When fluid flow passes a body, it will exert a force on the surface. As shown in the figure below, the force component that is perpendicular to the flow direction is called lift. The force component that is parallel to the flow direction is called drag. For simplicity, let’s assume that the flow direction is aligned with the coordinate system of the model. Later on, we will show you how to compute the lift and drag forces in a direction that is not aligned with the model coordinate system.
Schematic of lift and drag components when fluid flow passes a body.
There are two distinct contributors to lift and drag forces — pressure force and viscous force. The pressure force, often referred to as pressuregradient force, is the force due to the pressure difference across the surface. The viscous force is the force due to friction that acts in the opposite direction of the flow. The magnitudes of pressure force and viscous force can vary significantly, depending on the type of flow. The flow around a moving car, for instance, is often dominated by the pressure force.
COMSOL Multiphysics offers complete access to all of the internal variables and makes it very easy to compute surface forces via integration on a boundary. Here, we will demonstrate how to compute the drag forces on an Ahmed body. You can download this model from our Application Gallery.
Simulation of airflow over an Ahmed body. The surface plot shows the pressure distribution, and the streamlines are colored by the velocity magnitude. The arrow surface behind the Ahmed body shows the circulation in the wake zone.
There are several ways to compute drag depending on the physics. The most straightforward way is to integrate the total stress — which includes contributions from the pressure force and the viscous force — in each direction. To do so, we first need to define a surface integration operator under the Derived Values node, as illustrated below.
TIP: Alternatively, you can also use a boundary probe or integration operator in the component coupling to define such integration. The difference is that the operations defined in the physics setting can be used during the simulation — for example, drag force computed with a boundary probe as an objective or a constraint in an optimization study.
Next, we can select the boundaries to perform the integration. In this example, we chose all of the boundaries on the body. Drag in this model is in the ydirection. We can type in the expression: spf.T_stressy
, which represents the total stress in the ydirection.
Sometimes, engineers can obtain greater insight into designs by examining the pressure force and viscous force separately. COMSOL Multiphysics features a predefined variable, spf.K_stressy
, for viscous stress in the ydirection. We can readily evaluate the viscous force by integrating the viscous stress.
What about the pressure force? Pressure, denoted by the variable p
, is a scalar. To project in the direction of drag, we need to multiply pressure by the ycomponent of the normal vector on the surface, spf.nymesh
. Therefore, we can evaluate the pressure force by integrating spf.nymesh*p
on the surface.
In some special turbulent flow cases where the wall function is used, it is more accurate to compute the viscous force using the friction velocity, spf.u_tau
. In COMSOL Multiphysics, the kepsilon and komega turbulence models use the wall function.
To learn more about turbulence models in COMSOL Multiphysics, read our blog post “Which Turbulence Model Should I Choose for My CFD Application?“.
We can obtain the local shear stress at the wall by:
Therefore, the local shear stress in the ydirection is:
where u^T is the tangential velocity at the wall. We can further rewrite u^T as u_\tau*u^+, where u^+ is the tangential dimensionless velocity.
Without going into too many details on derivation, we can translate the previous equations into COMSOL variables. We can integrate the local wall shear stress in the direction of drag (the ydirection) with the following expression: spf.rho*spf.u_tau*spf.u_tangy/spf.uPlus
. In this expression, spf.rho
is the density of the fluid, spf.u_tangy
is the velocity in the ydirection at the wall, and spf.uPlus
is the tangential dimensionless velocity.
The table below summarizes the expressions used to compute each force.
Fluid Flow Without Wall Function  Turbulent Flow with Wall Function  

Pressure Force  spf.nymesh*p  spf.nymesh*p 
Viscous Force  spf.K_stressy  spf.rho*spf.u_tau*spf.u_tangy/spf.uPlus 
Total Force  spf.T_stressy  spf.nymesh*p + spf.rho*spf.u_tau*spf.u_tangy/spf.uPlus 
Note: In this example, the drag force is in the ydirection. You may need to change the projection direction based on the orientation of your model.
It is common that the geometry may not be aligned perfectly with the flow direction. The angle between the center reference line of the geometry and the incoming flow is called angle of attack (often denoted by the Greek letter \alpha). In aerospace engineering, the angle of attack is frequently used as it is the angle between the chord line of the airfoil and the freestream direction. The following figure shows the relationship between lift, drag, and angle of attack on an airfoil.
Schematic illustrating lift, drag, and angle of attack on an airfoil.
Using a 2D NACA 0012 model, we will show you how to compute lift with an angle of attack correction. This model is available for download in our Application Gallery.
There are two ways to change the angle of attack of the model. We can either rotate the geometry itself or we can keep the geometry fixed but modify the flow direction at the inlet. Here, we will use the second approach. It is much simpler to adjust the velocity field at the inlet boundary condition as we would not need to remesh the model for each angle of attack. As shown in the figure below, the airfoil is fixed while the streamlines show the flow at an angle of attack due to the adjusted inlet velocity direction.
Simulation of flow passing a NACA 0012 airfoil at a 14degree angle of attack. The surface plot shows the velocity magnitude along with the streamlines (shown in black).
This example uses the SST turbulence model, which does not use the wall function. Therefore, we will use total stress to compute lift. At a zero angle of attack, the lift is simply spf.T_stressy
. If the angle of attack is nonzero, we can project the force onto the direction of the lift using the following expression: spf.T_stressx*sin(alpha*pi/180)spf.T_stressy*cos(alpha*pi/180)
. Here, alpha represents the angle of attack in degrees.
You may also be interested in the nondimensionalized forms of lift and drag — the lift coefficient and the drag coefficient. It is often easier to use the coefficients instead of the dimensional forces for the purpose of validating experimental data or comparing different designs. The lift coefficient in 2D is defined as:
Since we have already calculated the dimensional lift, we can simply normalize the lift by the dynamic pressure and the chord length. With the dimensionless lift coefficient, we can compare our simulation results with experimental data (Ref. 1).
Note: In 3D, the lift coefficient is nondimensionalized by area instead of length: C_L = \frac{L}{\frac{1}{2} \rho U_\infty A}
Graph comparing simulation results and experimental data of the lift coefficient on a NACA 0012 airfoil at various angles of attack.
As illustrated in the above graph, no discernible discrepancy between the computational and experimental results occurs within the range of the angle of attack values used in this simulation. The experimental results continue toward a high angle of attack regime where the airfoil stalls.
In this blog post, we have explored ways to compute lift and drag on an Ahmed body and an NACA 0012 airfoil. We have demonstrated how to compute pressure force and viscous force, while also examining the special case where a wall function is used in the turbulence model.
Each of the approaches we have presented here are certainly not limited to these specific simulations. You can compute the body forces on any boundaries or surfaces, thereby gaining insight into designs through multiphysics simulations. With the Optimization Module, you can take this analysis one step further and optimize lift or drag.
Introduced by L.V. King in 1914, the hotwire anemometer represented the first of its kind: A device that could measure fluid flow using thermal sensing techniques. In a hotwire anemometer, a thin wire is electrically heated to a temperature greater than its surroundings. The surrounding flow cools down the device up to a given temperature. Because of the known relationship between the electrical resistance of the wire and its temperature, the fluid velocity can be obtained from the knowledge of the wire’s resistance.
Because of their delicate nature, hotwire anemometers are often not suitable for industrial use as many applications include dirt, which can cause damage to these fragile devices. Hotwire anemometers are also referred to as intrusive devices, because the sensors do not only measure the flow properties, but they also disrupt the flow. A more viable solution in such cases would be to use a thermal mass flow meter. The thermal mass flow meter is a nonintrusive device, i.e., it leaves the flow path unobstructed. While applying the same concepts as their predecessor, these instruments feature casing around the wires, enhancing their durability as well as their accuracy in measuring fluid flow.
A schematic of a thermal mass flow meter.
Thermal mass flow meters have been used extensively for measurement in gas flow applications, from thermal transfer to chemical reactions. These instruments are particularly favored in the industry for their simplistic design, as there are no moving parts included in the device.
