Science topic

# Turbulence Modeling - Science topic

Explore the latest questions and answers in Turbulence Modeling, and find Turbulence Modeling experts.
Questions related to Turbulence Modeling
Question
I have a specific case about internal pipe flow with constant heat flux. Although the inlet boundary condition is laminar, the flow is a passing transition (a significant part of the tube) and turbulent regime along the tube (because of the change of thermophysical properties depending on implied heat). SST models with intermittency term (For fully laminar flow, γ = 0 and the model reverts to a laminar solver. When γ = 1, the flow is fully turbulent.) can catch laminar/transitional and turbulent flow regimes. These models were designed for turbulent inlet boundary conditions (models solve intermittency term, so it needs extra boundary conditions such as turbulent intensity). Can Transitional SST Models be used for laminar inlet / turbulent outlet boundary conditions? If so, what is the approach?
Regards,
EB
Dear Dr. Youyun Shang thank you for your answer. I tried "enhance wall" in many different ways but couldn't achieve it yet. The transition model (by Menter) predicting transition was formulated for external flows. This model actually should be adapted to flow in pipes. J. P. Abraham conducted some studies in this context and presented modifications to the original transition model. Although I have adjusted my model considering these modifications, I couldn't take a proper solution (which is compared with experimental results).
Question
internal flow over cylindrical, rectangular and ellipse shapes.
outside is rectangular shape.
I would not use k-epsilon for this kind of problem. It is most valid for free stream turbulence like atmospheric flows. Near the walls k-epsilon behaves quite poor according to my experience and I believe that is where your heat transfer happens.
But you can try it yourself of course.
Question
Hi all, I have been encountering this problem shown in the pic with simulations with parameters:
• RNG k-epsilon Transient
• Pressure-based Coupled scheme
• massflow inlet and pressure outlet BC with Intensity 5% and Hydraulic Diameter 0.012m for Turbulence Specification Method
• URF and COurant number 0.2 while Turbulent Viscosity 1Three boxes for Frozen Flux Formulation, Warped-face Gradient Correction, Higher order term relaxation
• Timestep size 0.002 and 25 iteration/timestep
The problem occurs when the three boxes are checked, the number of cells overlimit starts very low and gradually builds up to such level after around 20 timesteps. When the three boxes are unchecked, overlimit cells range between 1 and 9 and disappear soon after.
Online posts suggested me to drop timestep size, max iteration per timestep, and URF but they don't seem to work for me. Especially when URF is quite low already. Assuming I wish to keep those 3 boxes checked, does anyone has any ideas?
I have been bugged for long. The model is also attached. Thanks a lot!
In such cases, modifying the BC or mesh configuration may be beneficial.
Question
Can we plot u-plus (U/Utao) Vs y-plus (Y/Ytao) plot for a turbulence model in ANSYS-Fluent post processing? Basically, I want to be ensure that the model will take into account the gradients in the viscous sublayer.
Hi Somenath, It should be possible with ANSYS as I have made it possible in STARCCM+ for my flat plate simulations. I will let you know the procedure in STARCCM+ and probably the same steps can be followed in ANSYS too.
1. Make a line probe where vertical measurements can be taken at the location or position where you want to have U+ vs Y+ plot.
2. Go for an XY plot where Y-axis is U+ and X-axis is a log scale of Y+.
3. Now the input part to this plot should be the earlier line probe.
4. Most of the software has Y+ defined so you just need to recall the expression for Y+ from the software database and assign it on the x-axis.
5. U+ may not be defined in most software. Hence create a custom field scalar function defining U+. (You will get a standard expression for U+ from any Fluid Mechanics Text Book, I follow Frank M White and it has expressions for U+ too).
6. Finally assign this newly defined U+ to the Y-axis.
Hope you too will get the same on ANSYS.
Question
I'm using Ansys Fluent to model a rotating cage setup to monitor Flow Accelerated Corrosion.
In general, for internal flows with curvature and rotations, k-Omega SST model performs the best. While k-epsilon models are used widely, they are not able to capture the near-wall effects (performs weakly under adverse pressure gradients and along curvatures). While k-Omega-SST model uses a blending function and allows us to go to y+ ~ 1, without having the adverse problems like in k-epsilon. In essence, it functions like the k-Omega model near the walls, and like a k-epsilon model in the far-fields.
Question
Is kw sst suitable for analyzing the flow over an airfoil after the airfoil has been stalled? specifically if we want to model the effective body of a stalled airfoil, can I do it with Kw sst or is there any better turbulent model to choose.(computational power is also limited )
Hello Mr Jayathilake,
the kOmegaSSTt is suitable for this problem in my opinion, especially when computational limits are low. With adequate refinement in the critical regions you might achieve good results. I don't know which code you are using for your simulations but, if available, you can also try the kOmegaSSTSAS approach. This "Scale Adaptive Simulation" approach is able to resolve turbulent length scales more precisely. It falls back to kOmegaSST if the mesh is coarse. But if you apply some further refinement you should get a more detailed results. Timesteps should be limited to CFL<=1. Compared to LES or DES mesh and solution order requirements are still lower I guess.
Computational effort for this model is not really higher than for the kOmegaSST.
You may have a look e.g. at these publications of the model developer Mr. F. Menter:
and many more.
I hope this helps.
Best Regards
David
Question
Hi all,
I am modeling a high-velocity (200 m/s) flow of water vertically entering the air. The water is supposed to hit the wall after traveling a 0.5 mm distance. The flow is highly turbulent, and I am using the k-omega phase-field approach for modeling.
The problem is that once the jet approaches the wall, the problem stops converging (Error: maximum number of segregated iterations reached). Any idea what is the root of the problem and how to solve it?
Majid
it may be caused by grid.
Question
First I simulated scramjet problem using k-e model in fluent. The results are validated using literature after that necessary modification was done in boundary conditions using same mesh. The results shows expected trends. After getting this results I refined the mesh and changed the turbulence model to K-w. The results are showing similar trends as k-e models but equivalence ratio of critical phenomenas are higher than k-e model. I want to know what are the possible reasons of high differnce of equivalence ratios? How I can verify which models are giving correct results?
First - changing two things in a simulation at the same time is obvious not a good approach (mesh AND turbulence model).
Further I need to say, that first you would need to find out, where your simulation comes to a mesh-independente solution (this question can be anbswered with no regard to which turbulence model you are using, if properly implemented in the CFD solver), and only on a mesh level, where the CFD solution is independent from the mesh resolution you can start to make judgements about model errors or about which turbulence model is more suitable for your particular application.
In contrary, if your solution is not yet mesh independent, i.e. the mesh is still too coarse, you are looking on a not known mix of discretization errors and model errors. This can mislead you to a misjudgement about a particular physical model and on the next following refinded mesh the situation (with the two models in question) might be reversed in comparison to what you have observed on the coarser mesh.
This CFD methodology has been outlined almost 22 years ago in the so-called "CFD best practice Guidelines for Industrial CFD".
The methodology says, that the following hierachy of CFD error quantification and elimination should be observed:
1) round-off error
2) iteration error (cut-off error with respect of stopping a solution process at a certain iteration number or by matchig a certain quantitative convergence criterion)
3) spatial and time discretization error
...and only afterwards you can investigate model errors of physical models.
Any attempt to investigate more than just one error source at the same time or to change the order of investigation of the errors from this error hierarchy potential will lead to erroneous CFD result.
