CFD Review  
Serving the CFD Community with News, Articles, and Discussion
 
CFD Review

User Preferences
Site Sponsorship
Headline Feeds
Mobile Edition
Privacy Policy
Terms of Service
twitter

Submit a CFD Story

Site Sponsors
Siemens PLM Software
Pointwise: Reliable CFD meshing
Software Cradle

Tell a Friend
Help this site to grow by sending a friend an invitation to visit this site.

CFD News by Email
Did you know that you can get today's CFD Review headlines mailed to your inbox? Just log in and select Email Headlines Each Night on your User Preferences page.

 
CFD Simulation of Nuclear Event
Posted Wed April 03, 2002 @06:25PM
Print version Email story Tweet story
News In the nuclear power industry, much effort is spent analyzing potential plant accidents. While the likelihood that any of these events would ever happen is extremely small, the analyses are an important component of ongoing research in the nuclear industry. These studies help engineers further reduce the risk of plant accidents. One way that engineers around the world participate in accident analysis is through international standard problems (ISP’s). An organizing body defines a standard problem, and researchers from various countries independently work to solve it. In one recent study, sponsored by the Committee on the Safety of Nuclear Installations (CSNI) within the Organization of Economic Cooperation and Development (OECD), the problem consisted of using computational fluid dynamics (CFD) to predict boron mixing in the downcomer of a pressurized water reactor (PWR).

Sponsor CFD Review

In a pressurized water reactor, soluble boric acid is added to the primary system cooling water as a means of reactivity control. Boric acid is a strong absorber of neutrons. The borated water is pumped through the reactor to carry heat from the fuel to steam generators. The organizers of this ISP postulated an accident initiated by a small leak in the reactor coolant system. The flow through the system stops as the coolant inventory is lost. During this time, a volume of pure, or unborated, water accumulates in the system at the heat exchanger used for steam generation. After some time, a significant slug of unborated water is assumed to form. Reinitiation of the flow in the system causes this slug of unborated water to travel back toward the reactor core. If the unborated slug does not mix sufficiently with the existing borated water in the reactor vessel, a reactivity excursion could occur with a potential for fuel damage.

Christopher Boyd of the U.S. Nuclear Regulatory Commission (NRC) was one of fifteen individuals from 10 countries who participated in this ISP. The goal was to predict the mixing of a volume of pure water as it is pumped into a reactor vessel filled with borated water. "This is an important issue but it's also important to understand that we are studying hypothetical scenarios based upon the occurance of a series of unlikely events," says Boyd. "Full scale testing of such events would be extremely costly and potentially dangerous. CFD provides a great way to take a look at these phenomona at a minimal cost and with no risk."

"CFD is a good tool for simulating the mixing of fluids, such as the borated and unborated water we studied in this ISP," says Boyd. A CFD simulation provides predictions throughout the solution domain which gives the user access to a wealth of information. More importantly, a researcher may change the geometry of the system or significant input parameters to determine the sensitivity of the solution to these assumptions. Detailed parametric studies can significantly enhance a researchers understanding of the phenomena governing a particular issue.

Boyd used the FLUENT CFD software from Fluent Inc. of Lebanon, NH to simulate this accident scenario. To do so, he needed a computational mesh of high quality, especially in regions of complex geometry. Pipe junctions, present in the ISP geometry definition, are one example of complex geometry that has traditionally been difficult to mesh uniformly. Without a mesh of good quality, it is difficult to achieve accurate computational results. Boyd used the paving algorithm and the cooper tool in GAMBIT, the FLUENT preprocessor, to generate a fairly uniform hexagonal mesh in those irregular areas with a minimal amount of effort. Boyd's CFD results showed details consistent with experimental observation that were missed by other researchers' predictions of the same problem and Boyd attributes this success to the quality of the mesh.

Difficult to model

The reactor geometry includes several pipe junctions, which make it difficult to create a high-quality mesh. "Much of the geometry was regular, such as the inlet and outlet pipes and the regions away from the pipe intersections. These areas could be meshed with a structured hexagonal mesh, which gives the most accurate results," explains Boyd. "But it has traditionally been difficult to create a uniform mesh in the pipe junctions, of which this model had many." Creating a structured hexagonal mesh in these regions is very time consuming and does not produce an ideal mesh. Another common approach is to use traditional unstructured meshing tools to create tetrahedral elements in these areas. This is an easy approach for the user but the tetrahedral elements are not considered ideal from an accuracy point of view.

Boyd used the FLUENT code and notes that the advanced meshing tools within its preprocessor, GAMBIT, are ideally suited to meshing this geometry. "Tools such as the 2D paving algorithm and the 3D cooper tool can be used to create a high quality hexagonal mesh in the pipe to vessel junction regions," Boyd says. FLUENT is also well suited to this ISP because it is a commercially available, general-purpose CFD code capable of solving a wide variety of fluid flow and heat transfer problems. "The code solves the Reynolds averaged Navier-Stokes equation set on a finite volume mesh," Boyd adds. "These equations describe the continuity of mass, momentum, and energy in a continuous fluid. Turbulence modeling accounts for the turbulent diffusion of momentum and energy. The FLUENT code includes a variety of turbulence modeling options."