A team from the University of Cambridge used COMSOL Multiphysics software to develop a 3D model of thermal flow sensors and analyze the dynamics behind the components’ operation. Let’s explore how simulation enabled this team to describe the behavior of this instrument under every physical aspect.
The design of the model used in the study was based on a silicon on insulator (SOI), complementary metaloxide semiconductor (CMOS) MEMS thermal flow sensor — or SOI CMOS MEMS thermal flow sensor, for short. The model features a validation chip that includes five parallel metal strips. The strip in the center is used to increase the temperature of the device to 300°C. All of the strips can be used to sense the temperature through the relationship between the metal resistivity and the absolute temperature. A fourwire measurement is used to obtain the resistance value.
When developing this validation chip, deep reactive ion etching was implemented at the back surface to remove the silicon substrate from beneath the sensing elements. This postprocessing step drastically reduced the thermal conductivity observed by the heating element and, consequently, lowered the power required to increase the temperature at the desired value.
The geometry of the thermal flow sensor. The image on the left shows the crosssectional view of the validation device, while the image on the right shows the top view. Image by C. Falco, A. De Luca, S. Sarfraz, and F. Udrea, and taken from their COMSOL Conference 2014 Cambridge paper submission.
In their analysis, the research team coupled three different physical domains — electric current, heat transfer in solids, and laminar flow — to create a multiphysics model. That is, the bias current is used to locally heat up the component, through the Joule heating effect, and conductive and convective heat transfer dissipate the excess heat.
Initially, the flow sensor was validated in still air. The plot below represents a validation of the relationship between dissipated power in the heater and the temperature sensed by alternate resistors without flow above the surface. The values from the simulation and the experiment are shown to mirror one another.
Comparing the temperature in all the resistors within the simulation and experimental data. Image by C. Falco, A. De Luca, S. Sarfraz, and F. Udrea, and taken from their poster submission.
The figure below provides a complete temperature profile for the current value of 10 mA.
Temperature profile in the area of interest. Image by C. Falco, A. De Luca, S. Sarfraz, and F. Udrea, and taken from their poster submission.
The wall shear stress, defined as the stress that a viscous fluid exerts on a wall, is chosen to characterize the fluid properties. In the next step, the research team calibrated the sensor, with the air movement above the chip included in the analysis, for varying values of wall shear stress. Comparing three values for the biasing current (6, 8.5, and 10 mA), the results showed good agreement between the temperature within the resistors and the experimental data for wall shear stress.
Plots depicting the sensor output as a function of wall shear stress. The graph on the top (a) shows the calorimetric approach and the graph on the bottom (b) represents the anemometric approach. An anemometric approach involves the measurement of the changes in the voltage across the heater; the calorimetric approach senses the variance in voltage between resistors that are placed symmetrically on opposing sides of the heater. Image by C. Falco, A. De Luca, S. Sarfraz, and F. Udrea, and taken from their paper submission.
Here, we have introduced research designed to investigate the behavior of thermal flow sensors. Coupling heat transfer, electric current, and laminar flow, the simulation provides accurate predictions of the sensor’s behavior and, by modifying the model’s geometry and material properties, can be applied to various applications of this technology. With its high precision and range of applications, the thermal flow sensor model serves as a powerful resource in optimizing the design of thermal flow sensors and developing prototypes more efficiently.
For our example, we will use a model that couples the NavierStokes equations and the heat transfer equations to model natural convection in a square cavity with a heated wall. The temperature on the left and right walls is 293 K and 294 K, respectively. The top and bottom walls are insulated. The fluid is air and the length of the side is 10 cm.
We will use this model to compare the computational cost of three different modeling approaches:
Each of these three approaches and their variables are defined here.
In COMSOL Multiphysics, the model is solved with a stationary study using the Laminar Flow, and Heat Transfer in Fluids interfaces, and the NonIsothermal Flow multiphysics coupling:
While setting up the model, it is important to check whether the flow is laminar or turbulent. For a natural convection problem, this is done by calculating the Grashof number, Gr. For an ideal gas, it is defined as
The Grashof number is the ratio of buoyancy to viscous forces. A value below 10^8 indicates that the flow is laminar, while a value above 10^9 indicates that the flow is turbulent. In this case, the Grashof number is around 1.5 \times \hspace{1pt} 10^5, meaning that the flow is laminar.
When using the full NavierStokes equation, we set the buoyancy force to \rho \mathbf{g}:
The buoyancy term is added using a volume force feature. The terms nitf1.rho and g_const represent the temperature and pressuredependent density, \rho, and the gravitational acceleration, \mathbf{g}, respectively.
When using the NavierStokes equations with pressure shift, we have to make three changes.
First, we need to change the definition of the volume force to (\rho\rho_0)\mathbf{g}, as such:
The term rho0 refers to the reference density \rho_0.
Next, we evaluate the reference density \rho_0 and the reference viscosity \mu from the material properties in a table of variables:
Here, pA and T0 represent the reference temperature and pressure.
The air viscosity is set to the constant \mu_{0}:
Finally, when using the Boussinesq approximation, we need to set the buoyancy force to \rho_0\frac{TT_0}{T_0}\,\mathbf{g}:
As with Approach 2, we also evaluate the reference density and viscosity from the material properties. A third and final step with Approach 3 is to set the fluid density to the constant reference density \rho_{0} (the Boussinesq approximation states that the density is constant except in the buoyancy term).
Note: If your model includes a pressure boundary condition (open domain), set the pressure to the hydrostatic pressure rho0*g_const*y for Approach 1 or to 0[Pa] for Approach 2 and Approach 3. The boundary conditions for models including gravitational forces are also discussed here.
The mesh is made of 15,000 triangular elements and 1,200 boundary layer elements. These are firstorder elements.
The resulting velocity magnitude and streamlines are nearly identical for all three approaches. The maximum temperature difference between Approach 1 and 2 is less than 2 \times \hspace{1pt} 10^{6} K and the maximum temperature difference between Approach 1 and 3 is around 5 \times \hspace{1pt} 10^{4} K. The only thing that differs is the simulation time.
Velocity magnitude and streamlines.
Because of the short running time of this 2D simulation (around 30 seconds), we look at the computational load by comparing the number of iterations it takes the solver to converge to the steadystate solution. The number of iterations, in this case, is nearly proportional to the CPU time.
The table below compares the number of iterations across all three approaches.
Approach 1  Approach 2  Approach 3  

Number of Iterations  39  55  55 
These results are very surprising!
While the Boussinesq approximation is supposed to reduce the nonlinearity of the model and the number of iterations required for convergence, the full NavierStokes equations (39 iterations) can be solved faster than the Boussinesq approximation (55 iterations). We also note that the use of NavierStokes equations with a pressure shift leads to the same number of iterations as the Boussinesq approximation.
To better understand these results, we can run a second set of simulations after disabling the pseudo timestepping algorithm. Pseudo time stepping is used for stabilizing the convergence toward steady state in transport problems. The pseudo time stepping relies on an adaptive feedback regulator that controls a Courant–Friedrichs–Lewy (CFL) number. The pseudo time stepping is often necessary to get the model to converge. In this particular case, however, it is not needed .
Here’s a look at the COMSOL Multiphysics settings window for the default solver settings with pseudo time stepping:
The following snapshot shows the updated solver settings without pseudo time stepping. We recommend that you always keep pseudo time stepping switched on, unless you feel comfortable tuning the solver settings.
Note on the solver settings for natural convection:
Due to the very strong coupling between the laminar flow and heat transfer physics in natural convection modeling, always use a fully coupled solver. The COMSOL software automatically switches to a fully coupled solver when a volume force is added in the laminar flow physics, meaning that you are modeling natural convection.
This second table shows the number of iterations without pseudo time stepping:
Approach 1  Approach 2  Approach 3  

Number of Iterations  9  7  7 
These results make more sense than the previous ones with pseudo time stepping. This is because Approach 3, the most linear problem, now converges faster than Approach 1. What is surprising is that Approach 2 and Approach 3 converge with the same number of iterations.
