[Aurora23]

Dear all,

I am doing a transient compressible flow in Fluent. I am using user defined real gas. Geometry has one Inlet and three outlets. The solver is density based. The formulation is Implicit

For all boundary conditions I have defined transient profiles, for static pressure and static temperature (as a result of experimental data).
Transient BC-s for Outlet1 and Outlet2 are the same.

one example of the profile:
((static_pressure_inlet transient 10 0)
(time
0.0001
0.0002
0.0003
0.0004
0.0005
0.0006
0.0007
0.0008
0.0009
0.001
)
(spi
4089179.75
4020958
3953923.5
3888054
3823323.5
3759711.25
3697189.75
3635747.25
3575362
3516014.75
)
)

Question1:

I have tried first to do a steady simulation as a initial condition, then changed to transient, and then changed boundary conditions to be profiles and started calculation again. Results show that in the calculation the profiles were not used. So I figured that before the transient calcilation I have to INITIALIZE the solution again, BUT in that case I guess that the steady solution is no longer used as an Initial.
If someone could clarify this it would be very useful. Is this some kind of limitation, and what should I do to overcome it?

Question2:

All the time I have been using STANDARD inicialization----compute from----all zones.
What kind of inicialization in this case would be the best? Hybrid or Standard, and what kind of Standard?

Question3:

Even when I initialize solution before transient calculation, and compute, ony few profiles are used during the simulation. Others do not change on the boundary conditions. Is there some reason for this?

For examlple temperature remains at some average value across the whole domain and it should change because of the temperature profiles.

Best regards,

[`e`]

Originally Posted by Aurora23

Question1:

I have tried first to do a steady simulation as a initial condition, then changed to transient, and then changed boundary conditions to be profiles and started calculation again. Results show that in the calculation the profiles were not used. So I figured that before the transient calcilation I have to INITIALIZE the solution again, BUT in that case I guess that the steady solution is no longer used as an Initial.
If someone could clarify this it would be very useful. Is this some kind of limitation, and what should I do to overcome it?

Initialising the domain would reset (initialise) the entire domain; not only the boundaries. Ensure your profile is updated at each iteration from Solve > Run Calculation... > Profile Update Interval: 1. Ensure you have applied your boundary condition from your file from Define > Boundary Conditions...

Originally Posted by Aurora23

Question2:

All the time I have been using STANDARD inicialization----compute from----all zones.
What kind of inicialization in this case would be the best? Hybrid or Standard, and what kind of Standard?

What is the geometry? If your solution is predominately similar to the inlet then use a standard initialisation computed from the inlet; this setting initialises the domain with your inlet conditions. You could solve your simulation in steady state, save the values (File > Interpolate... > Write Data), enable transience and then start with your steady state solution (File > Interpolate... > Read and Interpolate).

Originally Posted by Aurora23

Question3:

Even when I initialize solution before transient calculation, and compute, ony few profiles are used during the simulation. Others do not change on the boundary conditions. Is there some reason for this?

For examlple temperature remains at some average value across the whole domain and it should change because of the temperature profiles.

Are your simulation times greater than your profile time intervals of 0.0001 s? As with Question1: ensure you have applied these profiles correctly in your boundary conditions.

[Aurora23]

Originally Posted by `e`

Initialising the domain would reset (initialise) the entire domain; not only the boundaries. Ensure your profile is updated at each iteration from Solve > Run Calculation... > Profile Update Interval: 1. Ensure you have applied your boundary condition from your file from Define > Boundary Conditions...



What is the geometry? If your solution is predominately similar to the inlet then use a standard initialisation computed from the inlet; this setting initialises the domain with your inlet conditions. You could solve your simulation in steady state, save the values (File > Interpolate... > Write Data), enable transience and then start with your steady state solution (File > Interpolate... > Read and Interpolate).



Are your simulation times greater than your profile time intervals of 0.0001 s? As with Question1: ensure you have applied these profiles correctly in your boundary conditions.

First of all thank you very much for your reply.

Reading Iterpolated steady solution helped me to initialize after applying transient profiles, and before strarting transient calculation.

I checked everything else you mentioned and it is ok.

For example:
time stem is 5e-6
number of time steps: 200
max iter/time step: 10

Also my geometry has a lot of curves.

Question1:

I still get the following:
Pressure profiles are obtained during the calculation (I track them on surface monitor--Area wighted average--static pressure)
BUT the static temperature profiles on inlet and three outlets has some irregular change, as you cam see on one of the attached pictures.
Is that because it is not possible to obtain wanted temperature on boundarys because of the backflow condition boundary.
Maybe because the flow is too fast this happens.
I was wondering is there any other way to obtain these boundary temperatures with some other boundary condition?

I repeat, my boundary conditions are pressure inlet, and pressure outlets.
I don't know if target mass flow would help because this is a compressible transonic flow?

Question2:

As you can see on the pictures for the first 200 iterations there is no change in the profile. Is there a solution for that?
Should I define in the profile the time 0 zero also?





http://imgur.com/EunIizU



http://imgur.com/NSITMoL