CSP Component Analysis

This project consisted of three linked assignments done over 10 weeks: proposal, presentation & report. 

Design Briefs

Prior to either the progress report and video or the final report the project topic needed approval. This process involved:

"

1. Aim of the project: what are you trying to do?

2. Specific object under analysis: what are you modelling?

3. Specific application characteristics (quantitative constraints, specific loads, …).

4. Specific assumptions.

5. Key criteria for evaluation of the outcome. What quantities will you use to evaluate the achievement of the aim.

6. An outline of the FEM analysis type you are intending to use: which ANSYS modules? Which type of element? Please note that, to get a good mark in the reports, there is a general expectation for you to use at least two modules.

7. Validation and verification approach.

"

Progress Report and Video

For the progress report:

Same marking criteria and requirements as the Final Report.

For the progress video:

"

Make a ≤5 minute video demonstrating your progress. My suggestion is to prepare a short presentation (e.g. Powerpoint) to help you in the video, but any format is accepted as long as clear. The presentation must include FE results in ANSYS (screenshots or actual screen-recordings). The presentation must be narrated with your own voice. You must upload the video directly to the submission box as an accepted video format (no link to any external platform).

The video should answer the following questions:

• What is the problem I am trying to solve?

• How have I converted the problem in a FEM model?

• What are the key decisions that have gone into the analysis type, geometry, mesh, BCs, symmetry, etc…

• What do my preliminary results mean? How are they helping me answer the original problem?

• What is the model still missing that will be added before the final report is due?

It is a lot for 5 minutes, so make sure you are concise and focus on the key elements.

"

Final Report

Final Report

Executive summary

This study investigates the optimal absorber tube material within a PTC system through thermal stress. The result is that the currently used material, Kovar, performs the best with a maximum stress of 153.95 MPa observed by FEA. This result is within 5% of accepted literature results. A trend between the thermal expansion coefficient and the maximum stress produced on the absorber tube was established.

1        Introduction and Aims

1.1        Introduction

Since the invention of the light bulb in 1880 the need for electricity has only increased. In the year of 1880 an estimated 2,575 TWh of fossil fuels were consumed with an increase of 5,330% since to 2022 to a total yearly global consumption of 137,237 TWh [1] , this also coincides with a 90% increase in global emissions over the last 50 years [2]. The current use of fossil fuels is not sustainable, and the further development of renewable energy sources is required.

Concentrated Solar Power (CSP) is a renewable energy source that uses mirrors to focus sunlight onto a receiver to generate heat. One configuration of CSP is a parabolic trough, commonly referred to as a Parabolic Trough Collector (PTC). PTC’s use long trough shaped reflectors to concentrate sunlight onto a circular receiver tube at the focal point of the parabola as shown in Figure 1.

At the centre of the receiver tube is a heat transfer fluid which is heated by the sun and then used to generate electricity through a steam generator. Encapsulating the heat transfer fluid is a metallic absorber tube, air gap and glass envelope, this setup along with the heat transfer between each layer is shown in Figure 2.

When metals, such as the metallic absorber tube, are heated the atoms within the metal vibrate more vigorously causing thermal expansion to occur, this expansion can lead to a permanent deformation. In the case of a PTC if the absorber tube undergoes too much expansion the surrounding glass envelope can crack, or the heat transfer fluid (HTF) become blocked rendering the system incapable of capturing heat. Different metals have different coefficients of thermal expansions (CTE) which is a material property that describes the correlation between material expansion and temperature.

Thermal stress is a mechanical stress within a material due to a change in temperature. Thermal stress can be induced by non-uniform heating and constrained expansion within a PTC system. When non-uniform heating occurs such as a larger amount of solar radiation applied to one side of the tube thermal stress can occur, this occurrence is documented by Lei et al. in a 2019 study on thermal stress within PTC [3] where thermal stress was analysed using FEA and validated with experimental data. Constrained expansion within a PTC system would cause fracture to the glass envelope, constrained expansion of metals and the subsequent lateral buckling was studied in 1978 by Kerr [4], the study found that not allowing volume for expansion resulted in far more buckling then when metals were allowed room to appropriately undergo thermal expansion.

