CHT 001 - CHT in a manifold microchannel heat sink

Conjugate heat transfer in a manifold microchannel heat sink is considered.

Simulation setup guide

Below, you’ll find a simplified guide for setting up this simulation.

Step 0 - Define shared expressions

Start out in the Properties section by defining the following shared expressions for model dimensions:

Name	Description	Expression
l1	length 1 (m)	0.6e-3
l2	length 2 (m)	0.5e-3
l3	length 3 (m)	0.3e-3
l4	length 4 (m)	0.15e-3
m1	Number of mesh segments along l1	12
m2	Number of mesh segments along l2	10
m3	Number of mesh segments along l3	12
m4	Number of mesh segments along l4	5

Then, define the following shared expressions for other key values:

Name	Description	Expression
VolumeFlowRate	Volume Flow Rate (mL/s)	0.0001
UniformHeatFlux	Uniform Heat Flux (W/m^2)	220000
InletArea	Area of inlet (m^2)	l3 * l3
InletVel	Inlet velocity magnitude (m/s)	VolumeFlowRate * 1e-6 / InletArea
InletTemp	Inlet temperature (K)	293
Ahsbase	Base area for thermal resistance calculation (m^2)	10.02 * 11.4 * 1e-6

Finally, define the following Interpolated function type shared expression:

Name	Description	Arguments
nu	Kinematic viscosity as a function of temperature	T

Under Values, input the following 10 rows:

T	values
283	0.000001311
293	0.000001009
303	8.07e-7
313	6.61e-7
323	5.59e-7
333	4.79e-7
343	4.16e-7
353	3.67e-7
363	3.3e-7
373	2.95e-7

Now, your nu shared expression should look like in the image below.

 

Step 1 - Create the geometry

In the Model section, create the model geometry by building Box elements and using the Translation operation in the following order:

Name	Element type	Axis	Center point (m)	Size (m)	Rotation (deg)
box	Box	X	0	l4	0
		Y	-l3	l3	0
		Z	l2 / 2	l2	0

Name	Element type	Target volumes	Translation (m)	Copy	Repeat count
translate	Translation	1	X: 0	☑️	2
			Y: l3
			Z: 0

Name	Element type	Target volumes	Translation (m)	Copy	Repeat count
translate 2	Translation	1, 2, 3	X: -l4	☑️	1
			Y: 0
			Z: 0

At this point, your model geometry should look like in the image below.

Then, continue adding geometry elements:

Name	Element type	Axis	Center point (m)	Size (m)	Rotation (deg)
box 2	Box	X	0	l4	0
		Y	-l3	l3	0
		Z	l1 / 2 + l2	l1	0

Name	Element type	Target volumes	Translation (m)	Copy	Repeat count
translate 3	Translation	109	X: 0	☑️	2
			Y: l3
			Z: 0

Name	Element type	Target volumes	Translation (m)	Copy	Repeat count
translate 4	Translation	109, 110, 111	X: -l4	☑️	1
			Y: 0
			Z: 0

Now, your model geometry should look like in the image below.

Finally, add the following elements:

Name	Element type	Axis	Center point (m)	Size (m)	Rotation (deg)
box 3	Box	X	0	l4	0
		Y	-l3	l3	0
		Z	l3 / 2 + l2 + l1	l3	0

Name	Element type	Target volumes	Translation (m)	Copy	Repeat count
translate 5	Translation	217	X: -l4	☑️	1
			Y: 0
			Z: 0

Name	Element type	Target volumes	Translation (m)	Copy	Repeat count
translate 6	Translation	217, 218	X: 0	☑️	1
			Y: 2 * l3
			Z: 0

Now, your model geometry is finished, and should look like in the image below.

 

Step 2 - Define the materials

Proceed to the Properties section to define the model materials.

Water

First, pick the Water material from the materials database and assign it to volumes 112, 113, 114, 217, 218, 219 and 220. Save the target as a shared region.

Set the Dynamic viscosity of your water material as 998 * nu(T).

Copper

Then, pick the Copper material from the materials database and assign it to volumes 1, 2, 3, 4, 5, 6, 109, 110 and 111. Save the target as a shared region.

Now, your model materials are defined.

 

Step 3 - Define the physics

Proceed to the Physics section to define the physics.

In this example, the Laminar flow, Heat solid and Hear fluid physics are needed.

Laminar flow

• As laminar flow target, select the water volumes (112, 113, 114, 217, 218, 219 and 220).
• Add Velocity constraint and name it as Inlet.
  • As Target, select surfaces 57 and 61.
  • As Constraint value (X, Y, Z), select (0, 0, -InletVel).
  • 
• Add Pressure constraint and name it as Outlet.
  • As Target, select surfaces 66 and 70.
  • As Constraint value, select 0.
  • 
• Add Velocity constraint and name it as CHTWalls.
  • As Target, select surfaces 21, 25, 29, 30, 34, 35, 39, and 42.
  • As Constraint value (X, Y, Z), select (0, 0, 0).
  • 
• Add Velocity constraint and name it as AdiabaticWater.
  • As Target, select surfaces 49, 56, 60, 64 and 68.
  • As Constraint value (X, Y, Z), select (0, 0, 0).
  • 
• Add Velocity symmetry and name it as SymmetryWallX.
  • As Target, select surfaces 43, 47, 50, 54, 58, 62 and 67.
  • 
• Add Velocity symmetry and name it as SymmetryWallY.
  • As Target, select surfaces 44, 51, 55, 59, 65 and 69.
  • 
• Add the Heat fluid coupling Thermal fluid.

