(a) Badly ordered elements (b) Well ordered elements

Fig. 9.15. Examples of element ordering for frontal method.

9.4.7. Application of boundary conditions

Having created a mesh of finite elements and before the job is submitted for solution, it is necessary to enforce conditions on the boundaries of the model. Dependent upon the application, these can take the form of

• structural loads,

• heat transfer loads, or

• specification of active and inactive dof.

Attention will be restricted to a brief consideration of restraints and structural loads, which are sufficient conditions for a simple stress analysis. The reader wishing for further coverage is again urged to consult the many specialist texts.1-10


Restraints, which can be applied to individual, or groups of nodes, involve defining the displacements to be applied to the possible six dof., or perhaps defining a temperature. As an example, reference to Fig. 9.3(b) shows the necessary restraints to impose symmetry conditions. It can be assumed that the elements chosen have only 2 dof. per node, namely u and v translations, in the x and y directions, respectively. The appropriate conditions are along the x-axis, v = 0, and along the y-axis, u = 0.

The usual symbol, representing a frictionless roller support, which is appropriate in this case, is shown in Fig. 9.16(a), and corresponds to zero normal displacement, i.e. S„ — 0, and zero tangential shear stress, i.e. r, = 0, see Fig. 9.16(b).

In a static stress analysis, unless sufficient restraints are applied, the system equations (see §9.4.5), cannot be solved, since an inverse will not exist. The physical interpretation of this is that the loaded body is free to undergo unlimited rigid body motion. Restraints must be

(a) Symbolic representation (b) Actual restraint

Fig. 9.16. Boundary node with zero shear traction and zero normal displacement.

chosen to be sufficient, but not to create rigidity which does not exist in the actual component being modelled. This important matter of appropriate restraints can call for considerable engineering judgement, and the choice can significantly affect the behaviour of the model and hence the validity of the results.

Structural loads

Structural loads, which are applied to nodes can, through usual program facilities, be specified for application to groups of nodes, or to an entire model, and can take the form of loads, temperatures, pressures or accelerations. At the program level, only nodal loads are admissible, and hence when any form of distributed load needs to be applied, the nodal equivalent loads need to be computed, either manually or automatically. One approach is to simply define a set of statically equivalent loads, with the same resultant forces and moments as the actual loads. However, the most accurate method is to use kinematically equivalent loads5 as simple statically equivalent loads do not give a satisfactory solution for other than the simplest element interpolation. Figure 9.17 illustrates the case of an element with a quadratic displacement interpolation. Here the distributed load of total value W, is replaced by three nodal loads which produce the same work done as that done by the actual distributed load.

Total load W

(a) Actual uniformly distributed load (b) Kinematically equivalent nodal loads

Fig. 9.17. Structural load representation.

9.4.8. Creation of a data file

The data file, or deck, will need to be in precisely the format required by the particular program being used; although essentially all programs will require the same basic model data, i.e. nodal coordinates, element type(s) and connectivity, material properties and boundary conditions. The type of solution will need to be specified, e.g. linear elastic, normal modes, etc. The required output will also need to be specified, e.g. deformations, stresses, strains, strain energy, reactions, etc. Much of the tedium of producing a data file is removed if automatic data preparation is available. Such an aid is beneficial with regard to minimising the possibility of introducing data errors. The importance of avoiding errors cannot be overemphasised, as the validity of the output is clearly dependent upon the correctness of the data. Any capability of a program to detect errors is to be welcomed. However, it should be realised that it is impossible for a program to detect all forms of error, e.g. incorrect but possible coordinates, incorrect physical or material properties, incompatible units, etc., can all go undetected. The user must, therefore, take every possible precaution to guard against errors. Displays of the mesh, including "shrunken" or "exploded" element views to reveal absent elements, restraints and loads should be scrutinised to ensure correctness before the solution stage is entered; the material and physical properties should also be examined.

9.4.9. Computer, processing, steps

The steps performed by the computer can best be followed by means of applications using particular elements, and this will be covered in §9.7 and subsequent sections.