FEA is able to simulate the effects of radiation, convection and internal stresses within a PTC system. The need for FEA for the analysis of PTC systems is highlighted by Lei et al. [3] as FEA is able to consider the combined and individual effects of temperature gradients, gravity, support and internal constraints for which the experimental case cannot individualise. A 2009 study by Irfan et al. studies the thermal stresses within radiant tubes due to temperature distributions [5]. The visualisation of stresses within materials is often not visible until a stress has passed the materials yield strength. FEA is able to analyse stress a material undergoes at different temperatures to lead to better real-world understanding of how the materials in PTC systems interact with the surrounding environment.

The aim of this study is to identify the common metallic material that can withstand the highest thermal stress within a PTC system. This will be assessed based on the material that under the same conditions experiences the lowest Von-Mises Stress. Secondary properties that can be simultaneously studied are thermal expansion of materials, measured in mm through deformation, which correlate to the operational effectiveness of a PTC system.

2        Assumptions and Problem Specifics

IEC 62862 specifies the general requirements for the design of parabolic-trough solar thermal power plants [6]. Standard 9.2.1 (d) states that loads to be applied to the collector structural models may be obtained via computational modelling [6]. Standard 9.2.4 (c) states that the temperature of the receiver should match the operating temperature of the HTF [6]. The combination of these standards specifies that the problem is applicable to CFD assuming that the metals chosen to be evaluated are able to conduct heat at operational temperatures of HTF.

In a 2016 review into Solar Parabolic Trough Collectors by Jebasingh et al. the operating temperatures of a PTC system were found to be within a 350-400°C range [7]. This means that all materials are assumed to maintain a higher melting point then 400°C.

2.2        Heat Transfer

Within the real-world application of a PTC system heat transfer modes of conduction, convection and radiation exist. In the 2019 study into thermal stress within PTC only convection and radiation were modelled in a cross section of an absorber tube [3]. Therefore, an assumption for this study is that the effects of conduction within the absorber tube subsystem are negligible compared to the effects of both convection and radiation.

Radiation within the system occurs on the outside of the glass envelope due to solar irradiation as well as between the circular surfaces in surface-to-surface transport. Figure 3 shows the experimental result of concentrated solar flux on the glass tube, an assumption can be made for this study that this is constant over the defined region that the heat flux is applied. In reality the solar flux differs due to latitude, longitude and incident angle of solar irradiation, causing variability within the parameter. The management of the real problem, where solar flux changes at every degree, compared to the computational creation, where solar flux can be separated into geometric sections, can be managed by creating small division in sections of high variability resulting in lower possible error of values.

A 2016 study into differing solar irradiation based on global positioning found variance of 2-3 W/m­­2 across the globe [8]. Statistically this results in variation between results included in previous literature due to variations in solar flux of up to 10%.

Convection occurs from free convection with air on the outside of the glass envelope and from HTF on the interior of the absorber tube. The rate of convection can be changed by changing the rate at which the HTF flows through the absorber tube and by changing the temperature of the HTF.

2.3        Variability in Material Values

Studied literature provides experimentally derived material values which can contain errors from the accepted material values. The thermal expansion coefficient for Kovar found by Lei et al. was  whereas the accepted theoretical value is   [9]. The difference is close to a factor of 5 between the results which computationally would result in a vastly different result.

3        Model Setup and Methodology

3.1        Analysis Type

Two analysis systems are used, Thermal Steady State and Static Structural. Thermal Steady State is used to simulate the effect of solar irradiation onto the system. The resulting temperatures are then analysed in Static Structural to find deformation of the absorber tube from the temperature gradient across the tube as shown in Figure 4.

3.2        Geometry

The receiver tube is entirely enveloped by a glass outer layer with an air gap between the surfaces to allow for thermal expansion of the receiver tube and no conduction. The geometry of the tube used in real-world applications is shown in Table 1.

The computational cost of modelling 4000mm of length for a receiver tube does not represent a balance between fidelity and computational cost thus a key parameter in this study is created, length. Maximum temperature was found at different lengths with corresponding coarse meshes. The results from this study as shown in Table 2 show that at the full length of 4000mm a solution was unable to be converged upon mainly due to size of the model.

Comparing the results with results obtained by Lei et al. the length of 200mm provides the most accurate result.

