Once FEMGV is running, start the modelling session by typing

This will initiate FEMGEN with a model name of LUG. A workbox of approximately the size of the item being modelled can be created; this has the effect of scaling the view and checking dimensions as they are entered. In this case the command:

CONSTRUCT SPACE WORK-BOX 30 80 will be sufficient.

If the user does not define a workbox then the points will only be shown on the screen, if they are within the default scaling for the screen (as seen in the Getting Started section). To rescale the model the command EYE FRAME is used.

These are points needed to define the basic outline of the structure. No point names are specified and so they are generated automatically starting with P1.

GEOMETRY POINT COORD 0

GEOMETRY POINT COORD 20

GEOMETRY POINT COORD 20 27 .64

GEOMETRY POINT COORD 30 50

GEOMETRY POINT COORD 0 80

GEOMETRY POINT COORD 0 60

GEOMETRY POINT COORD 10 50

GEOMETRY POINT COORD 0 40

GEOMETRY POINT COORD 0 20

The next command will create a point at the centre of the arcs and for clarity it is given a specific name.

GEOMETRY POINT COORD C1 0 50

All the points needed for the definition of the shape now exist. The next step is to define the lines and surfaces to enable a mesh to be created. Arcs are defined with two end points and the centre.

GEOMETRY LINE P3 P4 C1

GEOMETRY LINE P4 P5 C1

GEOMETRY LINE P6 P7 C1

GEOMETRY LINE P7 P8 C1

GEOMETRY LINE P5 P6

GEOMETRY LINE P4 P7

GEOMETRY LINE P8 P9

In the same way as point names, line names are allocated automatically if no name is specified.

Surfaces are defined by closed loops of three or four lines. FEMGEN allows a surface to be created by defining three or four lines OR by defining the three or four vertices of the boundary being defined. If lines already exist between the points then these will be used, if not, then new lines will be created. Both methods of defining boundaries will be used in this example.

GEOMETRY SURFACE 4POINTS P1 P2 P3 P9

creates a surface as well as the four lines needed to define it.

Figure 5.2: Lines and points created so far

The adjacent region in the model has five sides and as such could not be a valid FEMGEN surface. The solution to this is to make a combined line from lines L10 and L1.

GEOMETRY LCMB LC1 L10 L1

This is a very useful technique and combined lines can be defined by a maximum of four ordinary lines. However, their use should be restricted to plate and shell structures only. There are a number of potential pitfalls which can be encountered if combined lines are used in three dimensional solid models.

GEOMETRY SURFACE 4SIDES LC1 L6 L4 L7

GEOMETRY SURFACE 4POINTS P7 P4 P5 P6

Each line that has been created has automatically been allocated four divisions, which is the default. (To change the default use MESHING DIVISION DEFAULT ). A mesh can now be created and viewed.

MESHING GENERATE

VIEW MESH

LABEL MESH QUALITY will check the resulting mesh. (See also the mesh quality section).

The transition mesh that is seen on surface 2 is caused by the inner arc having four divisions, whereas the combined line has a total of eight divisions. The ability to have unequal divisions on opposite sides of surfaces is very useful in the situation where a reduction in mesh density is required; however a smooth mesh is required in this case, so to get a smoother, finer mesh.

VIEW GEOMETRY +ALL

adds the geometry to the current picture.

LABEL GEOMETRY LINES

LABEL GEOMETRY DIV

labels the lines for identification and shows the current division settings.

Change the number of divisions on L4 to 8 and do the same for lines L3 and L2. (Note that as soon as any information used in generating the mesh is changed, the mesh is deleted so that the geometry and the mesh are always consistent.)

MESHING DIVISION LINE L4 8

MESHING DIVISION LINE L3 8

MESHING DIVISION LINE L2 8

Because the stress gradients near the hole will be greater than elsewhere in the model it is a good idea to bias the elements towards the hole.