Comparing these results with the first set of results, a speedup of 8 (from 55 to 7 iterations) is observed for the third approach — the Boussinesq approximation. These results also indicate that the number of iterations in the first set of results not only depend on the linearity of the problem, but also on the tuning of the pseudo timestepping algorithm.
Here, we have discussed the implementation and benefits of the Boussinesq approximation as well as using the pressure shift method. The results show that, for this particular model, there are no real benefits in terms of computational time for using the Boussinesq approximation, regardless of whether or not pseudo time stepping is enabled. This is generally the case since the Boussinesq approximation is only valid when the nonlinearity is small. A much shorter computational time for the Boussinesq approximation with respect to the full NavierStokes equations would indicate that the Boussinesq approximation might not be valid.
Because of the small speedup observed with the Boussinesq approximation and the fact it is not always easy to know a priori if the Boussinesq approximation is valid, we generally recommend solving for the full NavierStokes equations. Implementing the pressure shift (Approach 2 and 3), however, does avoid roundoff errors and simplifies the implementation of timedependent problems as well as models with open boundaries. This will be the object of a future blog entry.
Using Approach 3 (Boussinesq approximation with pressure shift) involves more implementation steps and does not reduce the number of iterations as compared with Approach 2 (NavierStokes equations with pressure shift). The final simulation time might be slightly shorter for Approach 3, since it does not require the evaluation of the temperature and pressuredependent density and the temperaturedependent viscosity, but this speedup might not be noticeable.
The number of iterations is reduced by a factor 4 to 8, depending on the chosen approach, by disabling the pseudo timestepping algorithm. Please keep in mind, however, that most problems will not converge without pseudo time stepping or other load ramping or nonlinearity ramping strategies.
You can set up and solve this model using the CFD Module or the Heat Transfer Module. If you have any questions about the models that I’ve presented here, contact our Technical Support team. If you are not yet a COMSOL Multiphysics user and would like to learn more about our software, please contact us via this form — we’d love to connect with you.
]]>
The drag coefficient quantifies the resistance of an object in a fluid environment. It is not an absolute constant for a body’s shape because it varies with the speed and direction of flow, object shape and size, and the density and viscosity of the fluid. The lower the drag coefficient of an object, the less aerodynamic or hydrodynamic drag occurs. In terms of a car, the lower the drag coefficient, the more efficient the car is. As well as affecting the top speed of a vehicle, the drag coefficient also affects the handling. Cars with a low drag coefficient are sought after, but decreasing the drag drastically can reduce the downforce and lead to loss in road traction and a higher chance of car accidents.
Most cars have an average drag coefficient of between .30 and .35. Boxy cars have a higher number, like the HUMMER® H2 vehicle at .57, while more streamlined and agile cars have a lower number, like the MercedesBenz® CClass® vehicle at .24. Again, this is just an average measurement. The exact drag coefficient of a car varies with the Reynolds number and various other factors.
There are certain ways to modify a car to optimize its aerodynamics and decrease the drag coefficient. To streamline the exterior, you can remove certain aftermarket items such as the roof rack, mud flaps, spoilers, and radio antenna. Professional car racers also take off their windshield wipers and side mirrors, but this isn’t recommended for the average driver! You can also add wheel covers, a partial grille block, an under tray, fender skirts, and a modified front bumper to improve the drag coefficient and make your car stand out in the process.
The Ahmed Body was first created by S.R. Ahmed in his research “Some Salient Features of the TimeAveraged Ground Vehicle Wake” in 1984. Since then, it has become a benchmark for aerodynamic simulation tools. The simple geometrical shape has a length of 1.044 meters, height of 0.288 meters, and a width of 0.389 meters. It also has 0.5meter cylindrical legs attached to the bottom of the body and the rear surface has a slant that falls off at 40 degrees.
The simple geometry of an Ahmed body.
In the Airflow Over an Ahmed Body verification model, our Ahmed body has a 25degree slant and is placed in the following domain, measuring 8.352by2.088by2.088 meters, to compute the flow field.
Computational domain and boundary conditions for the fluid flow simulation.
The front of the body is placed at a distance of 2 car lengths (2L) from the flow inlet. To reduce the computational cost, a symmetry plane is introduced to model half of the model.
The flow for this model is turbulent, which is based on the Reynolds number determined by the body length and inlet velocity. The simulation solves for the turbulent kinetic energy in addition to the velocity field. For this simulation, we need a larger mesh size than what is usually common to resolve the turbulent flow. More specifically, we use a finer mesh downstream of the model to capture the wake zone.
The flow for this model is turbulent, which is based on the Reynolds number determined by the body length and inlet velocity. The simulation solves for the turbulent kinetic energy and dissipation in addition to the velocity and pressure fields.
The total drag coefficient of the Ahmed body is the key measurement for this simulation. It is made up of measurements for the pressure coefficients in the front, slant, and base of the body as well as the body’s skin friction. In the results of our simulation, the total drag is very well predicted but the individual measurements deviate from the experimental results in varying amounts.
A few different factors cause these deviations in data. For the front and roof of the body, wall functions used in the simulation aren’t effective at predicting the flow transitions observed in the experiments.
In terms of deviations in the slant coefficient data, we see the flow along the slant shown by streamlines in the figure below. The thickness of these streamlines is determined by turbulent kinetic energy.
Streamlines behind the Ahmed body have thickness proportional to their turbulent kinetic energy.
In the experimental data, these lines show that the flow along the slant is attached almost everywhere and that there are two small recirculation zones behind the base. In the simulation results, this effect is captured but the extent of the recirculation zones is overpredicted.
Streamlines showing the recirculation zones past the Ahmed body.
The pressure drag for the slant coefficient is very sensitive to the exact shape and location of the recirculation regions, which accounts for the deviation in measurements.
Although the data has quantitative differences, it is qualitatively equal to experimental results because the total drag coefficients are so close. There may be deviating details in the smaller data but the simulation still captures the major features of the flow over an Ahmed body. This simulation is more than adequate for calculating the overall drag coefficient.
HUMMER is a registered trademark or trademark of General Motors LLC.
MercedesBenz and CClass are registered trademarks of Daimler AG Corporation.
]]>
The name syngas gives reference to the role of this fuel gas mixture — comprised mostly of hydrogen, carbon monoxide, and carbon dioxide — as an intermediate in the production process of synthetic natural gas. Syngas, however, is also used to create other products such as methanol, ammonia, and even hydrogen. The idea behind this is a process known as gasification.
In gasification, a solid feedstock is converted to a gas, which can then be used in numerous applications. The gas can be liquefied, for example, by compression. Gasification is particularly valued for its flexibility in the types of feedstock that can be used, with options ranging from coal to biomass. Additionally, this approach simplifies the task of capturing byproducts of the reaction like sulfur or carbon dioxide.
Here, we model syngas combustion in a roundjet burner, comparing our results with experimental data.
In the Syngas Combustion in a RoundJet Burner model, the burner is comprised of a straight pipe within a slow coflow consisting of air. A gas made up of carbon monoxide, hydrogen, and nitrogen is fed through the pipe with an inlet velocity of 76 m/s (Ma ≈ 0.25). Meanwhile, the coflow velocity of the air outside of the pipe is 0.7 m/s.
Upon exiting the pipe, the fuel gas mixes with the coflow, which generates an unconfined circular jet. The turbulent flow of the jet ensures efficient mixing of the two gases and sustains combustion at the exit of the pipe. This is a nonpremixed form of combustion as the fuel and oxidizer come into the reaction zone independently.
A schematic of the roundjet burner.
Within this example, we solve for the mass fraction of six chemical species — the five used in the reactions and the nitrogen initially in the coflow — to model the mass transport in the reacting jet. In the example, the jet features a Reynolds number of around 16700, meaning that the jet is fully turbulent. Because of this, we can assume that the turbulence of the flow has a significant impact on the jet’s mixing and reaction processes.
