2.3 The session

2.3 The session

When using the mouse, please use the left mouse button to select menu items.

Step 1

Start FEMGV

Step 2

Access FEMGEN with the name of TRAIN1

FEMGEN TRAIN1

Step 3

Create some points

GEOMETRY POINT COORD P1 0

GEOMETRY POINT COORD P2 1

GEOMETRY POINT COORD P3 1 .8

Scale the view to contain the points

EYE FRAME ALL

Step 4

Create some more points

Here's a mistake

GEOMETRY POINT COORD P4 0 .08

Point P4 is the fourth corner but it's in the wrong place!

Correct it by redefining it.

GEOMETRY POINT COORD P4 0 .8

Confirm the change of location of the point

Continue to define the rest of the points

GEOMETRY POINT COORD P5 .5 .4

GEOMETRY POINT COORD P6 .6 .5

GEOMETRY POINT COORD P7 .6 .3

GEOMETRY POINT COORD P8 .4 .3

GEOMETRY POINT COORD P9 .4 .5

Step 5

Create lines to define the shape

GEOMETRY LINE STRAIGHT L1 P1 P2

GEOMETRY LINE STRAIGHT L2 P2 P3

GEOMETRY LINE STRAIGHT L3 P3 P4

Here's another mistake

GEOMETRY LINE STRAIGHT L4 P4 P2

Delete this line and then re-enter the line

UTILITY DELETE LINE L4

Confirm the deletion

Continue with the line creation

GEOMETRY LINE STRAIGHT L4 P4 P1

GEOMETRY LINE ARC L5 P6 P7 P5

GEOMETRY LINE ARC L6 P7 P8 P5

GEOMETRY LINE ARC L7 P8 P9 P5

GEOMETRY LINE ARC L8 P9 P6 P5

Label the lines in the model.

LABEL GEOMETRY LINES

[002.bmp]

Figure 2.2: The lines created so far

Step 6

Define the surface

Create a region by creating two sets representing the plate and the hole respectively. The surface is then created by subtracting the second set from the first one.

CONSTRUCT SET OPEN PLATE

CONSRUCT SET APPEND L1 L2 L3 L4

CONSRUCT SET CLOSE

CONSTRUCT SET OPEN HOLE

CONSTRUCT SET APPEND L5 L6 L7 L8

CONSTRUCT SET CLOSE

GEOMETRY SURFACE REGION S1 PLATE HOLE

Show the surface that has been created.

LABEL GEOMETRY SURFACES

Find out how the surfaces are defined by tabulating them.

UTILITY TABULATE GEOMETRY SURFACES

Step 7

Create the mesh

Check and change line divisions for more refined mesh

VIEW GEOMETRY ALL

LABEL GEOMETRY DIVISION

LABEL GEOMETRY LINE

MESHING DIVISION LINE L2 8

MESHING DIVISION LINE L4 8

MESHING DIVISION LINE L3 10

MESHING DIVISION LINE L1 10

Generate the mesh.

MESHING GENERATE

And view it.

VIEW MESH

[003.bmp]

Figure 2.3: The final mesh as displayed by VIEW MESH

Step 8

Define materials and physical properties

Look at the geometry.

VIEW GEOMETRY ALL

Label the lines

LABEL GEOMETRY LINES

Define material properties (Young's Modulus, Poisson's Ratio and Density).

PROPERTY MATERIAL MA STEEL 209E9 .3 7900

Define the plate thickness.

PROPERTY PHYSICAL TH THICK .012

Attach the properties just defined to all of the structure.

PROPERTY ATTACH ALL STEEL THICK

Step 9

Apply the load

Create a load on the edge of the plate

(on line L2, value 123 units, normal to the edge of the plate).

PROPERTY LOADS PRES L2 123 X

Show the load just defined.

LABEL MESH LOADS

However, the load is in the wrong direction! So re-define the load direction

PROPERTY LOADS PRES L2 -123 X

Check that the load direction has changed.

(Note that if using ABAQUS please use PROPERTY LOADS PRES L2 123 0 in order to define load normal to elements ).

Step 10

Apply constraints

Fix the model to stop it moving.

PROPERTY BOUNDARY CONSTRAINT L4 X Y Z

Show the constraints and check them.

LABEL MESH CONS

[004.bmp]

Figure 2.4: The loads and constraints defined on the model

Step 11

Define an element type

For some analysis packages the default element type is not appropriate for this analysis, and so it is necessary to request a plane stress element in the analysis input file.

Analysis Package	Command
ABAQUS	MESHING TYPES ALL QU4 6
ANSYS	MESHING TYPES ALL QU4 3
FEMSOL II	No action required
FINEL	No action required
NASTRAN	No action required
PAFEC	No action required

Step 12

Create an analysis input deck

Choose the command relevant to your analysis package.

Analysis Package	Command
ABAQUS	UTILITY WRITE ABAQUS train1.inp
ANSYS	UTILITY WRITE ANSYS train1.inp
FEMSOL II	UTILITY WRITE FS2
FINEL	UTILITY WRITE FINEL
NASTRAN	UTILITY WRITE NASTRAN
PAFEC	UTILITY WRITE PAFEC train1.dat
etc	Etc

Confirm file creation.

Write the file

(In this example the analysis input file created is `train1.inp', certain analysis packages may require specific filename extensions, in which case the user should give the relevant extension. If no filename is given the default of `MODELNAME'.ANL will be used.)

Step 13

Stop the program

Stop!

STOP

Confirm saving of data

Give a title for the model to be saved.

Beginning FEMGEN

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