CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Compressible flow modeling in Fluent (http://www.cfd-online.com/Forums/fluent/91356-compressible-flow-modeling-fluent.html)

nikhil August 8, 2011 12:35

Compressible flow modeling in Fluent
 
Hello,

I have few questions on compressible flow modeling in Fluent

1. Can i use velocity inlet and pressure outlet BCs while modeling compressible flow?

2. Can i use pressure based solver to model the compressible flow?

3. I am using velocity inlet, pressure outlet in one of my cases and pressure based solver. However, when i initialize the solution, i am getting this error message

Error:
FLUENT received fatal signal (ACCESS_VIOLATION)
1. Note exact events leading to error.
2. Save case/data under new name.
3. Exit program and restart to continue.
4. Report error to your distributor.
Error Object: #f


can anyone please explain why am i getting such error message and how to overcome it?

Thanks,
Nikhil

Pavlos August 8, 2011 12:55

For questions one and two my answer is YES.
For last one, my oppinion is that mesh might be wrong or type of other BC are wrong.

If Im wrong, correct me.

nikhil August 8, 2011 13:16

Mesh is pretty much simple and without any error.
Its a 2D domain. Therefore apart from inlet and outlet; other two boundaries are walls which are fine from my consideration.

Vijay August 8, 2011 15:55

You cannot have velocity and pressure boundary condiitons in a single domain...I guess

Pavlos August 9, 2011 04:24

My apology. I really thought that velocity inlet can be used for compressible flow but there is a explanation in Fluent manual.

Velocity inlet BC:
"This boundary condition is intended for incompressible flows, and its use in compressible flows will lead to a nonphysical result because it allows stagnation conditions to float to any level. You should also be careful not to place a velocity inlet too close to a solid obstruction, since this could cause the inflow stagnation properties to become highly non-uniform."

Pavlos August 9, 2011 04:30

Quote:

Originally Posted by Vijay (Post 319371)
You cannot have velocity and pressure boundary condiitons in a single domain...I guess

You can easily use velocity and pressure BC in a single domain. There is no problem.


You can use three combinations of BC at the inlet and outlet.
1. Velocity inlet - Outflow
2. Velocity inlet - Pressure outlet
3. Pressure inlet - Pressure outlet


Instead of velocity inlet you can use mass flow inlet too, of course.

Karl August 9, 2011 07:07

For compressible flows only two combinations are valid:

1. Mass Flow Inlet + Pressure Outlet
2. Pressure Inlet + Pressure Outlet

Velocity Inlet and Outflow are incorrect BC's for modeling compressible flows with FLUENT.

Best Regards

Pavlos August 9, 2011 08:57

Quote:

Originally Posted by Karl (Post 319453)
For compressible flows only two combinations are valid:

1. Mass Flow Inlet + Pressure Outlet
2. Pressure Inlet + Pressure Outlet

Velocity Inlet and Outflow are incorrect BC's for modeling compressible flows with FLUENT.

Best Regards


Of course, I mean generally you can use velocity inlet and Outflow, not for case of combressible flows.

Velocity Inlet is incorrect and Outflow is incorrect too for compressible flows.

nikhil August 9, 2011 14:18

Thanks all...

With mass flow inlet and pressure outlet my case is running smoothly.


All times are GMT -4. The time now is 23:05.