[akash_max]

Hi All,

I am new to this domain. I have started recently working upon Ansys CFX. I appreciate if you all could help me out in clarifying my doubts.

I am trying to simulate the flow in a injector control volume. I have a inlet and outlet too. I model, mesh and give boundary condition as inlet and outlet. Now when I give a solve I get a message “ A wall has been placed at the outlet and try using opening boundary condition instead of outlet” and percentage goes upto 56%.

I am trying to solve the problem with cavitation and do follow the best practices as described in Ansys documentation.

Kindly let me know why there is problem when I use outlet as I tried refining my mesh size, down sizing my outlet length, solving without cavitation and then with cavitation and changing time step.

As using opening boundary solves my problem as the residuals are below RMS < 1e-6 and imbalances also reach to zero.

Will there be lot of difference in the results, as the results for viscor volume fraction, pressure and velocity are almost the same.

Kindly adive me on this.

Best Regards
Akash

[Graham81]

Dear Akash,

What is happening is the following:

There is a recirculating flow pattern across your outlet boundary. This conflicts with the uniform outward velocity you have prescribed on that boundary. CFX warns you that it is preventing flow inward (the recirculating part), by placing walls.

The best advise I can give you is to consider the importance of the outlet region to your simulation. Does it affect the macroscopic parameters you are after? Do you need detailled information on the flow in the outlet region? If so, you should place your outlet boundary condition away from the recirculating region. If not, the easy fix is use an opening.

Best regards,

Pieter

[akash_max]

Originally Posted by Graham81

Dear Akash,

What is happening is the following:

There is a recirculating flow pattern across your outlet boundary. This conflicts with the uniform outward velocity you have prescribed on that boundary. CFX warns you that it is preventing flow inward (the recirculating part), by placing walls.

The best advise I can give you is to consider the importance of the outlet region to your simulation. Does it affect the macroscopic parameters you are after? Do you need detailled information on the flow in the outlet region? If so, you should place your outlet boundary condition away from the recirculating region. If not, the easy fix is use an opening.

Best regards,

Pieter

Dear Pieter,

Thanks a lot for your kind response.

This would really help me lot. I am not much interested in the outward flow. I only concerned about the vapor fraction, which goes up as the wall percentage goes up.

I am specifying total pressure as 350bar at inlet boundary condition
I am specifying operating pressure as 0 bar at opening boundary condition.

Kindly let me know are these boundary conditions right or wrong.

Please correct me if I am wrong?

Regards
Akash

[Graham81]

Dear Akash,

if I understand correctly, the parameter you are after (vapor fraction) changes with the percentage of the outlet surface that is blocked by the solver to prevent the conflict above.

Specifying an opening boundary condition does not solve the fact that your boundary condtition at the outlet is ill-posed. I would suggest to extend your domain and place an outlet condition downstream from the recirculating region, far enough to prevent recirculation through the outlet condition.

Hope this helps,

Pieter

[akash_max]

Dear Pieter,

Thanks alot, I extended the domain at outlet and placed a outlet boundary condition and solved without cavitation first and then switched on the cavitation model. I model worked fine. There was no problem of recirculation and wall problems during solving.

Thanks for your kind response and help.

Best Regards
Akash A V

[Doginal]

Hello akash

Glad to see you got this working. As Pieter the first thing i would try is extending the domain to further downstream. If you are having flow inward at your outlet then even if your just looking at a specified control volume, the flow downstream from the control volume still has a large impact of what is happening in the CV.

As for the differences between an outlet boundary condition vs. an opening. From my understanding the differences stem from the solver equations. An Outlet is just a simplified version of an Opening. In the solver equations, an Outlet is simplified by assuming there is no inflow at that boundary. This allows the solver to reduce the number of terms it has to solve thus reducing computational demand.
An opening condition can be used in place of an outlet at any time. However it required more computational power to solve.
The other issue to worry about when solving using an opening boundary condition is the type of opening. Many of the options (including the default) use the assumption that the flow into the domain at that boundary is normal to the boundary. If this may not be the case (flow comes in at an unknown angle) then an Opening such as Entrainment may be preferred.

If i'm wrong in anything i said above please correct me.

Thank You,

DM

[Super Sonic]

Hi all,

may I aske you a question about a relevant issue. I have ANSYS 12 and in CFX I want to specify an opening boundary condition.Can some one please help me and specify me exaclty were I can choose that condition.

Thanks

[Graham81]

Basic Settings >> Boundary Type >> Opening

[Super Sonic]

Thank you very much for the advice, but now there is another issue. I run it in a transient state and after the first loop the solver stop and it's writing an error of overflow.So what about that now?

If you need any further information just let me know.

[Graham81]

Most likely its diverging because of your choice of boundary conditions. Can you state your problem setup?