MESHING DIVISION LINE L5 -204

MESHING DIVISION LINE L6 -204

MESHING DIVISION LINE L7 204

This will have the effect of making the divisions along these lines smaller near the start of the line and bigger (by a ratio of 2) at the end of the line. On the geometry the line name is positioned nearer the start of the line. Lines L5 and L6 have a negative value because of the orientation of the line.

Confirm that these changes have been made

DRAWING DISPLAY

MESHING GENERATE

VIEW MESH

The mesh created so far consists of four noded elements (which is the default for a four sided surface). To change to eight noded elements which will be better for this type of analysis

MESHING TYPES ALL QU8

(Note that the mesh has again been deleted).

Because QU8 elements have midside nodes the FEMGV treats the elements as having two divisions and so to keep the same number of elements the number of divisions on each line must be doubled.

MESHING DIVISION FACTOR ALL 2

MESHING GENERATE

VIEW MESH

At this stage a reasonable mesh has been created and so the next stage is to define the additional information that will be required for the analysis.

VIEW GEOMETRY ALL

LABEL GEOMETRY LINES

Figure 5.3: The final mesh with loads and constraints

The finite element model is one half of the actual object and consequently it is necessary to constrain the nodes on the line of symmetry to behave in a symmetric manner. This could be done by constraining each line individually but a far better way is to collect the relevant lines together in a set and then apply the constraints to the set. Sets are a means of collecting `parts' of the model together for a number of purposes (as will be seen later).

CONSTRUCT SET OPEN FIX

CONSTRUCT SET APPEND L5 L7 L11

CONSTRUCT SET CLOSE

The first item on the menu is FE-PROG which is not relevant in this case. (It is required when an analysis specific environment is available e.g. for ASAS, ABAQUS, PHOENICS, BEASY)

PROPERTY MATERIAL MA STEEL 209E3 .3 7800E-12

will define the Young's Modulus, Poisson's Ratio and density for a material called STEEL. The values used are those for Newtons and millimetres. If the user chooses not to work with S.I. units (i.e. metres and Newtons) then it is very important that consistent units are used or strange results will be obtained. The user should refer to the finite element user manual for further details.

Create a physical thickness property called PLATE1

PROPERTY PHYSICAL TH PLATE1 12.5

The material and the thickness have been defined, now they must be attached to the relevant parts of the structure (the complete model, in this case).

PROPERTY ATTACH ALL STEEL PLATE1

Continuing to move down the property menu, now specify the boundary conditions on the model. In this case, it is assumed as part of the modelling process, that the structure and loading are symmetric. The implication of this is that the nodes on the vertical line of symmetry must be prevented from moving across the line. The directions to be fixed are identified by numbers; 1, 2, 3, 4, 5, 6 corresponding to X, Y, Z, RX, RY, RZ respectively, all directions (freedoms) are fixed by using 9. In this case because plane stress elements are being used only X and Y freedoms will be available.

PROPERTY BOUNDARY CONSTRAINT CO1 FIX X

Also constrain the bottom of the model

PROPERTY BOUNDARY CONSTRAINT CO2 L8 Y

The load on the complete structure is 1500N therefore 750N needs to be applied to the finite element model.

PROPERTY LOADS PR LO1 L3 75 NORMAL

will create a load called LO1 which will apply a pressure load of 75N/mm² normal to line L3. (When resolved in the vertical direction and allowing for material thickness this will give 750N.) Similarly,

PROPERTY LOADS FOR LO2 2 P6 750 Y

will apply a point load of 750N to point P6 acting in the Y direction, the load name is LO2 and the loadcase number is 2.

Check that loads and constraints are applied in the correct directions.

LABEL MESH CONSTRNT

LABEL MESH LOAD

If the plate were being analysed by hand then it would be necessary to define the size and shape of the object, the loading, the material, the thickness and the boundary conditions. The same information is still required for f.e.; it has been defined and so the analysis can proceed.

A FEMSOL-II file for analysis can be written, this ascii file will contain all the relevant information required for the finite element analysis.

