JP | EN | ZH
TOP › Error Database › Solver Errors

Solver Error Resolution Database — FEA & CFD

Your solver just threw a cryptic error message and terminated. This database catalogs the most common FEA and CFD solver errors — the exact message text, what it physically means, and a precise step-by-step fix. Covers Abaqus, ANSYS Mechanical, OpenFOAM, and LS-DYNA.

How to use this page: Search your browser (Ctrl+F / Cmd+F) for the exact error message text to jump directly to the relevant entry. Each entry follows the format: exact message → meaning → root cause → fix.

Abaqus Errors

Too many attempts made for this increment
Abaqus/Standard Nonlinear Static / Dynamic Severity: Fatal

What This Means

Abaqus tried to converge the current load increment but could not satisfy the force residual and displacement correction criteria within the maximum allowed iterations (default: 16 iterations × up to 5 cutbacks). Each failed attempt halved the increment size, but even the minimum increment size couldn't produce a converged solution.

Root Causes

  • Load increment too large for the degree of nonlinearity
  • Contact instability — nodes chattering between open and closed states
  • Material model instability — hyperelastic constants causing non-positive-definite tangent
  • Physical instability — model approaching buckling, snap-through, or limit point
  • Rigid body motion — insufficient boundary conditions

Fix — Step by Step

1
Open the .msg file and find the last reported force residual. Note which DOF (node number and direction) has the largest residual — this localizes the problem area.
2
Visualize the deformed shape at the last converged increment. Does it look physically reasonable? If the model is distorting or rotating wildly, check for missing constraints or incorrect contact definitions.
3
In the *Step definition, add or tighten automatic incrementation: *Static, stabilize=0.0002, allsdtol=0.05. This adds viscous damping to absorb energy from unstable modes.
4
If the problem is contact, switch to softened contact: *Surface Interaction, name=INT-1 with *Surface Behavior, pressure-overclosure=EXPONENTIAL (or LINEAR). This eliminates the binary open/closed discontinuity.
5
As a final check, run a linear perturbation eigenvalue analysis (*Frequency) at the last converged increment. Negative eigenvalues confirm structural instability — switch to the Riks arc-length method if that's the case.
🧑‍🎓

I got "Too many attempts made for this increment" right at the beginning of the step — like, at increment 1 with a tiny applied load. That seems strange. Is this the same issue as convergence failure at a high load?

🎓

Failure at the very first increment with a tiny load is a completely different problem from convergence failure at high load. At increment 1 with near-zero load, the stiffness matrix should be well-conditioned and easy to solve. If it fails immediately, you almost certainly have one of three issues.

First, a rigid body mode — some part of the model is unconstrained and free to move infinitely with any applied force. Check that all parts are connected (no floating subassemblies) and that constraints prevent all rigid body motions (3 translations + 3 rotations in 3D).

Second, an incompatible mesh — if you imported geometry and meshed in separate operations, there might be unintended free surfaces at part interfaces. Use the mesh verification tool to check for free edges/surfaces at intended connection zones.

Third, a material definition issue — if you're using a user material subroutine (UMAT) that crashes on the very first material point evaluation, all subsequent iterations will fail. Check UMAT inputs at the initial state.

Excessive distortion at a total of N integration points in solid (continuum) elements
Abaqus/Standard & Explicit Large Deformation / Forming Severity: Fatal

What This Means

The Jacobian determinant at one or more integration points has become negative or near-zero, meaning the element has inverted or collapsed. The solver cannot compute valid stresses or strains from an inverted element and must abort.

