RunMat
  • Pricing
RunMat
GitHub
GitHub
Sign inTry in browser
DesktopRuntimePhysicsCADAdministrationAgent

Get RunMat updates

New releases, guides and examples.

Product+
  • Runtime
  • GPU
  • Parallel
  • Compile
  • Interop and MEX
  • Simulation
  • MCAD
  • ECAD
  • Enterprise
  • AI integrations
  • Pricing
  • Download
Math+
  • Signal processing
  • Linear algebra
  • Statistics
  • Curve fitting
  • Differential equations
  • Control systems
  • Optimization
  • Finance
  • Data and tables
  • Plotting
Physics+
  • Simulation overview
  • Structural
  • Thermal
  • Electromagnetic
  • Joule heating
  • Thermal stress
  • Acoustics
  • Fluid flow
  • Conjugate heat transfer
  • Fluid–structure
  • What is FEA
Industries+
  • Aerospace
  • Automotive and transportation
  • Defense
  • Electronics and semiconductors
  • Energy
  • Industrial machinery
  • Life sciences
  • Quantitative finance
Learn+
  • Guides
  • Docs
  • Function reference
  • Language reference
  • Migration guide
  • Changelog
  • MATLAB Online
  • MATLAB AI agent
  • For students
Compare+
  • RunMat vs MATLAB
  • RunMat vs Ansys
  • RunMat vs SOLIDWORKS
  • RunMat vs Altium
  • RunMat vs Cadence
  • RunMat vs COMSOL
  • RunMat vs Python
  • RunMat vs Julia
  • RunMat vs Physics AI
  • RunMat vs Octave
  • Benchmarks
  • MATLAB alternatives
  • All comparisons
Company+
  • About
  • Blog
  • Contact
  • Source code↗
  • License
  • Privacy
  • Terms

Product

  • Runtime
  • GPU
  • Parallel
  • Compile
  • Interop and MEX
  • Simulation
  • MCAD
  • ECAD
  • Enterprise
  • AI integrations
  • Pricing
  • Download

Math

  • Signal processing
  • Linear algebra
  • Statistics
  • Curve fitting
  • Differential equations
  • Control systems
  • Optimization
  • Finance
  • Data and tables
  • Plotting

Physics

  • Simulation overview
  • Structural
  • Thermal
  • Electromagnetic
  • Joule heating
  • Thermal stress
  • Acoustics
  • Fluid flow
  • Conjugate heat transfer
  • Fluid–structure
  • What is FEA

Industries

  • Aerospace
  • Automotive and transportation
  • Defense
  • Electronics and semiconductors
  • Energy
  • Industrial machinery
  • Life sciences
  • Quantitative finance

Learn

  • Guides
  • Docs
  • Function reference
  • Language reference
  • Migration guide
  • Changelog
  • MATLAB Online
  • MATLAB AI agent
  • For students

Compare

  • RunMat vs MATLAB
  • RunMat vs Ansys
  • RunMat vs SOLIDWORKS
  • RunMat vs Altium
  • RunMat vs Cadence
  • RunMat vs COMSOL
  • RunMat vs Python
  • RunMat vs Julia
  • RunMat vs Physics AI
  • RunMat vs Octave
  • Benchmarks
  • MATLAB alternatives
  • All comparisons

Company

  • About
  • Blog
  • Contact
  • Source code↗
  • License
  • Privacy
  • Terms
GitHubXLinkedIn

© Dystr, Inc. · RunMat v0.7.1, Nov 17, 2026

RunMat® is a registered trademark of Dystr, Inc. MATLAB® is a registered trademark of The MathWorks, Inc. RunMat is not affiliated with, endorsed by, or sponsored by The MathWorks, Inc.

/
    • Linear static analysis
    • Steady heat transfer
    • Modal analysis
    • Mesh refinement
    • Thermal stress
    • First static study
    • Reusable parameterized model
    • Transient study with generated inputs
    • Modal response-spectrum study
    • Run and plot a sweep
    • Scale from local to cluster
    • Publish and read large results
Docs>Physics>Guides

First static study

This guide uses the checked example at docs/simulation/examples/structural-static.fea. It uses a two-part STEP assembly so the complete exact import, mesh, multi-solid material coverage, model, solve, and result path can run in a release check.

