Week 6 - CHT Analysis on a Graphics card

Week 6 - CHT Analysis on a Graphics card.

Aim:

To simulate a Forced convection flow on a graphics card and study for the Conjugate heat transfer in the simulation, to perform mesh independent study and compare the results. We shall simulate for 3 velocities 1 m/s, 3m/s and 5 m/s with default mesh and for 5 m/s we shall study with a finer mesh.

Introduction:

CHT Analysis means Conjugate Heat Transfer, modes of heat transfer are generally conduction, convection and radiation. Conduction is observed within same kind of molecules (within a solid), convection occurs between different kind of molecules where bulk motion is involved (between solid and fluid). Any situation where both conduction and convection can co-exist within a system, then it is called as Conjugate heat transfer. Though conduction and convection co-exist either one can be dominating over the other, that is given by a non dimensional number called Nusselt number.

Graphics card has a processor which runs at its clocked speed, this produces heat. This heat has to be released or dispersed in order to keep the electronics up and running. Over heating can lead to permanent damage, now a days PC’s come with a preventive mechanism that allows automatic switch off of PC when it exceeds thermal limit, called as thermal trip.

Here cooling is facilitated by provision of cooling fans that allows forced convection, when ambient air is flowing over the graphics card, the mode of heat transfer between the ambient air and the fins is convection, and between the processor and the fins is conduction. Generally, the conduction between the processor and the fins is facilitated practically by application of thermal paste between the heat generating processor and the heat sink fins.

Solving and Modeling approach:

We shall solve for 4 cases as discussed in Aim.We will be using ANSYS Fluent solver to create the geometry and perform unstructured tetra CFD mesh with boundary definitions, setup the physics of fluid flow and run the iterations to get solutions, using post processing to interpret the data in form of plots,contours, vectors, streamlines etc.,

With velocity of 5 m/s and k-omega SST model we shall study grid independence for CHT analysis of exhaust port with RANS. When we say grid independence study we shall study for 4 cases as follows.

Case	Flow domain element size (mm)	Body element size (mm)	Velocity (m/s)
Case 1	Default (10.29)	Default (10.29)	5
Case 2	Default (10.29)	Default (10.29)	3
Case 3	Default (10.29)	Default (10.29)	1
Case 4	10	1	5

We shall keep in mind we are using a student version of ASNYS, so we are limited with the number of elements to play with. Then, we tabulate the case study results and compare it with the open literature or book data results to validate the simulation.

Preprocessing and Solver setting:

Let us open ANSYS workbench, now opening Fluent flow can be done by drag and drop in the schematic window or by double clicking on Fluent. The fluent workflow is in a series of steps such as GEOMETRY > MESH > SETUP > SOLUTION > RESULTS. Each step has to be completed for the next step to initialize.

we shall consider case 1 and discuss in detail,

GEOMETRY >

In the Fluent, right click on the Geometry and select New SpaceClaim Geometry. The space claim application opens, select FILE > OPEN and open the Graphics card model. It could be seen that the model already contains an enclosure. We need to perform SHARE TOPOLOGY so that there is interaction of nodes between the fluid volume and the solid volume. After performing share topology, we can quickly save the file.

We are good to go now. Once the geometry is ready, we can close space claim and check that the fluid flow (fluent) geometry is updated indicated by a green tick.

MESH >

Right clicking on the Mesh and selecting edit opens the Mesh window. Mesh window is preloaded with the geometry we have worked on earlier, so clicking on the GENERATE MESH should create a mesh automatically.

The default mesh size here is 10.29 mm. The elements are mixed in nature, meaning for prismatic structures, we get quad elements and for fluid volumes we get tetra elements, total elements is around 80000.

Any changes made, click on the update icon to update the mesh details or else there is an indication of a thunderbolt sign asking the user to update.

We shall name the entry and exit surfaces such as Inlet, Outlet, Wall by selecting the outer faces and using the ‘N’ button and name them as symmetry. We shall select the bodies and name them as PCB, Fins and Processor respectively. Once this is done, we should see a green tick near Mesh. we can close the mesh window.

SETUP >

Right clicking on the Setup, opens the Fluent launcher. In the Fluent launcher select 3D, Double precision and select the number of cores as per the user system configuration and click on start.

Upon opening, there are some selections to be done to define the simulation definitions, we shall select Type: Pressure based, Velocity Formulation: Absolute, Time: Steady. Under the Physics tab, we can turn on viscous and select k-omega > SST as well. Turn on Energy.

Under the materials we shall select air as our default material with material type as fluid. since we are dealing with the CHT analysis, we shall consider the solid volume also with aluminium as the default solid material. We need to add 2 more materials for Processor and the PCB which can be done by copying the aluminum and changing the properties like density, specific heat and thermal conductivity from standard data books for materials as follows,

Body	Material	Thermal conductivity (W/m.K)	Specific heat (J/Kg.K)	Density (Kg/m^3)
Fins	Aluminium	202.4	871	2719
Processor	Silicon	153	703	2330
PCB	Polystyrene	0.027	1210	55
Flow domain	Air	0.0242	1006.43	1.225

Under the cell zone conditions, select the solid volume and check for material selection is solid, and fluid material for fluid volume. For processor after selecting the material, enable source term and input 31250000 W.