Root Causes

  • Elements undergo large strains beyond the mesh resolution limit
  • Material flowing through an element (forming, forging) without adaptive remeshing
  • Hourglass mode amplification in reduced-integration elements
  • Excessively large time increment in explicit simulation

Fix — Step by Step

1
Identify the distorted elements using the field output EVOL (element volume) or by checking the Jacobian ratio in the mesh quality tool. Visualize the distortion history — when did it start?
2
For sheet metal forming: switch from solid to shell elements (S4R). Shell elements represent thinning through a thickness scaling parameter, not geometric distortion, and are much more robust for large bending/stretching operations.
3
For bulk forming (forging, extrusion): use Abaqus Explicit with adaptive remeshing (*Adaptive Mesh). Specify the remeshing frequency (every 5–10 increments) and quality criteria.
4
Check hourglass control. For reduced-integration elements (C3D8R, S4R), add *Section Controls, name=CTRL-1, hourglass=enhanced. This uses enhanced assumed strain to suppress hourglass modes that can cause artificial distortion.
5
As a last resort, enable element deletion: *Section Controls, element deletion=yes with a maximum degradation of 0.99. Deleted elements are removed from the model when they become too distorted, preventing abort.
🧑‍🎓

The Abaqus output shows "Excessive distortion at a total of 3 integration points" for my rubber seal under compression. I looked at the element and it's actually a corner element right where the seal contacts the housing. Could the contact itself be causing the distortion?

🎓

Absolutely — contact is a very common cause of localized extreme distortion. What's happening is that when the seal compresses against the housing, it has nowhere to go but outward (bulge). If the contact constraint is preventing that bulge — for example, if the housing geometry traps the rubber — the material pile-up causes elements in the corner to become very thin and eventually invert.

A few things to try: First, ensure your contact pair has sufficient clearance for the expected bulge direction — don't over-constrain the deformation path. Second, use hybrid elements for the rubber (C3D8RH or C3D8H) — these properly handle the nearly-incompressible behavior of rubber. Standard C3D8R elements will volumetrically lock under large compression of incompressible materials, causing artificial stiffness and extreme stress concentrations at corners.

Third, refine the mesh specifically in the contact corner region. The element that's distorting is probably too coarse to accurately represent the stress gradient at the contact edge. A finer mesh distributes the deformation over more elements, preventing any single element from taking all the strain.

The strain increment has exceeded fifty times the strain to cause first yield at N points
Abaqus/Standard Elastoplastic / Crashworthiness Severity: Warning → Fatal if widespread

What This Means

During plastic strain integration (radial return mapping), the proposed strain increment is 50× larger than the elastic yield strain. The integration algorithm can still compute a result, but accuracy is significantly degraded — the hardening slope and stress state may be wrong by a large factor.

Root Causes

  • Time increment too large for the strain rate in plastic zones
  • Explicit simulation with excessively large mass scaling (artificially inflated time step)
  • Crash/impact problem being attempted with implicit quasi-static solver
  • Localized plastic strain in a stress concentration without mesh refinement

Fix — Step by Step

1
Reduce the maximum time increment. Add to the *Static keyword: MAXINC=0.001 (or smaller if needed). The solver will apply smaller load increments through the plastic region.
2
For explicit analysis, check mass scaling factors. If mass scaling > 100×, the effective time step is too large for accurate plasticity. Reduce mass scaling or refine the mesh in the critical region to increase the stable time step naturally.
3
For crash/impact problems: switch to Abaqus/Explicit or LS-DYNA. The explicit method takes thousands of tiny steps automatically sized by the CFL condition, avoiding this problem entirely. Implicit quasi-static analysis is fundamentally not the right tool for dynamic crash events.
4
Review the stress-strain curve data. If your plastic data has a steep hardening slope with very few data points, add more tabular points in the region where yielding occurs to allow smooth integration.

ANSYS Mechanical Errors

Pivot term less than zero *** Zero or negative pivot term (DOF X, node Y)
ANSYS Mechanical / Mapdl Linear & Nonlinear Static Severity: Fatal

What This Means

During direct stiffness matrix factorization (ANSYS uses a sparse direct solver by default), a diagonal pivot element became zero or negative. A zero pivot means the matrix is singular — the system has no unique solution. A negative pivot indicates the stiffness matrix is not positive semi-definite, which typically means either structural instability or an incorrect material definition.

