The need for speed: Part 6 of 7 - Reducing output requests

In order to find a solution to a structural FEA model, an FEA solver must find the displacements that result from the applied loads and displacements.  What an analyst does with this solution for the model, which is now held in memory,will affect how much extra effort the FEA solver must put into finding other solution variables, and to saving all the requested output to disk.  The typical guidance is that excess output requests is a bigger impact on hard drive space than on solution times, but certain solution sequences can generate output so frequently that it can severely slow the solution speed, such as explicit, which will typically have time steps so small (maybe a millionth of a second) that even for short duration events an analyst may only care about the solution result every thousandth step. 

There are two types of output from an FEA solution: primary field variables and calculated variables.  Primary field variables are the actual solution, such as displacements for a structural simulation or temperatures in a heat transfer simulation.  As such, when they are requested they only require writing data to the disk and have a small impact on simulation speed.  The other type of variable, calculated variables, are found by using the solution variables and the properties of elements to back calculate other variables, such as stress and strain in a structural simulation or heat flux in a thermal simulation.  These require actual computation, and as such will have a much bigger impact on simulation speed.

Some practical tips for particular solvers:

Abaqus
Abaqus will only output the output variables that you request.  The most important thing in Abaqus is typically to reduce the frequency of output in a nonlinear analysis and explicit dynamic analysis.  Both of these solutions will find a converged result over and over again, and unless a model is new and being diagnosed these intermediate results typically do not need to be output very frequently.  Make use of the '*output, TIME INTERVAL=' or '*output, Frequency=' keywords to limit the frequency of these outputs.
  
There are two typical types of output in Abaqus: Field and History.  Field is usually used less frequently to output the complete solution, and history is more typicall used for global measures of model condition, such as total kinetic or elastic energy.

While using "*output, variable=preselect" will provide the most typically used variables in most cases, being more specific about which variables, and even which elements or nodes you wish to find solutions at, will provide even more savings

Do not use *restart unless you are fairly certian you need to use, as it will generate an ENORMOUS restart file.

Optistruct
Optistruct has an interesting behavior in that if no output is requested, it will generate the default outputs for you, similar to Abaqus' preselect.  Outside of not requesting things you dont' care about, the most important thing to do in Optistruct is to be careful how frequently a full result from an optimization is output.  This can be set on the card, 'OUTPUT,(OUTPUT TYPE),(FREQUENCY)'.  The best result is usually FL for the frequency, as this will generate the full results for the initial and final design.


Nastran
Similar to Optistruct, take care to request only the results you care about, using both selective choices of output requests in the case control and use of sets to only requests results for regions you care about.