The geometry used in this study is shown below in Figure 5.

3.3        Boundary Conditions

To define the solar flux that is acting on the exterior of the glass tube the average heat flux across the glass tube per angular section, as shown in Figure 1, was used. The heat flux applied is shown below (Table 3) and is derived from Figure 3, which is taken from literature [3].

Other thermal steady state boundary conditions are shown in Figure 7; surface to surface radiation between the absorber tube and glass envelope which occurs at an emissivity of 0.89 and convection on the interior of the absorber tube to model the flow of HTF within the system with the ambient temperature being set to the desired HTF temperature of 250°C.

Within the Static Structural Analysis, a symmetry boundary condition and a fixed boundary condition were used as shown in Figure 8. The symmetry boundary represents the remainder of the tube that is not modelled. The fixed boundary represents the real-world fixture where the tube is expected to not be able to rotate or displace in any direction.

These boundary conditions are modelled as ideal conditions. As discussed previously in Assumptions the heat flux applied to the system is not a perfect replication of experimental conditions with heat flux variation across the sections of the geometry being taken as an averaged value. Also as previously stated the nature of solar irradiance globally results in different heat fluxes based on geographical locations, meaning that to create an ideal boundary condition solar irradiance data would need to be taken from a specific location where the PTC is to be installed to create an ideal model of the boundary conditions.

The boundary conditions used in the Static Structural system create a correct, but simplified, model of the system that is in place within the PTC system. To create a perfect system an additional component such as end links, mirrors and ground supports would need to be added but the additional computational cost of modelling these systems only to use as boundary conditions is not ideal for this model.

3.4        Materials

The aim of this study is to determine which absorber tube material can withstand the highest thermal stress within a PTC system. To do these different materials can be parameterised with their respective properties as shown in Table 3. All materials maintain a higher melting point then the operational temperatures of the PTC system. These materials and the variation between their values are use parametrically within ANSYS Workbench & Mechanical to derive the solution.

In literature the best performing materials under thermal stress tend to have lower coefficients of thermal expansion [15]. Low thermal expansion can be defined as a coefficient of . The lowest thermal expansion material was the given coefficient for Kovar, with the variability of this value discussed previously in Assumptions and Problem Specifics. Next to Kovar is Invar 36 which is known to maintain an extremely low (0.01 ) thermal coefficient at temperatures below 50°C. As the application of the PTC absorber tube will face temperatures greater then 700K then the larger yet still small thermal coefficient of 4.18 was taken [14].

3.5        Meshing

Global meshing size of the system is compared in Table 5. The results from testing these meshing sizes are that 8mm strikes the best balance between fidelity and computational cost as the solution converges at this sizing and thus is a suitable global sizing. A mesh convergence study was also completed to show more variation in mesh sizes as shown in Figure 6.

The meshing method for all cases is set to Hex- Dominant due to the ability for hex elements to be packed more densely, thus reducing the total number of elements within the model as such requiring less resources to solve.

The thick edges of the cylinder provide little information related to heat transfer, stress, or deformation and as such can be meshed coarser. The edge sizing for all cylinder edges can be increased to a meshing size of 16mm. This allows for retainment of accuracy to the real-world model while reducing the computational cost of the simulation.

The creation of this mesh was based on meshing best practices with a balance between a finer resolution with computational cost [16]. The curvature of the body allowed for the hex-dominant mesh to be created.

3.6        Choosing Results

When choosing results, the main result is chosen based on the lowest Von-Mises Stress experienced between materials. Von-Mises stress is a good indicator of yield and failure in ductile materials as it takes into account all of the stress components, while not assuming that the material will fail under pure tension or pure shear. Thermal stress, the key result of this study, is a type of stress that is caused by change in temperature. If the material is constrained, such as the case is here, the thermal expansion caused by the change in temperature can cause stress to develop in the material. The amount of stress that develops depends on the material's coefficient of thermal expansion, the change in temperature, and the constraints. Thermal Stress can be accurately represented by Von-Mises Stress [17].

Secondary results such as maximum temperature of the absorber tube and maximum deflection can be determined by reviewing ANSYS results that coincide with results for maximum stress in the receiver tubes. This extraction of secondary results should aid to verify that the primary results are as expected.

