Dear all,

I am using CFX5.6 I have some sub domains in my problem where I specify momentum resistance terms, (pressure drop)

When I look at the results in post I do have the problem that the velocities in the sub domain are higher than they should be, meaning that the average does not fit with the correct mass flow. (it is not transient or compressible). Everywhere else, but the subdomain, are the average velocity correct. What is wrong? Thanks in advance Jens

Hi Jens,

Do you have recirculation in the subdomain?

-Robin

Thanks for your reply Robin,

No I do not have a recirculation in my domain. The pressure resistance is so high that I almost have a plug flow.

I have made a very simple test, where I have like a square duct

9 meter long, 1 meter 1 high. After 4 meter a have a sub domain on 1 meter. The inlet is a plug flow and the resistance in the subdomain corresponds to a pressure drop on 4 times the dynamic pressure.

I have tried different ways, 1 solid that covers the total domain and then the subdomain. and also using 3 solids and the subdomain, in this case is one of the solids the same as the "sub" solid.

I can in any case calculate a higher average velocity in the subdomain. The funny thing is also I can not calculate any value on a plane that lies on the face of the subdomain. Another funny thing is also when I look at the density, then it has the same value until the subdomain where it changes. The change is only very little, say from 1.26 to 1.255 and is not enough to explain the difference in the velocity. The average velocity calculated in the subdomain is also sensitive to the quadratic resistance coefficient I use.

Regards Jens

Are you trying to model flow through porous media with the geometry similar to what Gartling did in his paper?

I did the same thing while back and had some weird problems as well but as far as I remember it wasn't average velocity and my problem was in the pressure profile along the domain which wasn't similar to Gartling's case.

I will see if I can find my files on plug flow domain. Amir

Hi Jens,

Try forcing GGI connections at the interface to your subdomain. This will give you mass flows on the regions you are looking for, and will also correct some of the numerical problems which can occur when a 1:1 interface is used to connect a porous region (if you run CFX-5.7.1, the solver will do this automatically).

Regards, Robin

Hi Robin, Thanks for your help.

I assume that means I will have to split my main domian into smaller domain . I have tried your solution for the simple case with 3 solids and one in the centre. In pre I define domain interfaces on each side of the sub domain.

Even when I do this it looks strange. I have calculated the areAve on each domain interface and on inlet and outlet;

inlet,domain interface 1 side 1, domain interface 1 side 2, domain interface 2 side 1,domain interface 2 side 2

and get the following velocity area averaged 0.999182, 1.01522,0.999396,1.07884,1.0288,0.999382

That is a large variation, on one of the interfaces is the velocity around 8% above average

I will investigate this further, there must be a reason for why I have this problem.

I am happy that this have been solved in 5.7.1 Regards Jens

The area average won't necessarily be the same. How do the mass flows and volume flows compare?

-Robin

Hi Guys,

this is likely due to the treatment of the Rhie Chow pressure redistribution terms. You may or may not have heard of the issue but basically when using the Rhie Chow pressure redistribution there are 2 velocity fields:

1. The advected velocity field which is represented by the nodal velocites that you are looking at.

2. The advecting (also sometimes called the mass carrying) velocity field

The later will be conservative everyhwere and is what you use when you calculate mass flows on faces.

The two differ by a term which is proportional to grid size^3 * a pressure term. This is normally a very small term and reduces rapidly with grid refinement. Howver when you have large momentum sinks this can be significant. You can find a detailed explaination of this in the CFX-4.3 solver manual around equation: 3-641.

I am not exactly sure how this is handled in CFX-5.6 so you may want to look in the doc for the Rhie Chow treatments. There also are usually some expert parameters that you can use to improve the behaviour around momentum sinks. Regardless, you should try refining the mesh and see if the discrepancy goes with h^3...let us know what you find.

Best Regards,

Bak_Flow