Augmented Lagrangian Contact in ANSYS Mechanical: Settings That Actually Converge

If your static structural model with frictional contact keeps bouncing between substeps or reports visible penetration, the fix is usually not a smaller time step — it is switching the contact formulation from Pure Penalty to Augmented Lagrangian and tuning two numbers: the penalty factor and the stabilization factor. Done right, this typically cuts Newton‑Raphson iterations and drives average penetration to near zero.

Why Pure Penalty struggles with friction

Contact in ANSYS Mechanical is enforced numerically. The default Pure Penalty method treats the contact interface like a stiff spring: any penetration is resisted by a force proportional to a normal stiffness. To keep penetration small you raise the stiffness, but a very stiff contact makes the global matrix ill‑conditioned, so the solver needs many iterations or fails to converge. Lower the stiffness and the solver converges easily but the parts visibly sink into each other.

The Augmented Lagrangian method breaks this trade‑off. It starts with a moderate penalty stiffness, then adds iterative correction terms (Lagrange multiplier updates) that drive the residual penetration toward zero without raising the stiffness further. You get penalty‑like robustness with much lower final penetration.

A worked configuration: two blocks in frictional contact

Consider a steel block pressed onto a steel base with a downward load, friction coefficient 0.3, in a static structural analysis. In the Mechanical tree, select the contact region and apply:

• Definition → Frictional, Friction Coefficient = 0.3
• Behavior → Formulation = Augmented Lagrangian
• Normal Stiffness = Factor, Penalty Factor (FKN) = 0.1
• Stabilization Damping Factor = 0.5
• Interface Treatment = Adjust to Touch, with a small clearance of 0.001 mm if the mesh leaves a tiny gap

These values assume a 2023 R1‑or‑later Mechanical interface; the same options exist in older releases but some labels differ (older versions expose FKN and FTN via command objects).

The penalty factor scales the automatically computed normal stiffness. 0.1 is a common starting point for metal‑on‑metal contact; softer materials (rubber, polymers) often need 0.01 or lower because the default stiffness is derived from element stiffness and can be wildly oversized relative to the bulk material.

Stabilization damping adds artificial normal and tangential damping during the first substeps, which suppresses the rigid‑body rocking that occurs before contact fully engages. It should decay as the load ramps — check that it does, because leftover damping energy at the end of the step is a sign of a problem (more on that below).

Verifying the result

Insert a Contact Tool under Solution and evaluate:

• Average Penetration — should be near zero, on the order of 1e‑4 mm or less for this example. Persistent penetration means the penalty factor is too low or the mesh is too coarse at the interface.
• Contact Status — confirm the expected region is actually closed/sticking, not open or sliding everywhere.
• Stabilization Energy (via Solution Information → Energy summary) — should be a small fraction of total strain energy, typically a few percent at most. Large stabilization energy means the damping is carrying real load and your results are not trustworthy.

A quick sensitivity check: rerun with penalty factors of 0.01, 0.1, and 1.0. You should see iteration count and penetration trade‑off, with 0.1 usually near the sweet spot for stiff metals. If results change materially between 0.1 and 1.0, your model is contact‑stiffness‑sensitive and needs mesh refinement at the interface rather than more penalty.

Limits of the method

Augmented Lagrangian assumes small‑to‑moderate sliding per substep. Large relative sliding, gross rigid‑body motion, or contact that opens and closes violently (snap‑through, impact) can still diverge — those cases need smaller substeps, more substeps in the contact‑chattering region, or a different formulation such as Normal Lagrange for zero‑penetration requirements.

The penalty and stabilization factors are scale‑dependent. If you change materials, element size, or units, re‑evaluate them; a factor that worked for steel will be wrong for a silicone gasket.

Common mistakes

1. Cranking Pure Penalty stiffness to 10 or 100. This produces stiff, unstable contacts and long solve times. Switch formulation instead of escalating stiffness.
2. Zero clearance with Adjust to Touch. If the mesh gap is real geometry, forcing instant closure with no ramp introduces a sudden load step. Give the solver a small tolerance or ramp the load over substeps.
3. Leaving stabilization on at full strength for the whole analysis. Verify stabilization energy decays; if not, reduce the damping factor or fix the underlying instability (often insufficient constraints on one body).
4. Ignoring penetration output. Converged does not mean correct. Always inspect the Contact Tool after the solve.
5. Applying one factor globally. Different contact pairs in the same model may need different FKN values; set them per contact region.

For the underlying equations and recommended ranges, see the Contact Technology Guide in the ANSYS Help, specifically the sections on the augmented Lagrangian formulation and contact stiffness settings.