Written by: Ricky Gill (Last Updated: 2024-11-12) 

Primary Structure Finite Element Analysis

In this section we present the analysis methodology and results for the structural finite element analysis performed on the engineering model primary structure of LISSA. The primary structure of LISSA is defined as the structure consisting of the corner and centre rails combined with the module shells and 2U payload stand-in. All module specific components were removed from this analysis and are factored into the simulations in Phase D once all component positions are finalized. In addition to module specific components, the 6U and 3U solar arrays are also removed and are analyzed separately. 

In this analysis, the 2U controlled payload is modelled by simply using a open structure with the same dimensions as the payload using a nominal wall thickness of 2 mm. A more detailed analysis with the actual engineering model payload CAD will be conducted separately in Phase D and reported in a document which can be accessed by specialized personnel upon request. The following sections outline details about the model and how it is defined. Additionally, we define each of the different loading scenarios and analysis along with thier respective results. 

Model Definition

Model Materials

Three main materials were used in the structural simulations used for the Primary Structure of LISSA. Information for each material is summarized below.

• Aluminum Alloy, Wrought, 6061, T6: The standard library material for 6061-T6 aluminum is used.  Additionally, a custom S-N curve was added into the standard material model.

  • Density: 2713 kg/m3

  • Coefficient of Thermal Expansion: 2.278E-5 C^-1

  • Young's Modulus: 69.0 GPa

  • Poisson's Ratio: 0.33

  • Bulk Modulus: 67.9 GPa

  • Shear Modulus: 25.9 GPa

  • Tensile Yield Strength: 259 MPa

  • Tensile Ultimate Strength: 313 MPa

  • S-N Curve (data obtained from "Fatigue Design Curves for 6061-T6 Aluminum, G. T. Yahr, Engineering Technology Division, Oak Ridge National Laboratory, Oak Ridge, Tennessee" ):

• PCB laminate, Epoxy/Glass fiber, FR-4.0 (Df > 0.02 at 10 GHz): A standard library material was selected for the FR-4 epoxy laminate material. Additionally, a custom S-N curve was added into the standard material model.

  • Density: 1944 kg/m3

  • Coefficient of Thermal Expansion: 1.470E-5 C^-1

  • Young's Modulus: 24.3 GPa

  • Poisson's Ratio: 0.16

  • Bulk Modulus: 12.12 GPa

  • Shear Modulus: 10.46 GPa

  • Tensile Yield Strength: 298 MPa

  • Tensile Ultimate Strength: 298 MPa

  • S-N Curve (data obtained from "Cumulative Damage Model for Glass-Fiber Reinforced Composites under Two Blocks Loading, Athmane et al."):

• Structural Steel: A standard library material was selected for the structural steel material.

  • Density: 7850 kg/m3

  • Coefficient of Thermal Expansion: 1.20E-5 C^-1

  • Young's Modulus: 200 GPa

  • Poisson's Ratio: 0.3

  • Bulk Modulus: 166 GPa

  • Shear Modulus: 76.9 GPa

  • Tensile Yield Strength: 250 MPa

  • Tensile Ultimate Strength: 460 MPa

  • S-N Curve:

Model Geometry, Material, and Contacts

The information below summarizes each of the active components in the simulation, their defined material, and the type of elements used in the simulation. 

• Corner and Centre Rails :

  • Corner Rail 1 [UMS-0598]:

    • Material: 6061-T6 Aluminum

    • Element Type: Shell (Solid elements used on tabs).  

  • Corner Rail 2 [UMS-0599]:

    • Material: 6061-T6 Aluminum 

    • Element Type: Shell (Solid elements used on tabs).

  • Corner Rail 3 [UMS-0662]:

    • Material: 6061-T6 Aluminum

    • Element Type: Shell (Solid elements used on tabs).

  • Corner Rail 4 [UMS-0663]:

    • Material: 6061-T6 Aluminum 

    • Element Type: Shell (Solid elements used on tabs).

  • Contacts and Additional Information: All contacts were modelled using bonded connections, multi-point constraint formulation, and defined using a pinball region radius of 5 mm or program controlled contact definitions. Contacts were set between the inner walls of each of the corner rails and the respective structure which comes into contact with it. Most of the corner and centre rail geometry was simplified using shell elements since the length to thickness ratio was within the acceptable range . The tabs were left as solid elements since their dimensions did not satisfy the criteria needed for shell element simplifications. 