UTILITY WRITE FS2 lug.anl

Y

STOP

Save the work from this session.

Y

Give a relevant description:

simple 2d lug

The user can examine (and with experience modify) the finite element input file using an editor.

The pre-processing is now complete and the analysis should be run, using your analysis package.

The user should also check the output file for any warning messages and to ensure that the correct loads have been applied and that the reactions match the applied load.

Provided that the analysis has been successful then a file will exist called LUG.FVI which contains the model information as well as all the calculated results and it is this file which needs to be accessed in FEMVIEW to display the results.

Run FEMGV again, the first thing to do is to read in the .fvi file.

UTILITY READ VIEWDATA lug.fvi

this will create a FEMVIEW database file for the model containing the necessary information for viewing, and will also record in the database index file that viewdata for the model exists.

FEMV lug

will access the FEMVIEW environment and display the outline of the model.

There is a very wide range of operations that the user can perform to display results. However, before any of these can be performed the user needs to identify the loadcase that is to be considered.

In order to check on the names of the loadcases in the current model issue the command:

UTILITY TABULATE LOADCASES

which will list all the loadcases in the analysis. In this example there are only two loadcases.

Knowing the name of the load case(s) the user must select which loadcase is to be viewed.

RESULTS LOADCASE LC0001

It is usual to first check the displacements of the model. To do this select the appropriate attribute and component of nodal results:

RESULTS NODAL DISPLACE ALL

will select the resultant displacements at nodes for subsequent plotting.

PRESENT SHAPE

will show the original and the deflected outline. Check that the displacement is in the correct direction. If it is not then the loading will have to be modified and the analysis re-run.

PRESENT PEAKS

will show the positions of the maximum and minimum values of the resultant deflection and give the numeric values in the monitor box.

VIEW MESH

will show the full mesh and

PRESENT SHAPE

will superimpose the deformed mesh.

In some circumstances it may be clearer to show the undeformed shape as an outline and the deformed shape as a complete mesh. This is achieved by :

VIEW OPTIONS EDGES OUTLINE

It is now easier to identify the deformed shape.

Having looked at the deformed shape, the next stage is to consider the stresses. With FEMSOL the user has access to both the elemental stresses and the nodally averaged stresses. he averaged stresses are often used for post processing assessment purposes but the process of averaging will hide stress discrepancies at nodes which can result from an inadequate mesh. Plotting the unaveraged stresses will show any discrepancies across element edges enabling the user to make an assessment of the quality of the stresses calculated.

RESULTS ELEMENT STRESS SYY

will select the elemental stresses in each element in the global YY direction.

PRESENT CONTOURS LEVELS 10

will display the elemental YY stress contours. The contours obtained show only a few small discontinuities which indicates that this mesh is quite reasonable.

VIEW OPTIONS EDGES ALL

will switch back on the full mesh.

Other stress types can be plotted. To plot the averaged nodal stresses select the component required (XX stress in this case) and then display it:

RESULTS NODAL STRESS SYY

PRESENT CONTOUR LEVELS 10

Similarly the user can display any of the stress components available as contours. Additionally Von Mises or Tresca equivalent stresses can be displayed. The PRESENT menu shows the options available for displaying the stress values being considered. The ability to present numeric values using the command PRESENT NUMERIC will be useful for post processing tasks relating to, say, fatigue or yield etc.

The user can obtain a graph showing the variation along a line (which need not be straight) of any parameter that is available for plotting; for example this could show how the displacement or stress varies along one edge of the model being considered. Assuming that the mesh is displayed, then this is done by:

CONSTRUCT LINE NODE THROUGH /PICK

The user points at the two nodes defining a straight line along which the variation of the current parameter is to be displayed. If the line is not straight then CONSTRUCT LINE NODE LIST /PICK can be used to select the nodes to define the line. The selection of nodes is completed by selecting the same node twice.

It is suggested that the user should select a line of nodes around the inside of the hole.

PRESENT GRAPH LINE OLD

will show the graph.

STOP

Y