Best regards,
Dr. Th. Frank.
Question
Hi everyone,
I am trying to simulate turbulent flow over a sphere with the following conditions:
Freestream velocty= 100m/s
ambient density and viscosity
Sphere diameter = 0.82 m
Reynold's number = 5.6 x 10^6
experimental Cd = 0.195
Sphere enclosure = 42 x 28 x 28 m3
mesh Size 4.5 milllion
I tried using S-A model and K-omega SST model in fluent, using which I am getting Cd=0.14. which is almost 26% error.
Any suggestion as to how may I improve the result?
WMLES or SBES model with a well thought (and validated) mesh resolution.
Regards,
Dr. Th. Frank.
PS : Your question did not involve any limitations on the computational time of the proposed turbulence modeling approach. Therefore a scale-resolving simulation would clearly deliver the best possible results (I'm not proposing a diret numerical simulation, since you asked for turbulence modeling approaches; DNS is resolving turbulence, but not modeling it).
Question
I would like to start a discussion of this specific topic.
Here I would like to discuss the list of possible techniques helpful for performing the simulation of oscillating bodies in quiescent fluid.
This discussion is open to all the students, teachers, and researchers.
I request you to reply here if you are familiar with code development in OpenFoam, IBPM, NEEK1000, lilypad and CFX
Pradyumn Chiwhane I am posting here a previous answer I provided on submerged oscillating bodies in quiescent fluid. The total force exerted by the fluid on the cylinder, you should consider besides the drag the added mass force. Academic references are provided within the following research projects:
Question
Turbulence model for blood flow simulation
Volodymyr Brazhenko
could you please explain agree on what ?
Markus J. Kloker Asif S. could you please tell us what turbulence model is used and what particular modulation of the terms closures are completed to take into account the non-newtonian behavior of blood, particularly for relatively low apparent Reynolds numbers ?
Question
In my study, I have two cases for CFD which I performed on Ansys Fluent,
1) oscillating flow over a solid cylinder (blunt face perpendicular to flow direction)
and
2) solid cylinder (blunt face perpendicular to flow direction) oscillating in the stationary fluid. It involves dynamic meshing.
In both of the above cases, I am using the SST k-w turbulence model for this simulation.
[ ie what should be the input value for Turbulent Kinetic Energy and Specific dissipation rate? ]
What does it means if both these values are equal to 1.0?
I have attached a graph representing drag force as a function of time [calculated from the case (2)]. I want to know what might be the possible reason for this behavior in the initial time.
My UFD (equation for velocity of moving cylinder): V = 1.0 * cos(2*3.1415*1.55*t) m/s.
The initial spike? why does this occur?
The decreasing amplitude?
What would be the expected output if this was calculated for longer time values (amplitude behavior after 5 secs)?
Fluid: incompressible (water)
calculation settings:
time-steps = 500, time-step size = 0.01 sec, maximum iterations = 500.
Meshing (element size = 1.0 mm, element shape = triangles)
Pradyumn Chiwhane I am not used to performing calculations with CFX. Researchers in my group do.
If this is the total force exerted by the fluid on the cylinder, you should in my opinion deduce the added mass force to obtain the net Drag. You may consult academic references within the following research projects:
Question
In case of turbulent flow over an irregular shape, how can we find the first layer thickness near the walls of the irregular boundary.?
For flow over a flat plate, the skin friction co-efficient can be found by the direct formula, for irregular shapes how can we find the skin friction coefficient.
Academic resources on fluid Mechanics are provided on the project references:
SINGLE PHASE AND MULTIPHASE TURBULENT FLOWS (SMTF) IN NATURE AND ENGINEERING APPLICATIONS | Jamel Chahed | 3 publications | Research Project (researchgate.net)
Question
Some commonly used turbulence models include k-epsilon, k-omega and shear stress transport (SST) models. The k-epsilon model is a best candidate for flow away from the wall (e.g. free surface flow region), while the k-omega model is best suited for near the wall flow region (e.g. adverse pressure gradient flow region). The choice of most appropriate turbulence model for any turbulent flow problem may be extremely difficult for young computational fluid dynamists, hence the need for this germane question.
The SST k-ω model is a hybrid of the best of k-ω and k-ε. This model uses the k-ω model near walls, and transitions to k-ε model in the open flow field. It’s popular in aerospace and turbo-machinery applications.
So SST is the most effective model for young computational fluid dynamists.
Question
This paper is claiming there is a problem in k-epsilon model. Because in k-epsilon model, we assume that eddy viscosity(νT) is isotropy. But actually in real world, eddy viscosity(νT) is anisotropy for high Reynolds number and is isotropy for low Reynolds number. It means there can be error when we consider flow with high Reynolds number.
And I have a question in uploaded figure. How he can calculate fluctuation velocity?
What I know is fluctuation velocity can be calculated only when we assume that eddy viscosity(νT) is isotropy(like k-ε model).
When we use k-ε model, we can find k(Turbulence Kinetic Energy) by T.K.E transport eqation and k is same with '½(u'2+v'2+w'2)'.
Then if k(T.K.E) is found, we can calculate u', v' and w'
because u', v' and w' are same each other by assumption of isotropy.
But in this paper, author claims that we should consider flow as anisotropy and he suggests new Eddy viscosity(νT) with new Cμ. (I've uploaded expression of Cμ by picture.) So I think it is impossible to calculate fluctuation velocity because flow is considered as anisotropy.
But there is a fluctuation velocity profile that is calculated by CFD. And I think author calculated fluctation velocity using root mean square and T.K.E
Because we can find desription in figure that means he calculated fluctuation velocity by root mean square. (Figure 8: Profiles of rms velocities perpendicular (v) and parallel (u) to the wall in the impinging jet)
So it looks like contradiction to me.
How fluctuation velocity is calculated in anisotropic flow?
Actually I've thought that assumption of isotropy can be possible in the impinging jet sometimes. Because impingement occurs nearby wall, so there is a low Reynolds number nearby wall by No slip condition(dominant molecule viscosity). But, eventhough my deduction is right, I can't understand why there is a difference between v' and u'. In the case that r/D=2.5, there is a difference between v' and u' that I've marked in uploaded picture. Difference between v' and u' means this flow is anisotropy and this is contradiction against author's claim also.
Also I've infered about the one more reason why calculation of fluctuation can be possible in this paper.
I don't know well but what I've heard is
In RSM(Reynolds Stress Model) is suggested by the same claim of this paper.
I've heard RSM is suggested because flow with high Reynolds number is anisotropic in real world
and this is different with original k-ε model.
So in RSM, it is possible to calculate the each fluctuation velocities(u', v' and w') in anisotropic flow.
So RSM and this author's model has same purpose that pursue to consider anisotropic flow.
And RSM can calculate the the each fluctuation velocities(u', v' and w').
So I think this author's model can also calculate fluctuation velocity in the same reason.
Eventhough I don't know how RSM calculate each fluctuation velocities(u', v' and w'), I've tried to infer.
Summary
Anisotropic flow by using new eddy viscosity that has direction - Calculated fluctuation velocity
: I think there is a contradiction.
Left side: Anisotropic
Right Side: Should be isotropic
→ ???
Calculated fluctuation velocity - Difference between u' and v'
: I think there is a contradiction.
