Sketcher Workbench/ro

Introducere
Atelierul Sketcher Workbench este utilizat pentru a crea forme geometrice 2D cu intenția de a le utiliza în Atelierul Part Design Workbench și ale ateliere. În general, o geometrie 2D este considerată punctul de plecare pentru majoritatea modelelor CAD - o schiță simplă 2D poate fi "extrudată" într-o formă 3D, pot fi folosite și alte schițe 2D pentru a crea buzunare/cavități în suprafața acestei forme și schițele pot fi folosite pentru definesc "pad" (extrudări) pe suprafața obiectelor 3D. Pe lângă Boolean operations, formele Sketcher constituie nucleul proiectării generării formelor solide.

Atelierul de lucru Sketcher pune pe primul loc constrângerile - permițând definirea formelor 2D după criterii geometrice precise. Un solver matematic de constrângeri calculează nivelul constrângerii și permite explorarea interactivă a gradelor de libertate.



Elementele de bază ale constrângerilor schiței
Pentru a explica cum funcționează Sketcher-ul, poate fi util să îl comparați cu modul tradițional de redactare.

Schițarea tradițională
Modul tradițional de schițare CAD moștenește de la vechea drawing board. Vizualizări ortogonale (2D) sunt desenate manual și sunt destinate pentru realizarea desenelor tehnice (cunoscute și sub denumirea de planuri). Obiectele sunt desenate exact la dimensiunea sau dimensiunea dorită. Dacă doriți să desenați o linie orizontală cu lungimea de 100 mm începând cu (0,0), activați instrumentul Linie, faceți clic pe ecran sau introduceți coordonatele (0,0) pentru primul punct, apoi efectuați un al doilea clic sau introduceți coordonatele celui de-al doilea punct la (100,0). Sau vă veți trage linia fără a ține seama de poziția sa și o veți muta ulterior. După ce ați terminat desenarea geometriei, adăugați dimensiuni acestora.

Constrângeri în Sketching
Sketcherul se îndepărtează de această logică. Obiectele nu trebuie să fie desenate exact așa cum intenționați, deoarece ele vor fi definite ulterior prin constrângeri. Obiectele pot fi desenate și, atâta timp cât ele nu sunt restricționate, pot fi modificate. Ele sunt în fapt "plutitoare" și pot fi mișcate, întinse, rotite, scalate și așa mai departe. Acest lucru oferă o mare flexibilitate în procesul de proiectare.

Ce sunt constrângerile?
În loc de dimensiuni, constrângerile sunt folosite pentru a limita gradul de libertate al unui obiect. De exemplu, o linie fără constrângeri are 4 Degrees of Freedom (abreviat ca "DOF"): poate fi mișcat orizontal sau vertical, poate fi întinsă și poate fi rotită.

Aplicarea unei constrângeri orizontale sau verticale sau a unei constrângeri de unghi (relativ la o altă linie sau la una dintre axe) va limita capacitatea sa de a se roti, lăsându-l astfel cu 3 grade de libertate. Blocarea unuia dintre punctele sale în raport cu originea va elimina încă 2 grade de libertate. Și aplicarea unei constrângeri de dimensiune va elimina ultimul grad de libertate. Linia este apoi considerată  complet constrânsă .

Obiectele multiple pot fi constrânse între ele. Două linii pot fi unite prin unul dintre punctele lor cu constrângerea punctului coincident. Un unghi poate fi setat între ele sau poate fi setat perpendicular. O linie poate fi tangentă la un arc sau un cerc și așa mai departe. O schiță complexă, cu obiecte multiple, va avea o serie de soluții diferite, ceea ce înseamnă că "una dintre aceste soluții posibile a fost atinsă pe baza constrângerilor aplicate.

Există două tipuri de constrângeri: geometrice și dimensionale. Acestea sunt detaliate în secțiunea 'Instrumentele' de mai jos.

La ce nu este bun Sketcher-ul
Instrumentul Sketcher nu este destinat pentru realizarea planurilor 2D. Odată ce schițele sunt folosite pentru a genera o caracteristică solidă, ele sunt ascunse automat. Constrângerile sunt vizibile numai în modul Editare schiță.

Dacă doriți să creați numai vizualizări 2D pentru tipărire și nu doriți să creați modele 3D, consultați Draft draftbench.

