Requesting Outputs
Abaqus has two types of output: Field Output and History Output. Understanding the difference and knowing which variables to request is essential for getting useful results.
Field Output vs. History Output
Field Output stores results across the entire model (or large regions of it) at selected intervals during the analysis. It is what you visualize in the Visualization Module as contour plots, deformed shapes, and animations. Because it captures spatial distributions, field output files can be large.
History Output stores results at specific nodes, elements, or sets at every increment. It is used to generate XY plots — for example, plotting the reaction force at a support versus load step time, or the displacement at the wing tip versus applied load. History output is much smaller than field output and is the right tool when you want a single number as a function of time/increment.
A practical workflow: use field output to understand where things happen in the model spatially, and history output to track how key quantities evolve through the analysis.
How to request Field Output
- In the Step Module, open the Field Output Manager
- Select your load step and click Edit
- Expand the variable categories and check the outputs you need
- Set the output frequency — every increment is fine for debugging; for large jobs, save every N increments to reduce file size
- Click OK
How to request History Output
- In the Step Module, click History Output Manager > Create
- Name the output and select the step
- Set the Domain to a node set, element set, or surface (you must create the set first)
- Select the variables you want to track
- History output is saved at every increment by default — this gives you a full load-displacement (or similar) curve
To view history output: in the Visualization Module, click Create XY Data > ODB History Output, select the variable and node/element, and click Plot.
Output variable reference
Displacement and rotation
| Variable | Description |
|---|---|
| U | Translational displacement (U1, U2, U3) |
| UR | Rotational displacement / rotation angle (UR1, UR2, UR3) — relevant for shell and beam elements |
Stress and strain
| Variable | Description |
|---|---|
| S | Cauchy stress tensor components (S11, S22, S33, S12, S13, S23) and invariants (Mises, Max Principal, etc.) |
| E | Nominal (engineering) strain |
| LE | Logarithmic strain — use instead of E when NLGEOM is enabled (large deformation) |
Forces and reactions
| Variable | Description |
|---|---|
| RF | Reaction force at boundary condition nodes (RF1, RF2, RF3) |
| RM | Reaction moment at boundary condition nodes (RM1, RM2, RM3) |
| CF | Concentrated force applied at a node (CF1, CF2, CF3) |
| CM | Concentrated moment applied at a node (CM1, CM2, CM3) |
Shell section forces
| Variable | Description |
|---|---|
| SF | Section forces and moments integrated through the shell thickness — SF1 (N11), SF2 (N22), SF3 (N12), SM1 (M11), SM2 (M22), SM3 (M12) |
Surface tractions
| Variable | Description |
|---|---|
| TRNOR | Normal traction on a surface (component perpendicular to surface) |
| TRSHR | Shear traction on a surface (component tangential to surface) |
These are useful when you've applied a general surface traction and want to verify or separate its normal and in-plane components. To request them, expand the Contact or Forces/Reactions category in the Field Output editor, depending on your Abaqus version.
Which outputs should I always request?
For a standard structural analysis, request at minimum:
- S — to find stress distributions and check for yielding or failure
- U — to visualize deformation and extract displacements
- UR — if using shells or beams (rotation matters at connections)
- RF — to verify reaction forces at supports and check equilibrium
- RM — if any rotational boundary conditions or rigid bodies are involved
- SF — if using shell elements and you need section-level force/moment resultants
- LE — if NLGEOM is on
For history output, create at least one set at each support location requesting RF and RM, and one set at key displacement points requesting U or UR.
Tips
The default field output set Abaqus creates includes most of the common variables, but UR, RM, SF, and TRSHR/TRNOR are not always included by default — add them manually if your analysis needs them.
Requesting too many field outputs significantly increases the size of your .odb file. If you have a large model or many increments, be selective — request only what you need, and use history output for time-history tracking rather than loading the full field output for every increment.