arc of hyperbola: Draws an arc of hyperbola.
 * [[Image:Sketcher_CreateArcOfParabola.svg|32px]] Arc of parabola: Draws an arc of parabola.


 * [[Image:Sketcher_CompCreateBSpline.png|48px]] Create a B-spline: This is an icon menu in the Sketcher toolbar that holds the following commands:
 * Sketcher_CreateBSpline.svg Create B-spline: Draws a B-spline curve by its control points.
 * Sketcher_CreatePeriodicBSpline.svg Create periodic B-spline: Draws a periodic (closed) B-spline curve by its control points.


 * [[Image:Sketcher_CreatePolyline.svg|32px]] Polyline (multiple-point line): Draws a line made of multiple line segments. Pressing the key while drawing a Polyline toggles between the different polyline modes.


 * [[Image:Sketcher_CompCreateRectangles.png|48px]] Create rectangles: This is an icon menu in the Sketcher toolbar that holds the following commands:


 * [[Image:Sketcher_CreateRectangle.svg|32px]] Rectangle: Draws a rectangle from 2 opposite points.


 * [[Image:Sketcher_CreateRectangle_Center.svg|32px]] Centered Rectangle: Draws a rectangle from a central point and an edge point.


 * [[Image:Sketcher_CreateOblong.svg|32px]] Rounded Rectangle: Draws a rounded rectangle from 2 opposite points.


 * [[Image:Sketcher_CompCreateRegularPolygon.png|48px]] Create regular polygon: This is an icon menu in the Sketcher toolbar that holds the following commands:


 * [[Image:Sketcher_CreateTriangle.svg|32px]] Triangle: Draws a regular triangle inscribed in a construction geometry circle.


 * [[Image:Sketcher_CreateSquare.svg|32px]] Square: Draws a regular square inscribed in a construction geometry circle.


 * [[Image:Sketcher_CreatePentagon.svg|32px]] Pentagon: Draws a regular pentagon inscribed in a construction geometry circle.


 * [[Image:Sketcher_CreateHexagon.svg|32px]] Hexagon: Draws a regular hexagon inscribed in a construction geometry circle.


 * [[Image:Sketcher_CreateHeptagon.svg|32px]] Heptagon: Draws a regular heptagon inscribed in a construction geometry circle.


 * [[Image:Sketcher_CreateOctagon.svg|32px]] Octagon: Draws a regular octagon inscribed in a construction geometry circle.


 * [[Image:Sketcher_CreateRegularPolygon.svg|32px]] Create Regular Polygon : Draws a regular polygon by selecting the number of sides and picking two points: the center and one corner.


 * [[Image:Sketcher_CreateSlot.svg|32px]] Slot: Draws an oval by selecting the center of one semicircle and an endpoint of the other semicircle.


 * [[Image:Sketcher_CreateFillet.svg|32px]] Fillet: Makes a fillet between two lines joined at one point. Select both lines or click on the corner point, then activate the tool.


 * [[Image:Sketcher_Trimming.svg|32px]] Trimming: Trims a line, circle or arc with respect to the clicked point.


 * Sketcher_Extend.svg Extend: Extends a line or an arc to a boundary line, arc, ellipse, arc of ellipse or a point in space.


 * [[Image:Sketcher_Split.svg|32px]] Split: Splits a line or an arc into two, converts a circle into an arc while keeping most of the constraints.


 * [[Image:Sketcher_External.svg|32px]] External Geometry: Creates an edge linked to external geometry.


 * Sketcher_CarbonCopy.svg CarbonCopy: Copies the geometry of another sketch.


 * Sketcher_ToggleConstruction.svg Construction Mode: Toggles sketch geometry from/to construction mode. Construction geometry is shown in blue and is discarded outside of Sketch editing mode.

Sketcher constraints
Constraints are used to define lengths, set rules between sketch elements, and to lock the sketch along the vertical and horizontal axes. Some constraints require use of Helper constraints.

Geometric constraints
These constraints are not associated with numeric data.


 * Sketcher_ConstrainCoincident.svg Coincident: Affixes a point onto (coincident with) one or more other points.


 * Sketcher_ConstrainPointOnObject.svg Point On Object: Affixes a point onto another object such as a line, arc, or axis.


 * Sketcher_ConstrainVertical.svg Vertical: Constrains the selected lines or polyline elements to a true vertical orientation. More than one object can be selected before applying this constraint.


 * Sketcher_ConstrainHorizontal.svg Horizontal: Constrains the selected lines or polyline elements to a true horizontal orientation. More than one object can be selected before applying this constraint.


