9.3 The session

9.3 The session

To model the above specimen, we will start by modelling one end of the specimen by intersecting analytical shapes. Once the external surface definition of one end is completed it will be mirrored to create the other end of the specimen. The two ends then joined together by sweeping a number of lines to complete the definition of the external surfaces that bound the specimen. The next stage is to create a general body that contains the whole specimen and then meshed with tetrahedral elements.

Finally, to complete the FEA model we define the required boundary conditions and load.

Step 1

Define geometry points required to create analytical shapes to create the geometry of one end

GEOMETRY POINT COORD P1 0

GEOMETRY POINT COORD P2 100

CONSTRUCT SHAPE CYLINDER CYL1 P1 P2 15

CONSTRUCT SHAPE PLANE PLX40 X 40

CONSTRUCT SHAPE PLANE PLZ0 Z 0

CONSTRUCT SHAPE PLANE PLX70 X 70

GEOMETRY POINT COORD P3 40 35

GEOMETRY POINT COORD P4 40 35 10

CONSTRUCT SHAPE CYLINDER CYLTOP P3 P4 30

GEOMETRY POINT COORD P5 40 -35

GEOMETRY POINT COORD P6 40 -35 10

CONSTRUCT SHAPE CYLINDER CYLBOT P5 P6 30

Step 2

View shapes in different colour

VIEW GEOMETRY +ALL

VIEW SHAPE +CYL1 YELLOW

VIEW SHAPE +PLZ0 VIOLET

VIEW SHAPE +CYLTOP BLUE

VIEW SHAPE +CYLBOT RED

VIEW SHAPE +PLX40 WHITE

VIEW SHAPE +PLX70 WHITE

[00j.bmp]

Figure 9.2: Define analytical shapes to create geometry

Step 3

Create geometry surfaces by intersecting shapes

GEOMETRY SURFACE INTERSECT CYL1 PLZ0 -CYLTOP -CYLBOT +PLX40

-PLX70

The above command will create two surfaces based on shape CYL1 on both sides of the plane shape PLZ0 and it will be limited by taking the two cylindrical shape (CYLTOP and CYLBOT) off and also limited by the positive and negative sides of the plane shapes PLX40 and PLX70 respectively.

Now do the same thing to create the required surfaces at the top and bottom of the specimen end

GEOMETRY SURFACE INTERSECT S3 CYLTOP +CYL1 +PLX40 PLZ0

GEOMETRY SURFACE INTERSECT S5 CYLBOT +CYL1 +PLX40 PLZ0

VIEW GEOMETRY +ALL

Step 4

Complete the surface definition of the above part by creating a regional surface containing the two arc lines at the edge of the specimen

CONSTRUCT SET OPEN END

CONSTRUCT SET APPEND L9 L10

CONSTRUCT SET CLOSE

GEOMETRY SURFACE REGION S7 END

Step 5

Adjust line divisions

MESHING DIVISION L3 408

MESHING DIVISION L4 -408

MESHING DIVISION L5 408

MESHING DIVISION L6 -408

MESHING DIVISION L9 8

MESHING DIVISION L10 8

VIEW GEOMETRY ALL

Step 6

Copy a mirror image of one end to the other end.

Start by creating a mirroring transform, include all the surfaces into a set, then copy the set.

GEOMETRY POINT COORD PM1 100

GEOMETRY POINT COORD PM2 -100

CONSTRUCT TRANSFRM MIRROR TR1 PM1 PM2

CONSTRUCT SET OPEN END1

CONSTRUCT SET APPEND SURFACES ALL

CONSTRUCT SET CLOSE

GEOMETRY COPY END1 END2 TR1

VIEW GEOMETRY ALL

Step 7

Join the two ends to complete the surface definition of the specimen. This is achieved by sweeping a number of lines at one end.

LABEL GEOMETRY LINES

CONSTRUCT SET OPEN END3

CONSTRUCT SET APPEND L7 L8 L11 L12 L15 L14

CONSTRUCT SET CLOSE

To calculate the required transform, measure the distance between the two ends and use it to sweep the lines.

UTILITY MEASURE DISTANCE P13 P23

GEOMETRY SWEEP END3 SE6 TRANSLATE TR2 -80

EYE FRAME ALL

LABEL GEOMETRY OFF

Step 8

Two surfaces (S15 & S16) created in step 6 are not planar and needs to be projected into the cylindrical shape CYL1

MESHING SHAPE S15 CYL1

MESHING SHAPE S16 CYL1

Step 9

At this stage we have completed the definition of the bounding surfaces of the specimen and we can create a general body, however, before doing that it is worth generating a surface mesh with triangular elements to give us an idea about what the skin of the tetrahedral elements will look like. This is done because the tetrahedral elements will respect the surface mesh and will use it as seeds to the tetrahedral elements.

MESHING OPTIONS ALGORITHM DELAUNAY ALL

MESHING DIVISION ELSIZE ALL 4

MESHING GENERATE

EYE DIRECTION 1 1 1

EYE FRAME ALL

VIEW MESH

Step 10

Create a general body by including all the bounding surfaces of the specimen into a set, then issue the command GEOMETRY BODY GENRAL setname as follows:

CONSTRUCT SET OPEN OUTER

CONSTRUCT SET APPEND SURFACES ALL

CONSTRUCT SET CLOSE

(you can also use: CONSTRUCT SET OUTER APPEND SURFACES ALL)

GEOMETRY BODY GENERAL B1 OUTER

VIEW GEOMETRY B1

Step 11

Generate tetrahedral elements

MESHING GENERATE B1

VIEW MESH

VIEW HIDDEN SHADE

VIEW HIDDEN OFF

As you can see, the default element type for the general body B1 is TE4 and if you tabulate B1 you will find that the tabulation tells us that it has used a set called OUTER to create the general body and 9707 new TE4 elements was generated

UTILITY TABULATE GEOMETRY B1

[00k.bmp]

Figure 9.3: The specimen with tetrahedral mesh


Step 12	Define material properties and loading using the property manager option available under the <Tool> option within the tool bar as shown in the figure below:

[00l.bmp]

Figure 9.4: Property manager form to define material properties and loading

To define steel material properties select <Material> then click on the <Add> button. This will add a new field that allow you to type in the appropriate material properties in the right field

(alternatively you can use the command line option to add material properties using the command PROPERTY MATERIAL…..).

In order to define force at one end of the specimen you can use the property manager form again as follows:

Select <Load> then <Force>

Choose <Add> to add force

Edit the definition of the new force by typing a new force name, part name, force value and direction.

When finished click on the <Ok> button to accept the new definition of material properties and load.

(you can also define force using the command PROPERTY LOAD FORCE name part value dof).

Now attach the steel property to the model using the command:

PROPERTY ATTACH ALL STEEL

Step 13

Apply boundary constraints by fixing the other end of the specimen in the X, Y and Z translations

PROPERTY BOUNDARY CONSTRAINT CO1 S14 123

Step 14

Label the material properties, constraints and load

LABEL MESH MATERIAL

LABEL MESH CONSTRNT

LABEL MESH LOAD

Step 15

Create an analysis input deck

UTILITY WRITE ……………

That’s the end of this session. At this stage a file has been created which can be used for analysing the model.