Simulation & FEA

Set up and solve a stress, frequency, buckling, dynamic, nonlinear or thermal study by chat, read the results back, and drive a dimension toward a target — without leaving the chat panel or hunting through the solver's ribbon.

The short version

Describe the study the way you would to a colleague: what the part is made of, what is held, what pushes on it. SphereHarness creates the study, assigns the material, applies the restraint and the load, meshes, solves, and reports the numbers.

Run a linear static stress analysis on this steel bracket: fix the minX face and apply 300 N in -Z on the maxX face. Report displacement and von Mises stress.

First, check what you have

Simulation depends on which solver is licensed and installed on your workstation, so it is worth thirty seconds to find out before planning around it.

Is simulation available here? List the solvers you can see and their status.
What simulation capabilities does this CAD system support?

What each CAD system provides

CAD systemSolverStudy types available
Autodesk Inventor Autodesk Inventor Nastran (required — Inventor's built-in Stress Analysis has no programming interface, so it is not used) Parts: linear static, frequency (modal), buckling, harmonic and transient response, nonlinear (bilinear plasticity, large displacement, permanent set after unloading), steady and transient heat transfer with a fixed temperature, a heat flux or convection. Assemblies: linear static and frequency, with touching parts bonded automatically. See Inventor in detail.
Siemens NX Simcenter structural analysis (linear static, modal) plus an NX Nastran deck export for an external solver Linear static and modal natively; more through the deck-export bridge. Probe availability first — it depends on your NX configuration.
Solid Edge Solid Edge Simulation (Femap / NX Nastran) Linear static, frequency, thermal and buckling only. Nonlinear, dynamic, drop test, fatigue and topology are not exposed.
A limit worth remembering: Solid Edge optimisation is single-variable goal seek only, and a running Solid Edge solve cannot be cancelled from chat.

Inventor in detail

On Inventor every study runs through Autodesk Inventor Nastran. SphereHarness writes the analysis into the solver's input deck, reads that deck back before solving to confirm it says what you asked for, and takes every number from the solver's own output file — never from your request. Decks written this way and solved by Autodesk Nastran were checked against hand calculations: a cantilever's first natural frequency within 0.2 %, a column's buckling load factor within 0.2 %, a bar's mid-plane temperature exact, a plastic bar's stretch and permanent set within 0.1 %.

StudyOn an Inventor part
Linear staticDisplacement, von Mises stress, strain, factor of safety, reaction force — and where the maximum is
Frequency (modal)Natural frequencies, mode 1 first; ask for the number of modes
BucklingLoad factors; the critical load is the applied load times the lowest factor
Harmonic responseA frequency sweep of the study's load with the damping you name (modal, constant or Rayleigh); the response at each solved frequency and its peak
Transient responseThe study's load over a duration and time step you name; the response at each solved step and its peak
NonlinearBilinear plasticity (the material needs a yield strength and a tangent modulus — without one it is refused, nothing is assumed), large displacement, the number of load increments, and the permanent set after unloading
Heat transferSteady or transient, with a fixed temperature, a heat flux or convection on faces; the maximum, minimum and mean temperature. Parts modelled in millimetres (an inch part is refused for heat transfer)
Drop testThe part dropped from a height (or at an impact speed) flat face first onto a rigid floor; impact force, contact duration and peak element stress read from the solve
FatigueLife of the study's load cycled at constant amplitude, from a two-point S-N curve you give (stress amplitude and cycles at two points); a mean stress is Goodman-corrected against the ultimate strength you state
Two bodies in one partTouching flat faces are bonded automatically

Assemblies

Linear static and frequency studies run on an assembly as one model: each component keeps its own material, parts whose flat faces touch are bonded automatically, and a static result is reported per component as well as overall. Name the component when you pick a face or give a material — the occurrence name as it appears in the browser:

These two steel blocks are glued end to end. Fix the left end of Block A:1 and push the right end of Block B:1 down with 1000 N — how far does it move, and which block carries more stress?
Make Block B:1 aluminium and run it again

Refused by name on an assembly: sub-assemblies, a component with no solid body or with several, heat-transfer or nonlinear studies, separation contact, meshes over 200 000 grid points, and parts that touch only along a line or at a point. SphereHarness does not derive, merge or split your assembly unless you ask it to.

Refused, with the reason given: random vibration and response spectrum, separation or sliding contact, topology optimisation, a drop onto a corner, an edge or a curved face or onto a flexible floor, fatigue with a Soderberg or Gerber correction or a variable load history, and anything the model has changed since the last solve until it is solved again. Autodesk Nastran has no SOL 400. A refusal is a real answer, not a glitch: the chat quotes the reason rather than working around it.