 * Sketcher_ConstrainParallel.svg Parallel: Constrains two or more lines parallel to one another.


 * Sketcher_ConstrainPerpendicular.svg Perpendicular: Constrains two lines perpendicular to one another, or constrains a line perpendicular to an arc endpoint.


 * Sketcher_ConstrainTangent.svg Tangent: Creates a tangent constraint between two selected entities, or a co-linear constraint between two line segments. A line segment does not have to lie directly on an arc or circle to be constrained tangent to that arc or circle.


 * Sketcher_ConstrainEqual.svg Equal: Constrains two selected entities equal to one another. If used on circles or arcs their radii will be set equal.


 * Sketcher_ConstrainSymmetric.svg Symmetric: Constrains two points symmetrically about a line, or constrains the first two selected points symmetrically about a third selected point.


 * [[Image:Sketcher_ConstrainBlock.svg|32px]] Block: it blocks an edge from moving, that is, it prevents its vertices from changing their current positions. It should be particularly useful to fix the position of B-Splines. See the Block Constraint forum topic.

Dimensional constraints
These are constraints associated with numeric data, for which you can use the expressions. The data may be taken from a spreadsheet.


 * Sketcher_ConstrainLock.svg Lock: Constrains the selected item by setting vertical and horizontal distances relative to the origin, thereby locking the location of that item. These constraint distances can be edited later.


 * Sketcher_ConstrainDistanceX.svg Horizontal distance: Fixes the horizontal distance between two points or line endpoints. If only one item is selected, the distance is set to the origin.


 * Sketcher_ConstrainDistanceY.svg Vertical distance: Fixes the vertical distance between 2 points or line endpoints. If only one item is selected, the distance is set to the origin.


 * Sketcher_ConstrainDistance.svg Distance: Defines the distance of a selected line by constraining its length, or defines the distance between two points by constraining the distance between them.


 * Sketcher_ConstrainRadius.svg Radius: Defines the radius of a selected arc or circle by constraining the radius.
 * Sketcher_ConstrainDiameter.svg Diameter: Defines the diameter of a selected arc or circle by constraining the diameter.
 * Sketcher_ConstrainRadiam.svg Radiam: Automatically defines radius/diameter of a selected arc or circle (weight for a B-spline pole, diameter for a complete circle, radius for an arc)
 * Sketcher_ConstrainAngle.svg Angle: Defines the internal angle between two selected lines.

Special constraints

 * Sketcher_ConstrainSnellsLaw.svg Snell's Law: Constrains two lines to obey a refraction law to simulate the light going through an interface.


 * Sketcher_ConstrainInternalAlignment.svg Internal alignment: Aligns selected elements to selected shape (e.g. a line to become major axis of an ellipse).

Constraint tools
The following tools can be used the change the effect of constraints:


 * Sketcher_ToggleDrivingConstraint.svg Toggle driving/reference constraint: Toggles the toolbar or the selected constraints to/from reference mode.


 * Sketcher_ToggleActiveConstraint.svg Activate/Deactivate constraint: Enable or disable an already placed constraint.

Sketcher tools

 * Sketcher_SelectElementsWithDoFs.svg Select solver DOFs: Highlights in green the geometry with degrees of freedom (DOFs), i.e. not fully constrained.


 * Sketcher_CloseShape.svg Close Shape: Creates a closed shape by applying coincident constraints to endpoints.


 * Sketcher_ConnectLines.svg Connect Edges: Connect sketcher elements by applying coincident constraints to endpoints.


 * Sketcher_SelectConstraints.svg Select Constraints: Selects the constraints of a sketcher element.


 * Sketcher_SelectElementsAssociatedWithConstraints.svg Select Elements Associated with constraints: Select sketcher elements associated with constraints.


 * Sketcher_SelectRedundantConstraints.svg Select Redundant Constraints: Selects redundant constraints of a sketch.


 * Sketcher_SelectConflictingConstraints.svg Select Conflicting Constraints: Selects conflicting constraints of a sketch.


 * Sketcher_RestoreInternalAlignmentGeometry.svg Show/Hide internal geometry: Recreates missing/deletes unneeded internal geometry of a selected ellipse, arc of ellipse/hyperbola/parabola or B-spline.


 * Sketcher_SelectOrigin.svg Select Origin: Selects the origin of a sketch.


 * Sketcher_SelectVerticalAxis.svg Select Vertical Axis: Selects the vertical axis of a sketch.


 * Sketcher_SelectHorizontalAxis.svg Select Horizontal Axis: Selects the horizontal axis of a sketch.


