Fluids

Fluids

Wrong pressure results in the shell side of a shell and coil heat exchanger

    • mmoataz
      Subscriber
      When separately simulating each side of a shell and coil heat exchanger, physically correct results are obtained, however, when combining both sides together to simulate the whole system, wrong pressure distribution in the shell side is obtained after convergence!nMy questions are:nHow could the presence of the 2 domains together affect results?nWhat can be done to fix this?nnSummary of used settings:nAll solid and fluid bodies share topology (Conformal mesh)nSolver: Pressure based - CouplednWorking fluid in shell: airnWorking fluid in coils: thermal oil (density 850 kg/m^3, viscosity 590e-06 kg/m-s)nTurbulence model: SSTnBoth fluids mass-flow-inlet and pressure-outlet BCnEach fluid is initialized separatelynDefault methods and controlsnnNote that: nThe same mesh and settings are used when simulating each side separately and when simulating both of them togethernChanging to non-conformal mesh or using SIMPLE pressure-velocity coupling didn't helpn
    • Karthik R
      Administrator
      How are you simulating the combined model? Could you please share some screenshots to help us understand? Please embed them directly into your posts. nThank you.n
    • mmoataz
      Subscriber
      Attached here you can find 3 JPG files,In 1f.JPG you can see the simulation of the shell side only.It shows correct static pressure distribution for air (maximum at inlet and minimum at outlet).n2f.JPG shows the results when the shell and coil sides are simulated together. The thermal oil pressure distribution is correct, however, in 2fRescaled.JPG you can notice how the air pressure distribution becomes incorrect!nI used 2 ways to simulate the combined model:nFirst, by creating a conformal mesh for the whole model including (air, thermal-oil and solids) .nSecond, by creating 2 separate meshes for thermal-oil and air then defining coupled interface between them.nboth ways use the same settings defined in the main post and both of them generate the same problem!nn
    • Rob
      Ansys Employee
      Staff are not permitted to open or download attachments. nIf you check the flow field (other than pressure) is it as expected? n
    • mmoataz
      Subscriber
      No all the results for the air side (not only pressure) totally get incorrect when simulated with the thermal oil side.nI pasted the images again here so that you are able to see it.nPressure distribution for the air side only. Pressure distribution for the whole system scaled for thermal oil pressure.nPressure distribution for the whole system scaled for air side.nn
    • mmoataz
      Subscriber
      I'd like to add some new info that can help fix the problem. Today I tried to change the thermal-oil to air so that both sides are the same fluid and I got correct results, which means that the problem happens only when the 2 materials are not the same.nI guess this is happening due to some sort of averaging that happens between cells of different fluids which is not supposed to happen. I am not sure which fluid property is causing this problem exactly? Is it the large difference in densities between air and thermal-oil? or is it viscosity?nThere must be a way to prevent this from happening. nAny advise?n
    • Rob
      Ansys Employee
      What boundary conditions and density options are you using? n
    • mmoataz
      Subscriber