Heat solid

• As Heat solid target, select the copper region.
• Add Heat source and name it as UniformHeatFlux.
  • As Target, select all the bottom surface of the copper region (surfaces 5, 10, 15, 20, 24 and 28).
  • As Heat source, select UniformHeatFlux.
  • 

Heat fluid

• As Heat fluid target, select the water region.
• Add Constraint and name it as Tinlet.
  • As Target, select surfaces 57 and 61.
  • As Temperature constraint, select InletTemp.
  • 

Now, your simulation physics are defined. Before moving on, check that your physics tree looks like in the image below.

 

Step 4 - Generate the mesh

Proceed to the Simulations section and create a new structured mesh:

1. Set Mesh quality to Expert settings.
2. Scroll down to Structured meshing and click Add structured mesh entity 16 times in total.
3. Assign a different volume as target for each entity, so that each entity targets a different volume in the model.
4. Save your work so far by clicking Apply.
5. Assign lengths to your structured mesh entities segments according to this table:

   Entity target volumes	A Segments	B Segments	C Segments
   1, 2, 3, 4, 5, 6	m2 (5e-5)	m3 (2.5e-5)	m4 (3e-5)
   109, 110, 111, 112, 113, 114	m1 (5e-5)	m3 (2.5e-5)	m4 (3e-5)
   217, 218, 219, 220	m3 (2.5e-5)	m3 (2.5e-5)	m4 (3e-5)

6. Click Apply & mesh.

Your finished mesh should look something like in the image below:

 

Step 5 - Simulate

In the Simulations section, create a new simulation:

• In Simulation settings:
  • Set Analysis type to Steady state.
  • Set Solver mode to Direct solver.
• In Mesh, select the mesh you created.
• In Outputs, add the 13 following outputs (or only those interesting to you):

  Output type	Name	Output expression
  Field	p	p
  Field	V	V
  Field	T	T
  Custom value	flowratein	integrate(reg.inlet_target, transpose(V)*-normal(reg.water_target),2)
  Custom value	flowrateout	integrate(reg.outlet_target, transpose(V)*-normal(reg.water_target),2)
  Custom value	AvgCHTWallTemp	integrate(reg.chtwalls_target, T, 2)/integrate(reg.chtwalls_target, 1.0, 2)
  Custom value	PressureDrop	integrate(reg.inlet_target, p, 2)/integrate(reg.inlet_target, 1.0, 2)-integrate(reg.outlet_target, p, 2)/integrate(reg.outlet_target, 1.0, 2)
  Custom value	Tbasemax	maxvalue(reg.uniformheatflux_target, T, 2)
  Custom value	Tbasemin	minvalue(reg.uniformheatflux_target, T, 2)
  Custom value	Tbaseavg	integrate(reg.uniformheatflux_target, T, 2)/integrate(reg.uniformheatflux_target, 1.0, 2)
  Custom value	ThermalResistance	(maxvalue(reg.uniformheatflux_target, T, 2)-InletTemp)/(UniformHeatFlux*Ahsbase)
  Custom value	PumpingPower	(integrate(reg.inlet_target, p, 2)/integrate(reg.inlet_target, 1.0, 2)-integrate(reg.outlet_target, p, 2)/integrate(reg.outlet_target, 1.0, 2))*abs(integrate(reg.inlet_target, transpose(V)*-normal(reg.water_target),2))
  Custom value	MeanAbsoluteTemperatureDeviation	(abs(maxvalue(reg.uniformheatflux_target, T, 2) - integrate(reg.uniformheatflux_target, T, 2)/integrate(reg.uniformheatflux_target, 1.0, 2)) + abs(minvalue(reg.uniformheatflux_target, T, 2) - integrate(reg.uniformheatflux_target, T, 2)/integrate(reg.uniformheatflux_target, 1.0, 2)))/2.0

Run your simulation by clicking Not Run.

 

Step 6 - Results

In the Simulations section, add visualizations to see field output results. In a steady state simulation, only one data point is extracted for each custom value output. See custom value output data in the Summary. Some examples are given below.

• Velocity field V visualized:
  • Glyph, scale factor 0.00003
  • 
• Temperature field T visualized:
  • 
• Summary:
  • 

To extract multiple values for each custom value output, create a sweep or a transient simulation with enough time-steps.

References

[1] K. Tang, G. Lin, Y. Guo, J. Huang, H. Zhang, J. Miao. Simulation and optimization of thermal performance in diverging/converging manifold microchannel heat sink. International Journal of Heat and Mass Transfer, Vol 200, 2023. https://doi.org/10.1016/j.ijheatmasstransfer.2022.123495.