• Module Shells:

  • ADCS Shell 1 [UMS-0668]:

    • Material: 6061-T6 Aluminum

    • Element Type: Solid

  • ADCS Shell 2 [UMS-0669]:

    • Material: 6061-T6 Aluminum

    • Element Type: Solid

  • Reaction Wheel Shell 1 [UMS-0670]:

    • Material: 6061-T6 Aluminum

    • Element Type: Solid

  • Reaction Wheel Shell 2 [UMS-0671]:

    • Material: 6061-T6 Aluminum

    • Element Type: Solid

  • Thruster Shell 1 [UMS-0672]:

    • Material: 6061-T6 Aluminum

    • Element Type: Solid

  • Thruster Shell 2 [UMS-0673]:

    • Material: 6061-T6 Aluminum

    • Element Type: Solid

  • POW-COM Shell 1 [UMS-0674]:

    • Material: 6061-T6 Aluminum

    • Element Type: Solid

  • POW-COM Shell 2 [UMS-0675]:

    • Material: 6061-T6 Aluminum

    • Element Type: Solid

  • Contacts and Additional Information: All contacts were modelled using bonded connections, multi-point constraint formulation, and defined using a pinball region radius of 5 mm or program controlled contact definitions. For two shells within the same module (i.e. ADCS Shell 1 and ADCS Shell 2) bonded contacts were set between each of the connecting faces which couple the module shells using mechanical interference. Between two modules (i.e. the bottom face of Reaction Wheel Shell 2 and the top face of Thruster Module 1) contacts were simplified by defining a bonded connection. Both of the aforementioned contacts were simplified from real life conditions (bonded contacts used instead of frictional). This simplification was deemed acceptable since the rails connect the shells together in a manner which akin to a bonded connection. Contacts were also defined between each of the corner and centre rails as mentioned previously.

• Payload:

  • Payload [UMS-0788]:

    • Material: Assumed 6061-T6 Aluminum

    • Element Type: Shell

  • Contacts and Additional Information: All contacts were modelled using bonded connections, multi-point constraint formulation, and defined using a pinball region radius of 5 mm or program controlled contact definitions. Contacts were set with the corner and centre rails. An additional contact was defined between the bottom face of the payload and the top surface of ADCS Shell 1. 

General Boundary Conditions

Two different types of boundary conditions are applied. A fixed constraint is placed on the four corner rails which come into contact with the deployer. The aforementioned constraint is applied on either the top or bottom surface of the satellite that comes into contact with the deployer. Which face the constraint is applied on is selected based on the direction of the applied loading. An additional constrain is applied to the surface region on the corner rails where it comes into contact with the dispenser. The aforementioned boundary condition was modeled using an elastic support with an applied linear stiffness value of 215 GPa. 

Loading Scenarios and Boundary Conditions

Quasi-Static Structural Analysis: G-Force 

This set of quasi-static structural simulations were defined according to the Falcon 9 Flight Limit Load Factors as shown in the figures below. Based on the Falcon 9 documentation, five main conditions were considered for static structural simulations and are summarized in the following table. 

Quasi-Static Structural Analysis: Combined Axial Load on CubeSat Feet 

Section 3.3 in the ISISPACE QuadPack/DuoPack Payload User Guide defines the expected combined axial load transmitted from the dispenser door to the CubeSat feet. According to Figure 3.9 in the aforementioned document, the combined force is expected to be 45 N.  

Quasi-Static Structural Analysis: Dynamic Rail Force

According to Section 3.1 in the ISISPACE QuadPack/DuoPack Payload User Guide, there is one dynamic guide rail and three passive guide rails. The dynamic guide rails interfaces with LISSA by applying a force to one corner rail effectively pushing the CubeSat into the other passive guide rails. The dynamic guide rail is used to reduce the amount of rattling and vibration within the deployer. The amount of force imparted by the dynamic guide rail on LISSA was taken from Figure 3.3 in the ISISPACE User Guide.  According to Figure 3.3 the amount of force transmitted is approximately 38 N.

Modal Analysis

A modal analysis is a numerical linear dynamics analysis used to determine the natural frequencies of a structure. A modal analysis uses no loads (i.e. free vibration) to quantify the natural frequencies based solely on the mass and structural stiffness of the system. In short, a modal analysis in this context provides information which can be used to determine if the structure will have a natural frequency close to any externally applied dynamic loading frequencies. Avoiding resonance means ensuring the natural frequency of the nanosatellite is larger than the expected applied frequncies during launch. A modal analysis is also the basis of other more complex analysis such as response spectrum analysis, and random vibration analysis which use the results obtained from the mode combinations.  In this analysis, ANSYS Mechanical was used to evaluate the natural frequencies of the primary structure of the nanosatellite. 

Two different sets of modal analysis were completed based on the applied boundary conditions. Fixed supported are applied to both ends of the corner rails. Elastic supports are applied to corners rail where the nanosatellite rails interface with the deployer. 

Response Spectrum Analysis 

A response spectrum analysis is a numerical technique used to evaluate the effect of shock-driven loading conditions on structures such as satellites. A response spectrum analysis is used as an approximation to a full time-series analysis for loading conditions which are short and non-deterministic. In a response spectrum analysis, the maximum response of the structure is evaluated by defining a response input spectrum.  A response input spectrum defines base excitation using acceleration as function of applied frequency. Modal analysis results are used in combination to estimate the peak response of the structure under the applied shock loading conditions. In this analysis, ANSYS Mechanical was used to evaluate the structural response of the nanosatellite by defining a Shock Response Spectrum (SRS) as function of frequency in order to estimate the resultant displacement, stress, and strain in the nanosatellite. 

