In the aerospace industry, CubeSats have emerged as a low-cost, easily manufacturable solution for space-based optical systems. They offer a unique opportunity to develop a production line approach for a space-based product through the manufacture of a constellation of smaller, more affordable systems.
Companies that manufacture CubeSat optical systems need an accurate and reliable method for developing an optical design, opto-mechanically packaging the system, as well as modeling structural and thermal impacts that the system will experience in-orbit. This article series will walk through the high-level development of a CubeSat system by leveraging the Zemax and Ansys software suites. We will illustrate how an integrated software toolset can streamline the design and analysis workflow.
By: Matthias Schlich & Jordan Teich
Article Attachments
Introduction
For decades, optical systems have been developed for operation in low, medium, and high Earth orbit. For many optical systems, the packaging form factor and the opto-mechanics that stemmed from this form factor were designed on a system-by-system basis. CubeSats are a class of lightweight nanosatellite that can house optical systems for applications ranging from laser communications to earth imaging. They are unique in that they use a standardized size and form factor.
For this article series, the paper Optical Design of a Reflecting Telescope for CubeSat1 was used as a reference for developing the CubeSat optical design.
In Part 3 of this series, we will cover the export of the Opto-Mechanical model from OpticsBuilder to Ansys SpaceClaim. We will then demonstrate how the model was prepared for Finite Element Analysis in Ansys Mechanical and analyze the generated FEA results.
Preparing the design for FEA in Ansys Mechanical
With the opto-mechanical design finalized in OpticsBuilder, the full CubeSat model can now be imported into Ansys software to prepare for Finite Element Analysis. First, the geometry was exported from Creo in a STEP file format to Ansys SpaceClaim, a 3D modeling software. Within SpaceClaim, the model geometry was simplified to reduce complexity.
After reducing the complexity of the model geometry, the design was then brought into Ansys Mechanical to prepare for Finite Element Analysis.
For the structural analysis, only the core of the assembly is used. The CubeSat side panels and small components such as spring-loaded bolts were removed to achieve a simpler model for analysis. The results is showcased in the picture below:
Figure 1: Simplified Design in Ansys Mechanical
In Ansys Mechanical, the following material definitions were chosen for the design:
- Both mirrors are built out of a low CTE aluminum substrate (Al-MS40Si)2
- The main frame is built from carbon fiber reinforced polymers
- The metering rods are built out of invar
- The image sensor is assumed to be made from PCB laminate
Please note that the materials were chosen to illustrate this example and their selection was not based on any realistic considerations.
The image below showcases how materials are assigned in the design:
Figure 2: Ansys Material Definitions
Assigning Contacts and Developing the Mesh
With the materials assigned, contacts were then defined within the model. The mount of each mirror is designed to hold the mirrors in place through a combination of spring-loaded bolts and fixed stops. The spring-loaded bolts acting on one side of the mirror force it to contact the fixed stop at the opposite side. This is present 3 times per mirror constricting the movement in all 3 dimensions. This behavior is represented by 3 “No Separation” contacts in Ansys Mechanical without modeling the spring-loaded bolts individually.
Figure 3: No Separation Contacts
The mirror retainers are connected to four invar metering rods. The invar metering rods are held in the CubeSat frame at the ends of the system and can slide into the other connections:
Figure 4: Invar Rods
The frame itself is connected via bonded contacts:
Figure 5: Bonded Contacts
With the contacts defined, the mesh created by Ansys can now be slightly tweaked to suit our simulation needs. The mesh was adjusted in a few areas where the default mesh resulted in bad quality. The element size for both mirror surfaces was adjusted such that each surface reached at least 10,000 nodes. This number was needed to obtain good fit quality in OpticStudio’s STAR module. The pictures below showcase the final mesh used for the opto-mechanics and mirrors.
Figure 6: Mesh in Ansys Mechanical
Figure 7: Secondary Mirror Mesh
Loads and Boundary Conditions
For this design, the only load present is a thermal condition that causes the components to expand according to their thermal coefficient of expansion (TC). Discrete temperature conditions were chosen to resemble the operating temperature range that the CubeSat would experience during Low Earth Orbit operation. The assumption was made that the CubeSat’s radiation control system would insulate the optics from large fluctuations in temperature. This limits the operating temperature range of the optics to 15C +/- 3C.
The nominal design as built in OpticStudio is assumed to have been built in an ambient, room temperature environment of 21C. This is the reference temperature at which the geometry is defined.
The temperatures were implemented in Ansys Mechanical as follows:
Figure 8: Temperature Definitions
In a structural analysis, the assembly needs to be held in place. For the optical analysis, using weak springs would not be accurate enough. Therefore, the entire assembly is held in place through a combination of remote displacements. The translational movement is constrained at the sensor plane since this component represents the image plane where deformation effects cannot be assigned in OpticStudio. The rotations are constrained at the front frame so that bending of the sensor is not interpreted as rotations of the entire assembly.
Figure 9: Remote Displacements
Since the CubeSat is assembled on Earth, there are differences in the loads compared to an in-orbit state. During assembly, the CubeSat is subject to Earth’s gravity and about one atmosphere of pressure. In the vacuum of space, there is no pressure and no acceleration load acting on the assembly. To check whether these load differences affected deformation in a significant way, two additional finite element analyses were conducted.
The analysis for the pressure difference revealed that the deformation of the mirrors was below 180 nanometers.
The analysis for the influence of gravity resulted in large deformation of the mirror retainers if the assembly was only supported at one side of the frame. This deformation caused the mirrors to move more than 8 micrometers compared to their original position. Therefore, an additional support was considered in the analysis. This additional support was directly connected to the bottom of the mirror retainers and helps them take on the weight of the mirrors. With this setup, the deformation of the mirrors was below 20 nanometers.
Since we expected the deformations due to thermal expansion to be in the range of 10 micrometers, pressure and gravity effects are neglected in the main FEA analysis as the induced deformations were multiple orders of magnitude smaller.
FEA Results in Ansys Mechanical
With preparation completed, FEA analysis can now be run within Ansys Mechanical. In the following pictures, the results for the lowest operational temperature, 12C, are shown. The dominating deformation effect is caused by the mirrors shrinking due to the high CTE of the aluminum substrate.
Figure 10: Ansys Mechanical Deformation Data
If the mirrors are hidden in the model, the effects of the frame deformation can be made visible:
Figure 11: Deformation of Frame
The Z-component of deformation can also be viewed and the results for this design are as follows:
Figure 12: Z-Component Deformation
With the FEA analysis completed, the structural deformation data for both mirror surfaces can now be exported for all operating temperatures. With the Ansys ACT extension, this data can be exported to a series of text files. These text files are all that is needed to import the FEA data into OpticStudio’s STAR module for further analysis. You can read about how to use the ACT extension in the following Knowledgebase article: OpticStudio STAR Module: Ansys Data Export Extension – Knowledgebase (zemax.com).
Conclusion
In this article, we covered how the completed CubeSat design was brought into Ansys SpaceClaim to prepare the design for Finite Element Analysis. We then walked through the loads and boundary conditions that were considered for this analysis. Finally, we showcased the FEA results within Ansys Mechanical and how this data can be brought directly into the OpticStudio STAR module.
References
- Jin H, Lim J, Kim Y, Kim S. Optical Design of a Reflecting Telescope for CubeSat. J Opt Soc Korea. 2013;17(6):533-537. doi:10.3807/josk.2013.17.6.533
- Aluminum Alloys. AMT Advanced Materials Technology; 2022:1-2. https://www.amt-advanced-materials-technology.com/materials/aluminum-for-optics-electronics/. Accessed June 14, 2022.
Next article: From Concept to CubeSat Part 4: Using Ansys Zemax Software to Develop a CubeSat System