You can select as many geometrical elements as required. You can
select the origin, the H or V Direction of the sketch absolute axis.
Dependencies
To assume that the rigid body behavior can be managed, by
default the
app
includes element dependencies. When adding a spline, for example, all its
control points and control point tangencies are automatically added even if
they are not selected.
The following table lists geometric elements and their corresponding
dependencies:
Geometrical Element
Dependency
Line
Start point + End point
Circle/Ellipse
Center point
Arc of Circle/Ellipse
Center point + Start point + End point
Parabola/Hyperbola
Start point + End point
Conic by two points
Start point + End point + (Start Tangent
curve + End Tangent curve) or Tangent Intersection point + (Passing point or
Not)
Conic by four points
Four points + One Tangent curve
Conic by five points
Five points
Connect Curve
First point + Second point + First curve
+ Second curve
Spline
Control points + Tangent directions
Important:
You can revert to a group with all its
dependencies. To do so, see
Sketcher
User's Guide: Analyzing the Sketch: About Analyzing Sketched Geometries.
Number of Elements
You can select as many geometrical elements as required but a
single geometric element can be used by only one
Group constraint.
Whenever you want to remove elements from the group, remove it from
the list in the
Group.x dialog box. Alternatively, select the
element in the
work area
again.
Absolute Axis
You can select the origin, the H or V Direction of the sketch
absolute axis.
These three elements cannot be selected at the same time by a
selection trap. You need to explicitly select them one by one.
Edges Obtained Using Offset, Projection or Intersection
A rigid set including edges obtained via
Offset,
Projection, and
Intersection operations and sketched geometry
remains rigid as long as you do not move the initial 3D geometry.
To ensure permanent rigidity, apply
Isolate to the edges obtained by
Offset,
Projection, and
Intersection operations. This breaks the links
between the original 3D geometry and the edges.
Degrees of Freedom
The set of geometric elements constrained by
Group has three degrees of freedom whatever the
number of elements.
To be fully defined, the set needs to be dimensioned to fix geometry
taking up at least the three degrees of freedom (one rotation and two
translations).
A geometric element included in a set of elements constrained via
Group can also be
constrained using
Constraints Defined in Dialog Box. If, for example, a group constraint contains a fixed line,
the set of geometric elements has one single degree of freedom which is along
the direction of the line.
Edit a Group Constraint
You can add a geometric element to a group constraint provided
it belongs to the current sketch and is not already included in another group
constraint.
The selection or the pre-selection of the elements to add depends on
this verification during the group creation and editing.
You can add several elements at the same time either using the
Ctrl key or the selection trap. After a
selection:
Geometric elements not used for the definition are added.
Geometric elements that are already part of the definition are
removed.
Additional Constraints
No constraints are solved between geometric elements linked by
the same group constraint, except for Fix constraints.
Adding constraints between elements involved in a group and other
elements involved too in a distinct group constraint or free elements allows
you to position the group.
Adding a constraint to an element in a group brings about an
over-constrained system. But unlike other types of constraints, when you exit
Sketcher,
no inconsistencies are detected.
All existing or added constraints on geometric elements of a group
are seen as over-defined (in purple
when solving status is displayed).
Except for fix constraints, no constraints are solved between
geometric elements linked by the same group constraint. However, no update
error appears on such over-defined constraints (between geometric elements of
the same group) and the part is successfully updated.
Remove Geometrical Elements
You can remove geometrical elements from a group by deleting the
geometrical elements: dependencies are deleted too.
When the number of geometric elements in the set is less than two, the
group constraint is not automatically deleted.
Apply Operations onto Group Constraint
Copy/Paste
You can copy and paste a group set (not the constraint alone)
by right-clicking the paper clip, selecting
Group object > Select Geometrical Elements,
Ctrl + select the paper clip.
You can also select using the selection trap to ensure that the
paper clip and the associated constrained geometry are selected and applying
the
Copy/Paste capability.
Mirror
By switching off the
Geometrical Constraints mode, the
Group constraint is taken into account like the
other constraints when mirroring geometric elements and keeping the initial
constraints.
If the
Geometrical Constraints is selected, the
app
creates
symmetry constraints as requested.
Break/Trim/Corner/Chamfer
You can apply the
Break,
Trim,
Corner, and
Chamfer commands onto elements attached by a
group constraint.
When all the geometrical elements belong to the same group, the
constraint is updated accordingly. For example, when breaking a curve, the new
half curve is automatically added to the definition.
Methodology
Group is a way of
getting better solving performance and solving more complex systems including
rigid sub-parts.
Depending on your geometry and your needs, you can use
Group or
Auto Constraint:
The Group command creates
only one constraint for a group or elements.
The
Auto Constraint command detects all possible constraints between the
selected elements then creates these constraints. This means that sometimes you
may create a lot of unnecessary constraints just for imposing a rigid behavior.
For more information, see
Sketcher User's Guide:
Auto-constraining a group of elements.
Visualizing Grouped Constraints in the
Drafting
or
2D Layout for 3D Design
Tree
In the context of
Drafting
or
2D Layout for 3D Design,
all constraints created in a view, using the
Group command are
added in the
Groups node, under the appropriate view in the
tree.
(Constraints created directly in the sheet or the sheet background are not
displayed in the tree.)
The
Groups node is created by default when one or
more elements are grouped using the
Group command, but it is not displayed by
default. At any time, you can specify whether or not you want to view this node
in
Me > Preferences > App Preferences > 3D Modeling > Mechanical Systems
> Drafting > Display tab,
under
Tree, by selecting
Group check box.
Internal and External Constraints of a Group
When a constraint is created pointing geometries belonging to
the same
Group, an internal constraint is created.
Whereas when a constraint is created pointing a geometry of
Group and an external geometry, an external
constraint is created.
In a sketch, internal constraints of
Group are always seen as over-constrained when
the
Group constraint is active.
External constraints are transferred during
instantiation of
Group, only when the external constraints are
created between the geometry of
Group and an element of sketch absolute axis
(i.e. the origin, H direction or V direction).
Constraints of Group before Instantiation
Constraints of Group after Instantiation
The external constraint values pointing to an element of the sketch
absolute axis, are updated automatically according to the position of the
origin instance defined by the Smartpick.
However, note that,
Notes:
The external constraints of
Group pointing to an external geometry are
removed at the instantiation.
The external constraints type is changed or they are removed if
the external constraints are incompatible with the requested transformation.
For example, when imposing an angle value, the external
driving distance constraints are changed into driven angle constraint to
respect the rotation transformation.
can also be
constrained using
. If, for example, a group constraint contains a fixed line,
the set of geometric elements has one single degree of freedom which is along
the direction of the line.
when solving status is displayed).
:
