Context:
You select one face of the cube to define the sketch plane and extrude the
sketched profile through half the depth of the cube. The cube and flange are
shown in
Figure 1.
From the main menu bar, select
.
Select the face at the front of the cube to define the sketching
plane, as shown in
Figure 2.
When you stop moving the cursor during a selection procedure,
Abaqus/CAE
highlights the edges of the entity that it would select at the current cursor
position. This highlighting behavior is called preselection.
Note:
Two forms of preselection are available in
Abaqus/CAE:
one for object selection from the viewport and the other for selection from the
Sketcher.
For more information, see
Highlighting objects prior to selection,
and
Turning preselection on or off,
respectively.
Select an edge that will appear vertical and on the right side of the
sketch, as shown in
Figure 2.
Again,
Abaqus/CAE
uses preselection to aid you in selecting the desired edge.
The
Sketcher
starts and displays the outline of the base feature as reference geometry.
Abaqus/CAE
magnifies the view to fit the sketch plane; the sheet size and grid spacing are
also recalculated based on the size of the sketch plane. To change the sheet
size and grid spacing back to their original settings and disable their
automatic recalculation for the current session, use the options tool
, located in the
Sketcher
toolbox. On the General tabbed page, toggle off
Auto next to the sheet size text field and set the value
to 0.2; toggle off Auto
next to the grid spacing text field and set the value to
0.005.
The sketch of the flange that you will create is illustrated in
Figure 3.
To duplicate the view in the figure, use the options tool again to double the
grid spacing.
Zoom out to view the area where you will sketch the flange:
-
From the
View Manipulation toolbar,
select the magnify tool
.
-
Position the cursor near the center of the viewport.
-
Click mouse button 1 and drag to the left until the cube occupies
approximately half of the visible
Sketcher
space.
Reducing the view is necessary because the flange is created beyond
the edges of the selected sketch plane.
As before, the approximate shape of the new feature will be sketched
first. From the Sketcher toolbox, select the connected lines tool
.
Sketch the rectangular portion of the flange by drawing three lines as
follows:
-
Starting at any point to the right of the cube, connect the line
to the top-right corner of the cube.
-
Continue the next line to the bottom-right corner of the cube.
This line is automatically assigned a vertical constraint.
-
The final line extends from the bottom-right corner of the cube to
any point to the right of the cube.
Click mouse button 2 in the viewport to exit the connected lines tool.
Refine the sketch by defining the following constraints and dimension:
-
Use the constraints tool
to constrain the top and bottom lines of the sketch so that
each is horizontal.
-
Assign an equal length constraint to these two lines (use
ShiftClick to
select both lines).
-
Dimension either line so that it is
0.02 m long.
The sketch appears as shown in
Figure 4.
Close the profile by adding a semicircular arc using the 3-points
circle tool
.
-
Select the two vertices at the open end of the rectangle as the
endpoints of the arc, starting with the top one. Select any point to the right
of the sketch as a point that lies on the arc.
-
Define tangent constraints between the ends of the arc and the
horizontal lines to refine the sketch.
Click mouse button 2 in the viewport to exit the 3-points circle tool.
The resulting arc is shown in
Figure 5.
From the Sketcher toolbox, select the center-perimeter circle tool
to sketch the flange hole.
-
Place the center of the circle to coincide approximately with the
center of the arc created previously. The perimeter point should be placed to
the right of the center point. Apply a concentric constraint between the two
circular regions.
-
Use the dimension tool
to change the value of the radius to
0.01 m.
-
Dimension the vertical distance between the center of each circle
and its perimeter point. Edit this dimension so that the distance is
0. (If the distance is already
0, you cannot add a vertical dimension.) This
will adjust the location of the perimeter point so that it is on the same
horizontal plane as the center point.
Note:
When you mesh a part,
Abaqus/CAE
places nodes wherever vertices appear along an edge; therefore, the location of
the vertex on the circumference of the circle influences the final mesh.
Placing it on the same horizontal plane as the center point results in a
high-quality mesh.
The final sketch is shown in
Figure 6.
Click mouse button 2 to exit the
Sketcher.
Abaqus/CAE
displays the part in an isometric view showing the base extrusion, your
sketched profile, and an arrow indicating the extrusion direction. The default
extrusion direction for a solid is always out of the solid.
Abaqus/CAE
also displays the Edit Extrusion dialog box.
In the Edit Extrusion dialog box:
-
Accept the default Type selection of
Blind to indicate that you will provide the depth of the
extrusion.
-
In the Depth field, type an extrusion depth
of 0.02.
-
Click
to reverse the extrusion direction, as shown in
Figure 7.
Figure 7. Completed flange sketch showing the extrusion
direction.
-
Toggle on Keep internal boundaries. When you
toggle this option on,
Abaqus/CAE
maintains the face that is generated between the extruded solid feature and the
existing part. As a result, the extruded flange is maintained as a second cell
and is not merged with the cube. (When you mesh the model at the end of the
tutorial, the internal boundary allows you to mesh the flange without having to
first partition the cell and flange into separate cells.)
-
Click OK to create the solid extrusion.
Abaqus/CAE
displays the part composed of the cube and the flange. Use the auto-fit view
manipulation tool
again to resize the part to fit in the viewport.