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In this task, you will find the following
information:
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Open the
Constraint_Definition.CATPart document. |
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Double-click Sketch1 as the sketch to be
edited.
You are now in the Sketcher workbench.
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Double-click the Radius.6 constraint.
The Constraint Definition dialog box appears.
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Select the Reference option to make the
constraint a reference.
The Radius field is deactivated, indicating that the value is
now driven by modifications to the sketch.
Using the Reference mode, the offset value is displayed
between brackets indicating this mode and measured from the component
locations. When the offset constraint supporting elements are two
non-parallel lines or the offset constraint is over-constrained, the
offset value cannot be measured, the constraint is invalid, any value is
displayed and two pound signs are displayed between the brackets (##).
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Click OK to confirm.
The radius value is displayed in brackets in the geometry area.
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If you drag the corner center point, you can
check that the radius value is updated. |
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Double-click the Angle.9 constraint.
The Constraint Definition dialog box appears.
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Type 125deg and click OK.
The new value is displayed in the geometry area. It affects the
angle. The sketch shape is also modified due to the radius previously
converted into a measure.
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Double-click the Offset.14 constraint.
The Constraint Definition dialog box
appears.
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Click the More button to access additional
information.
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Click the Line.5 component.
The related geometry is highlighted.
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Click Reconnect... to redefine the constraint
component.
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Select Line.6 and type 52mm in the
Value field.
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Click OK.
The position of the profile is modified accordingly.
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Exit the Sketcher.
The application has integrated the modifications to the sketch.
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Double-click Offset.3.
The Constraint Definition dialog box appears.
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Type 30mm in the Value field and
click OK.
The offset is modified accordingly.
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In the 3D area, if you select the blue pad, the Edit
Parameters contextual command allows you to display all parameters
and constraints defined for that pad. |
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When you are in the Repeat mode (you double-clicked on the
command for creating a constraint), if you try to edit an existing
constraint while creating another constraint, the modification will only be
taken into account when you have finished creating this other constraint. |
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Modifying Constraint Values by Using the Shift Key
It is possible to edit dimensional constraint values just by dragging
constrained geometry. This is a quick way of editing constraints without
launching dialog boxes. |
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Press the Shift key and drag the vertical line to the
right as shown below.
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You can notice that the value of the angle
constraint is not only modified as you are dragging the cursor, but it is
also displayed between parentheses, meaning that it is temporarily
converted into a reference. In other words, you can move the geometry
freely, with respect to geometrical constraints. |
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Press the Shift key and drag the vertical line to the
right as shown below.
The modified angle value is displayed (137.913), and is no longer a
reference:
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If the Snap to Point
option is active, the geometry is moved according to the spacing you
defined for the grid. For more information, refer to the customization for
Sketcher). |
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About Diameter and Radius Constraints
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You can obtain a radius constraint by editing a
diameter constraint. You just need to double-click the diameter
constraint and choose the radius option in the dialog box that appears.
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If you need to create a formula remember that:
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the parameter corresponding to the radius or
diameter constraint is referred to as RadiusX.object
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this parameter always contains the radius value. As
a consequence you can only add a formula on the
radius, not on the diameter (the diameter is a way to display the
constraint, not the parameter itself).
For more information about formulas, refer to
Knowledge Advisor User's Guide. |
- You can add a formula to the radius value of a diameter constraint by
using Tools > Formula.
Deactivating or Activating Constraints
You can:
- deactivate a constraint by right-clicking it and selecting
XXX.N.object > Deactivate. In other words, this constraint will
still appear on the sketch but will not behave as such.
Deactivated constraints appear preceded by an open-close brackets symbol
in the geometry and in the specification tree.
- activate a constraint, use the Activate option from the
contextual menu.
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