4        Results

Table 6 shows the results of maximum stress. The validation case, Kovar, had the lowest maximum stress at 153.95 MPa followed by Invar at 277.62 MPa. From the remaining materials the next lowest thermal stress is in Aluminium with 1093 MPa.

These results are expected due to the low thermal expansion coefficients of the materials that performed well. Having a low thermal coefficient provides a correlation to lower induced thermal stress.

From these results a trendline can be established (Graph 1). This trendline displays a positive linear correlation between the variable of thermal expansion coefficient of a material compared to the maximum stress found in FEA.

4.1        Secondary Results

Secondary results of maximum temperature and maximum deformation within the absorber tube are shown in Table 7 and Table 8 respectively.

Invar achieved the highest absorber temperature (722.08 K) , ideal result, closely followed by Kovar (710.1 K). For the materials with higher thermal expansion coefficients the most heat absorbed is by Stainless Steel (702.41 K).

Kovar had the lowest amount of deformation (0.12853 mm), followed by Invar (0.3692mm). From the remaining materials Stainless Steel was again the best performing material deforming 0.95216mm.

4.2        Meshing Quality

The quality of meshing produced is evaluated using ANSYS mechanical, the results of this (Figure 9) show that low Thermal Error occurs. Thermal Error was chosen over Structural Error as Thermal Steady State was used prior to Static Structural being used. Hence the quality of meshing was important to gain an accurate result to be imported into Static Structural.

The computational cost of this mesh compared to a finer mesh is ideal as stated previously in the mesh sizing study where the sizing of the mesh and hence the amount of nodes is directly correlated to the computational cost of processing the mesh. The findings from the error in the mesh represent the expected outcome.

5        Validation and Discussion

5.1        Validation against literature

Comparing results of thermal stress with Lei et al. results shown in X shows that the Kovar validation case produces a maximum stress (153.95 MPa) within 4% of the accepted result (160 MPa) as circled in red in Figure 10.

Further results using Kovar were taken at differing HTF temperatures (Table 9)

These results can be compared to those in Figure 10 and are both plotted below.

Further validation on maximum temperature within the Kovar validation case shows the maximum temperature within the system (710.1 K) was within 1% of the accepted result (703 K) as shown in Figure 11.

5.2        Mathematical Validation

The formula for calculating thermal stress on a surface is:

Where σ represents thermal stress, E represents Youngs Modulus, α represents the coefficient of thermal expansion and ΔT is the change in temperature.

The hand working for Kovar is shown, it was replicated using Excel along with the error range for other materials.

E = 206 x 109 Pa

α = 1.7 x 10-6 K-1

Max Temperature from secondary results = 710.1 K

Ambient Temperature = 295.15 K

The computational result for Kovar was 153.95 MPa.

The error of 5.95% is a reasonable error in the thermal stress.

For the remaining materials a trend can be seen between a secondary effect of significance, thermal expansion coefficients, and error percentage. A larger coefficient of thermal expansion correlates to a larger discrepancy between the computational and mathematical stress.

6        Conclusions

This study aimed to determine which material used in a PTC absorber tube was able to withstand the highest amount of thermal stress. The result from this is that Kovar, with the experimentally defined material values, was able to withstand the most stress. This was followed by Invar which also contains a low thermal expansion coefficient. A trend was established within the materials for both error from mathematical calculation and thermal stress whereby a lower thermal expansion coefficient results in simultaneously less error and less thermal stress.

Secondary results were used in conjunction with the thermal stress to provide further credibility to the result. All results were compared against literature and found to be within 5% of the experimentally and computationally derived results.

7        Acknowledgements and Response to Peer Review

In the Progress Report the following goals were stated to be achieved within this report:

-        Local mesh refinement for a more accurate simulation

-        Further materials added for a wider comparison.

-        Different HTF temperatures evaluated.

-        Further Literature to be reviewed to provide a wider range of acceptable data.

-        Mathematical Calculations to be carried out.

The full range of comments given during peer feedback can be found in Appendix A. Key comments that were given were: Lack of Mathematical Validation, Needs Further Discussion on Computational Costs and Further References to Literature were needed.

Combining the defined goals and feedback into this report all of these tasks were undertaken and completed as shown earlier within the report. In more detail the material of Invar was added, mesh refinement on edges of cylinder was added, a comparative study to literature on HTF temperatures was done, further literature was added, and mathematical calculations were carried out. This led to overall improvement in the quality of the report.

I would also like to acknowledge the aid of Ray Clark in his work in troubleshooting and problems I may have and additional his expert insight into this project.

I would like to extend thanks to Matthew Overton-Clarke and Ishan Ray Chaudary for their aid in reviewing and reading this report.

Results

Progress Report and Video: 97/100

Final Report: 94/100

References

[1] H. R. a. P. Rosado, “Fossil Fuels,” OurWorldInData.org, 2017. [Online]. Available: https://ourworldindata.org/fossil-fuels#article-citation.

[2] EPA, “Global Greenhouse Gas Emissions Data,” 2019. [Online]. Available: https://www.epa.gov/ghgemissions/global-greenhouse-gas-emissions-data#:~:text=Since%201970%2C%20CO2%20emissions.

[3] X. F. Y. R. F. Y. Z. W. Dongqiang Lei, “Temperature and thermal stress analysis of parabolic trough receivers,” Renewable Energy, vol. 136, pp. 403-413, 2019.

[4] A. D. Kerr, “Lateral Buckling of Railroad Tracks due to constrained thermal expansions,” Railroad tracks mechanics and technology, pp. 141-169, 1978.

[5] W. C. Mohammad A. Irfan, “Thermal stresses in radiant tubes due to axial, circumferential and radial,” Applied Thermal Engineering, vol. 29, pp. 1913-1920, 2009.

[6] International Electrotechnical Commission, “Solar thermal electric plants – Part 3-1: Systems and components - General requirements for the design of parabolic-trough solar thermal power plants,” IEC, no. 1, 2022.

[7] G. J. H. V.K. Jebasingh, “A review of solar parabolic trough collector,” Renewable and Sustainable Energy Reviews, vol. 54, pp. 1085-1091, 2016.

[8] R. W. Mueller, “Solar Irradiance,” Solar Energy, no. https://link.springer.com/referenceworkentry/10.1007/978-1-4614-5806-7_447, pp. 553-583, 2016.

[9] MatWeb, “Kovar Alloy,” [Online]. Available: https://www.matweb.com/search/datasheet.aspx?matguid=c2fa45c3446f485692fc97b4b0962ac9&ckck=1.

[10] MatWeb, “Aluminium 6061-O,” [Online]. Available: https://www.matweb.com/search/DataSheet.aspx?MatGUID=626ec8cdca604f1994be4fc2bc6f7f63.

[11] MatWeb, “Eagle Brass 110 EPT COPPER, Annealed,” [Online]. Available: https://www.matweb.com/search/datasheet.aspx?MatGUID=d51a19947e624563bde3c3e7be245602.

[12] MatWeb, “Stainless Steel 409,” [Online]. Available: https://www.matweb.com/search/DataSheet.aspx?MatGUID=7f38db56864e46659a38760e6de4a5db.

[13] MatWeb, “Brass 464,” [Online]. Available: https://matweb.com/search/DataSheet.aspx?MatGUID=5d0f88a052c54ee28c7e66de6d7f0d92.

[14] MatWeb, “Carpenter Invar 36® Alloy, Cold Drawn Bars,” [Online]. Available: https://www.matweb.com/search/datasheet.aspx?matguid=b6fb00b235f0442da4d31a0cd04671c9&ckck=1. [Accessed 15 11 2023].

[15] D. A. a. H. A. M. Roy Rustum, “Very Low Thermal Coefficient Expansion Materials,” Annual Review Material Science, vol. 19, pp. 59-81, 1989.

[16] P. Borghesani, The Finite Element Library.

[17] K. v. d. W. R. W. M. J. K. a. J. B. D. N. Mbidi, “Mechanical design considerations of a double stage axial-flux PM machine,” Conference Record of the 2000 IEEE Industry Applications Conference. Thirty-Fifth IAS Annual Meeting and World Conference on Industrial Applications of Electrical Energy (Cat. No.00CH37129).

Appendix

Appendix A - Peer Review Feedback