These are all at x=-127 and at y=0, y=69 and y=80 respectively.

Use GEOMETRY SURFACE 4POINTS (with the cursor or the keyboard) to create a four sided surface at the lower left hand end; where lines exist already they will be used, otherwise new lines will be created.

Create a line from the top left hand corner to P2 and using GEOMETRY SPLIT split the line at 0.75 of the distance along the line (or use the cursor to choose the location of the split point).

Create another line from the point just created to the nearest point and a corresponding line at the top left hand corner of the model.

At this stage there is a five sided region that needs to be resolved. If this were a two dimensional mesh then a combined line could be used to create a suitable surface. However the use of combined lines in 3 dimensional brick models can lead to subsequent problems so it is necessary to subdivide this area. The quickest way to do this is to use GEOMETRY SPLIT again to create an extra point halfway along the arc from P1 to P7 and then create a line joining this point to the other point created using GEOMETRY SPLIT.

Create the additional surfaces required to define the two dimensional shape by use of GEOMETRY SURFACE AUTOMATIC. This will search through the existing lines and create surfaces from closed loops of three or four lines. It does a check to make sure that surfaces already defined are not duplicated.

The next stage is to create a suitable mesh on the two dimensional shape that currently exists. Mesh information is copied when transformations are used so creating a suitable cross section mesh at this stage will save time later on when the three dimensional mesh is being created and refined.

Create a mesh to see what the default will look like.

Change the divisions on the lines to produce a suitable mesh. The quickest way of doing this is to change the default for meshing divisions (MESHING DIVISION DEFAULT n) and then use the cursor (left button) to pick the lines where the number of divisions is to be changed to the default value. If just a few lines are to be changed then the middle button of the cursor can be used in a similar way except that the user is expected to give the new value for the number of divisions on each line selected.

Sweep the set just created by 8 in the Z direction, remembering to specify '2' for the number of divisions along the swept lines.

Using EYE ROTATE or EYE DIRECTION change the view of the object to a general orientation so that the model is more comprehensible.

The translation will automatically have put the surfaces etc created as copies of the original surfaces into a new set (probably called SE3). So view just this set and remove the surface (probably S9) corresponding to the region that does not require to be swept.

VIEW GEOM

LABEL GEOM SURF

CONSTRUCT SET OPEN 'setname'

CONSTRUCT SET REMOVE 'corner_pointname'

CONSTRUCT SET CLOSE

Note also that CONSTRUCT SET 'setname' REMOVE 'pointname' would have the same effect and can be used as a shortcut.

Sweep the set which has just been modified by 27 in the Z direction. Remember to specify that all swept lines are to have 4 divisions.

Figure 7.2: The solid model geometry

Generate the mesh, view and try using VIEW HIDDEN SHADE, VIEW HIDDEN FILL to get a better idea of the mesh. Remember to use VIEW HIDDEN OFF when returning to look at the geometry.

Assuming that the mesh is suitable the next stage is to create the additional information required for a finite element analysis. Material properties can be defined and attached as in the previous examples. Physical properties do not need to be specified because the model uses brick elements (and so there are no physical properties).

The pressure load will be applied to the cylindrical surfaces on the inside of the model and the constraints will need to be applied to the plane of symmetry and also the left hand end of the model. The easiest way of applying the loads and constraints is to make use of sets; the easiest way of constructing the sets is to make use of the CONSTRUCT SET 'setname' APPEND CURSOR functions.

Rotate the view back to the initial orientation (EYE ROTATE TO 0)

CONSTRUCT SET YSYM APPEND CURSOR

can then be used to pick two points just above the plane of symmetry, all the points defining parts on the plane of symmetry will be highlighted to confirm the selection.

With the same view

CONSTRUCT SET PRES APPEND CURSOR POLYGON

can be used to define a polygon inside which the inner surfaces are contained (in this case most of the vertices will be in between the inner and outer arcs of the housing. The first vertex of the polygon should be selected using the left mouse button, intermediate vertices are selected with the middle button and the polygon is closed with the left hand button. The points in the resulting set are highlighted.

Confirm the set contents by rotating to a general view and viewing the two sets SYM and PRES. When two or more sets (or in general parts) are to be viewed together this can be achieved by use of `+'.

VIEW GEOMETRY YSYM

VIEW GEOMETRY +PRES

Apply the pressure load to the surfaces in set PRES and label the mesh with the pressure load. The load arrows will all be pointing into the solid part of the model. This is because the load is being applied to brick elements (where the convention is that a positive pressure acts in the direction of the inward normal to the body). As a comparison the user should label the normals for the surfaces in the set PRES.

The main constraints to be applied to the model are the symmetry constraints. In practice this means constraining the Y freedom for the nodes on the plane of symmetry. However it will also be necessary to constrain other parts of the structure so that the structure is sufficiently restrained. To do this create a set of the faces at the left hand end of the model and constrain the X freedom and finally choose a point on the plane of symmetry at the left hand end and restrain the Z freedom.

The mesh can be labelled with the constraints, check that the constraints are applied to the parts of the structure and in the correct direction.

Change the element type from the default of HE8 to HE20; the element type can be changed even at this stage in the model because the load, constraint etc. information is associated with the geometric parts rather than the mesh.

Check that the model data is correct by using a combination of UTILITY TABULATE,

LABEL GEOMETRY and LABEL MESH.

Write the input file in the required format using UTIL WRITE...

If required the user can mirror the geometry created so far to create a model of the complete object.

GEOM POINT C1 0 -62

will create a point to be used in defining the mirror plane.

CON TRAN MIR MIR1 P1 C1

will create a mirror transform, where the plane for mirroring is halfway between the two points chosen.

CONS SET HALF APPEND ALL

will create a set for the mirroring and

GEOM COPY HALF MIR1

will create the geometry for the mirrored half of the model. The meshing information is copied from the other half of the model and so a complete mesh can be readily generated. As an exercise the user should also determine what other information is copied from the original half of the model.

Figure 7.3: Mesh load and constraints display