total pressure dynamic pressure static pressure
 

my operating pressure is 101325 (atm).

I am simulating a two-phase flow with a pressure inlet.
after initialization and patch
we have the following distribution of dynamic pressure, static pressure and total pressure.
Is total pressure really calculated as the sum of dynamic pressure and static pressure


dynamic pressure= u2/2g*rhou water * g (9.81)=51.2
http://tiebapic.baidu.com/forum/w%3D...03908fc1a0.jpg
static pressure=rhou water g h=approximately 1774 pa
http://tiebapic.baidu.com/forum/w%3D...c378311eb2.jpg
these two are all alright. however, the total pressure has a much smaller magnitude....the maximum is only 185...
http://tiebapic.baidu.com/forum/w%3D...136327cc2b.jpg

Not an apple to apple comparison
 

Hi Rui

Looking at the maximum and minimum is not the right comparison. The cell with the maximum static pressure most likely does not have the maximum dynamic pressure. Addition is done on cell by cell basis. Therefore, you should do the validation on cell by cell basis as well. Write out all the three profiles as ASCII files and then sum up the static and dynamic pressure. If you are satisfied with checking a small sample, then just pick up a few cells and report their static and dynamic pressures and compare against total.

Hi Vinerm Thank you for your reply
I created a line in the middle of the inlet plane
as we can see the plot directly from fluent is still not the sum
http://tiebapic.baidu.com/forum/w%3D...24aa1830f5.jpg
http://tiebapic.baidu.com/forum/w%3D...cb38db3df5.jpg
http://tiebapic.baidu.com/forum/w%3D...16082431f5.jpg

As you suggested, I export the three pressures at the line.... surprisingly, it is the sum of the two pressure now....
http://tiebapic.baidu.com/forum/w%3D...03728de9fc.jpg
I found the weird distribution of pressure at the beginning when I check my results at CFD post....however the same strategy to output the result at the line will not work ....I still get that weird pressure distribution as shown in the figure...
I might have to rerun all the cases and save static pressure and dynamic pressure as well at all the cells for CFDpost....:(

Dynamic pressure is derived not solved
 

Dynamic pressure is a derived variable and not a solved one. You may not need to rerun your simulations if the current ones are converged enough. Dynamic pressure is nothing but kinetic energy per unit volume, i.e., . So, you can use velocity in each cell to calculate it. Rather CFD-Post will do it directly for you.

Yes Vinerm. I checked the velocity distributions, and it looks reasonable. If the streamlines are parallel with each other, we can calculate the static pressure as rhou g h. we can then obtain the total pressure by adding them up. However, my cases involve recirculation zones and the paper I am comparing with only has the effective pressure distribution measured by manometer board. In the previous simulations, I forgot to save additional quantities in the simulations (e.g. dynamic pressure, static pressure), so I only have the total pressure distribution quantities in CFD post. The figures I showed in this thread is only the initial conditions.

So this time I am gonna save more additional quantities to figure out why it is like this..

I still do not understand why it doesn't show as the sum of the two quantities when I plot it directly in Fluent after initialization and patch even though the exported data has the correct magnitude.

Static vs Dynamic
 

It is difficult to get static pressure from the velocity field, however, if you already have total pressure field saved, you can calculate dynamic pressure field and subtract that from total.

Difference you observe, when you plot contours and when exported data is processed, is because exported data is sorted as per coordinates or cell IDs while the contour plots are not. But to verify further, for the case where all three pressure fields are available, you can create a new variable in CFD-Post or a CFF in Fluent that determines dynamic pressure using velocity and another one that is sum of dynamic and static pressure. Compare the contours of these CFF or new variables against contours of total. They should match.

1. All the questions about this thread originate from the situation that I do not have the accurate pressure distribution in CFD-post. In my current results in CFD post, they only show a default "pressure" quantity as shown in the link below, on the left part noting as "standard quantities" (the other three quantities on the right I am saving it in the new simulations). This default saved "pressure", I suppose it is total pressure, which is of the order 100, whereas the data from the experiment and hand calculated data from the hydrostatic situation (in the paper they say the static pressure is close to hydrostatic situation) is of the order 1000. Using a wrong pressure distribution to minus the correct dynamic pressure distribution might not give me static distribution. (I guess I have to rerun the case to output all the three pressures and check on if the static pressure is correct. As the available data in the paper is also hydrostatic pressure). So far the water elevation and velocity seem reasonable.

http://tiebapic.baidu.com/forum/w%3D...094b369a3e.jpg

2. for the second paragraph, "exported data is sorted as per coordinates or cell IDs while the contour plots are not". This might explain why the exported value is accurate. However, I am still confused that even the exported CFDpost "pressure" is incorrect. Maybe because fluent saved the wrong pressure distribution in the .dat file... Yes, I can try to compare using the suggested way to double-check the dynamic pressure.

http://tiebapic.baidu.com/forum/w%3D...12b21bee65.jpg

after running for a few time steps, yes the dynamic pressure can be replaced by rhou u2/ 2...

