.png){kind=small}
= .png){kind=small}
= .png){kind=small}
= 0Verifying the results of an FE analysis
A significant part of the power of any finite element analysis is the ability to model and analyse more complex structural geometries than would be achievable by more traditional manual calculation or wireframe modelling methods. But as the complexity of the structural form increases the more likely that the behaviour of the structure also becomes more complex and load paths may be less obvious. In this case, the need to validate the results becomes even more important, not only to prove results are correct, but equally important to identify parts of a model where the results are incorrect. Validation can also assist in identifying areas of the model where the behaviour is not as expected or intended.
There is no set method or algorithm for checking a model, but the following steps provide a basis for any validation exercise.
A vital step in the validation process of any model is to view the deflected shape of the structure under a range of loadcases. This can be done using the Graphical Analysis Results for the Line Elements, which will show the deformed shape of FE surfaces as well as line elements. For a validation exercise, the shape of the deformations are likely to be as important, if not more so, than the values of the deflection; the value of deflection will be of more importance in the next stage of checking and particularly at the detailed design stage.
When viewing the deflected shape, it can be useful to increase the magnification to exaggerate the deflected shape. While seemingly trivial, the following typical visual checks can provide clues to aspects of the model that require further review:
Are slabs showing sagging deflections in areas that would be expected to sag such as mid spans of slabs?
Are parts of the model deflecting excessively relative to adjacent parts of the model?
Are elements that would be expected to be in compression showing a shortening under load
Are parts of the structure that would be expected to deflect showing no deflections?
Are parts of the structure, or indeed the whole structure, showing excessive deflections under lateral loads?
A review of the deflected shape can assist in identifying potential problems such as loading being applied in the wrong direction or areas with incorrect restraint conditions, such as too many member releases or missing support conditions. It is best thought of as a qualitative check to identify potential areas for further investigation rather than a quantitative check.
The above points are equally applicable to a wireframe model as an FE model. When dealing with FE surfaces, it can be helpful to review both the overall behaviour of the model as a global entity and then to focus on specific FE surfaces by filtering the view to specific surfaces or areas of the model.
For all models in static equilibrium the following conditions must hold:
= = = 0
And
.png){kind=small}
= .png){kind=small}
= .png){kind=small}
= 0
A first stage check on any model should then be to review the support reactions versus the self-weight and applied loading on the model. The total reaction for each load can be viewed by going to Results>Tabular Analysis Results and viewing the support reactions. The total for each reaction is given at the foot of the table.
For initial checks, the total reaction for self-weight and imposed load should be carried out. This need not necessarily require a very detailed assessment of self-weight or an exact calculation of imposed load. A reasonable estimate of both loads is usually satisfactory to check that the total reactions from the analysis are of the correct magnitude.
Checking individual reaction forces is often more difficult, particularly as the geometry of the structure becomes more complicated. As for the overall loads, for checking purposes an estimate of the reaction forces is usually adequate for the validation process. Thus, in most cases attributing load on the basis of a simplified area of supported structure will usually give an indication if the results are of the correct magnitude and orientation.
Confirming reaction forces is simpler for nodal supports than is the case when dealing the FE surface edge restraints since nodal supports are explicitly given as part of the MasterFrame results. This is not the case for FE edge restraints and the FE surface results will need to be used. The used of line diagrams can often be more helpful than interpreting the results from a contour plot.
A first stage check is not aimed at identifying parts of a structure which are not satisfactory and require a modification to the structure to resolve, nor to identify the required reinforcement in concrete elements. This type of detailed design check is part of the design stage. The initial checks are carried out with the purpose of ensuring that the returned results are sensible, with the correct magnitude and orientation. As with the support reactions, an estimate of the results, say using standard formula based on a simplified geometry to determine representative spans, will generally be adequate to identify the correct magnitude of forces or stresses as required by a validation check.
In most structures it may be more convenient to check the magnitude and sign of bending moments, but there is no difference between checking forces or stresses and in some materials, it may be more convenient to use stresses.
The presence of peak values of forces or stresses due to either stress concentrations or singularities within the FE surface will lead to localised areas of high stresses and forces which can complicate the initial process of model results validation. In the first stage of validation of the model, it may be desirable to carry out checks in areas not affected by the presence of stress concentrations or singularities as an initial assessment.
