Learn how to evaluate centrifugal stresses in rotating components using static structural analysis in Ansys Mechanical — with theoretical validation, rotational inertia loads, and modal analysis for resonance risk assessment.
Centrifuge machines are widely used in industrial and laboratory applications to separate materials based on their density. During operation, these machines rotate at extremely high speeds, generating significant centrifugal forces. These forces act radially outward from the axis of rotation and induce stresses throughout the rotating components. Evaluating these stresses is critical for ensuring the structural integrity, safety, and performance of the system.
To analyse such stresses without explicitly simulating rotation, rotational velocity can be applied within a Static Structural analysis framework in Ansys Mechanical. In this approach, the part itself does not physically rotate; instead, rotational effects are represented as inertial body loads within the rotating reference frame formulation.
The primary aim of this study is to evaluate stress in a component rotating at a constant angular velocity. Since the rotation is steady (no change in speed), transient effects such as acceleration and damping are not significant. Including them would unnecessarily complicate the analysis, requiring additional unknowns to be solved.
Static analysis offers a simplified yet effective solution in such cases:
In this formulation, gravity, rotational velocity, and rotational acceleration are treated as inertial loads and included in the force term F(x) of the governing equation.
The centrifugal force on a particle moving with a velocity on a curve is given by:
F = ρ · ω² · r
Where: ρ = density (ton/mm³), ω = rotational speed (rad/s), r = radius (mm)
An important observation is that the centrifugal body force density increases linearly with radial distance from the axis of rotation. Therefore, elements located farther from the centre experience higher forces.
For a solid homogeneous circular disk of uniform thickness, the radial stress at any point at distance r from the centre is (Roark's Formula, 7th Ed., Page 746):
σᵣ = ρ · ω² · (R² − r²) / 8 · (3 + μ)
Although the outer edge experiences the highest centrifugal force, it is free to deform outward and therefore carries zero radial stress. In contrast, the centre must resist the cumulative outward pull of all surrounding material — resulting in maximum stress at the centre.
To simulate the system in Ansys Mechanical:
Key points to remember:
Theoretical verification at the outer edge (r = R = 203 mm): σᵣ = 0 MPa — confirming that radial stress is zero at the outer boundary.
At r = 12.5 mm (inner region), with R = 203 mm, μ = 0.25, ρ = 7.95×10⁻⁹ ton/mm³, ω = 209.44 rad/s: the theoretical radial stress = 5.82 MPa.
The FEA results show slightly higher stress values than the analytical calculation. This deviation is expected due to the influence of boundary conditions, geometric constraints, and numerical approximations within the simulation.
A pre-stressed modal analysis is linked from the static structural result to identify natural frequencies under the centrifugal loading state. The critical operating frequency is:
f₁ = ω / 2π = 209.44 / 2π = 33.33 Hz
Natural frequencies within ±10% of operating harmonics should be investigated for potential resonance risk:
Static structural analysis is an efficient and practical method for evaluating stresses in rotating components operating at constant angular velocity. By neglecting transient effects such as acceleration and damping, the governing equations are simplified, making the analysis more computationally efficient while still providing accurate stress predictions.
In this method, the component does not physically rotate; instead, the coordinate system rotates, allowing centrifugal effects to be modelled as inertial loads. When combined with modal analysis, this approach also enables identification of critical frequencies and potential resonance risks.
Static analysis serves as a powerful tool for preliminary design and validation of rotating systems, ensuring structural integrity without the need for complex transient simulations. — Wakar Ali Mohammad Khan, CADFEM Mechanical Business Unit
Fluids Tìm hiểu cách Ansys SimAI kết hợp với Ansys Fluent tạo nên quy trình AI-Driven Simulation mới, giúp tăng tốc thiết kế và tối ưu hóa nhanh hơn hàng trăm lần so với CFD truyền thống.
Read Article →
MBU Many structural failures originate at component interfaces. Learn how to use contact nonlinearity in Ansys Mechanical to capture separation, friction, sliding, and re-contact — phenomena that linear analysis consistently misses.
Read Article →
DME See how Ansys STK Astrogator transforms Sun–Earth L1 mission planning — from orbital injection and halo orbit refinement to station-keeping dynamics — entirely in simulation before launch.
Read Article →Connect with CADFEM experts for advanced simulation, automation, and engineering solutions tailored to your industry.