Root Causes

  • Negative stiffness (negative pivot): Material with negative tangent modulus (post-necking data past ultimate stress), numerical instability in UMAT/UANISO, or compressive preload exceeding Euler critical load
  • Zero pivot (singular): Rigid body mode — missing constraint, disconnected geometry, symmetry BC applied incorrectly
  • Near-zero pivot (warning): Extreme stiffness ratio between adjacent materials (e.g., steel + air in thermal-structural coupling)

Fix — Step by Step

1
Read the DOF and node number from the error message. In ANSYS Mechanical, use Tools > Worksheet > Select by Node ID to locate that node. What does the model look like there?
2
For a zero pivot (singular): run a modal analysis (Vibration > Modal) with the same BCs. A rigid body mode (near-zero frequency, ~0 Hz) confirms the singularity. Fix the missing constraint.
3
For negative pivot in a nonlinear analysis: plot the force-displacement curve. If the slope goes negative, the model is past a structural limit point. Apply a small stabilization damping in the step settings, or use arc-length control.
4
Check material data: in ANSYS, go to Engineering Data and plot the stress-strain curve. Ensure the slope (tangent modulus) is always positive. Do not input data past necking (ultimate stress) for standard plasticity models — this creates negative tangent modulus and a non-positive-definite stiffness matrix.
5
If using contact, check for initial penetration or grossly misaligned contact pairs. In ANSYS, use Contact Tool > Initial Information to check gap/penetration at the start of analysis.
🧑‍🎓

I'm seeing "Pivot term less than zero" in ANSYS for a pre-stressed bolt analysis. The bolt is modeled with pretension load. Could the pretension itself cause a negative pivot?

🎓

Yes, it can — and this is a subtle and common issue in pretension modeling. When you apply pretension using a pre-tension section (bolt pretension load), ANSYS introduces an internal displacement constraint that "shortens" the bolt. If the compressive axial force in the bolt exceeds the Euler critical buckling load for that cross-section length, the geometric stiffness matrix becomes negative definite and you get the negative pivot error.

For a typical structural bolt this shouldn't happen at realistic pretension values — but it can occur if the mesh at the pretension section is poorly conditioned, or if the bolt geometry is very slender (high length-to-diameter ratio).

More likely in your case is a Step 1 issue: in ANSYS bolt pretension analysis, the first load step locks the bolt at its specified pretension force. If the surrounding structure isn't adequately constrained at this step (for example, the flanges are free to separate or rotate), the under-constrained system produces the negative/zero pivot. Make sure all external boundary conditions are active from Step 1.

Element X has degenerated — Jacobian ratio exceeds limit
ANSYS Mechanical Meshing / Nonlinear Severity: Warning (meshing) / Fatal (nonlinear)

What This Means

The element's Jacobian ratio — the ratio of maximum to minimum Jacobian determinant values sampled at the element's integration points — exceeds the acceptable limit (default: 30 for most ANSYS element types, 10 for quadratic elements). This means the element is severely distorted and the isoparametric mapping from element coordinates to physical coordinates is numerically unreliable.

Root Causes

  • Highly curved geometry meshed with coarse elements
  • Sharp re-entrant corners where elements become warped
  • Thin features with aspect ratios above 20:1
  • Large deformation analysis where elements distort during solution

Fix — Step by Step

1
In ANSYS Meshing, run Mesh > Show Mesh Metrics > Jacobian Ratio. This colors elements by Jacobian ratio — identify the problematic regions visually.
2
Reduce element size in the flagged regions using local mesh controls: Insert > Sizing > Body of Influence around the problematic geometry. Aim for a Jacobian ratio below 10.
3
For sharp corners (re-entrant angles): add a small fillet (radius = 0.5–1× element size) to the CAD geometry before meshing. Sharp corners with angles less than 45° will always produce poor Jacobian ratios regardless of mesh refinement.
4
For quadratic elements on curved surfaces: reduce the element size so that element edges more accurately approximate the curvature. Alternatively, switch to linear elements (faster, less sensitive to distortion) if accuracy requirements allow.

OpenFOAM Errors

Matrix singular or near singular — residual from linear solver: INF or NaN
OpenFOAM (all solvers) Linear Solver Failure Severity: Fatal

What This Means

The linear algebraic system assembled for a field variable (pressure, velocity, etc.) could not be solved — the coefficient matrix is singular or the iterative solver diverged to infinity. This is typically a symptom, not a root cause: something in the CFD model or mesh caused the matrix to become ill-conditioned.

