Mismatch between H-Energy and massFlowInt(Static Enthalpy)
I am using CFX/12.1 and I have observed something which is of a bit of concern.
If I analyse results of my CFX case which is properly converged (to RMS residual of 1e-6 and conservation target of 0.001), I observe this strange mismatch:
1. In the .out file, solver lists the H-energy at the end at various boundaries under the section 'Boundary Flow and Total Source Term Summary'.
2. Now one can also calculate the H-energy flow at boundaries in CFX-Post using the function 'massFlowInt' on the variable 'Static Enthalpy'.
I observe that H-energy at inlet/ outlet boundary as printed in solver .out file is not equal to massFlowInt(Static Enthalpy) at inlet/outlet boundary.
I have taken care to use conservative values only in CFX-Post calculation.
As an example, I got the following values in two cases involving conjugate heat transfer :
Case 1: Simple channel laminar flow, viscous dissipation not included, RMS residual target=1e-6
H-energy from .out file
Boundary : Inlet 1.3883E+01
Boundary : Outlet -7.3882E+01
Values from CFX-Post
massFlowInt(Static Enthalpy) @ Inlet = 14.2419 [W]
massFlowInt(Static Enthalpy) @ Outlet= -80.6939 [W]
Case 2: Laminar Flow through channels and porous medium, viscous dissipation included, RMS residual target = 1e-6, conservation target= 0.001
H-energy from .out file
Boundary : Inlet fluid 5.2444E+01
Boundary : Outlet fluid -8.1517E+01
Values from CFX-Post
massFlowInt(Static Enthalpy) @ Inlet = 52.4475 [W]
massFlowInt(Static Enthalpy) @ Outlet= -81.4848 [W]
So the difference in Case 1 is larger but in case 2 smaller.
Why is this difference at all?
Thanks for your inputs
Presumably this imbalance in inlet and outlet is 0.001 of the total heat so is small. In this case it is just the convergence tolerance. If this is inadequate then define a tighter convergence tolerance.
Thanks Glen for your reply.
Please consider the case of a very simple laminar flow simulation of flow of water through a channel heated from below. As per your suggestion, i reduced conservation target to as low as 1e-6 from 0.001. Still, the difference between H-energy values in .out file for inlet and outlet boundaries and those calculated from CFX post using massFlowInt(Static Enthalpy) @ inlet and outlet is significant. Infact the difference between these values hardly changes as conservation target is reduced from 0.001 to 1e-6 although domain imbalance for H-energy reduces from 0.0006% to 0.0001%.
I am concerned and confused.
It will be great if you could have a look at the .out file for this simulation. I could not upload the other files due to forum limitations. I can send you those files (.res and .def files. size~ 5MB) in case you would like to have a look at them. The difference in values is as below>
| H-Energy-liquid |
Boundary : Inlet -1.8123E+02
Boundary : Outlet 1.3123E+02
Domain Interface : Domain Interface 1 (Side 1) 1.2428E+01
Domain Interface : Domain Interface 2 (Side 1) 1.1982E+01
Domain Interface : Domain Interface 3 (Side 1) 1.2428E+01
Domain Interface : Domain Interface 4 (Side 1) 1.3163E+01
Domain Imbalance : 1.7667E-04
Domain Imbalance, in %: 0.0001 %
massFlowInt(Static Enthalpy) @ inlet = -180.934 [W]
massFlowInt(Static Enthalpy) @ outlet = 125.557 [W]
This is just a test simulation that I ran to confirm the differences between .out file and CFX post values.
The most critical issue here is the following:
Water is flowing through channel which is heated. The net heat flux to channel is 50 W. With a simple control volume analysis, the following balance should hold:
massflow* enthalpy at outlet - massflow*enthalpy at inlet = Total heat input
Now Total heat input = 50 W as I mentioned above.
The solver .out file reports that
H-energy at outlet - H-energy at intlet = 181023-131.23 = 50 W which is good.
