[Deranda]

Hello,

Im working on a cyclone separator including an additional filter. So i want to simplify the filter as an isotropic porous medium. Now i have to define the inertial and viscous resistance, but I dont have a clue how to do this.

I have two measurements of pressuredrop on different volume flows to determine the coefficients.

Is it the right way to start like this

dp/d = Rv*v+Ri*v^2
dpressuredrop
d:filter thickness
v: velocity (volumeflow per area)
Rv: Viscous Resistance Coefficient
Ri: Inertial Resistance Coeddicient

does anyone knows how to do that?
Thanks a lot

[triple_r]

That's right, however, just using two measurements is not going to give you very accurate estimates of Rv and Ri.

You can fit a parabolic equation to three points (origin, and your two measurements) but this assumes there was no noise in your measurements. The more data points you have the more accurate values you get for Rv and Ri are going to be.

Also, if the two measurements are in the linear regime (Darcy regime) and your application is for low velocities, then it is better if you fit a linear equation to the two measurements (make sure that the fitted line has a zero intercept, so in form of y=mx and not y=mx+b) to find Rv and set Ri to 0. But use this only if your application is low velocity, and flow is in Darcy regime and not Forscheimer.

[Deranda]

tank u for your quick replay,

I've only got these two measurements, so I will try to work with them. Maybe with a linear relation.
Thank you

[triple_r]

Do you happen to have some information on the structure of the filter? For example, what is the porosity? Is it made of fibers? or fused particulates? If you have some of these information, you can use a correlation like Ergun's equation (https://en.wikipedia.org/wiki/Ergun_equation look under the "extension" section). It can at least give you an estimate, a value to compare to and start your simulation.

[Deranda]

Hey thanks,

I only have those measurement I named before.
The media should only drop the pressure... nothing more, so I'm happy with it now, it's working

[Rayman]

Originally Posted by triple_r

That's right, however, just using two measurements is not going to give you very accurate estimates of Rv and Ri.

You can fit a parabolic equation to three points (origin, and your two measurements) but this assumes there was no noise in your measurements. The more data points you have the more accurate values you get for Rv and Ri are going to be.

Also, if the two measurements are in the linear regime (Darcy regime) and your application is for low velocities, then it is better if you fit a linear equation to the two measurements (make sure that the fitted line has a zero intercept, so in form of y=mx and not y=mx+b) to find Rv and set Ri to 0. But use this only if your application is low velocity, and flow is in Darcy regime and not Forscheimer.

Dear Reza

I have a porous cylindrical rock saturated with gas under pressure 2185 psi. Outside the cylinder is gas with the same pressure at time zero. As time passes, the pressure outside the cylinder is reducing with time. I wanna see how the pressure inside changes. Where should I put the inlet and outlet surfaces? The outlet surface should look like a cylindrical layer around the cylinder? The How can I convert porosity 2% and permeability 0.016 Milli Darcy to fluent?

[triple_r]

Hi Ray,

Unfortunately, I don't have access to FLUENT, so I can't help you on the details. However, from FLUENT's user guide, it seems that the required viscous and inertial loss coefficients (D and C) are used as:



So, looking at that, the viscous coefficient should be the inverse of permeability (mind the units though, if you are using SI, then you need to convert from milliDarcy to m^2, which means multiplying by ~9.869e-10). You can set C to be zero if the flow is going to be "slow", otherwise you need to either measure it or use some correlation to find it.

FLUENT will also ask for porosity directly, so you can just use the 0.02 value that you mentioned.

With regard to boundary conditions, there is no inlet in your case, just one outlet which is going to be a cylinder bigger than the rock itself but large enough to make sure the boundary condition doesn't change your solution. Also, if everything is cylindrical, you can probably use an axisymmetric solution and model it as a 2.5D problem instead of the full 3D :-)

good luck

[Rayman]

Dear Reza

First I appreciate your reply and guidelines. I have still some small questions:
1) When I am inserting the D or viscous resistance coefficients in Cell Zone Cinditions, should I put these values for which Directions for my case i.e. direction 1 and direction 2? (In my case I have only radial from from inside the cylinder radiallt out).
2) In my case, in Cell Zone Conditions, there is place to tick Conical. Should I do that? When I do, the Direction 1 vector becomes 1, 0, 0 respectively for x, y, z and for point on cone axis, 39.37, 0,0 respectively for x, y, z. The 39.37 seems unusual to me! For my case, the cylinder cross section is in xz plane and the height is in y direction. Generally, I am confused by Direction 1, 2 and 3. Are these x, yand z?
3) You mentioned the value for porosity is asked. Where is it? Is it near the end of Cell Zone Conditions after clicking on prous zone (Fluid Porosity)? I think this should be 1 alwaus. Am I wrong? I guess I saw that in one porous media tutorial.
4) As I said, the outside pressure and inside pressure inside porous cylinder is zero in time zero. But then timing starts the outside pressure reduces with time and radial flow starts from inside out of cylinder. I know the function of outside pressure with time (2180 psi decrease in 10 hrs), do you think I should write a UDF or there is simpler way. The temerature is decreasing with time.
5) Do you think in this application, gravity should be consideted? Do you think thermal issue should be considered based on low temperature decreases of only 80 degrees farenheit.
Many thanks. You may later email me with rahman.ashena.313@gmail.com if possible.