The k\epsilon turbulence model is used to account for this turbulence within the flow field. To model the turbulent reactions, we use the eddy dissipation model, which provides a robust yet simple way of simulating such reactions. Because of heat release in the reactions, there is a significant increase in temperature of the jet — a defining characteristic of combustion. To accurately predict the temperature and composition, we account for the temperature dependence of the species properties as well as the physical properties of the fluid.
The syngas combustion model involves a high degree of coupling, combining turbulent flow with heat and mass transfer. A thorough overview of the solution steps to solve such a nonlinear model is shown in the Model Gallery entry.
The first figure below depicts the velocity field within the reacting jet, illustrating the expansion and creation of the hot free jet. Within the outer parts of the jet, turbulent mixing prompts the acceleration of fluid initially from the coflow and brings it into the jet, a process referred to as entrainment. This transition of fluid is evident in the coflow streamlines that bend towards the jet downstream of the opening of the pipe.
The velocity flow magnitude and field.
Next, we can analyze the temperature in the jet, using a revolved data set to visualize the model in full 3D. Here, we identify the maximum temperature within the combustion region as about 1960 K.
Jet temperature.
The following figure illustrates the carbon dioxide mass fraction within the reacting jet. CO_{2} is formed in the jet’s outer shear layer, right outside of the pipe. It is in the outer shear layer that the fuel reacts with the oxygen in the coflow, with turbulent mixing encouraging the reactions. Like the CO_{2} formation, the temperature increase depicted in the previous plot also takes place just outside of the pipe. This suggests no liftoff and the attachment of the flame to the pipe.
Carbon dioxide mass fraction.
Let’s now shift our focus to comparing the simulation results with experimental data. Our analysis begins with the jet temperature profiles along the centerline, as shown in the figure on the left, below. In this graph — and the ones that follow — lines represent the model results and symbols are used to indicate the experimental values. The plot of the centerline shows that the maximum temperature predicted in the model is close to that from the experimental results.
In the model results, you may notice that the temperature profile shifts in the downstream direction. This difference can be attributed to the fact that radiation has been left out of the model. Meanwhile, the figure on the right compares the temperature profiles along a horizontal line at two different positions (20 and 50 pipe diameters) downstream of the pipe exit. Again, there is a good agreement between the values obtained in the simulation and those from the experiment.
Left: A plot comparing jet temperatures along the centerline. Right: Jet temperatures at 20 and 50 pipe diameters downstream of the pipe exit.
When comparing the axial velocity of the jet with experimental data, we can observe that these results are in excellent agreement for both positions (20 and 50 pipe diameters). This is illustrated here:
Axial velocity at the same downstream positions as the previous plot.
Lastly, we evaluate the species concentration along the jet centerline. In the case of the species N_{2} and CO, the axial mass fraction development aligns closely with experimental data. H_{2}O and H_{2} are found to agree fairly well with the experimental values, with a slight shift on H_{2}O. The species CO_{2} and O_{2} feature a similar trend as the experimental results but, just as in the temperature, the profiles are found to shift downstream. Here, the discrepancy can be somewhat attributed to the lack of inclusion of radiation in the model. However, the simplified reaction scheme and the eddy dissipation model are likely to have an influence on the accuracy as well.
Comparing species mass fractions along the jet centerline.
Try pouring some wine into a glass. Don’t drink it yet — this is a scientific experiment. When you hold up your glass, you’ll see what look like teardrops running down the sides. These tears of wine are caused by the Marangoni effect, which describes a mass transfer along the surface of two fluid phases caused by surface tension gradients along the interface between the two phases (for example liquid and vapor).
The term tears of wine was first coined in 1865 by physicist James Thomson, the brother of Lord Kelvin. Italian physicist Carlo Marangoni later studied the topic for his doctoral research and published his findings in 1865. The Marangoni effect, which causes tears of wine and other phenomena observed in surface chemistry and fluid flow, is named after Marangoni and his research.
Tears of wine moving down the inside of the glass.
Study your glass. Do you see the tears? If not, it may be because you chose a wine of low alcohol content. If you want to see tears of wine, wine with a high alcohol content is more likely to display tears. Wine with a low alcohol content gives only small variations in alcohol concentration and surface tension along the wineair interface and will rarely show teardrops. The wine in the photo above has 13.5% alcohol content, which is on the lower side, but high enough to produce tears.
Surface tension is a property of the interface between two phases. It describes the amount of energy needed to expand the surface area of that interface by one unit. You can also look at surface tension as the force per unit length needed to create new surface area. The figure below illustrates a liquid phase in contact with its vapor. The surface molecules (shown in red) have only very small upwards interactions with the vapor molecules (shown in orange) causing them to experience asymmetrical force that pulls the surface of the liquid together. The molecules in the bulk of the liquid (blue) interact in all directions. To expand the surface area of the liquid, bulk molecules have to move towards the surface, breaking up upward interactions. Doing so requires energy.
Surface tension in a liquid interacting with its vapor. The molecules at the surface (red) experience asymmetric interactions. The molecules just below (violet) experience slightly more symmetric interactions, while the molecules in the bulk (blue) experience even more symmetric interactions.
Water has strong interactions in the bulk of the liquid due to its hydrogen bonds, so it has a relatively large surface tension since it requires breaking strong interactions. Liquidsvapor interfaces have surface tensions that depend on the strength of the interactions between the molecules in the bulk of the liquid. The Marangoni effect is the flow caused by gradients in surface tension along the liquidvapor interface surface in the figure above. Such a gradient can be caused by differences in composition or temperature of the solution along this surface.
We can see how this works by pouring a thin layer of water onto a plate and adding glitter or another kind of light material to better illustrate the effect. The interaction between the water and the glitter is due to the glitter particles being hydrophilic, or water loving. Adding a drop of soapy solution, alcohol, motor oil, or any liquid with a contrasting surface tension to the center of the surface causes all of the glitter to immediately rush to the sides of the surface, away from the center.
As you pour soap, the soap molecules form a thin film — only one or a few molecules thick — on the water surface. The surface experiences a difference in surface tension between the parts covered by soap and the parts with only water, which causes the soap film to spread and the glitter particles to flow to the sides — the Marangoni effect. Eventually, the soap molecules cover the whole surface, which lowers the surface energy, because now the surface water molecules are also able to interact with the hydrophilic end of the soap molecules.
In the next figure, the experiment is illustrated on a molecular level. The glitter particles rather interact with water, not with soap, because they have a hydrophilic surface. They are squeezed to the sides as the soap covers the surface because they “want” to continue interacting with water molecules.
Surface tension changes as soap is added to water. Soap is green, an ion with with a hydrocarbon “tail”. Water is blue in the bulk, red at the free water surface, and violet at the surface covered by soap or when they are just below other surface water molecules.
In tears of wine, a meniscus forms at the threephase junction between the wine glass walls, wine, and air. This is where the liquid loosely clings to the surface of the glass. The meniscus is formed because the walls of the glass have a hydrophilic surface, like the surface of the glitter particles. Wine contains alcohol that is continuously evaporating from the surface at a rate higher than water (since ethanol has a higher equilibrium vapor pressure than water), and this also takes place in the meniscus. The alcohol concentration decreases faster in the meniscus due to its higher surface area in relation to its small volume. Therefore, it causes an alcohol concentration difference between the meniscus and the flat interface surface between the wine and air. This then causes a surface tension gradient that moves the meniscus up the walls of the glass.
As the meniscus begins to form a film on the surface of the glass’ walls, it gets even more depleted of alcohol, which in turn causes a larger surface tension gradient. More wine gets pulled up the walls of the glass until droplets form. Gravity takes effect and tears of wine run down the sides of the glass and back into the bulk of the wine.
Tears of wine form due to the surface tension (γ) gradient between the meniscus and the flat surface of the wine.