Q = 2 W, Qg = Q/V

V = 8*8*1 e-9

Qg = 2/64 = 31250000 W/m^3

We can proceed to define boundary conditions, as follows

Inlet : velocity magnitude = 5 m/s

Outlet should be a pressure outlet.

For generating surface reports, click on the Solution > Reports > Definitions > New > Surface Report > Area weighted average > Wall fluxes > Surface heat transfer coefficient for the heat transfer coefficient in the processor. And create another report for the temperature of the processor also. Now, it's time to start the simulation. In order to start the simulation for the above set up physics, we need to initialize the entire flow field by clicking on the t=0 initialize icon. In the Run Calculation we can input the number of iterations to be run (in this case 150) and clicking on the Calculate should start the iterations. After iterations, we get scaled residuals, average temperature plot and surface heat transfer plot.

We need temperature contour as well, to get them we can colour the bodies to make new contour in Results > Graphics > Contours > New temperature for temperature contour. The scale can be edited by double clicking on it.

In the Outline view under Simulation Reports, clicking on the Report Outline > Generate should generate a Ansys Fluent Simulation Report which is automatically generated with all the information of the simulation in it. This can be exported as a PDF also. We are done with setup, we can close the setup.

SOLUTION >

Since some solution is calculated in the setup itself, we can see the green ticks in both setup and solution too.

RESULTS >

Right clicking on the Results should open the Post processor. Default view is a wireframe model, we can create a plane in XZ to view contours and vectors. Selecting the Vector and selecting the plane creates a velocity vector.

Similar to setup and solution, all contours and plots can be created here, in addition to that we can create an animation of the velocity contour by clicking on AUTOSAVE during the solution and clicking on ANIMATE select make movie and save in desired location.

For Case 2 and 3, we shall repeat the same except for changing the velocity in boundary conditions. We can simply DUPLICATE case 1 fluent file and edit in it.

For Case 4, we need to refine the mesh for bodies to 1 mm while maintaining the fluid domain mesh size as 10 mm, otherwise all steps are same as case 1.

RESULTS:

After repeating the similar manner of simulation procedures for all cases from aim, we have a handful of data to compare and study. We shall put in order all the contours, plots and vectors for us to compare and come to a conclusion. Here, only the results of all cases are displayed, its inference and interpretation shall be discussed briefly in conclusion.

Scaled Residuals

Temperature plot of Processor

Surface heat transfer coefficient plot of Processor

Temperature contour (body)

Temperature contour comparison with fins and without fins for case 1

Temperature contour comparison with fins and without fins for case 2

Temperature contour comparison with fins and without fins for case 3

Temperature contour comparison with fins and without fins for case 4

Temperature contour

Velocity vector

Velocity vector combined with Temperature contour

CONCLUSION:

From the results of all 4 cases, let us tabulate for surface heat transfer coefficient and maximum temperature of processor with respective grid sizes, velocities.

Grid Size	Case 1	Case 2	Case 3	Case 4
Flow domain mesh (mm)	10.29	10.29	10.29	10
Body mesh (mm)	10.29	10.29	10.29	1
No.of elements	81611	81611	81611	200426
Surface heat transfer coefficient (W/m^2.K)	12.634	8.779	3.995	11.998
Maximum temperature of processor (K)	328.15	335.30	361.92	322.58

Here, we can see that the heat transfer coefficient is directly depended on the inlet velocity. Also the maximum temperature of the processor, is inversely proportional to the inlet velocity. There is not much difference between coarse and fine mesh as far as the heat transfer coefficient, but the maximum temperature attained is lower in finer mesh. 5 m/s velocity is good for cooling when compared with 1 and 3 m/s.

INFERENCES:

From the grid independency study, we come to know that the finer and coarse mesh gives almost similar results. But the back flow vortices are clearly visible in post processing for finer mesh than the coarse mesh in case 1 and case 4.

As the finer size mesh elements doesn’t affect the surface heat transfer coefficient much, whereas the maximum temperature attained by the processor is lower in case of the finer mesh.

From the temperature contours, we can see that the average temperature of the PCB is very low when compared to fins because of the material properties such as low thermal conductivity. This area of heat affected in PCB is visible in Temperature contour without fins, where at low velocities the heat affected area is large. This can lead to potential thermal failure of PCB. Hence we need a good inlet velocity to maintain the temperature of processor, in this case 5 m/s is better.

There is an increase in the surface heat transfer coefficient plot before it reaches steady state, that is due to the source reaching its maximum temperature. As the simulation starts from zero initialization, the processor reaches its maximum temperature as the air velocity kicks in the heat transfer reaches a steady value in all 4 cases. The maximum point on the plot depends on the velocity of the inlet.

References:

Jurnal Kejuruteraan 31(1) 2019: 139-147

https://doi.org/10.17576/jkukm-2019-31(1)-17

Computational Fluid Dynamics Simulation on the Heat Sink Performance of a

Graphics Processing Unit Thermal Management

Zambri Harun*, Ng Jie Suang, W. M. Faizal W. Mahmood, Mahir Faris Abdullah & Eslam Reda Lotfy

Centre for Integrated Design for Most Advanced Mechanical System, Universiti Kebangsaan Malaysia, Malaysia