© 2023 Created by blog.championxperience.com
Introduction
Radar antennas, particularly those housed under radomes, must withstand challenging field conditions. They are exposed not only to static loads—such as gravity, mounting stresses, and clamping forces—but also to vibrational excitations from wind, platform motion, and other environmental factors. Maintaining signal integrity under these conditions is critical, as even minor deformations can compromise system performance.
To address this, we developed a comprehensive simulation workflow using SOLIDWORKS and ANSYS Mechanical for an Antenna + Jig + PCB system. The workflow combines static structural analysis with prestressed modal analysis, enabling engineers to:
Evaluate displacement and stress fields under static loads
Identify resonant frequencies and vibration modes under pre-stress
Assess potential risks to signal stability
Inform design improvements for reliable operation
This approach ensures that both structural robustness and dynamic performance are considered in early-stage design.
Theoretical Background
A standard modal analysis assumes no initial stress. But structures often operate under pre-stress (gravity, clamping forces, bolt preload, thermal loads). This pre-stress modifies the structure’s effective stiffness via geometric (stress) stiffness, altering natural frequencies and mode shapes.
In practice:
– Tensile pre-stress tends to increase modal frequencies.
– Compressive pre-stress may decrease them.
This effect is captured by chaining a static analysis to a modal analysis with stress stiffness included.
This methodology is recommended in ANSYS Innovation Course materials under “Prestressed Modal Analysis.”
Model Setup
Geometry and Material Properties
The simulation model consists of three primary components:
PCB: Modeled as FR-4, an orthotropic elastic material, capturing directional stiffness properties.
FR stands for flame retardant, and the number 4 indicates woven glass-reinforced epoxy resin. The characteristics of FR4 vary significantly depending on the manufacturer, although it is commonly known for its mechanical strength and water resistance. This material performs as an insulator in PCBs by isolating adjacent copper planes while also providing overall mechanical strength
FR4 Laminate Structure – Source Image from ProtoExpress
Jig: Aluminum alloy, representing the mounting fixture.
Base Plate: Aluminum alloy, providing structural support.
Figure 1: SolidWorks Antenna model.
Figure 2: Connections between plates and Jig.
Bonded contacts were defined at all interfaces (PCB ↔ Jig ↔ Base plate) to ensure unified load transfer.
Loads & Constraints
- Three fixed supports on the underside of support pillars (translations + rotations fixed).
- Gravity ≈ 9.8066 m/s² applied globally.
- No additional loads (e.g. aerodynamic, thermal) at this stage.
Figure 3: Loadings and Constraints.
This setup ensures that the pre-stress environment mimics realistic assembly conditions before dynamic analysis.
Meshing & Solver Choices
A refined mesh in critical zones (edge transitions, interfaces) ensures accurate stress capture. The static step is linear elastic; the modal (eigenvalue) step is run with Prestress enabled, linked to the static solution. In ANSYS Mechanical, one must set the modal “Pre-Stress Defined By” to use the static solution and choose how contact status propagates (e.g. True Status, Force Bonded, Force Sticking).
Figure 3: Mesh Details.
Static (Pre-Stress) Results
Figure 4: Total Static Structural Deformation.
| Quantity | Value |
| Average assembly stress | ~ 2.58 × 10⁴ Pa (≈ 0.0258 MPa) |
| PCB region deformation (probe) | ~ 5.07 × 10⁻⁵ m |
| Max total deformation | ~ 5.2 × 10⁻⁵ m (≈ 52 μm) |
| Max von-Mises stress | ~ 1.24 × 10⁵ Pa (≈ 0.124 MPa) |
Interpretation & checks:
Deformations are negligible, within typical PCB mounting tolerances.
Stress levels are well below material yield limits for both Aluminum and FR-4.
Mesh quality was validated to prevent unrealistic stress concentrations near contacts or constraints.
These results confirm that the assembly can safely withstand static loads before performing dynamic vibration analysis.
Prestressed Modal Results
Figure 5: Modal Results.
The first six natural frequencies (with pre-stress) were:
- 87.27 Hz
- 90.06 Hz
- 98.24 Hz
- 111.79 Hz
- 131.08 Hz
- 157.09 Hz
Observation:
Lower vibration modes show bending and warping of the PCB.
Bonded interfaces and stiff constraints increase overall rigidity, shifting frequencies higher compared to a standard modal analysis without pre-stress.
These results help identify resonant frequencies, which is critical for avoiding signal degradation under operational vibration.
Animation showing PCB bending
Video 1:Static + Modal simulation showing PCB bending modes.
Lower modes show significant deformation in the PCB in bending/warping shapes. Because of the bonded interface and stiff constraint, the structure behaves more rigidly, raising frequencies. Comparing against a modal run without pre-stress would highlight the shift introduced by the static load.
Design Guidance & Forward Steps
- Compare modal frequencies to real excitation spectra (vibration, PSD, wind loading) from the operating platform.
- Run harmonic or random vibration analyses using modal results to compute forced responses, amplification factors, and fatigue stress cycles.
- Incorporate damping or isolation (viscoelastic layers, absorbers, vibration isolators) where resonant peaks overlap excitation bands.
- Perform parametric studies varying geometry, stiffness, bonding layout to shift resonances.
- Refine contact definitions (e.g. frictional/slip interfaces) and rerun static + modal to assess possible stiffness degradation under dynamic loads.
- Benchmark with experimental modal testing to validate frequencies and mode shapes against physical measurements.
Alignment with Best Practices
This workflow adheres to ANSYS’s recommended approach for loaded modal analysis: static → modal with stress stiffness. The careful propagation of contact state and inclusion of pre-stress aligns with official tutorials and literature.
Conclusion
This study demonstrates a complete simulation workflow for an antenna-PCB assembly, covering:
Motivation and structural requirements
Model setup in SOLIDWORKS and ANSYS
Static pre-stress analysis
Prestressed modal analysis
Interpretation of results and design guidance
By combining SOLIDWORKS for modeling and ANSYS for simulation, engineers can predict performance under both static and dynamic conditions, identify potential risks, and implement design improvements that maintain signal integrity and reliability in the field.
Aerospace Design and Simulation Engineer at National Aerospace Science & Technology Park (NASTP)
Muhammad Ibrahim is a Mechanical Engineering student at the Institute of Space Technology, focusing on CAD design and engineering simulations. He is proficient in using SOLIDWORKS and ANSYS for product modeling and analysis.
Latest posts by Muhammad Ibrahim (see all)
- Static & Modal Analysis of an Antenna-PCB Jig in ANSYS - 9 October 2025
Subscribe
0 Comments
Oldest