Here’s a 3second timelapse video to further illustrate the effect:
We can model the Marangoni effect with COMSOL Multiphysics and the Microfluidics Module. To get started, we have a tutorial model that illustrates the concept — the Jet Instability model. This model simulates an inkjet printer and the breakup of an infinitely long liquid jet due to a spatially varying surface tension coefficient.
There are three ways to solve this model: via the moving mesh, level set, or phase field methods. If you go to the Model Gallery, you will find PDFs with modeling instructions for two of these (the moving mesh and level set methods). The moving mesh method is faster and easier to use than the level set method, as we saw in Fabrice Schlegel’s blog post Which Multiphase Flow Interface Should I Use? However, we can only use the moving mesh method to model the Marangoni effect in tears of wine if the wine layer on the side of the glass has a definite thickness. There can be no dry area between the tears and the rest of the wine. If that’s the case, we must use either the level set or the phase field method.
The Jet Instability model consists of a fluid domain in the shape of a cylinder with a radius of 20 microns and a height of 60 microns. The domain contains a cylinder of water with a radius of 5 microns. We need to define the ink properties such as density and dynamic viscosity, as well as the surface tension coefficient.
We use the Laminar TwoPhase Flow, Moving Mesh interface to solve the model, which is plotted on moving mesh geometry. For this simulation, the interface has no thickness and is represented by a boundary. This is better for practical mesh densities. The interface calculates the NavierStokes equations and boundary conditions and transforms it onto a fixed mesh.
A cylinder of an inkjet printer in the Jet Instability model.
The Laminar TwoPhase Flow, Moving Mesh interface can easily input other physics and it is faster and more accurate than the level set and phase field methods. However, the moving mesh method cannot handle topological changes. This means that it can only be used for calculations prior to the breakup of droplets. The Laminar TwoPhase Flow, Level Set interface calculates velocity field and pressure as described by the NavierStokes equations, periodic boundary conditions, and point settings.
The results below were modeled using the level set method and show the breakup of the jet into droplets over six time periods. At first, the liquid forms a perfect column, but the variation in surface tension disturbs the jet and causes a force due to surface curvature that eventually breaks up the jet into droplets.
The liquid regions of the model as the jet breaks up due to surface tension variation over time.
Ps. We’re currently working on a new Heat Transfer feature for modeling Marangoni convection. Stay tuned for the upcoming release of COMSOL Multiphysics version 5.1…
]]>
Journal bearings are typically used to support a rotating shaft. They are made of two parts: a shaft (or journal) rotating in a fixed bearing. To reduce the friction and wear between the fixed bearing and the rotating shaft, the thin gap between these two parts is filled with a viscous fluid, such as oil, thus avoiding surfacetosurface contact. This lubricant also damps undesirable mechanical vibrations. This thin layer of fluid is referred to as the lubrication layer. Its thickness is ideally in the realm of thousandths to hundredths of a millimeter.
Because of the loads applied to the bearing and the shaft, the lubrication layer’s thickness is not constant, and neither is the flow pressure. When the flow pressure drops below the ambient pressure, the air and other gases dissolved within the lubricant are released. This phenomenon, characteristic of loaded bearings, is known as cavitation or gaseous cavitation.
Schematic of a journal bearing.
In some cases involving highfrequency varying loads, as in internal combustion engines, the pressure might drop below the oil vapor pressure (which is lower than the ambient pressure). In this case, bubbles are formed by rapid evaporation/boiling of the oil. This phenomenon is known as vapor cavitation.
Being able to predict the onset and extent of cavitation in the lubrication layer is important for two main reasons:
The pressure of the lubricant can be computed from the Reynolds equation. This equation is not solved in the threedimensional fluid domain between the bearing and the shaft, but instead on a twodimensional surface within the gap.
Therefore, the clearance between the shaft and the bearing is not represented in the geometry, where the two parts are in contact. This “lower dimension” approach drastically reduces both the CPU usage and memory load during the model resolution. In the COMSOL Multiphysics simulation software, the Reynolds equation has been modified to account for gaseous cavitation effects.
This tutorial from our Model Gallery predicts the onset and extent of cavitation in the lubrication layer of a journal bearing. The color represents the mass fraction of the lubricant in the cavitation region. The white contour shows the outline of the region of cavitation. (This model requires COMSOL Multiphysics and the CFD Module.)
At the COMSOL Conference 2013 Rotterdam, Rob Eling from Mitsubishi Turbocharger & Engine Europe presented his work where he used COMSOL Multiphysics and the thin film physics interface to evaluate the risk of rotor instability caused by the interaction between the rotor and the bearings in a turbocharger.
Image Credit: R. Eling, Mitsubishi Turbocharger & Engine Europe, Almere, The Netherlands.
This highly nonlinear analysis involves two main components:
The coupled analysis of this problem enables the prediction of the following critical performance criteria:
Because of the complexity of the model, the problem was tackled in three steps.
The first step involved performing an analysis of the rotor dynamics (i.e., the structural mechanics problem without considering the bearings):
Image Credit: R. Eling, Mitsubishi Turbocharger & Engine Europe, Almere, The Netherlands.
In the second step, he performed an analysis of the hydrodynamic bearings:
Image Credit: R. Eling, Mitsubishi Turbocharger & Engine Europe, Almere, The Netherlands.
Finally, he ran an analysis of the coupled rotorbearing system:
Image Credit: R. Eling, Mitsubishi Turbocharger & Engine Europe, Almere, The Netherlands.
Eling ran simulations over the full operating range and showed the presence of many interesting — and potentially dangerous! — selfinduced vibrations of the system due to the fluidstructure interactions between the rotor and the bearings.
For more information on the research shown here, please refer to Eling’s paper “Dynamics of Rotors on Hydrodynamic Bearings“, as presented at the COMSOL Conference 2013 in Rotterdam. If you have any questions, please contact your local technical support team.
]]>
The COMSOL Multiphysics software’s multiphase flow capabilities cover a wide range of applications, including:
These application areas are covered by six different physics interfaces, and it is not always trivial to determine which physics interface is better suited to solve your particular application.
Screenshot of the model tree displaying the six interfaces.
In this blog post, we describe these six multiphase flow physics interfaces to make it easier for you to choose. Very specific application areas, such as twophase flow in porous media or cavitation problems, will be the object of future blog entries.
The six multiphase flow models can be split into two main categories, which we will refer to as the interface tracking methods and the disperse methods.
The interface tracking methods model the flow of two different immiscible fluids separated by a clearly defined interface. These methods are typically used to model bubble or droplet formation, sloshing tanks, or separated oil/water/gas flow. In the below example by the Philips® FluidFocus team, the meniscus between two immiscible liquids is used as an optical lens.
Image credit: Philips.
The shape of the meniscus in this device is controlled by changing the voltage applied to the conducting liquid, thus changing the focal point of the lens. The lens is then integrated within a miniature variablefocus camera. Because the exact location of the interface is of interest here, the FluidFocus team used an interface tracking method in their numerical model.
A tutorial showing how to reproduce this model can be found in our Model Gallery.
While the interface tracking methods are accurate and provide a clear picture of the flow field (velocity, pressure, and surface tension force), they are not always practical due to their high computational cost. Thus, the interface tracking methods are generally better suited to microfluidics problems in which only a few droplets or a few bubbles are tracked.
Largerscale simulations involving a greater number of bubbles, droplets, or solid particles require computationally cheaper methods. Cue: the disperse methods.
This second category of methods does not explicitly track the position of the interface between the two fluids, but instead tracks the volume fraction of each phase, thus lowering the computational load. A circulated fluidized bed, which is a very common apparatus in the food, pharmaceutical, and chemical processing industries, can be modeled using a disperse method.
In this example, the dispersed phase, consisting of solid spherical particles, is fluidized by air and transported upwards through a vertical riser:
Tracking every single solid particle would not be computationally practical here. Instead, we compute the volume fraction of solid particles. The disperse methods are typically used to model particleladen flow, bubbly flow, and mixtures.
In the next few sections of this blog post, I will discuss and compare the different tracking and homogeneous methods.
