Hello!

I am setting a profile data file as an OUTLET boundary condition of velocity in x,y,z. When I go to the post, I realized the velocity has changed throuhg the simulation.

I monitored some points in the outlet and it changes the values i set until it converges.

Can somebody explain why can this happen if it is boundary condition!!

My other B.C are Total pressure in the inlet, Temperature at the inlet and the profile data B.C of velocity in the outlet.

Thanks!!

Mari

Hi Mari,

If you plot the conservative values, they will be different as they represent the control volume values, not the boundary condition. The hybrid values should correspond to your profile.

Enforcing a profile at an outlet is generally bad practice, as the profile will be strongly influenced by the advected conditions upstream. Your profile will probably only have an effect very close to the outlet and will likely result in an uphysical static pressure distribution.

That said, there are other reasons why your profile may look different. What exactly did you set at the outlet. Can you copy the ccl for the outlet to the forum? (tip: put *pre* and */pre* html tags before and after your snippet of CCL. This will preserve the formatting. Replace my *'s with < and >).

Regards, Robin

Hello!

I dont think I am aloud to post the file on the forum. I will have to ask.

I am setting the outlet boundary condition from the results of previous calculations. I need to set the profile, because I need the preserve the direction of the flow in the outlet. I set the Cartetian coordinates in X, Y, Z from the exported file from a previous calculation (*.csv)

The problem is not how it looks in the post. Mainly that when monitoring a point of the outlet BC during the iterations, it changes, it is not kept constant from the data set in the PRE.

Thanks a lot

Hi Maria,

I wasn't actually suggesting you post the profile, just the CCL from Pre (what you get if you right click on the boundary condition and select "Edit in Command Editor". Anyway, I see your problem; monitor points in the solver only report the conservative values.

What you are attempting is still a bit fishy to me. I don't see the practical use of fixing the velocity at the outlet to be the same as a previous solution. It simply isn't physically realistic. Pressure influences travel upstream (assuming Ma<1), but the distribution of velocity or mass flow is advected (unless you are at very low speeds, in which case diffusion plays a larger role).

Regards, Robin

Hi Robin!

You were right about the conservative values. They change, but the hybrid values are kept constant in the boundary conditions.

About your comments of the advection of the velocity and the influence of the pressure upwind:

I set velocity distribution in the outlet because I did a previous simulation with a section of the geometry of a volute including the vanes. In this first simulation I did set pressure in the outlet. From here I took the velocity distribution profile behind the vanes, so I can simulate a bigger section of the geometry without the vanes, wich implies less computation time and requirements.

I also did a simulation taking instead of the velocity, the pressure profile in the outlet, as you suggested, but the velocity in the outlet after the simulation is pretty much different to the one I get with the vanes.

I am calculating pressure drop over the volute, that is my main goal, and setting the velocity direction in the outlet gives a better behaviour of the flow upwind than the pressure distritubion, in comparison with the original simulation with the vanes.

Thank you again for you comments! At least now I am sure that the B.C. in the wall are kept constant, even when I am not really sure why it changes so much in the control volume when looking at the conservative values. I would think they should not be very different than the ones in the nodes of the B.C. If you have any idea of this, I would appreciate your comments!

My best regards!

Mari

Hi Mari,

It is for exactly the reasons that I have stated. The velocity distribution is something that is transported downstream by advection. The only physical processes that can transfer information upstream are pressure and diffusion, so it is entirely sensible that the control volume values are different.

In the control volume equations, the diffusion term includes the velocity gradient, which would be influenced by nodes on the upstream and downstream side of the element. However, the advection term only includes values from upstream nodes (so-called upwind differencing). So the velocity at your boundary only effects the diffusion term and also sets the local mass flow distribution, which influences the pressure.

If you exclude geometry downstream, such as your vanes, you will not get the same results, but I appreciate your reason for doing so. However, I would suggest using a static pressure profile instead. It is static pressure which the upstream flow really feels anyhow. Alternatively, you could create a very coarse mesh around your vanes and GGI it to your outlet boundary. While you may lose some fidelity due to the coarse mesh, it is probably a lot better than your outlet.

Regards, Robin

Hi Mari,

I think that rather than set the outlet boundary condition to enforce the flow turning from your vanes, it might be better to add a body force to the flow equations to achieve this.

I am not a user of CFX and am not exactly sure how one would go about this, but I think that it makes more sense. The body force will be axisymmetric, but so is your outlet boundary condition.

An estimate of the value of the force could be obtained by calculating the force on the vanes. You could then apply it to the calculation, check the flow turning and tune the force as required.

I have never actually done this, but it seems like a reasonable approach.

Good luck!

Thanks Robin!

I set the calculation that you suggested, with a coarse mesh for the vanes and GGI it to the volute. This time, I can set Average Static pressure at the outlet.

I run the simulation with k-epsilon model and the mesh resolution of the volute is very high. But it is not converging to the RMS 1E-4. Instead it stays constant at RMS 4e-3.

I don't know if this has to do with the mesh quality of the vanes at the Fluid to Fluid Interfaces with the volute!

Any suggestions?

Thank you very much!!!

Hi Maria,

On the output control for backup and results there is an option to write the residuals to the results or backup files. I suggest writing them to the backup files then looking at where the residuals are still high. The normalized residuals are still signed, so it is useful to calculate a new variable in Post equal to the absolute value of the residual you are plotting (using the abs() function).

Once you have the abs value, create a Volume object in Post using the isovolume option. Se the volume to show elements where the residual is greater than 1e-3. This will then show you where the convergence difficulty is occurring.

Regards, Robin

Thanks for the suggestion, I will do that!

I have another question back to the hybrid and conservative values. When calculating the Pressure Drop of the volute, I am using the Mass flow average of the conservative values of total pressure at the inlet and the outlet, and calculating the drop in this way. I understand that the conservative values take the average over the control volume at my surface while the hybrid are a calcuated value in the nodes of the surface. But shouldn't be this values in average be similar? When I calculate the pressure drop with conservative values I get a pressure drop 3 times smaller than when using the hybrid values.

Why is such a difference? Any idea.

Thank you very much!