Name faces by geometry, not by number

This is the difference between a repeatable study and a lottery. A face number belongs to the exact solid that produced it, so the same number can be a different physical face on a part that was rebuilt or modelled in a different order — and the study will run happily either way and give you a plausible wrong answer.

Use a geometric selector instead:

  • minX, maxX, minY, maxY, minZ, maxZ — the extreme face perpendicular to that axis
  • largest, smallest — by area

Each call reports which face it actually took, with its area, centre and normal. Read that back before solving:

Which face did the fixture land on? Give me its area and normal.

An area of 200 mm² on an 80 × 25 × 8 mm bracket tells you it took the 25 × 8 end face, which is what “the end” should mean.

For a cantilever, fix one extreme of the long axis and load the opposite one — check the bounding box first so you know which axis that is.

What is the bounding box? Then fix the face at the minimum of the longest axis.

Name the load direction too

“Downward” is not a defined quantity, and getting it wrong is expensive in a way that is hard to spot. On an 80 × 25 × 8 mm bracket, loading across the 8 mm thickness and loading across the 25 mm width differ by a factor of about ten in deflection — and both results look entirely reasonable on their own.

State an axis, or a direction relative to the loaded face:

  • +X, -X, +Y, -Y, +Z, -Z — explicit, always unambiguous
  • -normal — pushing into the loaded face, which is what you usually want for pressure
  • down, up — interpreted by the usual part convention (sketch on XY, extrude along +Z)

For ordinary bending, ask for the bounding box first and load across the smallest dimension.

What is the bounding box? Then fix the minX face and load 300 N in -Z on the maxX face.

Setting up a study

Study lifecycle

Create a linear static study called "Bracket load case 1"
List the studies in this document
Make "Bracket load case 2" the active study
Delete the study called "scratch"

Material

What materials are in the simulation library? Show me the aluminium alloys with their yield strength.
Assign 6061-T6 aluminium to the study

Material properties at the interface are SI: stresses in pascals, lengths in metres, masses in kilograms. You can still type in the units you think in — “270 MPa” is understood — but the numbers reported back follow the study's own convention, so read the units on the reply.

Restraints

Fixture types: Fixed, Pinned, Roller, on a flat face, on a cylindrical face, symmetry, and prescribed displacement.

Fix the minX face completely
Apply a pinned restraint to the bore — the cylindrical face
Apply symmetry on the minY face so I can model half the part

Loads

Force (N, kN or lbf), pressure, torque, gravity and bearing load are available for structural studies. A force can be applied as a total, per unit area, or per selected entity. Which of them a given CAD system carries follows the table above; one it cannot carry is refused, never applied as something else.

Apply 2.5 kN total in -Z on the maxX face
Apply 0.4 MPa pressure into the top face
Apply a 40 Nm torque about the bore axis
Add gravity in -Z
Apply a 1200 N bearing load on the pin bore, pointing -Y

Heat-transfer studies take thermal conditions on faces instead: a fixed temperature (°C), a heat flux (W/m², into the part) or convection (a film coefficient in W/(m²·K) to an ambient temperature). A steady study needs at least one fixed temperature or convection. Heat flux and convection are carried on Inventor with Inventor Nastran; elsewhere they are refused by name.

Hold the minX face at 100 °C and the maxX face at 0 °C, solve, and tell me the temperatures
Put 100 kW/m² into the maxX face, hold the minX face at 0 °C, and give me the hottest temperature
Cool the maxX face by convection, 100 W/m²K to 20 °C air, with the minX face held at 100 °C

Mesh

Leave it alone unless you have a reason. Omitted, the element size is derived from the part — the bounding-box diagonal divided by 25 — which is repeatable for a given solid, so two identical requests produce an identical mesh. A fixed default cannot be right for both a 2 mm part and a 2 m one, which is why an invented number is worse than none.

Element types: solid tetrahedral, solid hexahedral, mixed solid, shell, beam or mixed, with curved (high-order) elements on by default.

Mesh it at 2 mm and run the study again so I can compare
What is the mesh quality — element count, aspect ratios and any failed elements?

Comparing two mesh densities is a good convergence check: displacement should barely move, while peak stress at a clamped edge will shift by a few per cent because that is a stress concentration.

Solving

Solve the study and wait for it to finish
What is the status of the running study?
Cancel the solve

Reading results

What were the maximum displacement and the maximum von Mises stress?
What is the minimum factor of safety, and where is it?
What is the maximum strain?
What is the total reaction force at the fixture?