The Falcon 9 User's Guide outlines the Payload adapter-induced  shock at the spacecraft separation plane table which defines how the Shock Response Spectrum (SRS) changes as a function of frequency. The data taken from the Falcon 9 User's Guide is outlined in table below. For this analysis, the same boundary conditions are applied as outlined in the Modal Analysis Section.

Random Vibration Analysis

During launch, the LISSA nanosatellite will experience random vibrations of varying frequency and amplitude. A random vibration analysis quantifies the response of structures under loading conditions which are random. The random loading conditions are quantified using a Power Spectral Density (PSD) curve which essentially a statistical representation of the applied loading conditions. In this analysis, a PSD-G curve was used to correlate applied acceleration loading conditions to vibrational frequencies. Since the applied loading conditions are statistical, the results also are non-deterministic and thus the resultant displacement, stress, and strain are probabilistic. In this analysis, ANSYS Mechanical was used to evaluate the response of the nanosatellite primary structure using modal analysis results.

The Falcon 9 User's Guide outlines the Falcon 9/Heavy Random Vibration Maximum Predicted Environment (P95/50) at top of PAF [5.13 GRMS] as shown in figure below. The aforementioned data is used as an input to ANSYS Mechanical to simulate the predicted response of the LISSA nanosatellite under random vibration loading conditions.  For this analysis, the same boundary conditions are applied as outlined in the Modal Analysis Section above.

Static Structural Analysis

Results are shown in the table below for a mesh sensitivity analysis that was conducted using Case 1. Overall, results are converged using a total of 2044504 elements. The same number of elements were used for all other simulations to obtain results. A similar procedure was used in general for all other simulations including the 3U and 6U solar arrays.

Quasi-Static Structural Analysis: G-Force 

The following results shown below are for the quasi-static structural simulations under gravitational loading for the five cases summarized above. 

Quasi-Static Structural Analysis: Combined Axial Load on CubeSat Feet

Quasi-Static Structural Analysis: Dynamic Rail Force

Modal Analysis

Response Spectrum Analysis

Random Vibration Analysis

3U Solar Panel Board 1

3U Solar Panel Board 2

Modal Analysis

Response Spectrum Analysis

Random Vibration Analysis

6U Solar Wing Analysis

Radiation Analysis

An analysis was conducted in SPENVIS to estimate the expected radiation dosage. The following parameters were used to perform the simulation:

• Assumed mission duration: 5, 10 years

• Circular Orbit

• Altitude [km]: 575

• Inclination [deg]: 97.6

• RAAN [deg]: 90

• Argument of perigee [deg]: 0

• True anomaly [deg]: 0

• Trapped particle species: Protons (AP-8, Solar Maximum, Energy [MeV] = 50.0, Threshold flux for exposure (/cm2/s): 50.0)

•  Trapped particle species: Electrons (AE-8, Solar Maximum, Energy [MeV] = 1.0, (AP-8, Solar Maximum, Energy [MeV] = 50.0, Threshold flux for exposure (/cm2/s): 1.0))

• Radiation sources and effects model: SHIELDOSE-2

Results are shown in the figure below. The nominal wall thickness of the satellite is 2 mm. Therefore, the expected radiation dosage is approximately 10 krad for 5 years and 20 kRad for 10 years. The results from this analysis should be used as the expected radiation dosage for all subsystems.

Total Mass and Center of Mass 

The total mass of the satellite with all structural components included as outlined per the assembly drawing ICDs is estimated to be 7681.62 grams.  Refer to the mass budget (LINK). 

A center of mass analysis was conducted through SOLIDWORKS to estimate the position of the center of mass of LISSA with respect to the overall geometric center. With respect to the coordinate system shown below the geometric is located at (X,Y,Z) = (15.7180 mm, -32.1265 mm, -10.7059 mm). The position of the center of mass in the closed configuration is located at  (X,Y,Z) = (21.98328 mm, -35.95817 mm, -10.92617 mm). The position of the center of mass in the open configuration is located at (X,Y,Z) = (34.03540 mm, -35.95817 mm, -10.92617 mm).

• For the closed configuration (wings stowed), the distance from the geometric center to the center of mass is 7.3 mm.

• For the open configuration (wings deployed), the distance from the geometric center to the center of mass is 18.7 mm.

According to the CAD model, the centre of gravity of the satellite is located within a sphere with a radius of 20 mm from the satellite’s geometric centre. Additionally, the center of mass is encompassed by the CubeSat feet contact points as seen the figure below.

Flight Model Static Structual Analysis

6U Solar Wing Analysis

Mesh Convergence Analysis

Static Stress Analysis

Modal Analysis

Shock Loading Analysis

Extended Fairing Case

Average Case

Random Vibration