6.3 The session

6.3 The session

Point and line input has already been dealt with in previous sections; it is assumed that the user will by now be able to create points and straight lines.

Step 1

Create the points and lines for the beam section

From the information given create the points and lines necessary to define the profile of the beam as below (using eight points and eight lines). The profile can be defined in any plane that the user requires but this example uses the X-Y plane for the profile and the Z axis for the span direction.

[00b.bmp]

Figure 6.1: The box girder

The next stages are to put all the lines defining the profile into a set, define a translation and then to sweep the profile to give the plate model of the beam.

Step 2

Rotate the view

Before doing this, rotate the view of the structure so that as the profile is swept the additional geometry can be seen. Views can be changed either by using EYE ROTATE or EYE DIRECTION, as shown:-

EYE DIRECTION 1 1 1

will give a general view of the model,

EYE ROT T 0

will rotate back to the initial 2D view.

E R R 40; E R U 40; E F

will rotate the viewer right by 40 degrees and up by 40 degrees and scale the view to fit the screen.

(Note that several commands can be combined on one line with the use of ";", this suppresses the redraw in between the two commands)

Step 3

Create a set to contain the 2D profile

Open a set and put into it all the geometry created so far. Finally close the set.

CONSTRUCT SET OPEN

The name of the open set will be included in the monitor box in the top left hand corner of the screen. The default name is SE1 as no specific name was given.

CONSTRUCT SET APPEND ALL

CONSTRUCT SET CLOSE

Step 4

Set the default for line divisions

All the lines joining the original shape and the new shape will have the default number of divisions for meshing. So change the default before these lines are created.

MESHING DIVISION DEFAULT 9

Step 5

Sweep set SE1

Sweep SE1 by 3000 units in the Z direction.

GEOMETRY SWEEP SE1 TR 0 0 3000

Note that the copy of the original part is put into the next available set SE2

Step 6

Scale the view

EYE FRAME

Step 7

Generate a mesh and view it

MESHING GENERATE

VIEW MESH ALL

Step 8

Change the element type and variant

Find out what type of elements are being used by either labelling the geometry or by tabulating the surface definitions. In this case it is required to use eight noded elements and so the element type needs to be QU8, but most finite element packages have more than one eight noded element and so it is necessary to decide which element variant is required. This is done by identifying which element in the fe package is to be used, then use UTILITY TABULATE FE package name which will give a table showing element type and variant number. Change the element type for the whole model to be eight noded quadrilaterals of variant type 3 (for example):

MESH TY ALL QU8 3

Step 9

Change the mesh density

Double the number of divisions on the lines to keep the same mesh density (in the same way as in the previous example).

Step 10

Show the line numbers

Go back to a view of the geometry and label the lines in order to create some sets :

VIEW GEOMETRY ALL

LABEL GEOMETRY LINES

Step 11

Zoom in

Zoom in now on the front of the model. To do this make two diagonally opposite cursor hits to define a box around the area to be enlarged.

EYE ZOOM IN

Step 12

Tabulate lines and sets

Tabulate the sets and the lines; note that SE2 contains the other end of the beam created by the sweep:

UTIL TAB SETS

UTIL TAB LIN SE1

UTIL TAB LIN SE2

Step 13

Re-scale the view

EYE FRAME

Step 14

Put all the swept lines into a set

Open a set called SLIN and append all the lines running along the length of the beam. Do this either by typing the commands below, or by using the cursor. The cursor can be used when the prompt CONSTRUCT SET APPEND LINE is seen; moving the cursor from the menu to the model area will show the 'picking' cursor, positioning this on the relevant line and using the left mouse button will add the line to the set. A similar technique can be used when the prompt is CONSTRUCT SET APPEND but to make sure that a line is selected rather than a point or a surface then "l" from the keyboard instead of the mouse button should be used (similarly if points are being selected then "p" should be used and so on for surfaces (s) and bodies (b)). If a wrong line is selected then this can be removed with CONSTRUCT SET REMOVE.

CONSTRUCT SET OPEN SLIN

CONSTRUCT SET APPEND L21

CONSTRUCT SET APPEND L22

CONSTRUCT SET APPEND L23

CONSTRUCT SET APPEND L24

CONSTRUCT SET APPEND L20 L19 L18 L17

CONSTRUCT SET CLOSE

Step 15

View just the last set

View the set independently to verify its contents:

VIEW GEOMETRY SLIN

Step 16

Bias the divisions along the beam

Increase the number of divisions on the lines in set SLIN to 12 and give a negative bias factor of 6:1. When the lines were swept, the command MESHING DIVISIONS DEFAULT could have been used set to -612 to automatically create 12 biased divisions on each of the swept lines.