Boyd was given a CAD model of the University of Maryland's experimental loop facility. Although it was in a format (Pro/ENGINEER) that he could import into GAMBIT, he opted to recreate the geometry himself. "The CAD model had too many details—small features such as gaskets and bolt holes, for example—that were not significant to the CFD analysis. I opted instead to recreate the geometry from scratch using GAMBIT," Boyd says. GAMBIT provides top-down geometry construction using 3D primitives. It enabled Boyd to create the geometry quickly, without forcing him to deal with the complexity of a full-fledged production drawing. The loop facility is basically a very simple structure and while Boyd left out some details, he made sure to include those that might affect mixing within the downcomer. For example, he included a small, inward-facing step change in downcomer width.

Tools simplify meshing

After laying out the geometry in GAMBIT, the next step was to develop the computational mesh. Boyd first created a uniform 3D structured mesh in regions surrounding the pipe junctions. Next, he needed to make transitions between these areas. Using GAMBIT features, a fairly uniform hexagonal mesh was quickly created in the pipe junctions which smoothly connected the surrounding structured mesh regions.

One of the tools he used was the software's paving algorithm, which can create a 2D surface mesh of nearly square elements given an existing mesh at the boundaries. "The paving tool let me automatically create smooth transitions between regions with different mesh topology, such as those on an inlet pipe and on the reactor vessel," explains Boyd. "With a structured mesh, you would have to compromise and give both regions the same mesh structure if you wanted to connect them. That prevents you from optimizing the structures separately. But with GAMBIT, I could optimize the mesh in each region independently, and then use the paving tool to make the transition between them with a fairly uniform mesh. This process produces a high quality, uniform surface mesh with a minimal user effort."

Next Boyd used GAMBIT's cooper tool to create a 3D volume mesh from the 2D surface mesh. This tool sweeps the mesh patterns created on a surface through a 3D volume. Boyd simply selected the volume to be meshed, and the software projected the surface mesh across the 3D volume. "This saved a lot of time for the cylinder to cylinder intersections," Boyd says. "GAMBIT's logic is very good. GAMBIT determines the projected surfaces and projection direction automatically in most cases. By using the cooper tool across the pipe intersections, I was able to obtain a good quality hexagonal mesh with minimal effort."

After creating an initial mesh and specifying boundary conditions, Boyd ran the CFD simulation on an eight-processor COMPAQ Alpha computer. He used FLUENT's segregated transient solver and allowed the solution to fully converge after each time step. Initial results were available one week after Boyd starting work on the problem. After getting the preliminary results, Boyd refined the model by performing a grid independence and time step study. A final grid was created and further optimized using the solution-based adaption feature in FLUENT. Solution adaption takes each cell in a user defined adaption region and divideds it into multiple, smaller cells. This study led to the use of a final mesh with 434,589 cells that had reduced cell sizes in regions requiring additional solution detail. The time step study showed that the initial model that solved the problem with time increments of ½ second was not completely time accurate. It was demonstrated that using 1/20-second increments provided the desired time step convergence.

In this ISP, the CFD results obtained by different researchers are compared with experimental data from two types of tests. One test, performed at the University of Maryland's integral 2 x 4 loop facility simulated the BORON mixing phenomena using hot and cold water. Inlet flow rates and temperatures at selected points in the domain were measured during several tests. In another test, a transparent replica of the University of Maryland's loop facility was constructed to allow for quantitative optical concentration and velocity measurements. This facility used a dye marker to represent the unborated slug. This ISP was conducted as a blind test, which means that Boyd and the other researchers conducting the CFD analyses were not given the experimental results until after their CFD predictions were submitted.

Predictions based on Boyd's CFD analysis compared very well with temperature data collected experimentally, coming to within the level of experimental uncertainty. The accuracy of his model was actually more evident in the prediction of flow patterns, however. Similar to the data recorded by the optical facility, Boyd's CFD results showed the slug entering the downcomer, and forming a stagnation region on the inner cylindrical surface. A wall jet spread out in all directions, and when it reached the step change in the downcomer width, it jumped from the inner to the outer wall. "Some other researchers' simulations showed the wall jet continuing to hug the inner wall after passing the step change. The flow pattern predicted by FLUENT is consistent with what the optical test data showed also," Boyd says.

This ISP showed that CFD analysis is capable of simulating boron mixing in a nuclear reactor, but only when the analysis is based on a valid CFD model. As this work illustrates, an optimized finite volume mesh is a key requirement for achieving a valid model. By using the tools available in FLUENT's preprocessor, Boyd was able to quickly create a high quality 3D mesh even in traditionally difficult areas, and then optimize the mesh in FLUENT to accurately predict real-world results. Lessons learned from this experience will allow the NRC to analyze boron mixing in actual nuclear reactors with greater confidence.

fig 1
Contours of velocity magnitude on the inner surface of the downcomer show the spread of the wall jet that entered through the inlet pipe.

fig 2
Contours of temperature on a vertical slice in the downcomer show thermal mixing prior to entry into the reactor.

fig 3
Average temperature at the downcomer exit from the ISP measurements and CFD predictions.

[ Post Comment ]

CFD for Combustion and Radiation Web Demonstration | Jobs Database News  >

 

 
CFD Review Login
User name:

Password:

Create an Account

Related Links
  • Fluent
  • More on Fluent
  • Also by nwyman
  • This discussion has been archived. No new comments can be posted.

    Just to have it is enough. All content except comments
    ©2017, Viable Computing.

    [ home | submit story | search | polls | faq | preferences | privacy | terms of service | rss  ]