The disperse methods include the following:
The EulerEuler model simulates the flow of two continuous and fully interpenetrating incompressible phases. Typical applications are fluidized beds (solid particles in gas), sedimentation (solid particles in liquid), or transport of liquid droplets or bubbles in a liquid.
This model requires the resolution of two sets of NavierStokes equations, one for each phase, in order to calculate the velocity field for each phase. The volume fraction of the dispersed phase is tracked with an additional transport equation.
The EulerEuler model is the correct twophase flow method to model the fluidized bed that I presented earlier. The model relies on the assumption that the dispersed particles, bubbles, or droplets are much smaller than the grid size.
The EulerEuler model is the most versatile of the three disperse models, but it comes at a high computational cost. The model solves for two sets of the NavierStokes equations, instead of one, which is the case for all other models presented here. Both the bubbly flow and mixture models are simplifications of the EulerEuler model and rely on additional assumptions.
The bubbly flow model is used to predict the flow of liquids with dispersed bubbles. It relies on the following assumptions:
In this model of an airlift loop reactor, air bubbles are injected at the bottom of a reactor filled with water:
The bubbly model solves one set of NavierStokes equations for the flow momentum, a mixtureaveraged continuity equation, and a transport equation for the gas phase. Although this model does not track individual bubbles, the distribution of the number density (i.e., the number of bubbles per unit volume) can still be recovered. This can be useful when simulating chemical reactions in the mixture.
The mixture model is used to simulate liquids or gases containing a dispersed phase. The dispersed phase can be bubbles, liquid droplets, or solid particles, which are assumed to always travel with their terminal velocity. While this model can be used for bubbles, it is recommended to use the bubbly flow model instead for gas bubbles in a liquid.
The mixture model solves one set of NavierStokes equations for the momentum of the mixture, a mixtureaveraged continuity equation, and a transport equation for the volume fraction of the dispersed phase. Like the bubbly model, the mixture model can also recover the number of bubbles, droplets, or dispersed particles per unit volume.
The mixture model relies on the following assumptions:
This tutorial models the flow of a dense suspension consisting of light, solid particles in a liquid placed between two concentric cylinders.
Particle concentration.
I have summarized the disperse models for you in a table:
EulerEuler Model  Bubbly Flow Model  Mixture Model  

Valid for these continuous phases: 



Valid for these dispersed phases: 



Assumptions: 



Equations solved for (laminar flow): 



Available turbulence models: 



These three multiphase flow models require the CFD Module. The mixture model for rotating machinery problems also requires the Mixer Module. More details on the required COMSOL products can be found in our specification chart.
The interface tracking methods include:
All these methods very accurately track the position of the interface between the two immiscible fluids. They account for differences in density and viscosity of the two fluids, as well as effects of surface tension and gravity.
With the level set and phase field methods, the interface is tracked using an auxiliary function, or color function, on a fixed mesh.
The NavierStokes equations and the continuity equation are solved for the conservation of momentum and mass, respectively. The color function, and therefore the interface position, is tracked by solving additional transport equations (one additional equation for the level set method and two additional transport equations for the phase field method). This color function varies between a low value (0 and 1 for the level set and phase field methods, respectively) in one phase and high value of 1 in the second phase.
The interface is diffuse and centered on the center value of these functions (0.5 and 0 for the level set and phase field methods, respectively). The material properties of both phases such as the density and viscosity are scaled according to the color function.
This plot shows the filling of a capillary channel using the level set or phase field method. The higher value of the color function (red region) shows the location of the fluid phase, while the lower value (blue region) represents the gas phase. The two phases are separated by a diffuse interface that is not aligned with the fixed mesh.
The phase field method, which is physically motivated, is generally more numerically stable than the level set method and is compatible with fluidstructure interactions. The level set method, however, usually represents surface tension slightly more accurately than the phase field method.
Unlike the level set and phase field methods, which are solved on a fixed mesh, the twophase flow moving mesh method tracks the interface position with a moving mesh using the ALE method.
Here, the same capillary filling simulation is implemented using the moving mesh method. This time, the interface is sharp and it follows the boundary between the fluid and the gas domain. Because the position of the interface is given by the boundary between the two meshes, it does not require any additional transport equations. Only one set of NavierStokes equations is solved on each mesh.
Since physical interfaces are usually much thinner than practical mesh resolutions, the twophase flow moving mesh technique offers the most accurate representation of the interface. This method also accounts for mass transport across the interface, which is very difficult to implement using the two other interface tracking methods. Finally, the sharp interface also means that different physics can be solved in the domains on either side of the interface.
The main drawback of the moving mesh methods is the fact that the mesh must deform continuously, which means that problems involving topological changes cannot be solved. This drastically limits its applications. Problems such as droplet breakup or the transition from jetting to dripping of a liquid jet cannot be modeled using the moving mesh method and require the level set or phase field method. This jet instability simulation shows the breakup of a jet into droplets over time using the level set method.
Liquid regions (shown in black).
Tutorials for the droplet breakup and jet instability simulations are available in the Model Library and our online Model Gallery.
As with the homogeneous models above, I have put the interfacing tracking methods in a table for an easy overview:
Level Set  Phase Field  Moving Mesh  

Applicability: 
Does not support topological changes 

Accurate representation of the interface:  Better  Good  Best 
Speed and convergence:  Good  Better  Best 
Equations solved for: 



Available turbulence models: 



Required COMSOL products for laminar flow:  
Required COMSOL products for turbulent flow: 
In this blog post, we compared six different twophase flow methods. The COMSOL Multiphysics simulation software does offer additional multiphase flow methods, including twophase flow methods in porous media or cavitation in thin films, such as journal bearings. These topics will be the object of future blog entries.
If you have any multiphase flow modeling questions, feel free to contact our Technical Support team. If you are not yet a COMSOL Multiphysics user and would like to learn more about our software, please contact us via this form — we’d love to connect with you.
PHILIPS is a registered trademark of Koninklijke Philips N.V.
]]>
The dielectrophoretic effect will show up in both DC and AC fields. Let’s first look at the DC case.
Consider a dielectric particle immersed in a fluid. Furthermore, assume that there is an external static (DC) electric field applied to the fluidparticle system. The particle will in this case always be pulled from a region of weak electric field to a region of strong electric field, provided the permittivity of the particle is higher than that of the surrounding fluid. If the permittivity of the particle is lower than the surrounding fluid, then the opposite is true; the particle is drawn to a region of weak electric field. These effects are known as positive dielectrophoresis (pDEP) and negative dielectrophoresis (nDEP), respectively.
The pictures below illustrate these two cases with a few important quantities visualized:
An illustration of positive dielectrophoresis (pDEP), where the particle permittivity is higher than that of the surrounding fluid \epsilon_p > \epsilon_f. At the surface of the particle, the induced surface charge is colorcoded with red representing a positive charge and green a negative charge. Yellow represents a neutral charge.
An illustration of negative dielectrophoresis (nDEP), where the particle permittivity is lower than that of the surrounding fluid \epsilon_p < \epsilon_f.
The Maxwell stress tensor represents the local force field on the surface of the particle. For this stress tensor to be representative of what forces are acting on the particle, the fluid needs to be “simple” in that it shouldn’t behave too weirdly either mechanically or electrically. Assuming the fluid is simple, we can see from the above illustrations that the net force on the particle appears to be in opposite directions between the two cases of pDEP and nDEP. Integrating the surface forces will indeed show that this is the case.
It turns out that if we shrink the particle and look at the infinitesimal case of a very small particle acting like a dipole in a fluid, then the net force is a function of the gradient of the square of the electric field.
Why is the net force behaving like this? To understand this, let’s look at what happens at a point on the surface of the particle. At such a point, the magnitude of the electric surface force density, f, is a function of charge times electric field:
(1)
where \rho is the induced polarization charges. (Let’s ignore for the moment that some quantities are vectors and make a purely phenomenological argument by just looking at magnitudes and proportionality.)
