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This
task shows you how to duplicate an element of the following type: line,
arc or circle. You can also duplicate by offset one of the following: an
edge, a face (all the boundaries of this face are offset) or a geometrical
feature (for example, by selecting a join or another sketch in the
specification tree).
Select a topic:
Offsetting 2D Geometry
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Create a line. |
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Click Offset
from the Operations toolbar (Transformation
subtoolbar).
OR
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Select the Insert >Operation>Transformation>Offset
command from the menu bar.
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There are two possibilities, depending on whether the
line you want to duplicate by offset is already selected or not:
- If the line is already selected, the line to be created appears
immediately.
- If the line is not already selected, select it. The line to be
created appears.
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Select a point or click where you want the new element to
be located.
The selected line is duplicated. Both lines are parallel.
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- If you were offsetting circles or arcs, these two circles would be
concentric.
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- If Geometrical Constraints
and Dimensional Constraints
are active in the Sketch tools toolbar when offsetting an
element, constraints are automatically created, based on the type of
element you are offsetting. Thus, if you move an element, or change
its geometry, the other element will be moved or modified accordingly.
Using offset tools
You can also apply one or more offset instances to
profiles made of several elements:
- by using tangency propagation or point propagation,
- by creating an offset element that is tangent to the first one,
- by creating several offset instances.
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This is not true for
generated elements (Generative Drafting workbench).
If the multi-selected elements do not make up a closed profile, the
offset will be applied to the selected elements only. As a result, you will
have as many offset elements as the first multi-selected elements.
Previews are not available when creating several offset instances (i.e.
when the value in the Instance(s) field of the Sketch tools
toolbar is higher than one). |
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Open the
Offset.CATPart document. |
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Click Offset
from the Operations toolbar (Transformation
subtoolbar).
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Select the desired option from the displayed Sketch
tools toolbar.
(These options are described further down in this section).
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Select the element you want to offset and if needed,
enter the desired number of instances. The element to be
created is previewed.
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Select a point or click where you want the new element to
be located.
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To offset a single element:
Activate No Propagation
.
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To offset an element and elements which are tangent to it:
Activate Tangent Propagation
.
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To offset an element using Point Propagation:
Activate Point Propagation
.
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To offset an element symmetrically to another:
Activate Both Side Offset
.
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To offset and duplicate multiple elements:
Type the number of elements you want to create in the Instances
field. |
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Note that if you position
the cursor outside the zone that is allowed for creating a given element,
the
symbol appears.
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Drafting Workbench
You can create offset geometry using 2D component elements and dress-up
elements (axis lines, center lines and threads). Note that by doing this,
you will not create offset 2D components or dress-up elements, but you will
create offset geometry. |
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- You can offset them only element by element.
- You cannot offset complex curves.
- This will only work if you first select the command and then the
element to offset.
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Offsetting 3D Geometry
You can create an associative offset with a 3D element.
Open the
Offsetpad.CATPart document. |
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Click Offset
from the Operations toolbar (Transformation
subtoolbar).
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Select the 3D surface to offset, Face.1 for example. The
profile to be created is previewed.
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You can do one of the following:
- specify the offset position or value in the Sketch tools
toolbar and press Enter to validate.
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- Move the cursor till the correct offset appears in the sketch, then
click to validate the position.
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The offset is created, with the offset value
displayed. |
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It appears as Mark.1 in the specification tree: |
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If you want to edit the offset value, you can
double-click it and enter a new value in the dialog box which is displayed. |
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- When offsetting a face, if there is an intersection between the face
and the sketch plane, by default, it is this intersection which is offset
(rather than the projection of the face edges). In this case, if you want
to offset the projection of the face edges, you can modify the offset as
explained in the section below.
- You can offset the intersection between a face and a sketch plane
without explicitly creating this intersection.
- lf you offset a multi-domain face, the face that is closer from the
cursor is offset.
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- If you isolate a composite mark, as many simple geometry elements as
the mark was containing are created, and associativity will not be
available anymore.
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Modifying a 3D Geometry Offset
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Double-click the offset in the specification tree or on
the sketch. The Offset Definition dialog box is displayed.
In this dialog box, you can modify the offset definition.
- Parallel corner type: specifies
whether corners should be round or sharp (when applicable).
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Note that this option applies only when the
offset results in extrapolated curves (as is the case in our example, for
instance).
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Parameters
These options let you specify the offset parameters.
- Object to offset: indicates which 3D element is offset. To
offset another element, select this field and then select the new element
in the sketch.
- Offset value: indicates the offset value. You can modify
it by typing a new value in this field.
- Offset mode: when offsetting a face, specify whether you
want to intersect and offset or to project and offset the face by
selecting the appropriate option from the list.
Propagation
These options let you offset a 3D element using the propagation of an
edge.
- Type: specifies what type of offset propagation should be
applied to the selected reference element: No propagation,
Tangent propagation, or Point propagation. Click
the appropriate icon.
- Reference element: indicates which edge should be used as
a reference for the propagation. Select this field and then select the
reference edge in the sketch.
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In the Offset value field, type 20mm.
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Choose Project and offset from the Offset
mode field.
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Click OK to validate. The offset is modified.
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- Only 3D elements can be offset with associativity.
- There is no propagation on 3D edges.
- Typing a negative offset value reverses the offset direction.
- Multi-domain elements cannot be offset in one shot.
- If you apply the Parents/Children... command to a sketch
containing an offset obtained after selecting a face or an edge, the
Parents command shows the last solid feature that modified the
offset geometry. To see an example of this, refer to Parents/Children
paragraph of Projecting 3D Elements onto the Sketch Plane.
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