In CFD-post, dynamic pressure is rhou u2/2, the pressure is static pressure. total pressure represents the sum of the two as highlighted in the figure.


All the problems now are "why I do not have a correct pressure distribution".... the results are off by about 12 times.... I could not figure out where did I go wrong.... I need to think about it now.

thank you Vinerm..

Off in what sense
 

Is it the maximum or the minimum pressure that is off by 12 times? Did you look at averaged values? As long as fluid is incompressible, pressure value does not matter, only its gradient is important.

Hi Vinerm, it is off by every location, not only the max or min, the ratio is not 12 at every location. I really care about this value, because I need to compare it with the pressure measurement on the sidewalls.

"pressure value does not matter, only its gradient is important." could you explain more about this sentence. why the value itself doesn't matter. I can compare the gradient as well, but I don't know how to explain the pressure magnitude difference

What I am doing is a two-phase open channel flow, the set up is pretty close to the experiment. It is not rigid lid simulation anymore.

Now I am thinking is my inlet boundary condition or initial condition is wrong.

First, Fluent works on gauge pressures. Don't forget to add back the operating pressure if you need to.



The value of pressure that resides in the .dat file is the solver pressure. Depending on the solver this may or may not include the hydrostatic component (rho*g*h) and so this may or may not be what you define as "static pressure." Usually, the pressure does not contain the gravity part. However, it's definitely not the total pressure.

1. gauge pressure is good. operating pressure is set to atmospheric pressure as well. What I need is the gauge pressure, which should be the same as the manometer board eliminating the elevation effect, as we also read the piezometric head with reference to atm.

2."solver pressure" part

https://www.afs.enea.it/project/nept...th/node306.htm
I am using VOF with an "open channel" option. The definitions of total pressure and static pressure on this page seem to be what I want them to be.

Importance of reference
 

Pressure value does not matter if the fluids are incompressible. If they are, then density is a function of pressure and the value becomes importance. For any multiphase flow, three things are very-very important.

1. Location of operating pressure. Easiest is to use the highest point of your domain as operating pressure location. If gravity is along z-coordinate, then value of x and y do not matter, however, highest point along z should be given as operating pressure reference location.

2. If gas phase is considered compressible, ensure that operating pressure and density are set to 0. If not, operating pressure can be set to 101325 or any value for that matter. For the operating density, always use the density of the gas.

3. Gravity must be enabled in the right direction.

Reference values are used to determine pressure values and Fluent reports total pressure as sum of static pressure and dynamic pressure. However, the static pressure used in the sub is gauge static pressure.

Thank you Vinerm! It worked...I will come back update more after obtaining the results...:)

1. In the first one, my location is not set to the highest point I am going to correct it. but this is not the main cause.

2.second I did not specify my operating density to be the density of gas: (I suppose that is the main issue)....As the atmosphere (top surface boundary) is chosen to be "pressure outlet", I don't want the gas to be compressible. Though between "Compressive" and" Modified HRIC" for "volume fraction solution method" I kept the default option "compressive". might need to work on this further



<explicit VOF requires a smaller time step compared to implicit> --https://www.cfd-online.com/Forums/fluent/103541-vof-implicit-explicit.html CFD online

<The modified HRIC scheme provides improved accuracy for VOF calculations when compared to QUICK and second-order schemes, and is less computationally expensive than the Geo-Reconstruct scheme.>--fluent manual

< "Compressive" counter-acts the numerical diffusion which would otherwise tend to smearing of the sharp volume fraction gradient at the free surface, and in particular if users cannot afford finely resolved meshes.>--Dr. Th. Frank research gate

In the end, I think "implicit" can save me some time, compressive or Modified HRIC is both suitable for what I expect. (A relatively sharp surface between air and water. Later on, I can locate the water depth in my channel)


Maybe the so-called Immiscible Fluid Model with explicit VOF can give a sharper surface...to look into further


3. this is correctly specified

Good
 

That's good, Rui.

Compressive is default and recommended when using Implicit scheme. You can use implicit if objective is not to predict very sharp interface.

If you wish to predict very sharp interface, use Explicit with Geo-Reconstruct. But you will be bounded by .

If you wish to get 0-thickness interface, then you can use LSM. This method is based on a hyperbolic equation that assigns a distance function and tracks it explicitly instead of reconstructing the interface based on fields like density or volume fraction.

Yes, what I am planning to use is taking 50% of the VF of water as the water surface to compare the experimental data as well.

I will check the influence of coupled LSM+VOF after this patch of simulations...