The induced polarization charges are proportional to the electric field:
(2)
Combining these two, we get:
(3)
But this is just the local surface force density at one point at the surface. In order to get a net force from all these surface force contributions at the various points on the surface, there needs to be a difference in force magnitude between one side of the particle and the other. This is why the net force, \bf{F}, is proportional to the gradient of the square of the electric field norm:
(4)
In the above derivation, we have taken some shortcuts. For example, what is the permittivity in this relationship? Is it that of the particle or that of the fluid or maybe the difference of the two? What about the shape of the particle? Is there a shape factor?
Let’s now address some of these questions.
In a more stringent derivation, we instead use the vectorvalued relationship for the force on an electric dipole:
(5)
where \bf{P} is the electric dipole moment of the particle.
To get the force for different particles, we simply insert various expressions for the electric dipole moment. In this expression, we can also see that if the electric field is uniform, we get no force (since the particle is small, its dipole moment is considered a constant). For a spherical dielectric particle with a (small) radius r_p in an electric field, the dipole moment is:
(6)
where k is a parameter that depends on the the permittivity of the particle and the surrounding fluid. The factor 4 \pi r_p^3 can be seen as a shape factor.
Combining these, we get:
(7)
This again shows the dependency on the gradient of the square of the magnitude of the electric field.
If the electric field is timevarying (AC), the situation is a bit more complicated. Let’s also assume that there are losses that are represented by an electric conductivity, \sigma. The dielectrophoretic net force, \bf{F}, on a spherical particle turns out to be:
(8)
where
(9)
and
(10)
is the complexvalued permittivity. The subscripts p and f represent the particle and the fluid, respectively. The radius of the particle is r_p and \bf{E}_{\textrm{rms}} is the rootmeansquare of the electric field. The frequency of the AC field is \nu.
From this expression, we can get the force for the electrostatic case by setting \sigma = 0. (We cannot take the limit when the frequency goes to zero, since the conductivity has no meaning in electrostatics.)
In the expression for the DEP force, we can see that indeed the difference in permittivity between the fluid and the particle plays an important role. If the sign of this difference switches, then the force direction is flipped. The factor k involving the difference and sum of permittivity values is known as the complex ClausiusMossotti function and you can read more about it here. This function encodes the frequency dependency of the DEP force.
If the particles are not spherical but, say, ellipsoidal, then you use another proportionality factor. There are also wellknown DEP force expressions for the case where the particle has one or more thin outer shells with different permittivity values, such as in the case of biological cells. The simulation app presented below includes the permittivity of the cell membrane, which is represented as a shell.
The settings window for the effective DEP permittivity of a dielectric shell.
There may be other forces acting on the particles, such as fluid drag force, gravitation, Brownian motion force, and electrostatic force. The simulation app shown below includes force contributions from drag, Brownian motion, and DEP. In the Particle Tracing Module, a range of possible particle forces are available as builtin options and we don’t need to be bothered with typing in lengthy force expressions. The figure below shows the available forces in the Particle Tracing for Fluid Flow interface.
The different particle force options in the Particle Tracing for Fluid Flow interface.
Medical analysis and diagnostics on smartphones is about to undergo rapid growth. We can imagine that, in the future, a smartphone can work in conjunction with a piece of hardware that can sample and analyze blood.
Let’s envision a case where this type of analysis can be divided into three steps:
The COMSOL Multiphysics simulation app focuses on Step 2 of the overall analysis process above. By exploiting the fact that blood platelets are the smallest cells in blood and have different permittivity and conductivity than red blood cells, it is possible to use DEP for sizebased fractionation of blood; in other words, to separate red blood cells from platelets.
Red blood cells are the most common type of blood cell and the vertebrate organism’s principal means of delivering oxygen (O_{2}) to the body tissues via the blood flow through the circulatory system. Platelets, also called thrombocytes, are blood cells whose function is to stop bleeding.
Using the Application Builder, we created an app that demonstrates the continuous separation of platelets from red blood cells (RBCs) using the Dielectrophoretic Force feature available in the Particle Tracing for Fluid Flow interface. (The app also requires one of the following: the CFD Module, Microfluidics Module, or Subsurface Flow Module and either the MEMS Module or AC/DC Module.)
The app is based on a labonachip (LOC) device described in detail in a paper by N. Piacentini et al., “Separation of platelets from other blood cells in continuousflow by dielectrophoresis fieldflowfractionation”, from Biomicrofluidics, vol. 5, 034122, 2011.
The device consists of two inlets, two outlets, and a separation region. In the separation region, there is an arrangement of electrodes of alternating polarity that controls the particle trajectories. The electrodes create the nonuniform electric field needed for utilizing the dielectrophoretic effect. The figure below shows the geometry of the model.
The geometry used in the particle separation simulation app.
The inlet velocity for the lower inlet is significantly higher (853 μm/s) than the upper inlet (154 μm/s) in order to focus all the injected particles toward the upper outlet.
The app is built on a model that uses the following physics interfaces:
Three studies are used in the underlying model:
You can download the model that the app was based on here.
To create the simulation app, we used the Application Builder, which is included in COMSOL Multiphysics® version 5.0 for the Windows® operating system.
The figure below shows the app as it looks like when first started. In this case, we have connected to a COMSOL Server™ installation in order to run the COMSOL Multiphysics app in a standard web browser.
A biomedical simulation app running in a standard web browser.
The app lets the user enter quantities, such as the frequency of the electric field and the applied voltage. The results include a scalar value for the fraction of red blood cells separated. In addition, three different visualizations are available in a tabbed window: the blood cell and platelet distribution, the electric potential, and the velocity field for the fluid flow.
The figures below show visualizations of the electric potential and the flow field.
Screenshot showing the instantaneous electric potential in the microfluidic channel.
Screenshot displaying the magnitude of the fluid velocity.
The app has three different solving options for computing just the flow field, computing just the separation using the existing flow field, or combining the two. A warning message is shown if there is not a clean separation.
Increasing the applied voltage will increase the magnitude of the DEP force. If the separation efficiency isn’t high enough, we can increase the voltage and click on the Compute All button, since in this case, both the fields and particle trajectories need to be recomputed. We can control the value of the ClausiusMossotti function of the DEP force expression by changing the frequency. It turns out that at the specified frequency of 100 kHz, only red blood cells will exit the lower outlet.
The fluid permittivity is in this case higher than that of the particles and both the platelets and the red blood cells experience a negative DEP force, but with different magnitude. To get a successful overall design, we need to balance the DEP forces relative to the forces from fluid drag and Brownian motion. The figure below shows a simulation with input parameters that result in a 100% success in separating out the red blood cells through the lower outlet.
Successful separation of red blood cells.
To learn more about dielectrophoresis and its applications, click on one of the links listed below. Included in the list is a link to a video on the Application Builder, which also shows you how to deploy applications with COMSOL Server™.
Windows is either a registered trademark or trademark of Microsoft Corporation in the United States and/or other countries.
]]>
Mm… Farm fresh tomatoes still warm from the sun… How about farm fresh tomatoes that were then cooled off in dirty water and shipped off to your local grocery store with bacteria inside of them?
Image of a tomato created by A. Warning and A.K. Datta and taken from their poster.
Hydrocooling is a form of precooling, which is a common practice at the harvesting site. Precooling is designed to keep the produce fresh longer; without cooling produce off soon after harvest, it will continue to age and start to degrade. The hydrocooling process, specifically, involves putting freshly picked and hotfromthesun batches of produce into containers of cold water. The water will then cool off the fruit or vegetables. How long that takes naturally depends on the size of the produce, ranging anywhere from a few minutes to a full hour.
But, it turns out, a method meant to improve the quality of our produce might actually introduce new bacteria.
At this year’s COMSOL Conference in Boston, I met Alexander Warning of Cornell University during the poster session. He was standing by the poster he had created with Ashim K. Datta (also of Cornell University) on fresh produce safety during hydrocooling.
