Next: Simple example problems Up: CalculiX CrunchiX USER'S MANUAL Previous: Units Contents

# Golden rules

Applying the finite element method to real-life problems is not always a piece of cake. Especially achieving convergence for nonlinear applications (large deformation, nonlinear material behavior, contact) can be quite tricky. However, adhering to a couple of simple rules can make life a lot easier. According to my experience, the following guidelines are quite helpful:

1. Check the quality of your mesh in CalculiX GraphiX or by using any other good preprocessor.

2. If you are dealing with a nonlinear problem, RUN A LINEARIZED VERSION FIRST: eliminate large deformations (drop NLGEOM), use a linear elastic material and drop all other nonlinearities such as contact. If the linear version doesn't run, the nonlinear problem won't run either. The linear version allows you to check easily whether the boundary conditions are correct (no unrestrained rigid body modes), the loading is the one you meant to apply etc. Furthermore, you get a feeling what the solution should look like.

3. USE QUADRATIC ELEMENTS (C3D10, C3D15, C3D20(R), S8, CPE8, CPS8, CAX8, B32). The standard shape functions for quadratic elements are very good. Most finite element programs use these standard functions. For linear elements this is not the case: linear elements exhibit all kind of weird behavior such as shear locking and volumetric locking. Therefore, most finite element programs modify the standard shape functions for linear elements to alleviate these problems. However, there is no standard way of doing this, so each vendor has created his own modifications without necessarily publishing them. This leads to a larger variation in the results if you use linear elements. Since CalculiX uses the standard shape functions for linear elements too, the results must be considered with care.

4. If you are using shell elements or beam elements, use the option OUTPUT=3D on the *NODE FILE card in CalculiX (which is default). That way you get the expanded form of these elements in the .frd file. You can easily verify whether the thicknesses you specified are correct. Furthermore, you get the 3D stress distribution. It is the basis for the 1D/2D stress distribution and the internal beam forces. If the former is incorrect, so will the latter be.

5. If you include contact in your calculations and you are using quadratic elements, use the face-to-face penalty contact method. In general, for contact between faces the face-to-face penalty method will converge much better than the node-to-face method. The type of contact has to be declared on the *CONTACT PAIR card.

6. if you do not have enough space to run a problem, check the numbering. The memory needed to run a problem depends on the largest node and element numbers (the computational time, though, does not). So if you notice large gaps in the numbering, get rid of them and you will need less memory. In some problems you can save memory by choosing an iterative solution method. The iterative scaling method (cf. *STATIC) needs less memory than the iterative Cholesky method, the latter needs less memory than SPOOLES or PARDISO.

If you experience problems you can:

1. look at the screen output. In particular, the convergence information for nonlinear calculations may indicate the source of your problem.

2. look at the .sta file. This file contains information on the number of iterations needed in each increment to obtain convergence

3. look at the .cvg file. This file is a synopsis of the screen output: it gives you a very fast overview of the number of contact elements, the residual force and the largest change in solution in each iteration (no matter whether convergent or not).

4. use the ``last iterations'' option on the *NODE FILE or similar card. This generates a file with the name ResultsForLastIterations.frd with the deformation (for mechanical calculations) and the temperature (for thermal calculations) for all non-converged iterations starting after the last convergent increment.

5. if you have contact definitions in your input deck you may use the ``contact elements'' option on the *NODE FILE or similar card. This generates a file with the name ``contactelements.inp'' with all contact elements in all iterations of the increment in which this option is active. By reading this file in CalculiX GraphiX you can visualize all contact elements in each iteration and maybe find the source of your problems.

6. if you experience a segmentation fault, you may set the environment variable CCX_LOG_ALLOC to 1 by typing ``export CCX_LOG_ALLOC=1'' in a terminal window. Running CalculiX you will get information on which fields are allocated, reallocated or freed at which line in the code (default is 0).

Next: Simple example problems Up: CalculiX CrunchiX USER'S MANUAL Previous: Units Contents