Sketching Workflow
A Sketch is always 2-dimensional (2D). To create a solid, a 2D Sketch of a single enclosed area is created and then either Padded or Revolved to add the 3rd dimension, creating a 3D solid from the 2D Sketch.

If the Sketch has segments that cross one another, places where a Point is not directly on a segment, or places where there are gaps between endpoints of adjacent segments, Pad or Revolve won't create a solid. The exception to this rule is that it doesn't apply to Construction (blue) Geometry.

Inside the enclosed area we can have smaller non-overlapping areas. These will become voids when the 3D solid is created.

The tools
The Sketcher Workbench tools are all located in the Sketch menu that appears when you load the Sketcher Workbench.


 * [[Image:Sketcher_NewSketch.png‎‎|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.png|32px]] Edit sketch: Edit the selected Sketch.


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


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


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


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


 * Reorient sketch : Allows you to change the position of a sketch


 * Validate sketch: It allows you to check if there are in the tolerance of different points and to match them.


 * [[Image:Sketcher MergeSketch.png‎|32px]] Merge sketches: Merge two or more sketches.


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

Sketcher geometries
These are tools for creating objects.


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


 * [[Image:Sketcher_Line.png|32px]] Line by 2 point: Draws a line segment from 2 points. Lines are infinite regarding certain constraints.


 * Create an arc: This is an icon menu in the Sketcher toolbar that holds the following commands:


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


 * [[Image:Sketcher CreateArc3Point.png|32px]] Arc by 3 Point: Draws an arc segment from two endpoints and another point on the circumference.


 * Create a circle: This is an icon menu in the Sketcher toolbar that holds the following commands:


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


 * [[Image:Sketcher CreateCircle3Point.png|32px]] Circle by 3 Point: Draws a circle from three points on the circumference.


 * [[Image:Sketcher_Conics.png|32px]] Create a conic:
 * [[Image:Sketcher_CreateEllipse.png|32px]] Ellipse by center: Draws an ellipse by center point, major radius point and minor radius point.
 * [[Image:Sketcher_CreateEllipse_3points.png|32px]] Ellipse by 3 points: Draws an ellipse by major diameter (2 points) and minor radius point.
 * [[Image:Sketcher_Elliptical_Arc.png|32px]] Arc of ellipse: Draws an arc of ellipse by center point, major radius point, starting point and ending point.
 * [[Image:Sketcher_Hyperbolic_Arc.png|32px]] Arc of hyperbola: Draws an arc of hyperbola.
 * [[Image:Sketcher_Parabolic_Arc.png|32px]] Arc of parabola: Draws an arc of parabola.


 * 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_Create_Periodic_BSpline.svg Create periodic B-pline: Draws a periodic (closed) B-spline curve by its control points.


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


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


 * [[Image:Sketcher_CreateHexagon.png|32px]] Create regular polygon: This is an icon menu in the Sketcher toolbar that holds the following commands:


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


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


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


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


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


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


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


 * [[Image:Sketcher_CreateFillet.png|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.png|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_External.png|32px]] External Geometry: Creates an edge linked to external geometry.


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


 * [[Image:Sketcher_ToggleConstruction.png|32px]] 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.


 * [[Image:Constraint_PointOnPoint.png|32px]] Coincident: Affixes a point onto (coincident with) one or more other points.


 * [[Image:Constraint_PointOnObject.png|32px]] Point On Object: Affixes a point onto another object such as a line, arc, or axis.


 * [[Image:Constraint_Vertical.png|32px]] Vertical: Constrains the selected lines or polyline elements to a true vertical orientation. More than one object can be selected before applying this constraint.


 * [[Image:Constraint_Horizontal.png|32px]] Horizontal: Constrains the selected lines or polyline elements to a true horizontal orientation. More than one object can be selected before applying this constraint.


 * [[Image:Constraint_Parallel.png|32px]] Parallel: Constrains two or more lines parallel to one another.


 * [[Image:Constraint_Perpendicular.png|32px]] Perpendicular: Constrains two lines perpendicular to one another, or constrains a line perpendicular to an arc endpoint.


 * [[Image:Constraint_Tangent.png|32px]] 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.


 * [[Image:Constraint_EqualLength.png|32px]] Equal Length: Constrains two selected entities equal to one another. If used on circles or arcs their radii will be set equal.