      In the images I sent in the above posts the energy equation was turned off and the exact settings were:nFor thermal oil:nConstant density 850 kg/m^3nConstant viscosity 590e-6 Pa.snMass flow inlet with 1.0675 kg/s, intermittency=1, k=0.012 m^2/s^2, omega= 80 1/snPressure outlet with 0 bar total pressure, intermittency 1, k=0.015 m^2/s^2, omega=880 1/snFor air:nConstant density 0.5 kg/m^3nConstant viscosity 34e-6 Pa.snMass flow inlet with 0.0113 kg/s, intermittency=0.7, k=0.28 m^2/s^2, omega=2750 1/snPressure outlet with 0 bar total pressure, intermittency 0.5, k=1.5 m^2/s^2, omega=9240 1/snI also tried outflow boundary conditions, its results look nicer but still wrong.nfor the final simulation, the energy equation will be turned on and the density, viscosity, specific heat, conductivity and radiation absorption coefficient will all be calculated by piece-wise polynomials.nI think to solve my problem something needs to be done to separate the solution of continuity and momentum for the 2 fluids and to let them only solved together for energy equation. Is there a way to do so?nOf course temperatures will affect both continuity and momentum by changing all fluid properties but still solutions of these equations must not interfere with one another.nI don't know also if fluent can deal with cases when the residuals for one fluid converge much faster than the other one and if this may cause a problem?n
    • mmoataz
      Subscriber
      So any suggestions?n
    • Karthik R
      Administrator
      Hi, nSorry, I missed your previous response.nTo answer your questions - No, you cannot solve the continuity and momentum equations separately for each fluid. And, for the second question - yes, Fluent should be able to deal with different convergence rates. However, you will only see one single curve for residuals when you solve the two fluids problem.nHaving said that, this is not a multiphase simulation you are running, right (just clarifying)?nAlso, can you show me the convergence plots (residuals and monitor plots) when you run the two simulations together? What is your overall mesh quality (max skewness and minimum orthogonal quality)?nWhat is the Reynolds number in your problem - both oil and air sides?nThanks.nKarthiknn
    • mmoataz
      Subscriber
      Yes this is not a multiphase simulation just 2 different working fluids of a heat exchanger.nOil Reynolds number = 62000nAir Reynolds number is not applicable but the complicated geometry will force the flow to get turbulent or transitional.nnThe mesh quality cannot be the reason behind this problem since the solution converges when each fluid is simulated separately using the same boundary conditions, but anyway here are the values just for your info.nMesh aspect ratio:Max:98, Average:5, Standard Deviation:9nMesh skewness:Max:0.99, Average:0.27, Standard Deviation 0.14nMesh orthogonal quality:Min:9.9e-4, Average:0.7, Standard Deviation:0.14nnI don't have residuals plot because I'm using HPC nodes. Next post you can find a copy of residuals of last few iterations instead. Note in this report the e-mass is a monitor for the air outlet mass flow rate (should reach -0.0113kg/s) and o-vel is the oil outlet velocity (correct value around 1.15m/s). Notice also how reverse flow at the air outlet insists (this doesn't happen when simulating air separately).
    • mmoataz
      Subscriber
