Bonded vs No-Separation Contact in ANSYS Mechanical Static Structural

The wrong contact type can hide a gap

Imagine a static structural model of two plates clamped together by a bolt. The operating load keeps the interface in compression, so it seems safe to assume the faces never part. An engineer sets the contact type to Bonded because it solves quickly and returns a smooth stress field. The problem is that a bonded interface artificially carries tensile shear across the joint. If the real clamp load drops or a local bending moment peels the plates apart, the model will not show it.

Useful takeaway: bonded contact should be reserved for interfaces that are physically joined, such as welded or adhesive bonds. For clamped surfaces that are expected to stay closed but may slide, no-separation contact is usually the more honest choice.

Assumes ANSYS Mechanical with the Static Structural system and the default penalty-based contact formulation.

What each contact type actually does

Bonded constrains the contacting faces to behave as one continuous region. It transfers both normal and shear traction and does not allow relative motion or separation. It is appropriate for welded seams, glued layers, or surfaces that are monolithic for analysis purposes.

No Separation allows compression and sliding but prevents tensile opening. The interface cannot carry tension, so if the load tries to pull the faces apart, the contact opens instead of transferring shear. This fits bolted, clamped, or bearing interfaces that remain closed under the expected operating loads. It assumes contact exists at time zero and cannot represent an initial gap or impact.

ANSYS Mechanical reports contact behavior through result objects such as Contact Pressure, Contact Status, and Sliding Distance. The contact formulation also matters: Small Sliding is cheaper and works when surfaces move only slightly relative to each other; Large Sliding is more expensive but better when contact areas shift significantly.

Worked example: clamped plate assembly

Model two aluminum plates joined by a single bolt in a Static Structural analysis. The bolt preload keeps the interface in compression, and the external load is transverse.

1. Open ANSYS Mechanical and create a Static Structural analysis.
2. Under Model, right-click Connections and insert Contact.
3. Select the contacting faces. Assign one surface as Contact and the mating surface as Target.
4. In the Details panel, set Contact Type to No Separation.
5. Set Contact Formulation to Small Sliding if the plates shift only slightly; choose Large Sliding if the contact patch is expected to move across the faces.
6. Leave Penalty Stiffness Factor at the default unless the solver reports convergence trouble or the contact shows excessive overlap. A value that is too high can stall convergence; a value that is too low allows artificial penetration.
7. Solve the analysis.
8. Insert results for Contact Pressure and Contact Status.

Expected checks: Contact Status should show the interface as closed over the loaded region, and Contact Pressure should be compressive. If large areas show open status under a load that should keep the joint shut, the no-separation assumption or the load path may be wrong.

To see why the choice matters, duplicate the analysis and change only Contact Type to Bonded. Compare the total reaction force at the supports and the maximum contact penetration. If the bonded model transfers shear that the no-separation model cannot, or if the no-separation model shows contact opening where the bonded model shows stress, the physical assumption is driving the result.

There is no automatic rollback after changing contact type. Save a duplicate project or duplicate the analysis before switching so you can compare both formulations.

Limitations and practical verification

• No-separation contact cannot model an initial gap, loss of contact at startup, or impact. If those conditions exist, use a contact formulation that allows separation.
• Bonded contact can hide real-world separation because it artificially carries tension across the interface.
• Nonlinear contact may fail to converge if load increments are too large. Enable Auto Time Stepping or use smaller load steps if the solver reports contact difficulty.
• Mismatched surface meshes at a contact pair can produce noisy pressure. Refine the contact surface mesh or use pairing controls, then confirm that pressure and reaction force stabilize between refinements.

Practical verification: compare the total reaction force and maximum penetration against a simplified hand calculation or a fully bonded reference model. Open Solution Information and check contact iteration counts. Refine the mesh once more and confirm that Contact Pressure and reaction force change by only a small amount. If they do not, the contact discretization is still too coarse.

Closing checklist

• Is the interface physically joined? Use Bonded.
• Is it clamped and expected to stay closed under compression? Use No Separation.
• Are there gaps, impact, or possible lift-off? Neither assumption is sufficient; allow separation in the contact definition.
• After solving, inspect Contact Pressure and Contact Status, compare reaction forces, and refine the contact mesh until results stabilize.