We all know that output files generated by most FEA solvers can be huge. In some cases, this can be problematic, especially if you’re working with limited hard drive space. There’s nothing more frustrating than running an analysis for many hours, only to have it stop before it finishes because you ran out of space!
So, How Do We Do It?
Luckily, there are a bunch of things that we can do to reduce the output file size in our FEA analyses, a number of which are summarized below. This post will be focused on how to do this in Abaqus, but the sentiment should carry over to any FEA tool that you happen to be using. Before you run your analysis, first ask yourself these questions:
1. What Field Outputs Do You Actually Need?
FEA solvers typically have a default setting for outputs. This means that the preprocessor is essentially guessing what it thinks you might be looking for in the results. However, many times we don’t need all of these, or even most of them. For example, if we’re running a structural analysis and we’re only looking for stresses, we might not need to output strains, deflections, pressures, slip, temperatures etc. Because field output is written for every node and element, this can result in huge space savings. To do this in Abaqus, we can either select relevant output variables in the ‘Field Output’ dropdown menu or by defining them in the *FIELD OUTPUT section of the input file.
2. Do You Care About Seeing Field Output At Every Increment?
If we’re running a highly nonlinear static analysis, we probably don’t care to see results at every single increment that the solver calculates. We may only care about the results at the end of the analysis. And even if we want to see progress, it may be that five or ten output increments is enough. In this case we can set write frequency=999 if we only need the last increment or any frequency that we think makes sense. Alternatively, it may be useful to tell the solver to stop and write data at a set number of equally sized increments, especially when there are going to be a large number of increments because of contact for example. In Abaqus, we do this by asking for field output at ‘Evenly Spaced Increments’ or ‘Every X Units Of Time’.
n
3. Which Nodes And Elements Do You Actually Need Data From?
In many cases, we’re only really interested in the results for a certain component or location in a larger FEA model. In these cases, field output can be limited to specific locations by way of node and element set definitions, meaning much less data in the output file and, therefore, much smaller file sizes. To do this, select only the sets you are interested in when viewing the Field Output dialogue box in Abaqus CAE or by including *NODE OUTPUT, NSET = node_set_name or *ELEMENT OUTPUT, ELSET = element_set_name in the input deck.
4. Do You Care About Interior Nodes And Elements
Similar to point 3, it is often unnecessary to output data for internal nodes and elements. In most 3-dimensional models, these nodes and elements will make up the bulk of the mesh, and so you’ll find yourself outputting tons of data for internal locations that you will never see. For example, in this (horribly meshed) ball, there are a total of 478,920 nodes and 347,265 elements. However, the skin only includes 2,407 of these nodes and 1,023 of the elements. If you were to analyze this ball (not sure why you would) and compare the amount of data from all nodes and elements vs only the exterior, you’d find a whopping 99.6% field output space saving! To request this from Abaqus CAE, select ‘Exterior only’ from the field output request dialogue box or include *NODE OUTPUT, EXTERIOR or *ELEMENT OUTPUT, EXTERIOR in your input deck.
5. Can You Use History Output Instead Of Field Output?
History output is a great way to extract the data you need from your FEA analyses in a clean and, more importantly here, efficient way. By requesting relevant information from a small number of nodes or elements, you can avoid the need for cumbersome field output postprocessing and access the data more easily in tabular form. Not that history data takes up a large amount of room in the output file, but it can start to add up if there are a large number of nodes/elements and variables requested.
To take it further, if you utilize the *NODE PRINT and *EL PRINT features in the Abaqus input deck, the data that you need will be neatly tabulated in the .dat file, which means you may not even need to retrieve the output file at all.
6. Can You Zip Your Output Files?
Finally, when transferring data, either to colleagues or storage, .odb file size can be reduced by 50-70% simply by zipping it up!
Final Thoughts
FEA model output databases can be cumbersome to say the least. If the model is large, or there are a large number of increments (or both) then the amount of data that is written out can spiral rapidly. Hopefully, this quick hitter will help you be more mindful of postprocessing time and disk space next time you run a simulation!
If you’d like to talk to one of our experts about anything simulation, don’t hesitate to reach out to our team!
