domain imbalance for enrgy equation
Hi all,,
the below is the last iteration of my simulation for buoyancydriven flow. I can see the domain imbalance for the NS equation and mass equation is nearly zero; however, for Heat equation is 0.0418 %. Do you this is quite enough? I can found that imbalnce of energy equations at interair and top boundaries is higher than other boundaries. I tried to refine the mesh over there, but still have high values. Do you think that can cause problem within my results? so to solve the problem how can I treat with this problem, Please? Any comments will be appreciated. Regards CFX user ****************** ================================================== ==================== OUTER LOOP ITERATION = 1529 CPU SECONDS = 1.932E+05   Equation  Rate  RMS Res  Max Res  Linear Solution  ++++++  UMom  1.00  8.8E06  4.9E04  4.7E04 OK  VMom  1.00  1.0E05  4.9E04  3.2E04 OK  WMom  1.00  9.1E06  8.9E04  4.7E04 OK  PMass  0.73  1.8E09  8.1E07  4.8 9.4E02 OK ++++++  HEnergy  0.42  2.7E08  1.2E05  5.6 3.9E04 OK ++++++  KTurbKE  1.00  5.1E07  3.1E05  5.6 1.2E05 OK  OTurbFreq  0.65  6.8E09  8.3E07  7.8 1.9E05 OK ++++++ CFD Solver finished: Tue Sep 4 04:01:52 2012 CFD Solver wall clock seconds: 5.3389E+04 ================================================== ==================== Termination and Interrupt Condition Summary ================================================== ==================== CFD Solver: All target criteria reached (Equation residuals AND global imbalances) ================================================== ==================== Boundary Flow and Total Source Term Summary ================================================== ==================== ++  UMom  ++ Boundary : back 5.8039E+03 Boundary : bottom 1.8993E06 Boundary : chimney walls 1.1411E03 Boundary : front 5.8039E+03 Boundary : inletair 1.0861E07 Boundary : left 7.7466E04 Boundary : right 4.4811E05 Boundary : top 8.2928E04  Domain Imbalance : 7.7249E04 Domain Imbalance, in %: 0.0000 % ++  VMom  ++ Boundary : back 1.9882E02 Boundary : bottom 2.5480E02 Boundary : chimney walls 2.3605E01 Boundary : front 1.9764E02 Boundary : inletair 1.2138E03 Boundary : left 2.0296E02 Boundary : right 2.0737E02 Boundary : top 1.1605E+04 Domain Src (Neg) : room 1.1605E+04  Domain Imbalance : 1.2969E02 Domain Imbalance, in %: 0.0001 % ++  WMom  ++ Boundary : back 8.3537E04 Boundary : bottom 2.9684E06 Boundary : chimney walls 1.2648E03 Boundary : front 6.9932E04 Boundary : inletair 1.7835E07 Boundary : left 5.8039E+03 Boundary : right 5.8039E+03 Boundary : top 1.5814E03  Domain Imbalance : 5.8874E04 Domain Imbalance, in %: 0.0000 % ++  PMass  ++ Boundary : back 1.2765E+00 Boundary : front 1.2474E+00 Boundary : inletair 6.2579E04 Boundary : left 1.2757E+00 Boundary : right 1.2716E+00 Boundary : top 5.0718E+00  Domain Imbalance : 1.9602E06 Domain Imbalance, in %: 0.0000 % ++  HEnergy  ++ Boundary : back 1.2937E02 Boundary : front 1.2638E02 Boundary : inletair 8.3896E+02 Boundary : left 1.2930E02 Boundary : right 1.2885E02 Boundary : top 8.3926E+02 Domain Src (Pos) : room 1.6441E03  Domain Imbalance : 3.5057E01 Domain Imbalance, in %: 0.0418 % ********************** 
Have you double checked your boundary conditions? Any source terms? Is this a transient or steady state case?
Give us more information of what you're doing and how are you modeling it. 
For most applications you have achieved a tight convergence. But to check you are OK in your case you should do a sensitivity analysis. Do a simulation with tighter and looser convergence and see the difference in parameters of importance to you. When it converges to an accuracy you are happy with then you know you have adequately converged.

more information
Quote:
I did not have any source for heat or momentum. I'm sure. my simulation is steadt state. Tin at inetrair=1300C and the top is opening with atmospheric pressure. left, right,front, and back B.Cs is opening with atmospheric pressure. my modeling is about flow driven by buoyancy. so what you think, is it enough? I'm asking because when I did mesh independence study, my intersted variable in some importnat region can not reach constant value or at least the variation is less than 1%. This has killed me, I can get any progress through my research. so that I'm asking enrgy imbalnec may cause this problem. thanks in advance. regards CFD user 
SST model&adiabatic wall
Hi again
does the model can cause the problem? By the way, I modeled the fluid region only and I considered the walls as adiabatic as well. any help will be great. 
You say you do not have a source term but it states you do in your energy imbalance???
fluctuations of 1% are pretty small for a buoyant flow problem as they sometimes do not have steady state solutions, 0.04% imbalance would be pretty damn good, but you should have set the reference enthalpy closer to your inlet conditions, or average conditions. You can see from looking at the numbers, your inlet and outlet enthalpies are very high compared to the rest of the boundaries, so this energy imbalance is divided by a very inflated number due to the enthalpy being so high. 
I just reread you original post, those are not the energy imbalance at the boundaries, that is the total energy going in/out of those boundaries. It is very high because your reference enthaly is probably at 20 deg C, not at 1300. Those being really high does not mean it is is imbalanced there.

Quote:
my fluid is air and my ave temp is 662.5 C. air=O2+N2. As well I went threough the CFX help, it report that: " he reference specific enthalpy is the enthalpy of formation at the specified Reference Pressure and Reference Temperature (often 1 atm, 25°C). The reference specific entropy is also evaluated at the specified reference pressure and temperature." the heat of formation of air is arount 162 cal/g entropy=162/1573=0.103 cal/ gm.K Regards 
Quote:
Do you expect that my results will change too much when I change myrefernce temp and enthalpy? Regards CFX user 
No the results should not change, just pointing out why they are high, and telling you those values are not imbalances, just the amount of total enthalpy traveling through those boundaries, which is based off the enthalpy at your reference enthalpy point plus the specific heat *difference in temperature from that reference point.
If you change this reference enthalpy now and try to continue iterating from your current solution, it will probably diverge, so I would not recommend changing it now. 
no heat source
Quote:
could U plz tell me where it states you do in your energy imbalance. Regards CFX user 
Not sure on this, I actually thought source terms didn't show here, but in you script it says:
Domain Src (Pos) : room 1.6441E03 
more information.
Hi Erik,,
I used T ref=25C and reference enthalpy=0 J/Kg& ref. enthropy=0 J/Kg.K; but now my Tref=662.5C, ref. enthalpy=681.78 kJ/kg & ref. enthropy= 728.67 J/kg. K. is it correct? or I should remain ref. enthalpy &enthropy=0 because it is reference point? I start calculating from the beginning. my residual is going to convergence. I should mention that i have inlet; however, I did not specify outlet where I set the top as opening with entrenment option for opening pressure. the problem was also at the top of my domain. Any comment could be helpful. regards CFX 
You are confusing me now.....
I was just trying to explain that it is not a problem. It is not an imbalance. It doesn't matter what the value is, its arbitrarily based off the reference point and reference enthalpy. Whatever you set it to shouldn't matter other than giving you different values in your enthalpy boundaries and changing you energy imbalance percentage. It shouldn't affect results. The large values at those two boundaries are not a problem. 
Quote:
you are right. Regards 
All times are GMT 4. The time now is 12:59. 