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To create simple geometry, you need to get familiar with a
certain number of options. This task shows you how to:
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Use Snap to Point
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Make sure that Snap to Point
is activated.
By default, this option is on.
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Select Rectangle
in the Profile toolbar.
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Drag the cursor to define the rectangle dimensions.
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As you are sketching, the points are snapped to
the intersection points of the grid. If this option is not activated, your
sketch is not influenced by the grid points. |
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Use SmartPick
The SmartPick tool helps you detect the constraints all along the sketch
creation. For instance, here a coincidence constraint is detected during
the rectangle creation with the H direction.
- The SmartPick tool is directly linked to the options that have been
checked in the Tools > Options dialog box.
- Therefore, if you do not wish to visualize the constraints detected
by the SmartPick, then simply uncheck the appropriate options in the
Smart Pick dialog box by selecting Tools > Options >
Mechanical Design > Sketcher > SmartPick.
- When the Smartpick detects a coincidence between a line and a point,
this symbol
is visualized in the geometry.
- When the Smartpick detects a coincidence between two points, this
symbol
is
visualized in the geometry.
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Use the Construction/Standard Elements Option
Once set to the Construction mode, elements cannot be published in the
3D area.
Standard Elements are created by default and they can be published in the
3D area.
The Construction/Standard Element option
is not active by default. |
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Create a rectangle.
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Select Corner
in the Operation toolbar.
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Select Trim all Elements
in the Sketch tools toolbar.
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Select the two parallel lines one after the other.
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An arc of circle is displayed and you can
position it as you like just by dragging the cursor.
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Drag the cursor to position the corner as shown here.
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Click in the geometry to finish the corner creation.
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Note that the corner is created and that the
two selected lines have been re-limited automatically.
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The corner is created and as the
Construction/Standard Element option is not activated, the elements
of this sketch are set to the standard mode.
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Select the rectangle line as shown here.
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Click the Construction/Standard Element
option from the Sketch tools toolbar.
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The
selected line has been swapped to construction mode and is
displayed as shown here.
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If you
want to generate a pad from this sketch it is important to set the
line in construction mode otherwise the pad generation will not be
possible.
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To swap
it back to the standard mode, simply select it and click again the
Construction/Standard Element.
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- Note that this is only one way of creating this sketch and that you
can get the same result using other commands such as Profile,
Circle, etc.
- When setting an element in construction mode, then this element is
not published once in the 3D area
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