9.4.10. Interpretation and validation of results

The numerical output following solution is often provided to a substantial number of decimal places which gives an aura of precision to the results. The user needs to be mindful that the fem. is numerical and hence is approximate. There are many potential sources of error, and a responsibility of the analyst is to ensure that errors are not significant. In addition to approximations in the model, significant errors can arise from round-off and truncation in the computation.

There are a number of checks that should be routine procedure following solution, and these are given below

• Ensure that any warning messages, given by the program, are pursued to ensure that the results are not affected. Error messages will usually accompany a failure in solution and clearly, will need corrective action.

• An obvious check is to examine the deformed geometry to ensure the model has behaved as expected, e.g. Poisson effect has occurred, slope continuity exists along axes of symmetry, etc.

• Ensure that equilibrium has been satisfied by checking that the applied loads and moments balance the reactions. Excessive out of balance indicates a poor mesh.

• Examine the smoothness of stress contours. Irregular boundaries indicate a poor mesh.

• Check inter-element stress discontinuities (stress jumps), as these give a measure of the quality of model. Large discontinuities indicate that the elements need to be enhanced.

• On traction-free boundaries the principal stress normal to the boundary should be zero. Any departure from this gives an indication of the quality to be expected in the other principal stress predictions for this point.

• Check that the directions of the principal stresses agree with those expected, e.g. normal and tangential to traction-free boundaries and axes of symmetry.

Results should always be assessed in the light of common-sense and engineering judgement. Manual calculations, using appropriate simplifications where necessary, should be carried out for comparison, as a matter of course.

9.4.11. Modification and re-run

Clearly, the need for design modification and subsequent fe. re-runs depends upon the particular circumstances. The computational burden may prohibit many re-runs. Indeed, for large jobs, (which may involve many thousands of dof. or many increments in the case of non-linear analyses), re-runs may not be feasible. The approach in such cases may be to run several exploratory crude models to gain some initial understanding how the component behaves, and hence aid final modelling.

Regardless of the type of structure to be analysed, irrespective of whether the loading is static or dynamic, and whatever the material behaviour may be, there are only three types of argument to be invoked, namely, equilibrium, compatibility and stress!strain law. Whilst these arguments will be found throughout this text it is worthwhile giving them some explicit attention here as a sound understanding will help in following the theory of the fem. in the proceeding sections of this chapter.

9.5.1. Equilibrium

External nodal equilibrium

Static equilibrium requires that, with respect to some orthogonal coordinate system, the reactive forces and moments must balance the externally applied forces and moments. In fea. this argument extends to all nodes in the model. With reference to Fig. 9.18, some nodes may be subjected to applied forces and moments, (node number 4), and others may be support points (node numbers 1 and 6). There may be other nodes which appear to be neither of these (node numbers 2, 3, and 5), but are in fact nodes for which the applied force, or moment, is zero, whilst others provide support in one or two orthogonal directions and are loaded (or have zero load), in the remaining direction(s) (node number 6). Hence, for each node and with respect to appropriate orthogonal directions, satisfaction of external equilibrium requires

9.5. Fundamental arguments external loads or reactions = summation of internal, element, loads

Fig. 9.18. Structural framework.

Nodes 1 & 6: Support nodes Node 4: Loaded node Nodes 2.3 & 5: Unloaded nodes

Fig. 9.18. Structural framework.

Then, for the yth node e=l where the summation is of the internal loads at node j from all m elements joined at node j.

Use of this relation can be illustrated by considering the simple frame, idealised as planar with pin-joints and discretised as an assemblage of three elements, as shown in Fig. 9.19. The nodal force column matrix for the structure is

Node number

Node number

Fig. 9.19. Simple pin-jointed plane frame.

Dof. numbers

Fig. 9.19. Simple pin-jointed plane frame.

and the element force column matrix for the structure is

{5} = {{S^HS^HS^}} = {UiVtUiVi, u2v2u3v3, U,VXU3V3)

It follows from the above that external, nodal, equilibrium for the structure is satisfied by forming the relationship between the nodal and element forces as i/r v, u2

0 0

Post a comment