In recent years, the demand for high-performance six-axis force sensors has grown significantly, particularly in applications such as robotic perception, space docking, and industrial automation. As a key component in intelligent sensing technology, the six-axis force sensor must not only provide accurate force and moment measurements but also exhibit high stiffness to withstand structural loads. Among various designs, the Stewart platform-based six-axis force sensor stands out due to its large load capacity, flexibility, and robustness. However, optimizing its stiffness remains a critical challenge, as traditional design methods relying on theoretical derivations and experimental tests often lead to prolonged development cycles and high costs. In this study, I focus on enhancing the stiffness of a Stewart-type six-axis force sensor through finite element analysis, leveraging software like ABAQUS to simulate and optimize key structural parameters.
The Stewart-type six-axis force sensor consists of six elastic limbs connecting upper and lower platforms, with its performance heavily influenced by parameters such as the distribution radii of spherical hinge points on the upper and lower platforms (denoted as \( R_B \) and \( R_A \)), the distance between platform centers (\( H \)), and the positioning angles of the upper and lower platforms (\( \alpha_B \) and \( \alpha_A \)). These parameters define the sensor’s geometry and directly impact its stiffness characteristics. Through theoretical parameter analysis, I first optimized the basic structural parameters to meet technical specifications, resulting in initial values: \( R_A = 145 \, \text{mm} \), \( R_B = 115 \, \text{mm} \), \( H = 82 \, \text{mm} \), with \( \alpha_A \) ranging from \( 96^\circ \) to \( 105^\circ \) and \( \alpha_B \) from \( 28^\circ \) to \( 32^\circ \). This optimization aimed to balance sensitivity and stiffness, laying the groundwork for further refinement using finite element methods.
To build a reliable simulation model, I employed ABAQUS, a powerful finite element analysis software. The process began with creating a detailed 3D model of the six-axis force sensor, which was then imported into ABAQUS for meshing and analysis. Mesh quality is crucial for accurate results, so I carefully selected tetrahedral quadratic elements (C3D10M) due to their suitability for complex geometries like cylindrical structures and holes. Using a combination of free and swept meshing techniques, I divided the model into simpler regions to ensure high-quality grids. The initial global mesh size was set to 10 mm, with local refinements near holes to maintain 6–8 tetrahedral elements per circular feature, resulting in mesh sizes between 1 mm and 5 mm. To validate the mesh, I applied ABAQUS’s built-in checks for shape factor, face corner angles, aspect ratio, and geometric deviation, ensuring that error counts were zero and warnings were minimal (less than 0.005%). Further, I conducted a mesh sensitivity analysis by varying the approximate global size and observing its effect on normalized strain at a specific strain gauge location. As shown in the analysis, when the global size was reduced to 4 mm or smaller, the strain output stabilized, indicating that a mesh with over 1.5 million tetrahedral quadratic elements provided sufficient accuracy for this six-axis force sensor model.
For boundary conditions and loading, I simulated real-world scenarios to ensure the model’s practicality. The six-axis force sensor was subjected to external force vectors applied through multi-point constraints (MPC) using beam elements. Specifically, I defined an MPC reference point where the resultant force and moment were applied, and the constraints distributed these loads proportionally to 24 threaded holes and 12 pin holes on the upper platform, mimicking actual force transmission. The lower platform’s threaded and pin holes were fixed with encastré constraints to represent a rigid base. To enhance realism, I also modeled an external loading plate attached to the sensor, as stiffness tests often involve such configurations. This included defining contact interactions between the sensor’s upper platform and the loading plate, with tied constraints for screw and pin connections. The full-scale load conditions were based on the sensor’s design capacity: \( F_x = 50,000 \, \text{N} \), \( F_y = 20,000 \, \text{N} \), \( F_z = 20,000 \, \text{N} \), \( M_x = 3,000 \, \text{N·m} \), \( M_y = 3,000 \, \text{N·m} \), and \( M_z = 4,000 \, \text{N·m} \). Stiffness parameters were calculated using the formula \( K = F / \delta \) for translational stiffness and \( K_m = M / \theta \) for rotational stiffness, where \( \delta \) is displacement and \( \theta \) is angular deformation.
To verify the reliability of the finite element model, I compared simulation results with experimental data from a prototype six-axis force sensor. The stiffness values obtained from the simulation—both for the sensor alone and with the external loading plate—were close to the experimental measurements, as summarized in Table 1. For instance, the translational stiffness \( K_x \) was \( 1.254 \times 10^8 \, \text{N/m} \) in the simulation with the loading plate, compared to \( 1.218 \times 10^8 \, \text{N/m} \) in tests, showing a deviation of less than 3%. Similar trends were observed for other stiffness components, confirming that the ABAQUS model accurately captures the behavior of the six-axis force sensor. Notably, the inclusion of the loading plate slightly reduced the simulated stiffness, highlighting the importance of accounting for auxiliary components in design analyses.