      iter continuity x-velocity y-velocity z-velocity k omega intermit retheta e-mass o-vel time/itern 2372 9.2141e-03 2.7577e-05 2.8067e-05 3.6201e-05 4.2041e-03 8.1038e-04 7.7550e-03 1.5072e-05 -1.1524e-02 1.1625e+00 0:01:05 28nn Reversed flow on 119 faces (49.0% area) of pressure-outlet 7.n 2373 1.1360e-02 3.7969e-05 3.8537e-05 4.9860e-05 3.2498e-03 6.5447e-04 1.1625e-02 1.1547e-05 -1.1577e-02 1.1626e+00 0:01:03 27nn Reversed flow on 119 faces (49.0% area) of pressure-outlet 7.n 2374 1.0697e-02 3.2648e-05 3.2890e-05 4.2381e-05 3.7730e-03 6.1632e-04 7.7845e-03 9.1525e-06 -1.1573e-02 1.1626e+00 0:01:00 26nn Reversed flow on 119 faces (49.1% area) of pressure-outlet 7.n 2375 1.1190e-02 3.8597e-05 3.9147e-05 5.4134e-05 3.2822e-03 6.9063e-04 1.2302e-02 1.5363e-05 -1.1655e-02 1.1627e+00 0:00:57 25nn Reversed flow on 119 faces (49.1% area) of pressure-outlet 7.n 2376 1.1125e-02 3.5669e-05 3.5944e-05 4.5598e-05 3.8605e-03 6.4259e-04 7.6449e-03 1.0010e-05 -1.1688e-02 1.1627e+00 0:00:55 24nn Reversed flow on 119 faces (48.8% area) of pressure-outlet 7.n 2377 1.1335e-02 3.9644e-05 4.0187e-05 5.6082e-05 3.2271e-03 6.7429e-04 1.2151e-02 1.5464e-05 -1.1785e-02 1.1628e+00 0:00:53 23nn Reversed flow on 119 faces (48.8% area) of pressure-outlet 7.n 2378 1.1341e-02 3.6850e-05 3.7169e-05 4.7515e-05 3.8157e-03 6.4426e-04 7.5501e-03 1.0847e-05 -1.1787e-02 1.1628e+00 0:00:50 22nn Reversed flow on 119 faces (48.9% area) of pressure-outlet 7.n 2379 1.1491e-02 4.0092e-05 4.0776e-05 5.7011e-05 3.2002e-03 6.6529e-04 1.2317e-02 1.4415e-05 -1.1920e-02 1.1629e+00 0:00:48 21nn Reversed flow on 119 faces (48.9% area) of pressure-outlet 7.n 2380 1.1453e-02 3.7606e-05 3.7874e-05 4.8981e-05 3.8741e-03 6.6408e-04 7.7514e-03 1.1709e-05 -1.1692e-02 1.1627e+00 0:00:47 20nn Reversed flow on 120 faces (49.5% area) of pressure-outlet 7.n 2381 8.5417e-03 1.9685e-05 2.0956e-05 2.6071e-05 2.1750e-03 4.7657e-04 1.2825e-02 2.1264e-05 -1.1982e-02 1.1627e+00 0:00:45 19nn Reversed flow on 118 faces (48.3% area) of pressure-outlet 7.n 2382 9.3098e-03 2.7927e-05 2.8467e-05 3.6966e-05 4.2165e-03 8.0904e-04 7.7451e-03 1.5115e-05 -1.1850e-02 1.1627e+00 0:00:42 18nn Reversed flow on 119 faces (48.9% area) of pressure-outlet 7.nn iter continuity x-velocity y-velocity z-velocity k omega intermit retheta e-mass o-vel time/itern 2383 1.1317e-02 3.7945e-05 3.8587e-05 4.9670e-05 3.2519e-03 6.5387e-04 1.1632e-02 1.1543e-05 -1.1868e-02 1.1628e+00 0:00:40 17nn Reversed flow on 119 faces (49.1% area) of pressure-outlet 7.n 2384 1.0677e-02 3.2646e-05 3.2879e-05 4.2599e-05 3.7854e-03 6.1643e-04 7.7726e-03 9.4815e-06 -1.1908e-02 1.1628e+00 0:00:37 16nn Reversed flow on 119 faces (48.8% area) of pressure-outlet 7.n 2385 1.1139e-02 3.8524e-05 3.9000e-05 5.3823e-05 3.2806e-03 6.8996e-04 1.2306e-02 1.5705e-05 -1.2009e-02 1.1629e+00 0:00:35 15nn Reversed flow on 118 faces (48.3% area) of pressure-outlet 7.n 2386 1.1075e-02 3.5661e-05 3.5888e-05 4.5736e-05 3.8477e-03 6.4128e-04 7.6188e-03 1.0554e-05 -1.2021e-02 1.1629e+00 0:00:33 14nn Reversed flow on 119 faces (48.9% area) of pressure-outlet 7.n 2387 1.1263e-02 3.9555e-05 4.0050e-05 5.5978e-05 3.2245e-03 6.7269e-04 1.2153e-02 1.6059e-05 -1.2125e-02 1.1630e+00 0:00:30 13nn Reversed flow on 118 faces (48.4% area) of pressure-outlet 7.n 2388 1.1269e-02 3.6675e-05 3.6909e-05 4.7405e-05 3.7974e-03 6.4279e-04 7.5514e-03 1.1557e-05 -1.2079e-02 1.1630e+00 0:00:28 12nn Reversed flow on 119 faces (48.9% area) of pressure-outlet 7.n 2389 1.1405e-02 3.9754e-05 4.0156e-05 5.6480e-05 3.1460e-03 6.6343e-04 1.2299e-02 1.5096e-05 -1.2068e-02 1.1631e+00 0:00:26 11nn Reversed flow on 117 faces (47.8% area) of pressure-outlet 7.n 2390 1.1386e-02 3.7066e-05 3.7263e-05 4.8453e-05 3.8204e-03 6.6158e-04 7.7695e-03 1.2374e-05 -1.1992e-02 1.1629e+00 0:00:24 10nn Reversed flow on 119 faces (48.9% area) of pressure-outlet 7.n 2391 8.5094e-03 1.9466e-05 