 * [[Image:Constraint_Symmetric.png|32px]] Symmetric: Constrains two points symmetrically about a line, or constrains the first two selected points symmetrically about a third selected point.


 * [[Image:Sketcher_ConstrainBlock.png|32px]] Constrain Block: Basically allows to block a geometric element in place with a single constraint. It should be particularly useful to work with 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.


 * [[Image:Sketcher_ConstrainLock.png‎|32px]] 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.


 * [[Image:Constraint_HorizontalDistance.png‎|32px]] 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.


 * [[Image:Constraint_VerticalDistance.png|32px]] 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.


 * [[Image:Constraint_Length.png|32px]] 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.


 * [[Image:Constraint_Radius.png|32px]] Radius: Defines the radius of a selected arc or circle by constraining the radius.
 * [[Image:Constraint_InternalAngle.png|32px]] Internal Angle: Defines the internal angle between two selected lines.


 * [[Image:Constraint_SnellsLaw.png|32px]] Snell's Law: Constrains two lines to obey a refraction law to simulate the light going through an interface.


 * [[Image:Constraint_InternalAlignment.png |32px]] Internal Alignment: Aligns selected elements to selected shape (e.g. a line to become major axis of an ellipse).


 * [[Image:Sketcher_ToggleConstraint.png |32px]] Toggle reference/driving constraint: Toggles the toolbar or the selected constraints to/from reference mode.

Sketcher tools

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


 * [[Image:Sketcher CloseShape.png‎|32px]] Close Shape: Creates a closed shape by applying coincident constraints to endpoints


 * [[Image:Sketcher ConnectLines.png‎|32px]] Connect Edges: Connect sketcher elements by applying coincident constraints to endpoints


 * [[Image:Sketcher SelectConstraints.png‎|32px]] Select Constraints: Selects the constraints of a sketcher element


 * [[Image:Sketcher SelectOrigin.png‎|32px]] Select Origin: Selects the origin of a sketch


 * [[Image:Sketcher SelectVerticalAxis.png‎|32px]] Select Vertical Axis: Selects the vertical axis of a sketch


 * [[Image:Sketcher SelectHorizontalAxis.png‎|32px]] Select Horizontal Axis: Selects the horizontal axis of a sketch


 * [[Image:Sketcher SelectRedundantConstraints.png‎|32px]] Select Redundant Constraints: Selects redundant constraints of a sketch


 * [[Image:Sketcher SelectConflictingConstraints.png‎|32px]] Select Conflicting Constraints: Selects conflicting constraints of a sketch


 * [[Image:Sketcher SelectElementsAssociatedWithConstraints.png‎|32px]] Select Elements Associated with constraints: Select sketcher elements associated with constraints


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


 * [[Image:Sketcher Symmetry.png‎|32px]] Symmetry: Copies a sketcher element symmetrical to a chosen line


 * [[Image:Sketcher Clone.png‎|32px]] Clone: Clones a sketcher element


 * [[Image:Sketcher Copy.png‎|32px]] Copy: Copies a sketcher element


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


 * [[Image:Sketcher RectangularArray.png‎|32px]] Rectangular Array: Creates an array of selected sketcher elements


 * Sketcher Element SelectionTypeInvalid.svg Delete All Geometry: Deletes all geometry from the sketch.


 * Sketcher Element SelectionTypeInvalid.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_BSplineApproximate.svg Convert Geometry to B-spline


 * Sketcher_BSplineIncreaseDegree.svg Increase degree


 * Sketcher_BSplineIncreaseKnotMultiplicity.svg Increase knot multiplicity


 * Sketcher_BSplineDecreaseKnotMultiplicity.svg Decrease knot multiplicity

Sketcher virtual space

 * [[Image:Sketcher SwitchVirtualSpace.png‎|32px]] Switch Virtual Space: Allows you to "hide" constraints and make them visible again. See https://forum.freecadweb.org/viewtopic.php?f=9&t=26614

Preferences

 * [[Image:Std_DlgParameter.png|32px]] Preferences...: Preferences disposable in Sketcher Tools.

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.

Tutorials

 * Sketcher tutorial for beginners
 * Sketcher Tutorial
 * Sketcher Micro Tutorial - Constraint Practices