Skip to content

Modeling Checklist

Use this checklist as a guide when building your Abaqus model from scratch. Each step builds on the previous — skipping ahead often means coming back to fix problems later.

1 — Create Parts

  • Create or import each structural component as a separate Part in Abaqus
  • Confirm units are consistent (geometry dimensions match your intended unit system)
  • For imported geometry (e.g., from SolidWorks), clean up any small edges or redundant entities — see Importing from SolidWorks
  • Verify the part looks correct in the Part Module viewport

2 — Partition Parts

  • Identify regions that need finer mesh (stress concentrations, load introduction zones, joints)
  • Partition parts to isolate those regions — see Meshing for methods
  • Add transition zones between fine and coarse mesh regions
  • Partition faces where loads or boundary conditions will be applied (so you can select them cleanly)
  • Partition faces where tie constraints or contact will be defined

3 — Define Material Properties

  • Create each material in the Property Module: Material > Create
  • Define Elastic behavior: Young's modulus and Poisson's ratio
  • For vibration analysis: define Density (confirm units — see Vibration Analysis)
  • For composites: define Engineering Constants or Lamina properties
  • Double-check all values against the material datasheet

4 — Assign Sections

  • Create a Section for each material/element type combination: Section > Create
    • Shell sections for thin-walled structures — specify thickness
    • Solid sections for 3D geometry
    • For composites: define the layup (ply angles and thicknesses) in the shell section
  • Assign each section to the corresponding part regions: Assign > Section
  • Verify section assignments are showing (color coding in the viewport)
  • For composites, check ply normal orientation: Assign > Shell/Membrane Normal

5 — Create the Assembly

  • Switch to the Assembly Module
  • Instance each part: Instance > Create — use Dependent instances if you plan to mesh in the Part Module, Independent if meshing in the Assembly
  • Position parts correctly using Translate, Rotate, and Constraint tools
  • Verify there are no unintended gaps or overlaps between mating surfaces
  • Check that contact/tied surfaces are aligned as expected

6 — Define the Analysis Type

  • Switch to the Step Module
  • Create a Step after the Initial step: Step > Create
    • Static, General — for nonlinear static analysis
    • Linear Perturbation, Frequency — for natural frequency analysis
    • Linear Perturbation, Buckle — for linear buckling analysis
  • Set time incrementation parameters (initial/min/max increment size, max increments)
  • Enable NLGEOM if large deformations or contact is expected

7 — Set Field and History Outputs

  • In the Step Module, open the Field Output Manager
    • Confirm S, U, UR, E, RF, RM are selected for your load step
    • Add SF (section forces) if working with shells
    • Add P (pressure) if you want to verify applied loads
  • Create History Outputs for specific sets (e.g., reaction forces at supports, displacements at key nodes) — see Requesting Outputs
  • Set output frequency — every increment for debugging; reduce for large jobs

8 — Define Contact Interactions

  • In the Interactions Module, create Contact Properties (friction coefficients, normal behavior)
  • Define all Surface-to-Surface Contact pairs: master and slave surfaces, sliding formulation
  • Define Tie Constraints for bonded interfaces (skin-spar, skin-rib connections)
  • Verify that contact/tie surfaces are correctly highlighted in the viewport

9 — Define Reference Points and Rigid Bodies

  • Create Reference Points (RP) at load introduction locations: Tools > Reference Point
  • In the Interactions Module, create Rigid Body or Coupling constraints linking each RP to its surface region
  • Verify RP locations are correct (they should be at or near the physical load application point)

10 — Define Loads and Boundary Conditions

  • In the Load Module, apply boundary conditions in the Initial Step (fixed constraints, symmetry)
  • Apply all loads in the Load Step: pressure, concentrated forces, moments, body forces
  • For aerodynamic loads: apply as pressure with correct sign convention — see Applying Loads
  • Verify load magnitudes and directions visually in the viewport
  • Check that the model is fully constrained (no unintended rigid body motion)

11 — Mesh

  • In the Mesh Module, assign mesh controls (element shape: quad/hex preferred)
  • Seed edges with appropriate element sizes — fine in critical regions, coarser elsewhere
  • Use biased seeds in transition zones
  • Generate the mesh: Mesh > Part or Mesh > Assembly
  • Run Mesh > Verify and check for poor-quality elements — fix by refining seeds or re-partitioning

12 — Submit and Monitor

  • Set your working directory before submitting — see Abaqus Tips
  • In the Job Module, create a new job: Job > Create
  • Submit the job: Job Manager > Submit
  • Monitor the job log in real time — look for warnings and errors
  • If the job aborts, check the .msg and .dat files in your working directory for the error description
  • After completion, open the .odb file in the Visualization Module to review results

!!! tip If this is your first run of a new model, submit with a coarse mesh first to confirm everything is set up correctly before committing to a long fine-mesh run.