Left side: Isotropic
Right Side: Anisotropic(Different fluctuation velcity.)
→ ???
I'm not good at Turbulent.
I'm just Senior.
I don't have bachelor's degree yet.
But I'm interested in Turbulence.
But I'm confused now :(
Thanks :)
Flows with greater anisotropy in the turbulence stress tensor render standard one equation and two equation RANS models not great as they make assumptions about the turbulent shear stresses which turn out to be untrue for specific cases. This anisotropy is commonly present in flows with large separations etc. Reynolds stress models remedy this by solving transport equations for each component of the stress tensor but these too have limitations and haven't proven to be of much advantage. If high accuracy is desired, LES or DNS are the only way. But for most engineering flows of interest, one equation and two-equation eddy viscosity models provide sufficient engineering accuracy with results in a reasonable time.
Question
Hello everyone.
I'm working on a flow simulation in an axial pump. in the literature, they recommend that y + should be kept below 1. however, my results have shown that y + is greater than 10.
how can I keep y + below 1?
Note 1: I am using TurboGrid for the mesh and I am using SST as the turbulence model.
Note 2: I am using TurboGrid as a mesh generation tool.
Mohamed Bounouib please follow the links attached herewith and follow the steps for the flow simulation in an axial pump. That will be easier for you
1. https://youtu.be/aY2HRp6zq2g (CFturbo turbomachinery design software.)
2. https://youtu.be/H07b2pXpCCM (ANSYS)
Regards
Question
I am designing a turbine and predicting the Performance of the Vertical Axis Turbine. I have the experimental results of the same turbine with me. The problem is after the optimum TSR, the performance of don't go down its continuously increasing and goes above the Bitz limit. May be its not concluding stall due to high TSR. How do i resolve it?
Geometry -- Mesh -- CFx
Doubt i have but need help to resolve,
* I unable to capture the correct boundary layer, if it so then how could i capture it?
*Maybe i am using Turbulence model which is not correct, But i have chosen shear stress transport which is be better choice, mabe?
* Also share if you any any other.
I will be very thankful, and please make it urgent.
Ahmed Gharib Yosry Thanks for your assistance. i tried to reverse the boundary conditions, replace the inlet and outlet with each other. but the torque doesn't goes down the optimum value.
Question
Hi.
I'm trying to simulate a fluid through a vertical channel, width = 0.2 cm - height = 60 cm - fluid == water - inlet v = 1, using the 2D model in COMSOL. Due to the characteristics mentioned a turbulent model is needed. When choosing Algebraic YPlus method the no-slip condition in the vertical walls states (u,v) = (0,0), which is what I thought, but when using the k-epsilon or k-omega model for de NO-SLIP condition (u,v).(nx,ny) = 0 [u = 0 and v is free] which i don´t understand why. Can anyone explain why in k-e or k-omega don'y use velocity=0 on the walls?
In the COMSOL documentation the no-slip BC is indicated to be (u,v)=(0,0).
What you described is slip condition. You can consult the COMSOL team for more clarification. You can also run a test simulation to see how the code performs.
Question
Dear CFD Fellows,
Is there a decision table, diagram or software you use for turbulence model selection? What I'm looking for is not a table with information for each model, but rather a visual with decision steps such as "if the flow contains a-b-c, these models can be used". In the relevant case, after following the characteristic factors of your flow, I expect turbulence models to be proposed in the last section that can best define the flow.
Best regards,
Güven
Dear Fellows,
We are all choosing a Turbulence Model for our flows. We are already creating decision chart in our heads. So, why not put these decision steps together and create a real chart? Please do not think so complicated. At the end of the chart there won't be only one Turbulence Model for relevant case, there will be list (at end of different decision steps same model could be listed too). After that you can do some literature search to select the best model in the list.
Best regards,
Güven
Question
Dear CFD Fellows,
Is there a decision table, diagram or software you use for turbulence model selection? What I'm looking for is not a table with information for each model, but rather a visual with decision steps such as "if the flow contains a-b-c, these models can be used". In the relevant case, after following the characteristic factors of your flow, I expect turbulence models to be proposed in the last section that can best define the flow.
Best regards,
Güven
Question
Hi all,
I'm planning to simulate flow past a floating body using CFD method with the main purpose of investigating its stability against hydrodynamic forces. A sketch of the problem is presented the the figure attached.
It seems that an accurate estimation of pressure field, and therefore hydrodynamic forces, is heavily dependent on correct prediction of flow topology, particularly separation and reattachment of the flow.
I'm wondering what turbulent models would best handle this problem. I would appreciate it if you provide details and specific reasoning.
Regards,
Armin
The Reynolds Stress Model is the most complete turbulence model with regards to representing turbulent flow.
Question
I have watched videos about wall function on youtube but still confused about understanding viscous sublayer, logarithmic region, and wall functions. I couldn't find relevant material. Where do I find these topics? Can someone suggest some material regarding viscous sub-layer/logarithmic region and to understand y+ (wall functions)?
I would add that the meaning of y+ is very very simple. It is nothing but that the local Reynolds number measured along a normal-to-wall direction. That is, y+=0 is the wall position and then the value increases according to y+=(u_tau/vi)*y.
Question
Hi everyone
I am working on a shell and helically coiled tube heat exchanger with laminar flow through the shell and turbulent flow through the coil tube. I have performed iterations for coil by selecting different types of turbulence models but in each case, energy starts to diverge after some iterations (images attached).
What is the possible reason for this?
I think it may be due to BCs. Can you please your problem in detail, so that I may help you in diverg. Issue
Question
Can you suggest where can I find video lectures on turbulent flows or turbulence modelling? Are there any video lectures on understanding turbulence modeling? Or any books to understand turbulence modelling? Can someone please help!
i have a project on how different turbulent models can be used on Naca aerofoil. and i am not knowing how to find material to understand turbulent flows.
Dear Vinay,
I would recommend you to follow the video lecturer on Computational Fluid Dynamics by Prof. Suman Chakraborty according to me it is one of the best.
You can also follow Prof. Fillipo Maria Denaro's technical report/ppt on CFD, available in the ResearchGate.. He is one the famous researcher in computational physics and CFD.
Question
in turbulent flow calculation is it acceptable to use an y+ of 15 with a wall function in k-e turbulence model?
Dear Prof. Th. Frank
Thank You very much for your explanation and suggestions on my error.
Question
I am performing CFD simulation upon NACA 4418 airfoil at 45 m/s free steam velocity and Reynolds number of 3 million. I am following a particular paper where the experimental results of NACA airfoils are shown. The turbulence model I am using is k-omega SST turbulence model and the transition is ticked on. The mesh is also properly refined and since my computational power is limited, therefore I am choosing my y+ value to be greater than 30. But the following problems are observant from my simulation
01. Lift coefficient seems to be around the mark but the error percentage is still a bit above 10%
02. Drag coefficient is the real issue as it is exceeds the supposed value and produces.much higher value. Almost double the value that I want
What is the issue here and what should I do? I have been going through the theory behind drag and lift coefficient and the Computational process used behind but it's not helping me so far and I really need help regarding this right now.
Thank you very much
Hi Nehal,
If you have refined the mesh and used the appropriate turbulence model, then I suggest you to please check the convergence of the result.