| Stiffness Parameter | Simulation (Sensor Only) | Simulation (With Loading Plate) | Experimental Test |
|---|---|---|---|
| \( K_x \, (\text{N/m}) \) | \( 1.338 \times 10^8 \) | \( 1.254 \times 10^8 \) | \( 1.218 \times 10^8 \) |
| \( K_y \, (\text{N/m}) \) | \( 1.493 \times 10^8 \) | \( 1.363 \times 10^8 \) | \( 1.311 \times 10^8 \) |
| \( K_z \, (\text{N/m}) \) | \( 3.121 \times 10^8 \) | \( 2.859 \times 10^8 \) | \( 2.773 \times 10^8 \) |
| \( K_{mx} \, (\text{N·m/rad}) \) | \( 2.179 \times 10^6 \) | \( 1.881 \times 10^6 \) | \( 1.658 \times 10^6 \) |
| \( K_{my} \, (\text{N·m/rad}) \) | \( 2.303 \times 10^6 \) | \( 1.962 \times 10^6 \) | \( 1.735 \times 10^6 \) |
| \( K_{mz} \, (\text{N·m/rad}) \) | \( 4.017 \times 10^6 \) | \( 3.513 \times 10^6 \) | \( 3.205 \times 10^6 \) |
With the validated model, I proceeded to optimize the stiffness of the six-axis force sensor by analyzing the effects of the positioning angles \( \alpha_A \) and \( \alpha_B \). Since \( R_A \), \( R_B \), and \( H \) were fixed after initial theoretical optimization, I varied \( \alpha_A \) from \( 96^\circ \) to \( 105^\circ \) and \( \alpha_B \) from \( 28^\circ \) to \( 32^\circ \) in increments of \( 1^\circ \), conducting multiple simulations to evaluate the six stiffness components: \( K_x \), \( K_y \), \( K_z \) (translational stiffness along x, y, z axes) and \( K_{mx} \), \( K_{my} \), \( K_{mz} \) (rotational stiffness about x, y, z axes). The results revealed that these angles significantly influence stiffness, with optimal values depending on the specific component. For example, \( K_x \) reached its maximum of \( 1.639 \times 10^8 \, \text{N/m} \) at \( \alpha_A = 102^\circ \) and \( \alpha_B = 29^\circ \), while \( K_z \) peaked at \( 3.655 \times 10^8 \, \text{N/m} \) with \( \alpha_A = 100^\circ \) and \( \alpha_B = 30^\circ \). Similarly, rotational stiffness showed distinct optima, such as \( K_{mz} \) achieving \( 4.823 \times 10^6 \, \text{N·m/rad} \) at \( \alpha_A = 100^\circ \) and \( \alpha_B = 30^\circ \). To determine the overall best configuration, I considered the combined effect on all stiffness parameters, leading to the selection of \( \alpha_A = 100^\circ \) and \( \alpha_B = 30^\circ \) as the optimal angles. This choice balanced the improvements across all components, as detailed in Table 2, which compares the stiffness of the initial prototype with the optimized six-axis force sensor.
| Stiffness Parameter | Initial Simulation | Optimized Simulation | Improvement (%) |
|---|---|---|---|
| \( K_x \, (\text{N/m}) \) | \( 1.338 \times 10^8 \) | \( 1.563 \times 10^8 \) | 16.82 |
| \( K_y \, (\text{N/m}) \) | \( 1.493 \times 10^8 \) | \( 1.767 \times 10^8 \) | 18.35 |
| \( K_z \, (\text{N/m}) \) | \( 3.121 \times 10^8 \) | \( 3.655 \times 10^8 \) | 17.11 |
| \( K_{mx} \, (\text{N·m/rad}) \) | \( 2.179 \times 10^6 \) | \( 2.482 \times 10^6 \) | 13.91 |
| \( K_{my} \, (\text{N·m/rad}) \) | \( 2.303 \times 10^6 \) | \( 2.651 \times 10^6 \) | 15.11 |
| \( K_{mz} \, (\text{N·m/rad}) \) | \( 4.017 \times 10^6 \) | \( 4.823 \times 10^6 \) | 20.07 |
The optimization resulted in stiffness improvements ranging from 13.91% to 20.07%, demonstrating the effectiveness of fine-tuning \( \alpha_A \) and \( \alpha_B \) for the six-axis force sensor. To further validate the design, I conducted a safety analysis by examining stress distributions under extreme loading conditions. Using a combined load case of \( M_x = 2,000 \, \text{N·m} \), \( M_y = 2,000 \, \text{N·m} \), \( M_z = 2,000 \, \text{N·m} \), \( F_x = 5,000 \, \text{N} \), \( F_y = 5,000 \, \text{N} \), and \( F_z = 5,000 \, \text{N} \), I compared the von Mises stress in the initial and optimized models. The maximum stress in the optimized six-axis force sensor was 941 MPa, significantly lower than the 1,231 MPa in the initial design. This reduction indicates a higher safety margin, as the optimized structure distributes loads more evenly, minimizing stress concentrations in the limbs and joints. Such improvements are critical for ensuring the longevity and reliability of the six-axis force sensor in demanding applications.
In conclusion, this study successfully optimized the stiffness of a Stewart-type six-axis force sensor through finite element analysis, focusing on the positioning angles \( \alpha_A \) and \( \alpha_B \). The results show that setting \( \alpha_A = 100^\circ \) and \( \alpha_B = 30^\circ \) enhances overall stiffness by 13.91% to 20.07%, while also reducing maximum stress under load. The use of ABAQUS for simulation proved highly reliable, with close agreement between modeled and experimental data. This approach not only accelerates the design process but also provides deep insights into the structural behavior of the six-axis force sensor, enabling more robust and efficient sensor development. Future work could explore dynamic stiffness optimization or the integration of material variations to further advance the performance of six-axis force sensors in smart sensing technologies.