1. Inspect the geometry

Before writing selectors, inspect the CAD file:

runmat run inspect_geometry.m

In RunMat code, geometry.inspect(path) reports units, topology roles, persistent ids, imported names and tags, assemblies, and AP242 capabilities. Choose selectors from that inventory. Do not guess a face ordinal from a viewport.

2. Declare geometry and regions

The example declares both solid occurrences, a support on each disconnected part, and a load face on the left part. Each region states its topology role and expected cardinality. Run runmat check after this step; a stale or ambiguous selector should fail before meshing.

The included STEP file carries the authored body and end-face names the study selects; select name resolves only names authored in the CAD file. The study stays in one readable source file; exporting the project preserves its CAD names.

geometry bracket {
    file = "./geometry/two-box-assembly.step"
    units = m

    region left_body : solid { select name "left_body"; expect exactly_one }
    region right_body : solid { select name "right_body"; expect exactly_one }
    region left_support : face { select name "left_support"; expect exactly_one }
    region left_load_face : face { select name "left_load_face"; expect exactly_one }
    region right_support : face { select name "right_support"; expect exactly_one }
}

3. Declare the mesh

The mesh targets the same geometry by reference. target_size controls nominal volume resolution; maximum_deviation bounds geometric approximation. Start with a coarse mesh for model setup, then perform a governed refinement study before using results quantitatively.

mesh bracket on geometry.bracket {
    tetrahedra {
        order = linear
        target_size = 1.5 m
        maximum_deviation = 0.05 m
    }
}

4. Define and assign material behavior

The steel declaration supplies elasticity and mass density. Separate assignments cover both solid occurrences, not their faces. The fixed constraints and force target face regions. This distinction lets the compiler prove complete constitutive coverage and correct boundary dimensionality; the second support also prevents the disconnected right occurrence from retaining rigid-body modes.

material steel {
    mass_density = 7850 kg/m^3
    elastic {
        youngs_modulus = 200 GPa
        poisson_ratio = 0.3
    }
}

model loaded_bracket {
    assign material.steel to geometry.bracket.region.left_body
    assign material.steel to geometry.bracket.region.right_body
    constraint left_support {
        structural.fixed { target = geometry.bracket.region.left_support }
    }
    constraint right_support {
        structural.fixed { target = geometry.bracket.region.right_support }
    }
    load service_traction {
        traction on geometry.bracket.region.left_load_face = [166.6666666667, 0, 0] Pa
    }
    load_case service { include load.service_traction }
}

The traction tuple is expressed in global XYZ coordinates. The selected end face has an area of 6 m26\,\mathrm{m^2}6m2, so [166.6666666667, 0, 0] Pa retains the original 1 kN1\,\mathrm{kN}1kN resultant while boundary quadrature distributes it consistently over the surface mesh. Targeting a face does not implicitly rotate an arbitrary traction vector onto that face normal.

5. Define the study

The study binds geometry, mesh, and model, then names one structural static analysis and the result fields to publish.

study structural_static {
    geometry = geometry.bracket
    mesh = mesh.bracket
    model = model.loaded_bracket
    analysis static { structural static {} }
    output displacement = analysis.static.field.node.displacement
    output von_mises = analysis.static.field.element.von_mises_stress
}

6. Check, plan, and run

runmat check docs/simulation/examples/structural-static.fea
runmat plan docs/simulation/examples/structural-static.fea
runmat run docs/simulation/examples/structural-static.fea

Read check diagnostics before planning. In the plan, verify the selected root, geometry, mesh, model, and logical phases. After execution, inspect mesh quality, property coverage, constraint rank, convergence, balance, and formulation evidence before reading the displacement or stress field.

7. Plot an output

From RunMat code, select a typed result field and pass it to ordinary plot:

run = fea.run(study);
results = fea.results(run);
stress = fea.field(results, fea.StructuralField.vonMises());
plot(stress, "Edges", true);

The .m object-construction path and .fea file path share canonical study and result contracts, but their current public entrypoints differ. runmat run file.fea is the file workflow; fea.run(study) accepts a typed fea.Study object, not a path.

On this page
  • 1. Inspect the geometry
  • 2. Declare geometry and regions
  • 3. Declare the mesh
  • 4. Define and assign material behavior
  • 5. Define the study
  • 6. Check, plan, and run
  • 7. Plot an output