Question
hi everyone I need a little help here; Im new to fluent and recently I am trying to simulate a two phase flow in a pipe-tank system where I want to see and analyse the intake vortex with the air core. i am using vof+cls and les as turbulance model, I don't have problem with convergence but after simulating 100s of the flow, I can't see the formation of vortex and air core of in getting sucked in to the pipe. can any body help? has anyone experienced this problem too? I really need help at this point📷
Hi,
this is not an easy to setup simulation, also it may look like this on the first glance.
Why?
1) Vortices leading to air entrainment are rather small flow structures of thin diameter and having substantial velocity gradients over the diameter of the vortex. This velocity gradients need to be fairly good resolved in order to resolve the low pressure occuring in the center of the vortex leading to the air entrainement. For that a very fine mesh resolution is required.
2) Usually such vortices - if they are not artificially and by geometric design measures stabilized - are not stationary in space. So the vortex is moving around / precessing and that makes it even harder to establish a well resolved numerical mesh with fine mesh resolution at the vortex center. It might be suitable to use adaptive mesh refinement, but without a coarsening algorithm there is the danger, that the geometrical space more and more fills with refined mesh cells, making the simulation rather very expensive.
3) Standard 2-equation turbulence models are by default not capable of capturing the strong velocity gradients in flows with strong streamline curvature / rotation. A SST k-omega-based turbulence model with curvature correction is at least recommended.
4) It has to be made sure, that the turbulence conditions at the free surface between liquid and air are capturing the physical valid conditions. Usually a fine mesh resolution at the free surface is required for that in addition with turbulence model damping terms at the free surface, i.e. the turbulent kinetic energy at the free surface needs to be dampended to zero or small values.
Regards,
Dr. Th. Frank.
Question
Hello guys,
I am running a simulation of a mixing tank in unsteady-state( transient) with turbulence model SST K-omega and multiphase model VOF. And I gave a number of time steps as 10000 and time step size as 0.0003 and max iteration as 50 and the solution is converging at each time step. So my question is how do I know my simulation is completed ? or I need to wait till 10000-time steps to complete?
Regards
Johnny
I try to address better the question. If the flow problem admits a statistically steady state you start from an initial condition and run until you flow variables are statistically steady, that is you see them oscillating in time around a constant value. From that moment the solution is physically correlated.
Conversely, if you have a problem that has an unsteady behavior also in the mean values, you need to simulate at least the largest time period of your problem.
This approach is typical for DNS/LES formulations, sice you are using a URANS approach the real physical meaning of your unsteady simulation can be debated. If your flow problem is statistically steady, your URANS shouldn't be somehow different from a RANS solution.
The key is that you cannot fix arbitrarily a number of time steps without knowing the nature of your flow problem.
I suggest to monitor in time the mean values
Question
I am performing CFD simulation over a NACA 4418 airfoil on Ansys FLUENT and I have collected a data chart of NACA (from 1945) for the purpose of validation.
The Reynolds Number chosen for this CFD simulation is 3,000,000 and the free stream velocity is 45 m/s. Since the simulation for my case is 2D simulation both the characteristics length and area is 1m. The value of y+ considered is 1 and that is ensured by calculating the wall spacing and putting that on First Wall thickness and I have even gone through Report in Ansys FLUENT to check the maximum facet value is below 1. I have used both Spalart Allmaras and K-omega SST Turbulence model. But the following problems are prevalent:
01. For Spalart Allmaras Turbulence model,my lift coefficient is within the range i.e less than 5% difference in between but drag coefficient is way too much high in value sometimes even 200% more
02. For K-omega SST Turbulence model, my lift coefficient is significantly higher in value and as Angle of attack increases this difference gets higher but the highest it gets is below 30% however drag coefficient is also over predicted but in this case the difference is around 50% higher.
I have tried it again for both Turbulence model with a bit more refined mesh but the value of lift coefficient increases in both the cases and but the difference for drag coefficient decreases for K-omega SST Turbulence model
I have been trying this for months now and haven't come to a proper solution. I tried everything at my disposal. Read aerodynamic books and gone through understanding how it is represented on CFD but so far I am not able to find the solution. If anyone can explain it to me what is going on for my case and how can I find a solution for this, that will be really helpful and appreciated.
Best
Question
I have a case, which is about internal flow with constant heat flux. Although the inlet boundary condition is laminar, the flow is passing transition and turbulent regime along the tube. As known, the intermittency term is 1 (so, admitted as turbulent inlet BC) for freestream velocity for external flow, I would like to learn that whether using the transitional SST model by laminar inlet boundary condition in the pipe is the corrects way or not.
Best regards,
The problem I faced while using SST I need to put the value of turbulence intensity at the entrance, and if I specify it to zero then my solution does not converge.
Question
I am interested in broadening my understanding of the physical assumptions needed to simplify its mathematical description. From these assumptions i will to choose a suitable turbulence model to run the simulation in Ansys.
The problem is fairly basic;
Inlet flow conditions: Velocity in= 44.2 m/s, Mach number inlet = 0.128, atmospheric total pressure and temperature. Turbulent boundary layer thickness @ 4H upstream of the step is 1.9 cm.
Outlet flow conditions: Fully developed flow.
Any advice would be much appreciated
Kind regards
Anton
If you want to use the RANS formulation you should assume your flow field is totally developed. That means you can set the inflow profile according to a statistically mean velocity in a channel
Question
I want to determine the aerodynamic coefficients of a 2D model (solid boosters). To be clear with the model, It is a 2D axisymmetric model, with blunt nose and flared aft body. There is a plume exiting from the nozzle. The jet plume interacts with the freestream flow, to form plume induced flow separation (PIFS). The interaction will affect the aerodynamic coefficients.
Experimentally the axial force coefficient was found to be decreasing at increased jet pressure ratio (Jet pressure/free stream pressure). I've solved it using pressure based solver with standard, K-e turbulence model (I've tried using other turbulence model too). But results from Ansys Fluent showed no change with change in jet pressure ratio.
Am I missing something or is there any other method to find axial force coefficient.
Question
I am trying to run a transient simulation of a stirred tank reactor. Initially, I am simply trying to using water as the only fluid with the k-epsilon turbulence model. I ran the steady-state simulation first and then in the same workbench's fluent file, I simply changed the option of steady-state to transient and set the simulation to run using for 0.0008-sec timestep, 2000 timesteps, 25 iterations per time step (in order to use that steady-state data as the initial condition for the transient case). I had also used report definition function for plotting turbulence kinetic energy as a function of time and had used the option of autosave for every 5 steps along with export data of certain parameters for every 5 steps. (pl find the ss) But after around 200 timesteps, I am getting the error of (Error: GUI-domain-label: no domain selected Error Object: 1522351816) and the simulation stops at the next iteration. I am able to click ok and the simulation runs for another timestep but the error crops up again every timestep.
simply you can save your case and data file at the current time step , and then reopen it and procced the calculation again . the error at each time step will disappear.
Question
Both PANS (Girimaji, 2006) and TFLES (Pruett et al, 2003) provide a self-consistent formulation that allows one to recover RANS versus DNS at opposite limits. Are the two approaches fundamentally different (e.g., in the sense that RANS vs LES employ different ansatz and thus yield different types of closures to be modeled: the Reynolds stress vs the subfilter stress)? Or are they conceptually the same approach, independently developed and thus mainly differing in preferred modeling choices/perspectives?