Root Causes

  • All-Neumann pressure boundary conditions (no pressure reference point) — system is underdetermined
  • Extreme mesh non-orthogonality causing off-diagonal coefficients to dominate
  • Velocity field has blown up, making the convection matrix non-diagonally dominant
  • Physical time step is too large — cell Courant number >> 1

Fix — Step by Step

1
Check your pressure boundary conditions. For an incompressible flow with only inlet velocity and outlet zero-gradient conditions, the pressure is indeterminate by a constant — add a reference pressure point. In OpenFOAM, use pRefCell 0; pRefValue 0; in fvSolution under the SIMPLE or PISO block.
2
Run checkMesh and look at the non-orthogonality statistics. Maximum non-orthogonality above 85° almost always causes matrix singularity. Fix the mesh before attempting to solve.
3
Reduce the time step. For incompressible flows with explicit-type schemes, the Courant number must be below 1. Use adjustTimeStep yes; with maxCo 0.5; in controlDict.
4
Check for errors in boundary conditions that may have created unphysical initial velocity values (e.g., a typo setting velocity to 10000 m/s). The blockMesh or initial condition setup step should be reviewed.
FOAM FATAL ERROR: Maximum number of iterations exceeded
OpenFOAM (simpleFoam, icoFoam, pimpleFoam) Iterative Solver Severity: Fatal

What This Means

The iterative linear solver (GAMG, PCG, PBiCGStab, etc.) assigned to solve a field variable reached its maximum iteration count without achieving the specified tolerance. This means the linear system is either extremely ill-conditioned, the initial residual is too high for the tolerance setting, or there is an underlying physical instability causing the system to be non-convergent.

Root Causes

  • Residual tolerance set too tight (tolerance 1e-12) for an ill-conditioned problem
  • Max iterations set too low (maxIter 100) for a large or complex mesh
  • Preconditioner not suitable for the equation type (e.g., PCG for asymmetric matrix)
  • Diverging outer iterations feeding increasingly ill-conditioned linear systems to inner solver

Fix — Step by Step

1
In fvSolution, increase maxIter for the failing field. For pressure with GAMG, set maxIter 200; as a starting point. Also check that the relTol (relative tolerance) is set to 0.1 or similar — this allows early exit when the relative reduction is sufficient even if absolute tolerance isn't met.
2
Switch the pressure solver to GAMG with appropriate settings for your problem type. Example for incompressible pressure: 
p
{
    solver          GAMG;
    smoother        GaussSeidel;
    tolerance       1e-6;
    relTol          0.1;
    maxIter         200;
}
3
For asymmetric systems (convection-dominated, turbulence equations), use PBiCGStab (bi-conjugate gradient stabilized) with DILU preconditioner, not PCG (which requires symmetric matrices).
4
Reduce the outer iteration under-relaxation factors. If the outer SIMPLE loop is diverging, the linear systems it generates become progressively worse. Lower relaxationFactors for U, k, epsilon to 0.4, 0.3, 0.3 respectively and retry.
🧑‍🎓

I see "FOAM FATAL ERROR: Maximum number of iterations exceeded" for the pressure equation specifically. I increased maxIter to 500 but it still fails. The mesh looks fine in checkMesh. What else could cause this?

🎓

If the mesh is clean and increasing maxIter doesn't help, the problem is likely that your velocity field has diverged enough that the pressure correction equation — which depends on the velocity field through the divergence of velocity — has become completely unsolvable. It's not a solver settings issue; it's that you're asking the linear solver to solve an incoherent system.

Look at the preceding output lines. Before the fatal error, you should see the outer residuals for U (velocity). Are they growing, or have they already gone to infinity? If U residuals went to infinity first, the pressure failure is a secondary effect.

The velocity divergence typically comes from CFL violation or a boundary condition error. Check: (1) your inlet velocity magnitude — is it physically reasonable? (2) your outlet boundary condition — for incompressible flows, inletOutlet or zeroGradient is correct; do not use a fixed-value velocity at the outlet. (3) Any rotating regions or MRF (Multiple Reference Frame) zones — improper MRF setup is a common source of velocity blow-up that then kills the pressure solve.