Best, Rahman

[Rayman]

When I put 273 kelvin temperature as operating temperature in Cell Zobe Conditions, then if the outlet temperature is 310 kelvin, should I put 310 minus 273 equal to 37 ?

[Rayman]

How can I make it axisymmetric?

[triple_r]

This is getting too detailed for what I can remember from using FLUENT over 4-5 years ago, so I suggest taking these with a grain of salt :-)

1. There should be an option in FLUENT to let you specify an isotropic tensor for D and C, which is just a scalar, so you don't have to worry about the directions. I would assume the three directions will depend on the coordinate system that you are using (Cartesian: x, y, and z. Cylindrical: r, theta, z. ...)

2. Unfortunately don't remember what "conical" does :-(

3. It should be "cell zone porosity" not "fluid porosity" (if I remember correctly), so it might be in later menus when you specify the cell zone to be porous. FLUENT will need to know porosity to calculate correct velocity from superficial velocity, and to account for correct mass balance between inside and outside the porous media. Is the porous media tutorial that you are talking about available online? or is it from FLUENT's tutorial guide?

4. Do you know how to create a profile file for FLUENT? That should be a lot easier than writing a UDF. Something like:

((pressprofile transient 2 0)
(time 0 36000)
(p 1.503e7 0))

should do it.
The first line says this is a profile called "pressprofile", is a transient boundary profile data, has "2" data points, and is not periodic.
The second line says there are two values for time "0" and "36000" which are 0 and 10 hours in SI units (seconds).
The third line says the corresponding pressure values for the boundary are 1.503e7Pa ( = 2180psi) for the first time point in the data, and 0Pa for the second time point. This assumes these are gauge pressure values from the lowest pressure in your solution (atmospheric pressure, for example), if that is not the case change the profile to match what you need.

Again, check the actual format and how to load the profile and apply it to a boundary condition, I'm relying too much on my memory and internet :-)

5. To model this problem, you have to at least use an ideal gas model (if not a real gas), so you have to include energy equation in it (even if you want to model a isothermal process, you have to have a compressible fluid model, otherwise the mass balance won't be satisfied no matter how hard FLUENT works on it). With regard to gravity, depends on the height of the cylinder, but because the fluid is a gas (even under this much pressure, density should be low) I don't think you need to include gravity, but check it against the size of the problem, and your intuition for sure :-)

6. Temperature is always "absolute" and never "gauge" or "relative" for compressible fluids, so the boundary condition should be 310K (if you are using Kelvin as the units). Even if the fluid was incompressible, you should always use consistent units and use (273 and 310) or (0 and 37).

7. In FLUENT, you can model a problem as axisymmetric if you take the x axis (if I remember correctly) to be your axis of symmetry and have your geometry be on the x-y plane (no parts of the geometry should be in negative y half of the x-y plane). So, if you create a rectangle with one side on x axis (height of the cylinder) and the other side on positive y axis (radius of the cylinder), then if you tell FLUENT that this is an axisymmetric model (you need to set the dimensions to 2D not 3D to have the option of selecting axisymmetry) FLUENT will solve the problem as if there was a cylinder. This will make the problem run faster. I think there is an option for axisymmetry with swirl as well, that you can ignore unless the cylinder that you are studying is also rotating :-)

I hope these answer your questions. But again, check these with others and with FLUENT's user/tutorial/theory guide, as I didn't (and still don't) have access to FLUENT for over 4 years.

Good luck.

[Rayman]

No Dear Reza, I do not know how to write profile files. I tried, but should I write in excel? I do not know why my excel has a problem to connect to fluent?! Can you help me?

Dear Reza, you are good help, however do you know someone with more recent experience here in cfd-online? Thank you.

About gravity, the size of problem is not big. It is a cylinder of 4 inch diameter and 54 inch length. Now, do you think I should consider gravity based on your past experience?

[Rayman]

The excel can get connected now, but the first thing I should know is where I should type the below and then what to do:

((pressprofile transient 2 0)
(time 0 36000)
(p 0.503e7 0))

[triple_r]

As far as I can remember, you should put that into a file (a text file), and then load it as a profile. When you load the profile file, then you can select the profile in the appropriate boundary condition. This is very vague, I know, but I haven't used FLUENT for a very long time now, and just don't remember the exact steps. I would suggest asking about this in FLUENT forum :-( Sorry.