(note: I am unfamiliar with PANS and only marginally familiar with TFLES; apologies for any misinterpretations)
in RANS-like formulation the numerical discretization has much less implication as the turbulence model acts on all the scales.
I don’t know the specific issues in PANS but only for the case of a scale separation the numerical discretization assumes relevance
Question
I want to add the penalty term as you suggested in the paper "Topology optimization method with finite elements based on the k-ε turbulence model" Could someone guide me on how to add the penalty terms for Eq. (11) and (12) as shown:
Question
Hi everyone,
I'm simulating a 3D turbulent pipe flow using the SST K-W turbulence model in ANSYS Fluent. Is there any quantity among the postprocessing quantities that represent "eddy size" or "eddy length scale"? If there is not such a quantity, How can I define it in Fluent?
Thank you.
You have to define for example your desired Kolmogorov scale through UDF.
Cheers,
Question
Hello All,
I have 2D mesh defined in x and y directions.
Now I would like to extend just once cell in Z direction so that it is 3D Mesh due to requirement of 3D mesh for turbulence model and type of input mesh.
How can I do this in Ansys Fluent Mesh Modular?
The easiest way (which I know about) is to read this 2d Fluent mesh into CFX-Pre. During that CFX will ask you, whether this is a 2d planar or rotational symmetric mesh and it allows you to extend the mesh i z-direction (you can choose the extension in z in terms of dimensional units [m] and number of cells). Once this is saved as a CFX-Pre DEF file, you can re-import the DEF file into ANSYS Fluent again and it becomes a 3d Fluent CAS file.
Regards,
Dr. Th. Frank.
Question
The methodology I am using was
Type- 2D Axis-symmetric behaviour
Flow domain is divided into finite number of unstructured quadrilateral cells
2D double precision, implicit, density based solver of flux type Roe-FDS
2 equation SST k-w turbulence model and RANS energy equations are solved
Air of ideal gas density as fluid with 3 coefficient Sutherland’s viscosity
Pressure far-field, stationary wall and ensured no slip condition
Free stream conditions
Mach number 6
Pressure 1064 Pa
Temperature 234 K
Thermal condition for wall : constant wall temperature of 300k
Turbulence intensity of 5% and Viscosity ratio of 10
First order upwind discretization scheme for first few iterations and followed by second order upwind for further till convergence
Higher Order Term Relaxation, Convergence Acceleration for Structured Meshes and Warped face gradient correction were enabled
All the residuals were set to 1e-06
You should decrease the residuals. How many residuals did you have when you used the transient calculation. If you can not decrease the residuals you should increase the number of elements. If you have a separation zone then the residuals periodicity will remain.
Question
Hello
Just before I start I am new to CFD modelling and I am trying to simulate a numerical wave tank with a wave of amplitude 0.1m and wavelenght of 1.561m using stokes third order. I am using the VOF method Implicit model with 2 Eulrian phases. The turbulence model is K-omega SST and I am using a water as my second phase where I have selected compressible so it is able to interact with the air. I have set up numerical beach at the end of my domain and the BC I am using are as follows.
Inlet-Velocity inlet
outlet-pressure outlet
Atmosphere-pressure outlet
bottom and side walls-Wall(no slip)
cylinder-wall(no slip)
I am using the PISO algorithm and have decreased the relaxation factors for momentum,k and omega. For some reason I am not able to reach similar results to an experiment. I am not to sure where I am going wrong. If anyone could help I would be extremely grateful.
My answer is a bit late. But might be of help to others.
I am not a user of Ansys. I cannot tell you whether you need a used defined routine to obtain the wave kinematics at inflow.
However, I have experience with generating waves in CFD and recently published a paper in which I also compare a generated CFD wave with the Stokes 5th order theory and I also computed wave loads on a vertical surface piercing circular cylinder , but both with incompressible fluids. The results of the latter are also compared against experiments.
Your inflow BC should include wave kinematics (e.g. orbital velocity vectors for a regular wave) and the volume fraction according to the wave you are using (Stokes 3rd order). Some codes allow also coupling with potential flow codes that include several irregular wave spectra. The wave theory should also be chosen according to their applicability ranges. See e.g. Lé Méhauté.
Depending on the domain, you might see reflections at outflow, sides, objects, etc. Therefore, you need to tune your damping algorithm to your case. Further details see .
As Mohammad Mehdi Baseri pointed out, the grid/mesh is important. Usually, people try to relate the cell size in vertical and propagation direction to the wave height and length, respectively. However, this also depends on the steepness of the wave. A steeper wave might need different resolution. And it also depends on the structure you investigate, i.e. the diameter of the cylinder or any other difficult areas.
Furthermore, the time discretisation is also very important. Time discretisation can also be related to the wave period. Time discretisation is important because it influences the iterative convergence. Some interface capturing schemes like HRIC depend on the CFL (Courant-Friedrichs-Lewy) number. They switch to lower order methods for larger CFL numbers for robustness but this depends also on the CFD code you use. Thus, you will need to investigate different time step sizes. If you see irregular waves for regular inputs, the iterative convergence might be the problem. When you do the grid and time step sensitivity study, try to follow ITTC guidelines for refinement. If you want to read more about this, you are welcome to read my paper: Towards credible CFD simulations for floating offshore wind turbines . I believe test case 2 is similiar to yours. I will add a couple of further reading material below.
The iterative convergence is also important. To achieve convergence is usually difficult for simulations with VOF, see . Residuals in the order of Linf<1e-3 might be okay for a first investigation. Then, you can check the influence for 1e-4, 1e-5 etc. But this comes once your grid and time step are acceptable and the results in the same order as the experiment. The iterative convergence is also influenced by the relaxation parameters, the number of iterations per time step, the numerical schemes, the grid quality, etc.
Good luck!
Cheers, SImon
09377255.2015.1119921
Question
I'm trying to develop a code to solve the stream function-vorticity equations using the Finite Element Method in order to simulate a 2D incompressible flow problem. I was wondering what the pros and cons are, whether coupling a turbulence model is possible, whether formulating the boundary conditions may face difficulty and whether the evaluation of the pressure field is flawed possibly due to decoupling of the pressure variable from the governing equations. Note an accurate evaluation of the pressure field is particularly important for my case of study.
I very much appreciate helping me out.
Good topic
Question
Hi everyone
I'm doing a steady state simulation using ANSYS fluent and k-epsilon turbulence model to investigate thermal mixing in a T-junction and I need to get a temperature contour at a specific time steps. How can I achieve that?
Any help will be much appreciated. Thanks in advance.
Dear Md Nuruzzaman,
Use ANSYS FLUENT 12.0 Tutorial Guide to develop temperature contour data at specific time set up. Use the solution animation feature to save contour plots of temperature every five time steps. .ANSYS FLUENT to update the animation sequence at every time step and contour plot in Fluent at specified intervals of a calculation.
Step Condition
1. Geometry and boundary conditions.
2. Overall mesh generation
3. Independence studies. (a) Grid Independence; (b) Time Independence
4. Temperature contour for different time step sizes (top = 0.5 s, middle = 0.01 s, bottom = 0.005 s)
5. Animation
6. Post solution and save
Ashish
Question
I'm currently working on a project that is using the SST k-w turbulence model. This model, reads velocity flow on the near wall region of a bluff body as well as the far wall region which is the combination of k-w and k-e turbulence model. The SST k-w model can be the best approach in solving this type of flow problem. The only issue is defining this model onto the CFX pre process.