He explained to me that the water used during the hydrocooling process might be contaminated. For example, a farmer might touch soil containing manure for fertilization, pick a tomato, then dump it in the water with the rest of the batch. This then becomes a sort of bath tub of bacteria (my words, not his).
According to Warning, when you place warm produce in cold water, a negative pressure differential is established because of the condensation of water vapor inside the produce. Next, a vacuum is formed that may suck in water through an opening.
What about the tomato’s protective skin? The skin does a good job keeping contaminants at bay when the tomato is still attached to the plant, but when it’s removed from the stem, the tomato is no longer completely sealed.
A tomato undergoing the hydrocooling process. Image created by A. Warning and A.K. Datta and taken from their poster.
Warning and Datta decided to create an engineering model to test how contaminated water might affect tomatoes during the hydrocooling process.
To begin, the researchers scanned a tomato wedge using magnetic resonance imaging (MRI). They used these images to create a geometry from symmetry for their porous media model. Then, they ran simulations to analyze the water infiltration in the tomato at different times and water temperatures.
The researchers used MRI scans of the tomato wedge to create the geometry. Image created by A. Warning and A.K. Datta and taken from their poster.
The tomato starts out at 35°C and is placed in water that is 5°C. After 15 minutes, the tomato has cooled down significantly on the outside, but is still relatively warm at the center (called the core and placenta). After 30 minutes, the tomato is roughly 15°C in the placenta and around as cold as the water closer to the skin (the cuticle and vascular bundles).
Analogously, the longer the tomato is sitting in the water, the more water seeps in through the stem scar, and the higher the concentration of bacteria. (View all of the results in the presentation and poster.)
Surface plots of the tomato at three different times. A) Spatial variation in tomato wedge of temperature. B) Pore water saturation. C) Gauge pressure. D) Bacteria concentration. Image created by A. Warning and A.K. Datta and taken from their poster.
To combat the contamination issue, water used for hydrocooling should first of all be of drinking quality. If we can’t drink it, don’t bathe our produce in it. Another recommendation is typically to add some form of sanitizer to the water to keep microorganisms from spreading. One common sanitizer, which Warning mentioned during his live presentation at the conference, is chlorine.
When using chlorine, it’s important to control the pH and turbidity levels in the water. There are varying regulations for how much free chlorine can be used depending on whether the farm is organic or conventional. Intuitively, higher levels of chlorine can be used for produce grown conventionally than that grown according to organic standards. (Learn more about postharvest chlorination here.)
After talking to Warning at the poster session and hearing his presentation the following day, I couldn’t stop thinking about their research. While most people might cut the stem scars out anyway because of their indelicate texture, I used to not bother with it. I don’t know for sure exactly how the tomatoes I buy were precooled, but I’m no longer taking any chances…
Because I learned at the #COMSOLconf14 that the bacteria is right around where the stem is attached to the tomato pic.twitter.com/6J8p9E3cxk
— Fanny Littmarck (@fannylittmarck) October 18, 2014
As I’m writing this, it’s Friday and we’ve had a long and very productive week. Like me, you’re probably wondering what type of IPA you will order with your nachos later. We are quite lucky to have such a wide selection of beers available in the U.S., thanks to the recent rise of craft beers. But rather than going to our local micro brewery, we could take it a step further and attempt to make our own beer.
Here, we give you a crash course on beer brewing and explain how you can improve the brewing process with CFD simulations. The main purpose is to find out how to cool down five gallons of boiling water as quickly as possible. But, first: Some context.
Making your own beer is relatively straightforward. If you can make tea, you can probably make beer.
Here’s my list of seven steps to brewing beer:
That’s the standard procedure. But, why settle for standard when we can improve the process? Most of the above steps can be optimized with simulations. Let’s start with the most crucial one — Step 3: Cooling the wort.
In Step 3, the boiling wort needs to be cooled down very quickly for several reasons.
First of all, it needs to be cool enough for the yeast to survive. Second, cooling it limits the production of sulfur compounds and other contaminants during the cooling process. These compounds are associated with offflavors in the finished beer. Finally, some proteins need to be thermally shocked in order for them to precipitate.
We won’t go into these reasons in detail, as we prefer to focus on the engineering aspect of the process. The size of a typical home brew batch is between five and ten gallons. The problem of cooling down the liquid quickly becomes even harder in an industrial setup, where the amount of wort to be cooled down is massive.
I’ve seen on YouTube that you might try throwing ice in the boiling kettle. I would not recommend this as it might introduce contaminants in the beer and will dilute it.
How about placing the boiling kettle in an ice bath in our kitchen sink? While this is the cheapest way, it is not the most efficient. I will let you find that out on your own using our Conjugate Heat Transfer interface (included in the CFD Module and the Heat Transfer Module.)
The cooling of the kettle in an ice bath can modeled very similarly to the Free Convection in a Water Glass model tutorial, found in our Model Gallery.
Free convection in a glass of water.
This model treats the free convection and heat transfer of a glass of cold water heated to room temperature. Initially, the glass and the water are at 5°C and are then put on a table in a room that’s 25°C warm. The boiling kettle cooling problem could be modeled the same way by setting the initial wort temperature to 100°C and the external wall temperature to 0°C.
Alternatively, we could use a wort chiller. Basic wort chillers consist of a long helicoidal pipe that you immerse in the kettle at the end of the boiling process. You will then run cold water from your sink into the pipe to cool down the wort.
Sketch of a wort chiller.
As you can deduce by the shape, the modeling procedure for this wort chiller is identical to the one found in our geothermal heating problem model of a pond loop:
In this example, a pond is used as a thermal reservoir and fluid circulates underwater through polyethylene piping in a closed system. The model finds out how much heat is transferred from the pond to the working fluid in the pipes. To this end, the NonIsothermal Pipe Flow interface sets up and solves the equations for the temperature and fluid flow in the pipe system.
In the pipe flow physics interface, the pipes are represented by 1D lines, rather than actual 3D pipes, which drastically reduces the computational load of such a model. The following snapshot shows a possible design for the wort chiller, immersed in the boiling kettle, and the corresponding temperature field within the pipes:
We could also combine method 2 and 3 for faster results, i.e., use a wort chiller while the kettle is in an ice bath.
Another option is to use a flat plate or counterflow heat exchanger. A heat exchanger is a device that transfers heat from one fluid to another. Water, initially at a low temperature and used as the coolant, is being heated up while the wort is being cooled down. The following picture shows a flat plate heat exchanger.
Flat plate heat exchanger used to cool down beer at a local “brewyourownbeer” establishment. (You might recognize it from a similar picture on our Instagram account, COMSOL_.)
These types of heat exchangers are very popular due to their compact size. Many brewers also use counterflow heat exchangers.
You can model these devices by following the stepbystep instructions in the ShellandTube Heat Exchanger model, which shows the basic principles of setting up a heat exchanger model. In the model, two separated fluids at different temperatures flow through the heat exchanger, one through the tubes (tube side) and the other through the shell around the tubes (shell side).
Using a heat exchanger is not only the fastest way to cool down your wort, it is also the most efficient. Indeed, most of the heat taken form the wort is transferred to the water. This water can then be reused to steep the next batch of malted barley. This way, no energy is wasted!
Here, we have discussed conjugate heat transfer problems, a pipe flow model, and a heat exchanger model. I encourage you to try modeling these different cooling strategies in COMSOL Multiphysics and find out what works best. You can set up and solve these models using the CFD Module, Heat Transfer Module, and Pipe Flow Module.
After all this modeling, your beer must be pretty tasty and your friends are probably asking for more. It’s time to scale up and use a larger mixer tank, so that you don’t need to stir it manually anymore. Mixing tanks can be modeled using the Mixer Module, an addon to the CFD Module that allows you to analyze fluid mixers and stirred reactors.
Model of a turbulent mixer with a threebladed impeller. The model also considers the shape of the free surface.
If you have any questions about the models that I’ve presented here, contact our Technical Support team. If you are not yet a COMSOL Multiphysics user and would like to learn more about our software, please contact us via this form — we’d love to connect with you.
]]>