Sketcher Ограничение касательности
Sketcher ConstrainTangent |
Системное название |
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Sketcher ConstrainTangent |
Расположение в меню |
Sketch → Ограничения эскиза → Ограничение касательности |
Верстаки |
Sketcher |
Быстрые клавиши |
T |
Представлено в версии |
- |
См. также |
Constraint point on object |
Описание
Ограничение касательности делает две кривые касающимися друг друга. Линии полагаются бесконечными, а дуги как полные окружности или эллипсы. Ограничение так же может соединять две кривые, заставляя их идти по касательной в точке соединения, делая переход гладким.
Использование
Возможно четыре варианта назначения ограничения:
- между двумя кривыми (доступно не для всех кривых)
- между двумя конечными точками кривой, делая гладкое соединение
- между кривой и конечной точкой другой кривой
- между двумя кривыми в точке, определённой пользователем
Для назначения ограничения касательности следует:
- Выделить две или три элемента эскиза.
- Вызвать ограничение, кликнув его иконку на панели инструментов или выделив в меню, или использовав клавиатурное сокращение.
Между двумя кривыми (прямое касание)
Две прямые станут касательными, но точка касания будет неопределённой. Этот режим назначается, когда выделены две кривые.
Допустимые выделения:
- линия + линия, окружность, дуга, эллипс, дуга эллипса
- окружность, дуга + окружность, дуга
Если прямое касание между выделенными кривыми не поддерживается (например, между оуружностью и эллипсом), автоматически будет добавлена вспомогательная точка, и будет применено tangency-via-point.
Не рекомендуется реконструировать точку касания созданием точки и установкой принадлежности её обоим кривым. Это будет работать, но конвергенция будет значительно медленнее, сложнее, и потребует вдвое больше итераций чем в норме. Используйте другие режимы этого ограничения, если нужна точка касания.
Between two endpoints (point-to-point tangency)
In this mode, the endpoints are made coincident, and the joint is made tangent (C1-smooth, or "sharp", depending on the placement of curves before the constraint is applied). This mode is applied when two endpoints of two curves were selected.
Accepted selection:
- endpoint of line/arc/arc-of-ellipse + endpoint of line/arc/arc-of-ellipse (i.e., two endpoints of any two curves)
Between curve and endpoint (point-to-curve tangency)
In this mode, an endpoint of one curve is constrained to lie on the other curve, and the curves are forced tangent at the point. This mode is applied when a curve and an endpoint of another curve were selected.
Accepted selection:
- line, circle, arc, ellipse, arc-of-ellipse + endpoint of line/arc/arc-of-ellipse (i.e., any curve + endpoint of any curve)
Between two curves at point (tangent-via-point) (v0.15)
In this mode, two curves are made tangent, and the point of tangency is tracked. This mode is applied when two curves and a point were selected.
Accepted selection:
- any line/curve + any line/curve + any point
"Any point" can be a lone point, or a point of something, e.g. a center of a circle, an endpoint of an arc, or the origin.
For the constraint to work correctly, the point must be on both curves. So, as the constraint is invoked, the point will be automatically constrained onto both curves (helper constraints will be added, if necessary), and the curves will be forced tangent at the point. These helper constraints are plain regular constraints. They can be added manually, or deleted.
Compared to direct tangency, this constraint is slower, because there are more degrees of freedom involved, but if the point of tangency is needed, it is the recommended mode because it offers better convergence compared to direct tangency + point on two curves.
The placement of the point before the constraint is applied is a hint for the solver for where the tangency should be. With this constraint, one can constrain two ellipses to touch each other in two places.
Scripting
Tangent Constraint can be created from macros and from the python console by using the following:
# direct tangency
Sketch.addConstraint(Sketcher.Constraint('Tangent',icurve1,icurve2))
# point-to-point tangency
Sketch.addConstraint(Sketcher.Constraint('Tangent',icurve1,pointpos1,icurve2,pointpos2))
# point-to-curve tangency
Sketch.addConstraint(Sketcher.Constraint('Tangent',icurve1,pointpos1,icurve2))
# tangent-via-point (plain constraint, helpers are not added automatically)
Sketch.addConstraint(Sketcher.Constraint('TangentViaPoint',icurve1,icurve2,geoidpoint,pointpos))
where:
Sketch
is a sketch objecticurve1
,icurve2
are two integers identifying the curves to be made tangent. The integers are indexes in the sketch (the value, returned bySketch.addGeometry
).pointpos1
,pointpos2
should be 1 for start point and 2 for end point.geoidpoint
andpointpos
inTangentViaPoint
are the indexes specifying the point of tangency.
- General: Create sketch, Edit sketch, Attach sketch, Reorient sketch, Validate sketch, Merge sketches, Mirror sketch, Leave sketch, View sketch, View section, Toggle grid, Toggle snap, Configure rendering order, Stop operation
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- Sketcher constraints:
- Dimensional constraints: Dimension, Horizontal distance, Vertical distance, Distance, Auto radius/diameter, Radius, Diameter, Angle, Lock
- Geometric constraints: Coincident (unified), Coincident, Point on object, Horizontal/vertical, Horizontal, Vertical, Parallel, Perpendicular, Tangent or collinear, Equal, Symmetric, Block
- Other constraints: Refraction (Snell's law)
- Constraint tools: Toggle driving/reference constraint, Activate/deactivate constraint
- Sketcher tools: Fillet, Chamfer, Trim, Split, Extend, External geometry, Carbon copy, Select origin, Select horizontal axis, Select vertical axis, Array transform, Polar transform, Scale transform, Offset geometry, Symmetry, Remove axes alignment, Delete all geometry, Delete all constraints
- Sketcher B-spline tools: Convert geometry to B-spline, Increase B-spline degree, Decrease B-spline degree, Increase knot multiplicity, Decrease knot multiplicity, Insert knot, Join curves
- Sketcher visual: Select unconstrained DoF, Select associated constraints, Select associated geometry, Select redundant constraints, Select conflicting constraints, Show/hide circular helper for arcs, Show/hide B-spline degree, Show/hide B-spline control polygon, Show/hide B-spline curvature comb, Show/hide B-spline knot multiplicity, Show/hide B-spline control point weight, Show/hide internal geometry, Switch virtual space
- Additional: Sketcher Dialog, Preferences, Sketcher scripting
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