LS-DYNA Errors

*** Error *** Negative volume in brick element N at time T
LS-DYNA (Explicit) Crash / Impact / Forming Severity: Fatal (terminates analysis)

What This Means

A hexahedral (brick) element has undergone inversion — its volume has become negative, meaning the element is physically inside-out. In LS-DYNA's explicit algorithm, a negative volume is detected at the element level and immediately terminates the simulation. This is one of the most common fatal errors in crash and forming simulations.

Root Causes

  • Time step too large — explicit CFL condition violated, element advances past inversion threshold in a single step
  • Excessive hourglass energy amplification in single-point (reduced) integration elements
  • Contact penetration — impactor penetrates through target element, causing inversion
  • Initial geometry issue — element is nearly flat or has near-zero volume before loading even begins
  • High-velocity impact causing plastic strain localization faster than the mesh can resolve

Fix — Step by Step

1
Find the failing element in the LS-DYNA log (d3hsp file) — the element number N and time T are reported. In LS-PrePost, isolate that element and check its initial geometry. Is it already distorted before loading?
2
Reduce the time step scale factor. In *CONTROL_TIMESTEP, default is TSSFAC=0.9. Reduce to 0.67 or 0.5. This gives the element more integration points per unit deformation and prevents jumping past the inversion threshold.
3
Check hourglass energy. In *DATABASE_GLSTAT or *DATABASE_MATSUM, look at the hourglass energy (HE). If HE/IE (internal energy ratio) exceeds 0.10 (10%), hourglass modes are dominating. Change the hourglass control in *SECTION_SOLID: set ELFORM=2 (fully integrated) or switch to Type 1 with IHQ=6 (Belytschko-Bindeman enhanced).
4
Enable element deletion as a fallback: in *MAT_XXX, set FAIL parameter (effective plastic strain at failure). Elements exceeding this strain are deleted rather than going negative. This is physically justified for ductile fracture simulations.
5
Check contact penetration in the initial configuration. In *CONTROL_CONTACT, enable automatic surface orientation (IOSENFLAG=1) and initial penetration checking (IGNORE=2). Initial penetrations cause immediate large contact forces that invert elements in the first few time steps.
🧑‍🎓

I'm running a car door impact simulation in LS-DYNA. It works fine up to 15 ms, then at 15.2 ms I get "Negative volume in brick element 47823." I looked at element 47823 and it's in the foam energy absorber inside the door panel. Why would the foam element go negative?

🎓

Foam elements going negative in an impact simulation is a classic and painful problem. Automotive foam (polyurethane, polystyrene) can be compressed to very high strains — 80% volumetric compression is not unusual in a door impact. At such extreme compression, the element literally runs out of room to deform and inverts.

The key issue is the material model. For foam, you should be using *MAT_LOW_DENSITY_FOAM (MAT_57) or *MAT_CRUSHABLE_FOAM (MAT_63) in LS-DYNA. These models include a load curve for compressive crush behavior and handle large volumetric compression without numerical issues. Do not use a simple elastic or elastic-plastic model for foam — these models don't have the compaction response needed and will invert when compression is large.

Also: if you're using brick elements for the foam, switch to ELFORM=1 (default single-point hexahedral) with IHQ=4 (viscous hourglass control). The viscous option is better than stiffness-based hourglass for highly compressible foams. Additionally, ensure the foam mesh is fine enough to resolve the crush front as it propagates through the material — typically 3–5 elements through the crush direction is the minimum for reasonable accuracy.

Articles in This Section

Singular Matrix
Zero / Negative Pivot
Ill-Conditioned Matrix
Indefinite Matrix
Factorization Error
Rank Deficiency
Numerical Overflow / NaN
Out of Memory
BLAS/LAPACK Error
License Failure
Author: NovaSolver Contributors (Anonymous Engineers & AI)

Related Topics

Error Database Convergence Errors Mesh Quality Errors Material Errors Verification & Validation Open Source Solvers