¶ Goal(s) of the study
This document aims to present the method used to analyse with finite elements software the glued female coupler of the Firehorn rocket. Indeed, it is subjected to important loads during the flight, especially at the opening of the parachute.
¶ 214201_Glued
¶ Geometry
The couplers are made of only one part, manufactured in 2050-T84 aluminum alloy. Below is an image of the glued female coupler.
¶ Function
The glued female coupler’s function is to link the recovery bay to the payload bay and resist the different forces applied to the structure especially at the deployment of the parachute. The glued female coupler is found at the top of the recovery bay.
¶ Material
The coupler is machined in 2050-T84 aluminum alloy. This alloy has the following properties:
¶ Load case
Being part of the main structure of the rocket, the most important load the couplers will have to support is the tension due to the deployment of the parachute which corresponds to a 30g acceleration. This gives us the following force:
The 13.2 kg being the total mass that the coupler must absorb which includes its own weight, the male coupler, the shockplate, the payload, and the nose cone.
However this is the load case for FH 30, the coupler will only need to withstand the 4800 N of axial loads for FH 9.
As a coupler the part shall also withstand an bending moment of 7500 Nm and a compressive force of 15000 N.
- 2024_C_SE_ST_COUPLER_REQ_07 Mechanical axial loads
The CPLRs shall resist axial parachute deployment loads of [30]g with an additional FoS of [2]. - 2024_C_SE_ST_RECOVERY-BAY_REQ_13 Upper shockplate load case
The shockplate in the recovery bay of the FH I LV shall withstand [4800]N of axial tensile loads. - 2024_C_SE_ST_COUPLER_REQ_21 Coupler load case - bending
The Coupler shall withstand [7500]Nm of bending moment. - 2024_C_SE_ST_COUPLER_REQ_20 Coupler load case - compression
The Coupler shall withstand [15000]N of compression loads.
¶ Finite Element Analysis
¶ Software
This FEA analysis was performed with the ANSYS Mechanical software for a static structural analysis. The CAD of the part was designed using Solidworks.
¶ Type of simulation
The simulation performed was a static structural analysis to estimate the Von mises constraints for the load cases of 7.77 kN, 15000 N in compression and 7500 Nm in bending.
¶ Inputs
The set of units used for this simulation is: mm, t, N, s, mA, mV.
The geometry has been modified using ANSYS spaceclaim. We have specified the surfaces in contact with the shockplate, where the load will be applied :
The couplers are manufactured in 2050-T84 aluminum alloy. We used only the isotropic material properties, where we know the Young's modulus, the poisson ratio, the density, the Yield strength and the tensile strength. The following image shows the material properties implemented in the software.
Time was not taken into account for this simulation.
The following boundary contitions were applied:
¶ Force load case
- Clamped surfaces: The glued surface of the coupler has been blocked in all directions and rotations.
- An downwards (positive y) force of 7770 N has been applied on the surfaces in contact with the shockplate, corresponding to 1980 N per face.
¶ Compression load case
-
Clamped surfaces: The glued surface of the coupler has been blocked in all directions and rotations.
-
An upwards force of 15000 [N] has been applied on the conical surface of the coupler.
¶ Moment load case
The following boundary contitions were applied:
-
Clamped surfaces: The conical surface of the coupler has been blocked in all directions and rotations.
-
A moment of 7500000 Nmm around the x-axis has been applied on the glued surface of the coupler.
Analysis settings were left program controlled for both cases which gives the following settings:
¶ Mesh
We choose to use the 3D solid elements to realize our analysis. The mesh is constituted of tetrahedral mesh of quadratic element order (Tet10).
To verify mesh convergence, we probed the stress under the force load case, at the same node under a part that supports the shockplate as it is the area most prone to high stress:
The 'size' quantity refers to the sizing setting applied on the geometry.
| Size (mm) | 5 | 2 |
|---|---|---|
| Stress (MPa) | 285.43 | 283.65 |
| Deltas (%) | / | -0.62 |
We use the mesh with an element sizing of 5 mm as it is sufficiently refined (less than 2% difference with the finest mesh).
The final mesh is the one generated with an element sizing of 5 mm on the whole geometry. It contains 226059 elements and 354210 nodes. The average element quality is around 75%.
The following pictures illustrate the mesh as well as the element quality of the mesh.
¶ Outputs
¶ Force load case
The maximal stress is found on the curve under an overhang supporting the shockplate. It has a value of 285.43 MPa. The couplers being manufactured in 2050-T84 aluminum alloy, its yield strength is of 476 MPa, which is not exceeded.
¶ Compression load case
The maximal stress is found on one of the extrusions through which the screws go. It has a value of 19.725 MPa. The couplers being manufactured in 2050-T84 aluminum alloy, its yield strength is of 476 MPa, which is not exceeded.
¶ Moment load case
The maximal stress is found inside the grove under the glued surface. The following image shows a close up of this area :
We can see that the maximal value of 161.26 MPa is atteigned only on one node, with most of the nearby nodes having a value of about 116.5 MPa. However the difference is not very high so we will still consider the maximal stress to be 161.26 MPa. The couplers being manufactured in 2050-T84 aluminum alloy, its yield strength is of 476 MPa, which is not exceeded.
¶ Margin of Safety
The formula of the minimum Margin of Safety being the following:
We have:
¶ Force load case
¶ Compression load case
¶ Moment load case
which is greater than the required 0.25 in all cases.
¶ Conculsions
The main focus of the simulation was to determine if the yield strength of the material is exceded under the loads which the coupler is supposed to withstand, i.e 7770 N applied by the shockplate, 15000 N in compression or 7500 Nm of bending moment.
¶ Force load case
The simulation results indicate that under such a load, the maximal von mises equivalent stess within the part has a value of 285.43 MPa which corresponds to a margin of safety of 0.67 which is over the 0.25 required. Therefore, this load being higher than the 4800 N required we can conclude that the following requirement is verified.
- 2024_C_SE_ST_RECOVERY-BAY_REQ_13 Upper shockplate load case
The shockplate in the recovery bay of the FH I LV shall withstand [4800]N of axial tensile loads.
¶ Compression load case
The simulation results indicate that under such a load, the maximal von mises equivalent stess within the part has a value of 19.725 MPa which corresponds to a margin of safety of 23.13 which is well over the 0.25 required. Therefore, we can conclude that the following requirement is verified.
- 2024_C_SE_ST_COUPLER_REQ_20 Coupler load case - compression
The Coupler shall withstand [15000]N of compression loads.
¶ Moment load case
The results indicate that under the load case of 7500 Nm, the maximal von mises equivalent stess within the part has a value of 161.21 MPa which corresponds to a margin of safety of 1.95 which is well over the 0.25 required. Therefore, we can conclude that the following requirement is verified.
- 2024_C_SE_ST_COUPLER_REQ_21 Coupler load case - bending
The Coupler shall withstand [7500]Nm of bending moment.
Overall, all requirements are verified so we can validate the design for FH 9.