2.0625e-05 2.5828e-05 2.1649e-03 4.7615e-04 1.2856e-02 2.2677e-05 -1.2154e-02 1.1629e+00 0:00:21 9nn Reversed flow on 116 faces (47.3% area) of pressure-outlet 7.n 2392 9.2599e-03 2.7686e-05 2.8141e-05 3.6622e-05 4.1889e-03 8.0928e-04 7.7368e-03 1.5160e-05 -1.2002e-02 1.1629e+00 0:00:19 8nn Reversed flow on 118 faces (48.3% area) of pressure-outlet 7.n 2393 1.1302e-02 3.7607e-05 3.8045e-05 4.9345e-05 3.1918e-03 6.5214e-04 1.1603e-02 1.2124e-05 -1.1992e-02 1.1630e+00 0:00:16 7nn Reversed flow on 119 faces (48.9% area) of pressure-outlet 7.nn iter continuity x-velocity y-velocity z-velocity k omega intermit retheta e-mass o-vel time/itern 2394 1.0608e-02 3.2059e-05 3.2246e-05 4.1709e-05 3.6890e-03 6.1313e-04 7.7885e-03 1.0183e-05 -1.1899e-02 1.1630e+00 0:00:14 6nn Reversed flow on 118 faces (48.4% area) of pressure-outlet 7.n 2395 1.1071e-02 3.8132e-05 3.8447e-05 5.3475e-05 3.2071e-03 6.8922e-04 1.2299e-02 1.6369e-05 -1.1815e-02 1.1631e+00 0:00:12 5nn Reversed flow on 116 faces (47.3% area) of pressure-outlet 7.n 2396 1.1031e-02 3.5161e-05 3.5235e-05 4.4931e-05 3.7846e-03 6.4184e-04 7.6237e-03 1.1207e-05 -1.1687e-02 1.1631e+00 0:00:09 4nn Reversed flow on 117 faces (47.8% area) of pressure-outlet 7.n 2397 1.1240e-02 3.9228e-05 3.9461e-05 5.5507e-05 3.1630e-03 6.7124e-04 1.2144e-02 1.6575e-05 -1.1602e-02 1.1632e+00 0:00:07 3nn Reversed flow on 120 faces (49.3% area) of pressure-outlet 7.n 2398 1.1210e-02 3.6306e-05 3.6340e-05 4.6677e-05 3.7583e-03 6.4165e-04 7.5329e-03 1.2121e-05 -1.1521e-02 1.1632e+00 0:00:05 2nn Reversed flow on 119 faces (48.8% area) of pressure-outlet 7.n 2399 1.1421e-02 3.9725e-05 4.0099e-05 5.6607e-05 3.1535e-03 6.6447e-04 1.2316e-02 1.5506e-05 -1.1465e-02 1.1633e+00 0:00:02 1nn Reversed flow on 117 faces (47.8% area) of pressure-outlet 7.n 2400 1.1395e-02 3.7083e-05 3.7255e-05 4.8431e-05 3.8384e-03 6.6315e-04 7.7690e-03 1.2790e-05 -1.1793e-02 1.1630e+00 0:00:00 0n
    • Rob
      Ansys Employee
      A skew of 0.99 and an ortho quality below 0.05 is a problem, you may just have got away with it for the earlier models but running two domains may be enough to cause the problem as the stability functions are now trying to deal with two systems. n
    • mmoataz
      Subscriber
      But this high skew and low ortho quality values occur only in less than 0.001% of the cells. Does this small % still affect the results that much?! nAnd if stability functions are the reason, then why do they work fine when both fluids are set to be the same (keeping Reynolds constant as the original case)?! Which means they can deal with 2 systems.nn
    • Karthik R
      Administrator
      I'd definitely try to improve the overall mesh and see if the two system results improve. As Rob was saying, it is possible that the overall mesh quality might be what is causing the solution to diverge. Please let us know your findings.nThanks.nKarthikn
    • mmoataz
      Subscriber
      Is there a way to delete this whole discussion? or delete one of its posts?n
    • Karthik R
      Administrator
      Which post would you like us to delete? We can do it for you if you wish to do so.nThank you.nKarthikn
    • mmoataz
      Subscriber
      I would like to delete the 2 posts containing screen shots. Both of them were in 21 September. Thank youn
    • Rob
      Ansys Employee
      Done, note if you're working with a company on a project with an academic licence you MUST review the T&Cs as all work should be publishable. n
    • mmoataz
      Subscriber
      Thank you Rob. This is required for my master thesis not a company project.n
