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In this task, you will learn how to create a
positioned sketch, in which you specify the reference plane, and the origin
and orientation of the absolute axis. Creating a positioned sketch
enables you to define (and later change) explicitly the position of the
sketch absolute axis. This offers the following advantages:
- You can use the absolute axis directions like external references for
the sketched profile geometry.
- When the geometry of the part evolves and the associated position of
the sketch changes, the shape of the sketched profile (2D geometry of the
sketch) remains unchanged (even if the sketched profile is
under-constrained).
Creating a positioned sketch also ensures associativity with the 3D
geometry. |
Open the
Positioned_sketch.CATPart
document. |
You will now create a positioned sketch that
will enable you to design the retaining bracket for this part.
You will position the sketch absolute axis as follows:
- its origin will be on the axis of revolution,
- its horizontal (H) direction will be parallel to the flat face,
- its vertical (V) direction will be normal to the flat face.
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Click Positioned Sketch
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The Sketch Positioning dialog box appears.
In the Type field in the Sketch
Positioning area, two options are available:
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Positioned (pre-selected): creates
a positioned sketch for which you specify the origin and orientation of
the absolute axis.
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Sliding: creates a "non-positioned"
sketch, i.e. a sketch for which you do not specify the origin and
orientation of the absolute axis. This option is mainly used for
compatibility with non-positioned sketches, and to enable you to turn
them into positioned sketches. With the Sliding option, the sketch
absolute axis may "slide" on the reference plane when the part is
updated.
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Keep the Positioned option selected.
You will now specify the reference plane for the sketch.
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Make sure the Reference field is active, and
select the blue surface (Shaft.1).
The Sketch Positioning dialog box is
updated: the Reference field now indicates the reference plane.
Also, the Type fields of the Origin and
Orientation areas are activated and the Implicit mode is
pre-selected.
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With the Implicit mode, the sketch
origin point and the sketch orientation are positioned according to the
geometry used for the sketch plane:
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When the sketch support is a plane, the sketch
origin point is a projection of the part origin point in the sketch
plane, and the sketch orientation is parallel to the reference plane
directions.
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When the sketch support is defined by two
secant lines, the origin is at the intersection of these. The H direction
is co-linear to the first line, and its orientation directly depends on
the orientation of this line. The V direction is deduced from the second
line, which is not necessarily orthogonal to the first line. This second
line simply defines, depending on its orientation, the side where the V
direction will be positioned in relation to the H direction.
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You will now specify the absolute axis origin so
to make it coincident with the axis of revolution of the part. |
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Select Curve intersection in the Type
field of the Origin frame.
The Reference field is activated.
The options available for defining an origin are:
- Implicit
- Part origin
- Projection point
- Intersection between 2 lines
- Curve intersection
- Middle point
- Barycenter
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Select the cylindrical surface to make its axis intersect
with the absolute axis origin.
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The absolute axis of the sketch is now
positioned on this axis. Its orientation has not changed. |
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You will now specify the absolute axis orientation
according to an edge of the flat face. The options available for defining an orientation are:
- Implicit
- X Axis
- Y Axis
- Z Axis
- Components
- Through point
- Parallel to line
- Intersection plane
- Normal to surface:
you just need to select a surface intersecting the sketch plane.
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Select Parallel to line in the Type
field of the Orientation frame. The Reference field is activated.
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Select an edge of the flat face.
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The absolute axis of the sketch is now oriented
like the selected edge. |
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You will now invert the H direction and make the
V direction normal to the flat face. To do this, start by selecting
V Direction in the Orientation area to specify that you
want the orientation to be defined according to the V direction. |
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Select Reverse V to revert the V direction and
select the Swap check box to swap H and V directions.
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The sketch is now positioned as wanted. |
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Click OK to validate and exit the Sketch
Positioning dialog box.
You are now in the Sketcher workbench and ready to sketch a profile for
the retaining bracket.
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The absolute axis (its origin point, both its
directions and the grid) can be used to specify the position and
dimensions of the 2D geometry because it is associative with the part.
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With positioned sketches, the origin and
directions of the absolute axis are similar to external references
(Use-Edges) obtained using additional projections or intersections when
creating non-positioned sketches.
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In this exercise, you did not create any
constraints on 2D geometry: the geometry is under-constrained. Yet, if
you move or resize the part (no matter how significantly), the profile
you sketched will remain absolutely unchanged. Its shape will not be
altered: thanks to the fact that the position of its absolute axis is
explicitly defined, it is automatically pre-positioned in 3D before its
2D resolution.
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At any time after creating a positioned
sketch, you can change the reference plane, the origin and the
orientation of the absolute axis by specifying the new geometry in the
associated Reference field. To do this from the 3D,
right-click the positioned sketch in the specification tree, point to
[sketch name] object in the contextual menu, and then select
Change sketch support.
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