Maybe turn on the interfacial anti-diffusion as well.
https://ieeexplore.ieee.org/stamp/st...number=7396360

The following pic is what I previously got:
contour of Water volume fraction at a plane

http://tiebapic.baidu.com/forum/w%3D...a1cc112a52.jpg
If the layer is thin enough, I might not need to use the 50% VF of water approximation

Using a test case with a very coarse mesh, the coupled LSM together with interfacial anti diffusion effect seem not to be as good as the paper cited above

LSM and Anti-diffusion
 

LSM and anti-diffusion are two completely different approaches. LSM does not require anti-diffusion since the interface is defined based on the value of a function for which the equation is solved. Function maintains a value, say 0, as the interface moves. Iso-surface of this function with a value of 0 is the interface and it is always sharp. There are other issues with LSM, such as mass loss and maintaining the distance function, however, those are addressed within the tool by adding an equation.

Anti-diffusion is applied to VOF, particularly to Implicit VOF because Geo-Reconstruct is available with Explicit VOF and that is already quite sharp.

Sharp interfaces are desired only when surface effects, such as surface tension, are important because curvature calculation is required for surface force calculation. Curvature prediction are bad if interfaces are not sharp. Therefore, if you do not have surface forces, apart from what is being resolved, such as drag, then you can just look at 0.5 volume fraction iso-surface.

Oh, I see. Then I will stop the interfacial anti-diffusion, which is for the surface tension.
I do not want any mass loss involved, though the 0-thickness surface and the distance function are pretty fascinating

http://tiebapic.baidu.com/forum/w%3D...58cdbf4ea7.jpg
I might understand by mistake the option Coupled Level set+VOF as shown in the photo. That is why I was saying to combine everything. I assume it's a combination of the two.



More importantly, let us go back a little bit to the THREE RULES you suggested in the previous replies

<1. Location of operating pressure. Easiest is to use the highest point of your domain as operating pressure location. If gravity is along z-coordinate, then the value of x and y do not matter, however, the highest point along z should be given as operating pressure reference location.>
Reference Pressure Location: sets the location of the cell whose pressure value is used to adjust the gauge pressure field for incompressible flows that do not involve any pressure boundaries. --FLUENT Manual

For cases that do not have pressure-related boundary conditions (e.g., pressure inlet, pressure outlet, pressure far-field, etc.), you need to specify the Reference Pressure Location at a point in the problem domain. If pressure boundaries are involved, the adjustment is not needed and the reference pressure location is ignored. --FLUENT Manual

Maybe that is the reason why the location doesnot matter to my case as I am using pressure inlet and outlet.


<2. If gas phase is considered compressible, ensure that operating pressure and density are set to 0. If not, operating pressure can be set to 101325 or any value for that matter. For the operating density, always use the density of the gas.>

By default, ANSYS FLUENT will compute the operating density by averaging over all cells. In some cases, you may obtain better results if you explicitly specify the operating density instead of having the solver compute it for you. For example, if you are solving a natural-convection problem with a pressure boundary

Could you please explain a little more why \rho_{\rm0} is set to the density of air... I tried to set it to water. it is very close to what I got at the very beginning.

Depends upon your objective
 

Whether you wish to use combination of LSM with VOF or not is dependent upon what you wish to achieve. Interfacial Anti-Diffusion is not for surface tension rather when surface force like surface tension are required to be involved, it requires accurate calculation of the surface curvature. With anti-diffusion, curvature calculation becomes more accurate, hence, surface tension forces are applied more accurately. If objective is not to predict very sharp interface, then you do not need anti-diffusion algorithm. If you are using Explicit Scheme, then also this is not required. When you combine VOF with LSM, then LSM tracks the interface explicitly. However, Fluent does not have pure LSM, it is combined with VOF and has certain limitations, such as, simulation has to be transient and no transfer of mass is allowed from one phase to the other. You can use the setup that you have shown in the image. However, if you face convergence difficulties, remove coupling of LSM and VOF and run VOF with anti-diffusion.

As far as operating pressure and density are concerned, these are used to off set the round-off error when single phase flow is solved. But for multiphase, they play another role. Buoyancy force is important in multiphase flows and it is the reference density provided by user that is used by Fluent to calculate the buoyancy. If there is no input provided by the user, Fluent uses value that is averaged over whole domain. Since water is quite dense as compared to air and occupies most of the space in your simulation, Fluent will use water density but then the buoyancy force calculation will go wrong. Recommended is to use density of the lightest fluid, which is air in your case.

Yes, if you have a pressure inlet, then it takes it from boundary. However, if you have more than one pressure inlet, then it averages over those. This value is again not useful since this might predict water on top of the air. Therefore, it is always recommended to provided the highest point (since lightest fluid is expected to exist there) as the reference location.

Thank you Vinerm!

I will try a little bit coupled LSM and VOF later on and understand better the suggestions you gave. :)