    • mmoataz
      Subscriber
      I tried to simulate again with a mesh that doesn't contain inflation layers and has:nMesh skewness: Max: 0.87, Average: 0.25, Standard Deviation 0.11nMesh orthogonal quality: Min: 0.127, Average: 0.74, Standard Deviation: 0.107nOf course in this case y+ values are large but I just wanted to see if the same problem happens, and yes it happens unfortunately.nTo get closer to identifying the problem I tried the simulation with air and a hypothetical fluid that has the same density as air but the same viscosity as the thermal oil keeping mass flow rate and though Reynolds number the same. Surprisingly, I got a correct result! which means that the large difference in density (not the difference in viscosity) is probably the source of the problem!nIs it advisable to do an extra step in the setup when simulating 2 such systems of large difference in densities?nUnfortunately, I didn't find any similar heat exchanger tutorial on the internet that has 2 working fluids of large density differences. It is always either water-water, air-air or water-external air heat exchanger which doesn't apply to my case.nI hope you can help me on that.nThank youn
    • Rob
      Ansys Employee
      Have you set the operating density in the system? n
    • mmoataz
      Subscriber
      No, I didn't. I left the default operating conditions without specifying operating density. If I should, then the question is which density should be used the low air density or the high oil density or a mean density between them. There is only one field for one operating density.nn
    • mmoataz
      Subscriber
      Thank you very much Rob for your suggestion. Now I set the operating density to be that of air and I got results similar to the ones I get when each side is simulated separately. Of course I still need to judge the results more accurately but they seem OK from the first look.nTo understand how this actually worked I found the following paragraph from Fluent user guidenEven though I've read this before but just now I can notice the highlighted part averaging over all cells. nDoes that mean that fluent has calculated the operating density by averaging densities of air and oil?! how about densities of the solids in the heat exchanger are they included as well?nAlso, since now I've used air density as an operating density, can that make the results for the oil inaccurate some how?n
    • Rob
      Ansys Employee
      Given it's in the buoyant flow section of the manual I assume it uses the fluid properties only. The same section also notes that setting the operating density helps with convergence and shouldn't influence the end result: so now it's got a fixed value to work with the solver should be happier. CFX has an independent (maybe detached, will know) volume option for their equivalent operating pressure and density settings, and we've asked for the same in Fluent given the confusion this can cause. n
    • mmoataz
      Subscriber
      Yes, it averages over fluid properties only because when I simulate air side with the solid parts added I still got correct results.nI agree that calculating operating density by averaging causes confusion especially in applications having non-mixing 2 or more fluids with large density differences (like in many heat exchanges). I think for this case there should be separate operating conditions for each fluid in the system.nFinally I'm happy with the results and thank you all for your help nn
Viewing 25 reply threads
  • You must be logged in to reply to this topic.