[cwl6750084]

I appreciate if any person can offer some ideas on the following issues?

I am running an axisymmetric simulations of a nozzle. However, the pressure along a large portion of the axis is always equals to the value I set at the outlet boundary. Does anyone knows how to solve the problem? In particular, the pressure value of the outlet (to the right of the figure) is 2.5 MPa, the inlet pressure is 10 MPa.

Moreover, for some reasons, the values of pressure on the nodes immediately before the outlet BC at much higher (at about 9 MPa), then, it suddenly drops to the boundary value in only a distance of one mesh cell. Does this have anything to do with the weird pressure distribution on the axis? Any idea how to correct these issues?

[vinerm]

Could you confirm if axis is really defined as axis type under boundary condition? It should not be defined as any other type. Furthermore, it should really be aligned with the x-axis to behave like an axis. This is not a requirement for axisymmetric scenario, such as, an annulus, but for the cases that have their domain touching the axis.

[cwl6750084]

Hi,

Thanks for your reply.

Yes, the axis is defined using the axis type and perfectly aligned along the x-axis. There are no nodes lying below the x-axis.

When I plot the pressure contour using cell values, the pressure-field looks continuous. I do not understand the discrepancy. Should the contours from both not be the same? When should I look at node values versus cell values.

Do you think this is related with the suddenly drop of pressure (other other flow variables) at the outlet boundary?

[vinerm]

Fluent calculates everything at cell centers. Values at the nodes are interpolated using gradients. Therefore, there is always a difference. However, that cannot explain what you observed.

Though the details of the mesh show minimum y as 0.0, still why are there two lines near the axis in the image you shared? Or it could be just visual.

[cwl6750084]

The two lines should be just the resolution. For some reason the image downloaded from here looks kind of blur when zoomed in.

I actually exported the ASCII data file and the minimum y-coordinate for each given x-coordinate are actually 0.00000. There are no nodes below the x-axis.

[vinerm]

That's good. Fluent does not run if it detects even a single node on negative y. However, it is not must to have any element lying on x-axis. E.g., if the geometry represents annular region, all nodes will have y > 0 and none with y=0.

Is the solution properly converged then? And if you plot y-velocity, does it show any negative velocity near the axis? As per the pressure field, it should show that. That implies the solution is not fully converged. If that is the case, try using some other numerical scheme.

[cwl6750084]

Hello,

Based on the residual curves, they are all at least 3 orders of magnitude smaller than the initial values. Moreover, when I checked the averaged values at the nozzle exit (the second vertical line from the right in the mesh), they are pretty constant even I ran the simulation for 800000 iterations. That is why I am not sure that this is an issue with not sufficiently converged.

Per you suggestions, it seems that there is slight negative radial velocity at the beginning of the nozzle. But that does not correspond the region where P_axis = P_out.

Is there a general rule on Node Values versus Cell Values. The simulation is about liquid water being evaporated to water vapour. I am treating the vapour as ideal gas as the real gas law does not work.

I am using Coupled scheme with 2nd order Upwind for all variables. This is the only possible scheme for the simulation as anything else would crash.

[vinerm]

If the simulation is multiphase, operating conditions will have a lot of effect. Do check the following

1. Value and direction of gravity. It must be either -9.81 or 9.81 in x-direction. Gravity cannot be in y-direction for axisymmetric case.

2. Reference location for the operating pressure should be the highest point in the domain. If gravity is -9.81, then maximum value of x in the domain should be used as reference location and vice-versa.

3. Operating density should be the density of the gas phase.

[cwl6750084]

Originally Posted by vinerm

If the simulation is multiphase, operating conditions will have a lot of effect. Do check the following

1. Value and direction of gravity. It must be either -9.81 or 9.81 in x-direction. Gravity cannot be in y-direction for axisymmetric case.

2. Reference location for the operating pressure should be the highest point in the domain. If gravity is -9.81, then maximum value of x in the domain should be used as reference location and vice-versa.