???
Just go to flow domain --> turbulence model and select the Shear-Stress Transport (SST) model. So what is here the issue?
Regards,
Dr. Th. Frank.
Question
Hi all. I am running simulations on a compressor fluid domain (Turbocharger compressor for a passenger car) in Ansys fluent 19.3. I am using tetra element and k-omega SST turbulence model. But y+ is still high after refinement. How to reduce to get y plus value <5 ? Could someone give me any suggestion.
Hi,
you could use a combination of refinement on the wall surfaces and then apply inflation layers of your choice ( you may input the first layer height), thus you could generate a mesh of good quality in terms of skewness as well as aspect ratio.
hope it helps.
Regards,
Rajesh.
Question
Hi
I am trying to model an impeller rotating at a certain angular speed using MRF technique in Ansys fluent. Overall i expect clean attached flows and I am not really interetsted in resolving the boundary layer as I am more interested in studying the mixing of 2 liquids by the impellers. As i understand K-omega reliazable model is computationallly expensive and more for resolving the boundary layers. Which turbulence model is better for my flow as I want to keep my model light weight so that it is easier for convergence and computationally less expensive. Your advise will be really appreciated
Thanks/Regards
You can begin by trying different k-epsilon models (standard, RNG, realisable ) and compare it with experimental data.
Question
I am running a simulation for a turbocharger compressor fluid domain with turbulence model k-omega SST.
I am going to refine the mesh as the solution does not converge. What I know is that for a turbulence model k-omega, the Y plus value has to be <5.
I am looking to calculate the Y plus value before running the simulation.
Currently, I have a model of 3 Million of mesh elements.
Can someone explain what total mesh element number approximately should I refine to reach the Y plus value of <5?
The Y+ value depends on the grid points that are near the wall. The more grid points near the wall the less Y+. FLUENT has the Y+ plot option.
Question
I have problem in making my turbine simulation work with SST turbulence model
the other models: k-e, k-omega, BSL converge without problems
Another and similar approach would be to make a very coarse mesh solution. Due to high numerical diffusion on coarse meshes this is usually easier to converge. Than this coarse mesh SST solution could be interpolated on the productive mesh as a flow initialization. The coarse mesh could be extremely coarse for this purpose.
Regards,
Dr. Th. Frank.
Question
To analyze the thermal stratification of solar hot water storage tanks using numerical simulations, is it possible to apply the turbulence model? What are the parameters of using the model?
In my opinion, it depends on the model that you are going to develop. Turbulence is a 3D phenomenon caused by inlet jet mixing, plume entrainment, heat losses, etc. Using CFD, of course, you can model the turbulence. However, it is not the case for one-dimensional models since temperature gradient is only considered in axial direction, but turbulence should also be considered in radial and angular directions. Followings are papers that give some hints to solve this issue:
Question
In air-water multiphase flow CFD simulation's it is common to use a VOF = 0.5 to track or identify the position of interface or free surface. I would like to know why this criteria is used and if it can always be assumed the same. Otherwise, I would like to know if volume fraction can be taken different to 0.5 and, if so, ask them about a methodology to find this volume fraction.
Below I describe a case that I am simulating in Ansys Fluent:
-Sewer pipe with Length L=6 m (aligned with the x axis), Diameter D=200 mm (8 in) and longitudinal slope So = 0.005 m/m.
-Simulation in steady state of sewer pipe considering biphasic flow air-water flow.
-Model Volume of Fluid (VOF) with implicit formulation and Open Channel's submodel.
-Boundary conditions: Inlet as mass flow rate = 26.51 kg / s; outlet = Pressure outlet. The mass flow entered is such that the ratio y / d = 0.61 (that is, occupation of 61%).
-Turbulence model: k-epsilon RNG with Enhanced Wall Treatment function (y + <5).
-Pressure-Velocity Coupling method: Coupled + Pseudotransient solver.
-Spatial discretization: Least Squared Cell Based; PRESTO!; Momentum, k and epsilon with 2nd order schemes; Volume Fraction = Compressive.
-Run Calculation: Time Step Method = Automatic with Length Scale Method = User-Specified; Length Scale = 0.064 (Hydraulic Radius); Time Scale Factor = 0.3.
To verify convergence I did the following:
* Residuals at 10-4 for all variables.
* Mass balance between input and output.
* Pressure drop between inlet and outlet.
* Velocity at Inlet and Outlet.
* VOF fraction for various orthogonal planes to the pipe at x = 0.5m, 1.0m, 1.5m, 2.0m, ..., 5.5m. I configured them as Surface report-Area Weighted Average, for the Field Variable=Volume fraction and Phase=water.
Convergence is good in terms of residuals, mass flow rate (1x10-6), drop pressure, velocity. In VOF monitors the trend also stabilizes towards values between 0.40 and 0.75.
I know a flow profile along the pipe. In my initial simulation with refined mesh, with elements of 0.02mx0.005mx0.003m, [this is (dx) (dy) (dz)], I noticed that the theoretical profile is closer when I choose VOF = 0.7 and not VOF = 0.5 as is usual in the practice.
From the above my doubt arises about the VOF fraction to choose.
Thanks!
Leonardo Henao; Use the HRIC Scheme and refine the mesh in the z-direction (the wave elevation direction).
Question
How can calculate the value of Y+ for each turbulent models in Fluent CFD?
Yes, you can easily plot the value of y+ on the plot function of turbulence. There is "wall y plus" option.
Question
I am working on an open-channel multi-phase (water+air) flow with k-epsilon turbulence model. How can the computational cost of the model be minimized, while the accuracy and convergence are ensured?
There are various ways to decrease the computation cost in CFD problem as below:
- Use a coarse meshing in unimportant sections of domain,
- Apply a more powerful processor,
- Utilize all processors of your system.
Question
Hi,
I am simulating a turbine in Fluent that it has curve. Mesh is structure completely. but there is high Skewness in tip clearance and some parts of around of the blade:
When i use SIMPLEC Method, one factor (Skewness correction) appear under the SIMPLEC method in ANSYS Fluents method.
How i must adjust this factor? i dont know which number must be set?1< or 1 , 2, 3,
I used K-e turbulence model and when I set Skewness correction to 5 or 20, the following error is appeared:
"Error: Divergence detected in AMG solver: k
Error: Divergence detected in AMG solver: k
Error Object: #f"
Why does this happen?
Please suggest a way to reduce the skewness in ansys fluent and how can i check Skewness in Fluent?
Thanks.
Best.
Ali
Question
Hi
in ansys fluent's dacuments it has been said that : (( ANSYS Fluent has taken steps to offer more advanced wall formulations, which
allow a consistent mesh refinement without a deterioration of the results. Such -independent formulations are the default for
all omega-equation-based turbulence models. For the epsilon-equation-based models, the Menter-Lechner and Enhanced Wall Treatment (EWT)
serve the same purpose. A -insensitive wall treatment is also the default for the Spalart-Allmaras model and allows you to run this model
independent of the near-wall resolution. ))
so, is it true that for models mentioned above like k-omega or k-epsilon(EWT,Menter-lechner)there is no need to check y+ value to be in a certain range ?
for example can i use k-epsilon model with enhanced wall treatment and y+ value changes between 0.5 to 600 ?
if my assumption is'nt true , what is the certain range of y+ value for all turbulence models like k-epsilon with wall functions or k-omega
without wall functions ? please give me a reliable source ...
thanks...