MESHING DIVISION LINE SLIN -612

Step 17

Create the mesh and view it

MESHING GENERATE

VIEW MESH ALL

Step 18

Reduce the divisions across the top flanges

VIEW GEOMETRY ALL

LABEL GEOMETRY LINES

LABEL GEOMETRY DIV

MESHING DIVISION LINE L4 2

MESHING DIVISION LINE L6 2

MESHING DIVISION LINE L12 2

MESHING DIVISION LINE L14 2

MESHING GENERATE

Step 19

Label the surfaces

UTILITY TABULATE SETS

LABEL GEOMETRY SURFACES

Step 20

Define a set called FLAN

Open a set called FLAN and append the surfaces that form the beam flanges. The quickest way of doing this is to append all the entities to the set FLAN and then remove the unwanted surfaces S7 and S8 which are the webs

CONSTRUCT SET OPEN FLAN

CONSTRUCT SET APPEND ALL

CONSTRUCT SET REMOVE S7 S8

CONSTRUCT SET CLOSE

Check the contents of the set FLAN

VIEW GEOMETRY FLAN

Step 21

Create a set called WEB

CONSTRUCT SET OPEN WEB

CONSTRUCT SET APPEND S7 S8

CONSTRUCT SET CLOSE

VIEW GEOMETRY WEB

VIEW GEOMETRY ALL

Step 22

Zoom in on the original profile of the beam

Label the lines and zoom in on the bottom left hand end to get a better view of lines L1, L2 and L3:

LABEL GEOMETRY LINES

EYE ZOOM IN

The zoom operation is completed by using the cursor to define two diagonally opposite corners of a box that is to be scaled to fill the viewing area.

Step 23

Create a set called END for the support location

Open a set called END and append the three lines along the bottom edge of the profile, this set will be used for constraining the end of the beam:

CONSTRUCT SET OPEN END

CONSTRUCT SET APPEND L1 L2 L3

CONSTRUCT SET CLOSE

Check the contents of this set.

VIEW GEOMETRY END

(The set SE2 that was created as result of the sweep operation is on the plane of symmetry of the model and will subsequently be used to apply the symmetry constraints.)

Step 24

Rescale the view and zoom in to the other end.

VIEW GEOM ALL

EYE FRAME

EYE ZOOM IN

Step 25

Create a set called CENT for applying the loading

Open a set called CENT which will be used for applying the loading. Note the use of colour to identify the set:

CONSTRUCT SET OPEN CENT

CONSTRUCT SET APPEND L9 L11

CONSTRUCT SET CLOSE

VIEW GEOMETRY +CENT RED

EYE FRAME

Step 26

The PROPERTY menu

Having created a number of relevant sets for loading and constraints work down the PROPERTY menu, defining the material and physical properties, attach these to the relevant parts of the structure and then define the boundary and loading conditions.

Step 27

Define the material

Give the model material properties of mild steel for all parts. Use Young's Modulus of 2.1E5 N/mm² and Poisson's ratio of 0.3:

PROPERTY MATERIAL MAT MST 2.1E5 .29

Step 28

Define the thickness

Define thickness of 6mm and 15mm for the web and flange respectively:

PROPERTY PHYSICAL THICKNESS WEBT 6

PROPERTY PHYSICAL THICKNESS FLNT 15

Step 29

Attach the material and the physical properties

Attach material properties and physical properties to the relevant parts of the model.

PROPERTY ATTACH WEB MST WEBT

PROPERTY ATTACH FLAN MST FLNT

Step 30

CHECK

Re-scale and then check that the material and physical properties have been correctly allocated:

LABEL GEOMETRY MATER

LABEL GEOM PHYSICAL

Turn off the geometry labels.

LABEL GEO OFF

Step 31

Apply constraints

Apply symmetry constraints to the mid-span and simply support the end of the beam. To do this use the sets previously defined, SE2 and END.

PROPERTY BOUNDARY CONSTRAINT CO1 END PINNED

PROPERTY BOUNDARY CONSTRAINT CO3 SE2 Z RX RY

Step 32

Check the location and direction of the constraints.

LABEL MESH CONSTRNT

Step 33

Apply the load

Apply the loading downwards in the y-direction using the set CENT

PROPERTY LOADS PRES LO1 CENT -250 Y

The value of the distributed line load is calculated as half the total load divided by the distance over which it acts (50000*.5/100 = 250N/mm).

Switch off the constraint labels and check the location and the direction of the loading

LABEL MESH OFF

LABEL MESH LOADS

Step 34

Write an analysis file

If all is satisfactory write an output deck for the installed analysis package.

UTILITY WRITE FS2 girder.dat

If no filename is given as part of the UTIL WRITE command then the default filename will be GIRDER.ANL.

Step 35

Finish session

Finally stop the program, saving the current work and give a title for the model:

STOP

girder model