The reply tells you which source each number came from — the CAD system's own results browser, or the solved deck. That matters when the two disagree, which is itself informative.

Always compare against something independent. For a cantilever, tip deflection is PL³/3EI and peak bending stress is PLc/I. A model that disagrees with those by more than a few per cent is telling you the setup is wrong, not that the formula is. The reaction force is a second free check: it should equal the applied load.

Reports

Export the simulation results as a Word document to C:\reports\bracket.docx

Word, HTML, Markdown, CSV and PDF are rendered directly, with the metric table and any charts the solution produced. You can embed viewport images too — capture them first:

Set an isometric view, take a screenshot, then export the report to C:\reports\bracket.docx with that image included
There is also a “native” export that hands off to the CAD system's own report generator where one exists. Inventor Nastran has none that can be driven, so on Inventor the rendered formats above are the report.

Optimisation and design studies

SphereHarness can drive dimensions toward a target — minimum mass at a stress limit, for example — rather than you running studies by hand.

  1. Declare what may change.
    Make the rib thickness a design variable between 4 and 12 mm, in 1 mm steps
  2. Declare the limits.
    Constrain the maximum von Mises stress to 180 MPa and the tip displacement to 0.5 mm
  3. Declare the goal.
    The objective is to minimise mass
  4. Run it.
    Run the design study over at most 15 iterations and show me the results table
  5. Apply the winner — deliberately.
    Apply the optimised dimensions to the model, then re-measure the mass and re-run the stress study to confirm

Search strategies available: AI-driven (the model proposes the next candidate from what it has seen), full factorial, Latin hypercube, gradient descent, NSGA-II for multi-objective problems, the CAD system's own design-of-experiments, and topology optimisation.

On Solid Edge, only single-variable goal seek is available. For a multi-variable design study use Inventor Nastran.

Other study types

Run a frequency study and give me the first five natural frequencies
Run a buckling study and report the load factor
Shake the free end with 100 N from 100 to 1500 Hz with 2 % damping — at which frequency is the response largest, and how large?
Apply 1000 N suddenly at the tip and run it for 12 ms — what is the peak deflection and when does it happen?
The steel yields at 250 MPa with a tangent modulus of 2.1 GPa. Pull the bar with 30 kN, then let go — how much does it stretch, and how much stays?
Run a drop test from 1.2 m onto a rigid floor and report peak stress
Cycle the current load fully reversed. The S-N curve is 360 MPa at 1000 cycles and 200 MPa at a million — how many cycles does the part last?
Run a topology optimisation targeting 40% mass reduction, preserving the two mounting pads, and export the result to C:\reports\bracket_topo.stl

Availability follows the tables above — the advanced types need Inventor Nastran, and on Inventor topology is refused and a fatigue study needs the S-N curve stated (see Inventor in detail).

The external Nastran bridge

Where the CAD system exports a deck rather than solving in place, the three steps are visible to you and can be driven separately:

Export the Nastran deck for this study to C:\fea\bracket.dat
Run the external Nastran solver on that deck
Import the results back into the study

This is also the route for handing a deck to a solver your organization already trusts.

What appears in your CAD system

Studies are built inside the CAD system's own simulation environment, so the analysis, node and element counts, the loads and restraints and the result sets all appear where you would expect, with mesh and load glyphs drawn in the viewport. Inventor caveats worth knowing:

  • The part must be saved to a file before it can be meshed properly. An unsaved part falls back to an approximation of its bounding box, which is roughly twice as stiff. If that happens the reply says so — do not ignore that note.
  • What Inventor Nastran's own browser shows is its own model. Thermal conditions, contact between bodies, plasticity and the dynamic settings are written into the solver deck SphereHarness solves, so they do not appear there, and the numbers in the chat come from that deck's output — not from the browser's result sets.
  • Loads and restraints stay inside the part file; each study keeps only its own when its deck is written.

Before you rely on any of it

A stress number is the end of a chain of automatic choices — material, restraint, load, direction, mesh — and any one of them can be wrong while the result still looks credible. The checklist:

  • Read back which face each fixture and load landed on, with its area and normal.
  • Confirm the load direction was the axis you meant.
  • Check the reaction force equals the applied load.
  • Compare against a hand calculation for the nearest simple case.
  • Re-run at a different mesh size and see what moves.

Read Verifying results before a simulation figure informs a real decision. SphereHarness is not certified for safety-critical, medical, aerospace-airworthiness or nuclear work, and you remain the engineer of record.

See also