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 Y 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
Y
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
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
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
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.
Y
Write the file
w
(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
Y
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.