The SOLID65 element in ANSYS is specifically designed for modeling the nonlinear behavior of concrete structures, including cracking under tensile loads and crushing under compression. This post provides a comprehensive guide on how to effectively use SOLID65 for reinforced concrete simulations, covering material property definitions, reinforcement modeling, crack propagation, and convergence strategies.

How to Use the SOLID65 Element in ANSYS

1. Defining Basic Input Data

The SOLID65 element in ANSYS is designed for modeling concrete behavior, including both the bulk material properties of concrete and the embedded reinforcement (typically steel rebar). The MAT command is used to define concrete material properties, while reinforcement is specified using real constants, including:

• Material type
• Volume fraction of reinforcement within the concrete
• Rebar orientation angles (THETA and PHI)

If the reinforcement volume fraction is set to zero or assigned a code of 0, ANSYS will ignore reinforcement effects, treating the material as plain concrete.

To define reinforcement properties:

Main Menu > Preprocessor > Real Constants > Add/Edit/Delete
This menu allows users to input values such as rebar material, volume fraction, and orientation angles (THETA, PHI).

Reinforcement Placement Considerations

• If rebar is uniformly distributed, using real constants is appropriate.
• If rebar placement is non-uniform, alternative modeling techniques should be used, such as explicit reinforcement elements (beam or truss elements).

From a shear resistance perspective, placing stirrups randomly may not always be ideal. Instead, reinforcement should be properly arranged within the concrete structure. If reinforcement is not uniformly distributed, alternative modeling approaches may better simulate tensile load resistance in longitudinal rebars.

Tip: If reinforcement is highly concentrated in certain areas, explicit reinforcement modeling is recommended for more accurate results.

2. Keyoption (KEYOPT) Definitions for SOLID65 in ANSYS

When defining SOLID65 in ANSYS, several keyoptions (KEYOPT) are available to control element behavior, including deformation, reinforcement modeling, and solution output. Below are the keyoptions commonly used for reinforced concrete modeling:

• KEYOPT(1): Extra Displacement Shapes
  • 0 → Include extra displacement shapes (default).
  • 1 → Suppress extra displacement shapes (reduces computation time).
• KEYOPT(3): Behavior of Fully Crushed Elements
  • 0 → Base setting (standard crushing behavior).
  • 1 → Suppresses mass and applied loads for fully crushed elements, preventing numerical instability.
  • 2 → Applies Newton-Raphson load vector correction for crushed elements.
• KEYOPT(5): Concrete Linear Solution Output
  • 0 → Print concrete linear solution at centroid only (default).
  • 1 → Repeat solution at each integration point.
  • 2 → Print nodal stress output for linear solution.
• KEYOPT(6): Concrete Nonlinear Solution Output
  • 0 → Print nonlinear solution at centroid only.
  • 3 → Print nonlinear solution at all integration points (provides more detailed stress distribution).
• KEYOPT(7): Stress Relaxation after Cracking
  • 0 → No tensile stress relaxation after cracking.
  • 1 → Include tensile stress relaxation, improving convergence stability in nonlinear analysis.
• KEYOPT(8): Warning Messages for Crushed Elements
  • 0 → Print warning messages when elements fully crush (default).
  • 1 → Suppress warning messages for fully crushed elements (useful for large models with excessive warnings).

🔹 Example ANSYS Implementation

ET,1,SOLID65   ! Define SOLID65 element type
KEYOPT,1,1,1   ! Suppress extra displacement shapes
KEYOPT,1,3,2   ! Apply Newton-Raphson correction for crushed elements
KEYOPT,1,5,2   ! Enable nodal stress output for linear solution
KEYOPT,1,6,3   ! Print nonlinear solution at all integration points
KEYOPT,1,7,1   ! Include stress relaxation after cracking
KEYOPT,1,8,0   ! Print warning messages for crushed elements

This detailed explanation improves the understanding of SOLID65 keyoptions while ensuring proper setup for realistic concrete behavior modeling in ANSYS. 🚀

3. Defining Concrete Material Properties

Concrete material behavior is set in:

Main Menu > Preprocessor > Material Props > Material Models > Concrete

Important parameters include:

• Shear Transfer Coefficient (ShrCf-Op & ShrCf-Cl): Governs shear force transmission across open and closed cracks.
• Uniaxial Tensile Strength (UnTensSt): Determines when concrete cracks under tension.
• Uniaxial and Biaxial Compressive Strength (UnCompst & BiCompSt): Defines how concrete behaves under compressive loads.
• Hydrostatic Pressure Sensitivity (HydroPrs): Adjusts the concrete’s volumetric response under pressure.
• Crack Softening Factor (TenCrFrac): Regulates post-crack stress degradation.

Recommended Shear Transfer Coefficients

• For open cracks: 0.5 (standard beams), 0.25 (high-stress beams)
• For closed cracks: Between 0.9 - 1.0.

Note: If the uniaxial tensile strength (UnTensSt) is set to -1, ANSYS will ignore crack-related effects, making the concrete behave like a Von Mises plasticity model (which does not accurately capture brittle failure behavior).

Before concrete exceeds its elastic limit, the SOLID65 element can be used for:

• Linear elastic behavior
• Nonlinear elasticity
• Elasto-plastic deformation

Available material models in ANSYS include:

• Multilinear Isotropic Hardening (TB,MISO)
• Multilinear Kinematic Hardening (TB,MKIN)
• Drucker–Prager Model (TB,DP) (used for high-pressure concrete applications)

Caution: If concrete deforms excessively, it will lose its brittle behavior, making some plasticity models unsuitable.

4. Additional Considerations

When monitoring crack formation and failure in concrete, attention should be given to time-dependent crack propagation to avoid situations where tensile loads are transferred through cracks.

• Poisson’s effect can amplify stress concentrations near crack tips, which should be controlled.
• Crack propagation typically occurs perpendicular to the direction of maximum tensile stress.

After cracks form and propagate, load transfer depends on the bond-slip effect between concrete and reinforcement. If a crack crosses reinforcement without proper bond strength, the load transfer will be weak, leading to structural instability.

To prevent highly localized stress concentrations, it is advisable to:

• Increase element size in high-stress regions.
• Apply damping layers to reduce stress intensification.

5. Convergence Issues in ANSYS Simulations

The primary factors affecting convergence in ANSYS simulations of concrete structures include:

• Element size
• Number of substeps
• Convergence criteria settings

Element Size Effects

• Smaller elements capture local stress concentrations better but may cause convergence issues.
• Larger elements may smooth out stress variations but reduce accuracy.

If highly localized stress areas appear, increasing element size may help reduce computational errors.

Number of Substeps (Time Steps)

• More substeps improve accuracy but significantly increase computation time.
• Too few substeps can lead to convergence failures.

For nonlinear reinforced concrete analysis, excessively high or low substep numbers can both negatively impact convergence. It is best to adjust the substep count dynamically based on the model’s stress state.

Convergence Accuracy Settings

• Increasing accuracy tolerance does not always fix convergence issues.
• Expanding the convergence criteria range may improve simulation speed.

Recommendation: Convergence tolerance should not exceed 5% (default is 0.5%).

6. Conclusion

To ensure accurate and stable ANSYS simulations of reinforced concrete structures using SOLID65, follow these key principles:

1. Define concrete and reinforcement properties accurately.
2. Use proper reinforcement modeling techniques (real constants vs. explicit rebar elements).
3. Carefully control crack formation and propagation parameters.
4. Optimize meshing and convergence settings to ensure numerical stability.