 * Sketcher_Symmetry.svg Symmetry: Copies a sketcher element symmetrical to a chosen line.


 * Sketcher_Clone.svg Clone: Clones a sketcher element.


 * Sketcher_Copy.svg Copy: Copies a sketcher element.


 * Sketcher_Move.svg Move: Moves the selected geometry taking as reference the last selected point.


 * Sketcher_RectangularArray.svg Rectangular Array: Creates an array of selected sketcher elements.


 * Sketcher_RemoveAxesAlignment.svg Remove Axes Alignment: Remove axes alignment while trying to preserve the constraint relationship of the selection.


 * Sketcher_DeleteAllGeometry.svg Delete All Geometry: Deletes all geometry from the sketch.


 * Sketcher_DeleteAllConstraints.svg Delete All Constraints: Deletes all constraints from the sketch.

Sketcher B-spline tools

 * Sketcher_BSplineDegree.svg Show/hide B-spline degree


 * Sketcher_BSplinePolygon.svg Show/hide B-spline control polygon


 * Sketcher_BSplineComb.svg Show/hide B-spline curvature comb


 * Sketcher_BSplineKnotMultiplicity.svg Show/hide B-spline knot multiplicity


 * Sketcher_BSplinePoleWeight.svg Show/hide B-spline control point weight,


 * Sketcher_BSplineApproximate.svg Convert geometry to B-spline


 * Sketcher_BSplineIncreaseDegree.svg Increase B-spline degree


 * Sketcher_BSplineDecreaseDegree.svg Decrease B-spline degree,


 * Sketcher_BSplineIncreaseKnotMultiplicity.svg Increase knot multiplicity


 * Sketcher_BSplineDecreaseKnotMultiplicity.svg Decrease knot multiplicity

Sketcher virtual space

 * Sketcher_SwitchVirtualSpace.svg Switch Virtual Space: Allows you to hide all constraints of a sketch and make them visible again.

Preferences

 * [[Image:Preferences-general.svg|32px]] Preferences: Preferences for the Sketcher workbench.

Best Practices
Every CAD user develops his own way of working over time, but there are some useful general principles to follow.


 * A series of simple sketches is easier to manage than a single complex one. For example, a first sketch can be created for the base 3D feature (either a pad or a revolve), while a second one can contain holes or cutouts (pockets). Some details can be left out, to be realized later on as 3D features. You can choose to avoid fillets in your sketch if there are too many, and add them as a 3D feature.
 * Always create a closed profile, or your sketch won't produce a solid, but rather a set of open faces. If you don't want some of the objects to be included in the solid creation, turn them to construction elements with the Construction Mode tool.
 * Use the auto constraints feature to limit the number of constraints you'll have to add manually.
 * As a general rule, apply geometric constraints first, then dimensional constraints, and lock your sketch last. But remember: rules are made to be broken. If you're having trouble manipulating your sketch, it may be useful to constrain a few objects first before completing your profile.
 * If possible, center your sketch to the origin (0,0) with the lock constraint. If your sketch is not symmetric, locate one of its points to the origin, or choose nice round numbers for the lock distances. In v0.12, external constraints (constraining the sketch to existing 3D geometry like edges or to other sketches) are not implemented. This means that to locate following sketches geometry to your first sketch, you'll need to set distances relative to your first sketch manually. A lock constraint of (25,75) from the origin is more easily remembered than (23.47,73.02).
 * If you have the possibility to choose between the Length constraint and the Horizontal or Vertical Distance constraints, prefer the latter. Horizontal and Vertical Distance constraints are computationally cheaper.
 * In general, the best constraints to use are: Horizontal and Vertical Constraints; Horizontal and Vertical Length Constraints; Point-to-Point Tangency. If possible, limit the use of these: the general Length Constraint; Edge-to-Edge Tangency; Fix Point Onto a Line Constraint; Symmetry Constraint.
 * If in doubt about the validity of a sketch once it is complete (features turn green), close the Sketcher dialog, switch to the [[Image:Workbench_Part.svg|24px]] Part Workbench and run.

チュートリアル

 * Sketcher tutorial by chrisb. This is a 70-page long PDF document that serves as a detailed manual for the sketcher. It explains the basics of Sketcher usage, and goes into a lot of detail about the creation of geometrical shapes, and each of the constraints.
 * Basic Sketcher Tutorial for beginners
 * Sketcher Micro Tutorial - Constraint Practices
 * Sketcher requirement for a sketch Minimum requirement for a sketch and Complete determination of a sketch

Scripting
The Sketcher scripting page contains examples on how to create constraints from Python scripts.