Dear Amir,
Let me give you some more explanation concerning y plus. Y plus is an analytical profile covering the viscous sublayer and the buffer layer. In fact, the boundary layer thickness composed of three regions when going far from the wall, started with viscous sublayer, the buffer layer, and the turbulent layer. Y plus is designed to cover only the first two parts and it is expected to be started from the very beginning of the turbulent layer. Now as an assumption keep these figures in your mind:
Yplus> 500 for the outer layer
31<Yplus<500 for log low region
5<Yplus<30 for the buffer layer
Yplus<5 for viscous sublayer
considering above applying the wrong value for Yplus could shift the calculation from one layer to the other, where it is not supposed to be. In this regard, you need to run your model first by a fix y plus let say 50 for all parts of the model, thereupon check the model in postprocessing and determine the regions with high-velocity gradient, calculate boundary layer again for local Reynolds value, then you would realize how much YPlus value you need for different region and where you need to reduce it and up to what figure. In other words, reducing y plus means that regions are exposed to much more intensified turbulent flow, and thereof you need to close the grid to the wall. If we suppose sigma as the boundary layer thickness the ration of 0.02<y/sigma<0.2 represents the region one needs to locate the starting grid.
To put it in another way, the best solution could be obtained without using Y plus and by direct meshing right from the wall surface, but we made use of y plus to decrease computational costs associated with direct meshing.
Question
Hello everyone,
I have problem on settings of farfield boundary condions. I want to increase turbulence intensity on the airfoil as inlet turbulence intensity but if i enter %2 , it decreases to 0.9% on the point front 1 meter from leading edge. I want to know if there is any equation of Turbulence intensity for C shape mesh domain on airfoil to have needed turbulence intensity.
Thank you so much...
Greetings @Emre Güler
I am not sure if this would help you but @turbulence intensity (%) can be specified as I = 0.16Re^(-1/8).
So from what I understand and from the equation above, even if you specify your turbulent intensity at 2 %, there will be fluctuations in it as the flow over the airfoil will not have the same initial velocity you had set. When the flow over the airfoil changes, the corresponding Reynolds number also changes, hence calculated turbulence intensity slightly changes and it depends on Reynolds number.
So for example, if your inlet velocity is specified to be Re No 100000 which corresponds to 10.47 m/s if density taken is 1.1839 kg/m^3 and viscosity to be 1.86 E-05 m^2/s. Then your flow over the airfoil (upper surface and lower surface and trailing edge) will not be 10.47 m/s. It will change. Based on the velocity changes as the flow travels, this could be the reason why your turbulence intensity changes as well.
Question
Hello, I am doing a 3D simulation of a wind turbine using S-A turbulence model. Without wall function, I need to make y+ in the order of 1. So, I must use a finer boundary layer grids, but when I decrease the value of the first layer thickness, the solution diverge.
I agree with Aditya Vedanth ,
It is better to make a literature study to know which turbulence model gives the best results for your case....
Question
Can anyone please define me Linear Eddy Mixing model, and how can it be implemented in a quasi 1d combustion model for a pulsative combustor ?
Question
To me, a CFD is solve a fluid mechanics problem using mathematical approaches with the help of a computer. In other words, it is like a marriage between a mathematical model and numerical methods for solving a fluid mechanics problem.
According to the above, I ask the following questions and answer what I think:
1). Is a CFD a tool to solve only 3D problems?
According to the definition, No. A CFD is not restricted to dimension.
2). Can any software tool that solves a fluid mechanics problem be considered a CFD?
No. I would say that the mathematical model to be solved has to come at least from a simplification of the Navier-Stokes equations.
3). Based on what we understand as a cfd, please mention the CFD softwares you know. For now, exclude the computational algorithms programmed by you.
In 3D: Ansys Fluent; Ansys CFX; Flow3D; OpenFOAM.
In 2D: Iber; Hec-Ras 2D.
In 1D: EPA Swmm.
Simply CFD relaxes you from a wide variety of coding for fluid dynamics, particularly for general purposes or in the primary steps of design where coming and experimental approaches are time-consuming or expensive to be employed.
Question
- I'm trying to simulate a turbulent flow around an airfoil. I'm using Ansys software. The problem is my concern focus on the near wall region and I want to know which turbulence model is successful in such case?
Hi,
I would suggest you use the K-W SST or K-epsilon model for a near-wall phenomenon. There is nothing called the best turbulence model. No turbulence model is 'universal', each and every turbulence model is having its own advantages and disadvantages however, applicable for specific problems on an individual requirements basis. For more details, you can read my recently published article (uploaded in my Researchgate profile).
Thank you.
-Arnab.
Question
Hello Everyone,
Im performing a CFD study using ANSYS 18.1 on a 3D inverted Ahmed model to investigate the effect of an active underbody rear diffuser (Re > 1.4 e+6), my study was supposed to be performed using a wind tunnel, but due to the corona pandemic, i had to change the method to CFD, which is new to me, so i have some questions if anyone can help.
1- is there a specific rule for the enclosure (domain) dimensions? i made it 10-12 times the model L,H,W.
2- im using the k-omega SST turbulent model as it predicts well near walls, what value for y+ should i aim for? and is there a redcommended limit for the number of inflation layers?
3- how can i perform a local refinement for the area around the model in ANSYS 18.1?
Hello,
Question 1) : This is Ok. These dimensions should be sufficient so that the boundary conditions on the side faces of your domain are not influencing the pressure field near the investigated model (too much).
Question 2) : SST model is the best possible choice for a (U)RANS model. In particular if you study the effect of a diffusor.
Usually one aims for y+ values in the order of y+~1-2.
The number of inflation layers depend on the targeted y+ value, because at the same time you should aim for a smooth mesh transition between the last prism layer (last counted from the wall surface towards the free open volume) and the adjacent tertahedrons in the volume mesh. The change in volume between the outermost prism layer elements and the next following tetrahedral elements should be in the order of 1-5, not larger. Since the prism layers directly at the surface are very thin (small volume) and we need to resolve the profile of the boundary layer at the wall surfaces with approx. 10-15 prism elements, we usually end up with 15-20 prism layers for such a smooth transition. In regions, where walls are in close proximity (e.g. the road surface and the car floor surface) the things might be more squeezed. Consequently their might be either none tetrahedral elements or they are small as well. In this case a slightly smaller number of prism layers might be sufficient.
Question 3) : Largely depends on what mesher do you use. ANSYS Meshing? Fluent Meshing? ICEM/CFD? ANSA?
The usual way is to enclose the car body in a series of enclosed rectangular boxes. One box placed inside of the next slightly larger box. Usually 2-3 boxes are enough. Each box gets its own meshing parameters, so that the most aggressive meshing parameters are gettign assigned to the innermost box. Then a mesh size transition is planned and takes place to the next following box and so forth. By that you end up with a fine mesh in the car's surrounding without transitioning this fine mesh to the all over outer (virtual) wind-tunnel volume and to the area in front of the car, where essentially there is not so much change in the fluid field of motion.
If ever possible I would recommend to use ANSYS 2019.R3 instead of the old 18.x.
Hopefully this helps.
Rgeards,
Dr. Th. Frank.