For validation checks on specific parts or areas of a structure, while the contour plots give a good indication of the results in 2D, the use of FE section diagrams can be helpful in looking at results on specific lines in a format that is more similar to usual shear force and bending moment diagrams. Line diagrams can also be displayed with strip averaging active and this can aid in averaging out, to a degree, the effects of peak values. Refer to the Results chapter for more information on viewing section diagrams.
Whether in the form of nodal supports, spring supports or applied as FE Surface edge restraints, the behaviour of a model is highly influenced by the defined restraint conditions. Support conditions determine how and where the reaction forces are developed and so influence the load path, deflected shape and the forces generated in the model. A crucial stage of any validation process is, therefore, to review the applied supports and restraint conditions on the model. This applies equally to a wireframe model as to a FE model.
Nodal supports can be reviewed either graphically or by reviewing the nodal supports definition area. FE surface edge restraints are often easiest to review graphically, by going to Display Options drop down and expanding the Finite Element Display Options and selecting the Label Continuous Supports option.
.png)
Given the influence of the support conditions on the analysis results, the effect of applied restraints can also be reviewed by examining the deflected shape of the structure and the analysis results. Areas with much less deflection than expected or, conversely, areas with excessive deflections, are likely to indicate localised issues with restraint conditions. Large moments at locations where the bending would be expected to be zero may indicate either rotational restraints or continuity where the structure should be pinned.
The accuracy of an FE analysis is generally related to the mesh size. However, simply using a small mesh everywhere is not effective, since the analysis time will be significantly increased and for areas where the rate of change of results is low, the increase in analysis time is not leading to a real increase in accuracy. It is more important to ensure that the mesh size is appropriate to the rate of change in the results and that smaller mesh sizes are used in areas of high stress concentration.
As part of an initial validation check, the contour outputs can be used, either in a flat map form or using a 3D contour map, to identify areas with high stress concentrations, usually associated with areas where the contours are close together indicating a large rate of change in the results. This can then be used to identify areas where the mesh size may need to be refined or reduced locally.
In terms of identifying an appropriate mesh size, there are no clear or definitive rules and to some degree the mesh size is influenced by the underlying formulation of the finite elements. One approach is to run the model initially with a coarse mesh and review the effect on the results as the mesh size is decreased. As the change in the results reduces to a small percentage of the previous run, confidence can be gained that the mesh size is appropriate.
It is important to note that when carrying out an FE analysis, the analysis results are calculated at the node points and at selected points (Gaussian points) within each element, but the distribution of the results between these points is estimated using the elements shape function. So, the results within any given finite element are approximations. Therefore, if overly large finite elements are used, it is possible that the approximations of the results within the element can effectively miss or average out areas of higher stresses.
An important part of the analysis validation process is to check the load paths in the model and to determine if the model is behaving as expected or required. If loads are not going where expected, this may indicate an issue with the stiffness of elements in the model, or could be related to incorrect restraints such that load is effectively being directed to different locations. However, there are circumstances where the analysis is correct and the expectation of the design is incorrect. This often occurs where the stiffness of certain elements is not sufficient to attack the load. This can particularly occur with transfer structures, where the deflection of the transfer structure is such that the structure above is effectively acting to support itself rather than to transfer load.
One specific area of concern related to transfer structures is the construction sequence. The 3D model is based on the full structure, but the real structure will have a construction sequence that will affect the load path of the structure and may result in a significant divergence in the behaviour of the model when compared to the actual structure.
An extremely useful and important step in the validation process is to calculate check values of the results manually. In simple cases where the loading and geometry are such that the FE results can be checked directly by manual calculation, it is possible to use standard solutions to produce validation results from which the FE analysis results can be compared. But even where the structure is sufficiently complex so that manual calculation of an exact solution is not possible, estimation of the results by means of simplified manual calculations are extremely useful and can provide significant levels of confidence in the results of the finite element analysis even where they are used to simply verify the magnitude of the FE results.
A very significant part of the power of FEA is the ability to analyse complex structural geometries, loads and restraint conditions. But the more complex the model, the more important that the results are validated to ensure that the model is correctly set up and also that it produces a valid representation of the structure under consideration. There is no set method or process to validate a model, but within the software there are a variety of tools that can be used to assist the process.