However CFX Post calculates:
massFlowInt(Static Enthalpy) @ outlet-massFlowInt(Static Enthalpy) @ inlet 180.934 - 125.557 = 55.377 [W]
So CFX Post shows an imbalance in energy of 5.377 W even when CFX solver shows none !!
Have you looked at the total enthalpy in CFD-Post?
I calculated massFlowInt(Static enthalpy + 0.5*Velocity*Velocity)@ inlet and outlet and it does not change the situation. This is because the kinetic energy contribution is of the order of 1e-5 W only.
Can you repeat this calculation in the current version of CFD-Post?
The above CFX-Post calculations were done in CFX/12.1.
I have repeated the calculations in CFX/13.0 and the result is same :
Mass Flow Integral of Static Enthalpy on Inlet
Mass Flow Integral of Static Enthalpy on Outlet
I think the doc describes how Post calculates these results and explains that they are approximate in some case. Always trust the .out file values. The solver has access to all the integration point data and conservative face fluxes, so it can calculate an accurate value. Depending on exactly what you are calculating, Post will only have access to the nodal data written to the res file, so it simply doesn't have the data needed to perform a conservative calculation. To accurately calculate massFlowInt(Static Enthalpy) I expect you need mass flux data at the faces and enthalpy data at the integration points. Using monitor points and/or Additional Variables is a good way to get the solver to perform post-processing calculations rather than Post.
But CFX Post should be able to give accurate values. The case above has a difference of nearly 10% from .out file which is too much.
Also, in the above case, I found that CFX post calculations for total heat flux on solid boundaries and on all solid-liquid interfaces matched those from .out file. It was only the fluid energy calculation at inlet and outlet that did not match the values from .out file.
In addition mass flow rate at inlet and outlet is also correctly calculated by CFX Post. Now the solver would be providing the nodal enthalpy values in the same way as it provides velocity and density values. Then it seems very strange why mass flow integral of enthalpy should deviate from .out file value inspite of all this info available to CFX Post.
Actually I had contacted Ansys support once for this issue but they never came back with the answer.
My understanding was the CFD-Post used the full integration point data, but I might be wrong.
But it is quite possible you have found a bug specific to mass flow integrals on inlets and outlets. If this is the case the only way you will be able to do anything about it is by contacting support and reporting the issue.
Yes that is also what I think.
However, the case 2 that i mentioned in the first post in this thread does not show as much difference as the simple channel simulation. Dont know if mesh density can have any role to play. Although if the same integration data is available to solver and Post, then the results should be same between solver and Post for any mesh density.
As I said above, I reported this issue to Ansys about a year back. They kept dragging and finally did not answer. I also lost track at that time as from then on I did not have much confidence in CFX Post calculations and I started exporting all data to text files and doing all summations on the exported nodal data externally for evaluating various integrals. We discussed this very recently in the thread: http://www.cfd-online.com/Forums/cfx...rgy-flows.html
But CFX post , if accurate, makes life much easier. One can do all the calculations inside Post and export only the relevant calculated data. For example, doing something like what I mentioned in my other thread (http://www.cfd-online.com/Forums/cfx...ing-plane.html) would be very difficult for non-uniform mesh without using CFX Post functions.
Do you know of any specific person in Ansys support whom I could directly report this issue?
Your local ANSYS support person is the one to speak to. Hopefully if you explain that you may have found a bug in CFX that should get their attention.
In general Post doesn't have access to integration point data. However the solver writes out certain common quantities to the results file to enable accurate calculations in Post. Inlet/outlet mass flows are one of these quantities I believe and heat flows too, hence you get accurate values. Try calculating your own mass flow as areaInt(var)@inlet, where var = Density * <velocity normal to the boundary>. I would guess you get an inaccurate result. This is similar to your enthalpy calculation.
|All times are GMT -4. The time now is 07:07.|