Question
I'm currently working on a research of thermal-hydraulic performance of artificially roughened pipes using Ansys Fluent.
I have a 2D model of pipe section (upper boundary is wall with rectangular juts which are supposed to be elements of artificial roughness, their height and step are widely varied). I also created a structured mesh in Ansys Mesher. The first layer's height is chosen so y+ is equal to 1 at the highest Reynolds number I'm working with.
The problem is that Fluent does not give any proper results no matter what turbulence model I'm choosing. The heat flux is 2 times lower than in plain pipe, which is physically impossible.
That may be something wrong with the mesh or with the turbulence model settings. Could you help me?
Hi Nikita,
The issue could be many things.
1. Validation: Have you validated the hydrodynamics for a plain pipe to ensure the turbulence model you are using is predicting correct velocities especially near the wall. You can check and compare your velocity profile with analytical results, esp the law of the wall: u+=y+.
2. Grid convergence: As Meisam mentioned you need to make sure your results are grid independent.
3. Convergence: Generally residuals do not give a good indication of the convergence of the solution. As Rajesh mentioned make sure you are monitoring shear stress at wall (for hydrodynamics) or temperature (for heat transfer) when you solve the equations in Fluent.
Once you are sure the above issues are resolved for a plain pipe, then introduce roughness and see the impact. Generally, a pipe is considered rough based on the roughness height and the viscous sub-layer height. Make sure your pipe is indeed rough for a given flow condition.
Hope this helps.
Keep safe!
Question
I am working on the turbulence simulation. The scaled residuals of x, y & z velocity before going upward 1 e-5. The solution seems not to be converging. I am using K-E turbulence model to capture turbulence characteristics. Same issue is occurred in RSM model.
I used under relaxation factors as follows.
1. mass flow rate = 0.5
2. Pressure = 0.1
3. Density = 1
4. Body Forces = 1
5. Momentum= 0.5
6. Turbulent Kinetic Energy = 0.5
7. Turbulent Dissipation Rate = 0.5
8. Turbulent viscosity = 1
SIMPLE scheme is used for pressure coupling velocity, with least square cell based gradient , standard for pressure and all discretization are first order upwind . I hereby attached the sample picture of residual plots.
Kindly suggest what are the possible issues.
First of all improve the quality of the mesh and than run it with different turbulence models
Question
I am trying to calculate friction factor and heat transfer coefficient for flow in pipe, I am using Ansys Fluent as a solver when k-e model was used with 32 as Y+ but after analysis Y+ computed by solver was 23. Same was repeated for with k-w model in which Y+ was initially taken as 0.7 and the computed Y+ was 0.31.
Each time the used and computed Y+ values are different as a result friction factor and heat transfer coefficients don't match with the computed friction factor and heat transfer coefficient from cool-brook and Dittus-Boelter respectively.
Ansys ICEM was used to create geometry and mesh.
what concept I am missing here please guide me.
The question is very interesting. in CFX you can calculate it directly for post process
Question
What the differences between the SST k-omega and LES turbulence models for Pumps ?
The real difference is that LES is NOT a turbulence model but a different formulation of the governing equations based on local filtering of the variable.
That strongly differs from the formulation based in the statistical averaging (RANS/URANS).
The variables that are computed are totally different.
Question
I'm modelling a combustion simulation for a liquid rocket, regarding chemical equilibrium, radiation and gas phase instead liquid phase for propellants. I would like to know what is the best turbulence model for this case.
Question
I am working to simulate single and cavitation model in an axial flow pump can anybody provide me any tutorials in this field please. Thanks
...because this is one of the best validated 2-equation turbulence models with a good balance between accuracy and computational effort. In particular more sensitive to flow separations.
Question
The instantaneous kinetic energy k(t) of a turbulent flow can be categorized to the sum of the mean kinetic energy K and the turbulent kinetic energy k.
Question 1:
How the mean kinetic energy will be applied in engineering?
Question 2:
And for turbulent kinetic energy, it's obviously much more important in instantaneous kinetic energy when we try to understand the engineering principles and catch the effects of turbulence. So, after solving the k-equation, ε-equation along with 6 partial differential equations for Reynolds stresses, should we just focus on turbulent kinetic energy k and ignore the mean kinetic energy K?
Question 3:
The rate of deformation sij(t) can be split into two components as well: a mean Sij and a fluctuating component sij'. The question is elicited from the use of Sij in equations of K and k. Why the rate of destruction of K in the equations for mean kinetic energy K and the rate of production of k in the equation for turbulent kinetic energy k use the same term ρui'uj'*Sij but an opposite operating symbol? Won't that term be neutralized?
I guess the Hamed point is right.
Question
Hello all.
I am simulating a centrifugal pump. Before I started simulating, I ran few test cases on a simple setup to look into the y+. In the test case (which is a simple pipe flow), I could see that the yplus value specified for inflation matches the post-processing results. I am using SST turbulence model with automatic wall treatment.
When I am taking the same yplus to pump, which consists of rotating flows, the yplus fails. Now, as I did the sensitivity analysis using (10-15 layers in the boundary layer), y+ <1 and yplus 20-200 (where SST behaves like k-epsilon),l. However, I could not find the yplus specified for inflation to be matching with that of the post processing results. The difference is atleast an order near the blade walls. Now, I assume that it might be due to the large separation zone in the pressure side. Besides, the effect of y+ variation is not significant to compute the performance for the pumps.
My question is: Has any researcher found yplus value to be fully satisfied in case of turbomachines in CFX? Is it important to verify yplus (for Journal Papers) value even when we know that the wall function is not affecting our parameters of study?
Hi,
from my perspective this is rather logical. The estimates calculated for y+ in the meshing process for specifying the inflation layer parameters are based on correlations for a fully developed turbulent boundary layer. For a long pipe this is a pretty valid assumption, since the flow has enough length along the wall to develop from the inlet boundary conditions to fully turbulent flow conditions, so that after some pipe length the postprocessing y+ is in pretty good agreement with what was used during the generation of the inflation layers in the mesh.
For a more complicated geometry like your centrifugal pump the cord length of the blades of the centrifugal pumps is rather much too short to develop a fully developed turb. boundary layer. Furthermore flow development over the blade surfaces is disturbed by flow separation and so forth. Consequently the underlying assumption of a fully developed turb. boundary layer is violated (for this assumption being taken into account for mesh property estimates) and you end up with differing y+ values in the postprocessing. But the values in the postprocessing are the physically valid values. Consequently you need to carry out a few iterations between mesh generation --> flow simulation --> postprocessing --> mesh generation in order to find good mesh properties and consequently tolerable y+ values. If for example you encounter a wide-spread y+~10 in the first results, than you might to reduce the 1st layer height in the inflation layers by approx. the same factor (10) in order to end up with y+~1 in your next flow simulation in the same place.
And regarding your last question: over wide parts of the blade surfaces it is possible to have reasonable low y+ in the order of 1. But in front stagnation points, where the flow hits the front of a blade or other parts of the geometry it is usually not possible with reasonable efforts to reduce y+ to 1, but this concerns usually only very minor part of the overall surface areas.
Best regards,
Dr. Th. Frank.
Question
Hello Everyone !
It is alway said that SA model is apporopriate for adverse pressure gradients then how come it lacks the ability to accurately predict separation ?
It depends on your simulation's circumstances, for example, input boundary condition should be rechecked.
Question