3. Operating density should be the density of the gas phase.

I used 9.81 for gravity in the position x-direction and the minimum value of x (inlet) for operating condition. However, I used 0 for the operating condition per the instruction in Fluent for compressible phase (water vapour). It seems that the pressure field does not match the outlet BC because the domain is not long enough, though I do not know why - as I thought the boundaries are always matched.

However, the nodal pressure along the axis are still very low (almost equals to the outlet pressure and I am not sure what else can alter that).

[vinerm]

If you are using ideal or real gas, then operating density as well as operating pressure, both should be set to 0. And the pressure at the outlet should have some positive value.

[cwl6750084]

Originally Posted by vinerm

If you are using ideal or real gas, then operating density as well as operating pressure, both should be set to 0. And the pressure at the outlet should have some positive value.

Yes, I have been using both as zeroes for both operation density and operation pressure.

The value at the outlet boundary, for some reasons, will not match when I turn on the phase change (evaporation from water to steam). When I run single phase simulation (i.e. without evaporation), the values at both ends match well.

For multiphase calculation, the outlet boundary value will only match if the mesh is very long.

Does Fluent treat single phase and multiphase calculations differently?

[vinerm]

I am sorry, I could not understand what you mean by the statement

The value at the outlet boundary, for some reasons, will not match

Which boundaries are you comparing for matching the pressure values?

[cwl6750084]

Originally Posted by vinerm

I am sorry, I could not understand what you mean by the statement Which boundaries are you comparing for matching the pressure values?

If you look at the graph for multiphase, the pressure at the right edge of the graph (corresponds to the pressure outlet in the computational domain), the pressures is much higher than the pressure specified at the outlet. When I downloaded the numerical data, the pressure simply dropped from the node right before the outlet boundary to the specified value on the outlet boundary. I do not understand why there is such a discontinuity right before the outler boundary for the multi-phase case.

[duri]

Originally Posted by cwl6750084

I am running an axisymmetric simulations of a nozzle. However, the pressure along a large portion of the axis is always equals to the value I set at the outlet boundary. Does anyone knows how to solve the problem? In particular, the pressure value of the outlet (to the right of the figure) is 2.5 MPa, the inlet pressure is 10 MPa.

Moreover, for some reasons, the values of pressure on the nodes immediately before the outlet BC at much higher (at about 9 MPa), then, it suddenly drops to the boundary value in only a distance of one mesh cell. Does this have anything to do with the weird pressure distribution on the axis? Any idea how to correct these issues?

Try to plot the cell values which is the actual solution. The sudden drop in pressure and probably the strange pressure distribution in axis may be due to interpolation to node values.

The solution indicate the interior zone is ignorant of exit pressure. It probably means supersonic flow condition exist near the outlet condition. There could be other reasons as well but I couldn't guess from the given information. (Mach number plot, solver settings and boundary condition can help) Typically for a CD nozzle when supersonic flow is reached the outlet boundary condition is transferred through boundary layer which helps to produce over expanded condition. But in this case, the picture shows boundary layer ceases to exist after divergent wall. Try to initialize from subsonic solution.

[cwl6750084]

Originally Posted by duri

Try to plot the cell values which is the actual solution. The sudden drop in pressure and probably the strange pressure distribution in axis may be due to interpolation to node values.

The solution indicate the interior zone is ignorant of exit pressure. It probably means supersonic flow condition exist near the outlet condition. There could be other reasons as well but I couldn't guess from the given information. (Mach number plot, solver settings and boundary condition can help) Typically for a CD nozzle when supersonic flow is reached the outlet boundary condition is transferred through boundary layer which helps to produce over expanded condition. But in this case, the picture shows boundary layer ceases to exist after divergent wall. Try to initialize from subsonic solution.

Thank you for the very insightful comment. Actually, the flow should be subsonic throughout the nozzle, the maximum velocity is only 270 m/s and the temperature is over 500 K. The sonic speed for steam is over 500 m/s at that temperature and even higher for liquid water. (I could not figure out how to define the sonic speed for two-phase flow.)

What did you mean by "initialize from subsonic solution"?