TAGGED: conjugate-heat-transfer, energy-error, fluent, temperature
February 1, 2021 at 7:15 amvsjay3Subscriber
I am modelling a pipe carrying fluid through a solid domain (sand) in Fluent. Flow is turbulent. The pipe is embedded inside the sand layer which is heated. I want to see how the water in the pipe will get heated up by the sand layer's high temperature. But after I modelled it, I get negative temperature (negative values of Kelvin). The sand layer is supposed to be only heated to 55C, so there is no way the temperature can be negative. I am assuming something is not right with my heat transfer because the residual plot for energy starts increasing after sometime and then becomes constant (image attached below).
Any advice is very much appreciated!
Thank you!February 1, 2021 at 9:10 amDrAmineAnsys EmployeeReally negative values? Temepature is limited per deault to 1 K. nCan you share more details about case settings and boundary conditions?.The image you are sharing does bot provide any value (perhaps only that case is not converging)nFebruary 1, 2021 at 9:33 amvsjay3SubscriberHi Arraythanks a lot for helping. I am new to Fluent, so any help is truly appreciated. The Geometry is below, where the top layer which has the pipe embedded, is the sand layer and the bottom layer below the sand is soil.nI am using the standard k-omega turbulence model. The fluid (0.25m/s) enters the pipe from the left side (where the fluid temperature at inlet is set to 20C) and exits the pipe (right side). The boundary condition for pipe outlet is outflow. Also the pipe wall and sand layer is thermally coupled. The boundary condition at top of the sand layer is a constant temperature of 55C. The bottom of the soil layer (very bottom surface) is set to constant 24C. nAbout the temperature I am sorry, it was negative Celsius values, which still is a big problem since this is a simple problem and I do not have such temperatures in my system. Results are attached below (which makes no sense). The heat is supposed to flow downward from sand to soil while mixing with the fluid in the pipe.nnYour advice is much appreciated!nnFebruary 1, 2021 at 2:54 pmRobAnsys EmployeeLooking at the temperature range I think the solution has diverged: you shouldn't be cooler than 20C or warmer than 55C based on your comments. Given it's a fairly simple model check the mesh in the pipe fluid and solid if the pipe wall is included. nFebruary 1, 2021 at 4:09 pmDrAmineAnsys EmployeeVerify if you have the interfaces well set if using non-conformal mesh.nFebruary 1, 2021 at 4:09 pmDrAmineAnsys EmployeeDouble check all wall boundaries: I assume you have two zones right?nFebruary 1, 2021 at 5:14 pmvsjay3SubscriberHi Array and Array ,nI have four zones : the sand layer (top rectangle), soil layer (bottom rectangle), pipe material and the coolant (water). The pipe and coolant were meshed using sweep mesh. The pipe wall and the sand layer are thermally coupled (wall-wall shadow). The meshes of all components are conformal since in designmodeler I made all bodies into one single part. So it is just one part with 4 bodies. I did not make the mesh super fine since I am using academic version from my university and I hit the mesh limit. But I'm not sure if mesh resolution is the real problem here, since what I am facing is not a slightly inaccurate solution but a complete failure of the model to give a sensible solution. Attached below is an image of the mesh for your referencennHowever, I did notice a slightly strange thing - the sand and pipe wall contact region was initially identified in the boundary conditions as interior (highlighted in blue below)nThat is the only strange thing I noticed in the model.nFebruary 2, 2021 at 4:44 amYasserSelimaSubscriberHow deep is the clay?nWhat is the boundary condition on the clay sides?nFebruary 2, 2021 at 4:55 amvsjay3Subscriberthank you for answering. The whole setup is in millimeter scale actually. The soil is 120mm depth. The mesh element size for the soil is hexahedral 10mm (because nothing much happens in the soil region I did not make it very fine). The boundary condition for clay sides I tried adiabiatic wall and even system coupled (even though there is no other system im using in ansys). But both cases don't give good results. When i tried the same model with a one bend pipe (one U shape pipe) and put same boundary conditions, it worked. Just when i used this three bend pipe it does not seem to converge.nFebruary 2, 2021 at 5:19 amYasserSelimaSubscriberI am not sure about this system coupled!! But adiabatic should work.nThe clay cells are ok. I am assuming you are using the same adiabatic boundary for the sand sides, nwhat is your time step? nFebruary 2, 2021 at 5:24 amYasserSelimaSubscriberAlso I can see the temperature contours, every where is around 317 ... this is 44 C. nFebruary 2, 2021 at 5:25 amvsjay3SubscriberHi Array, yes sand sides are same condition. Just top of sand and bottom of clay have constant temperature. The modelling is steady state. When I meant system coupled in my previous comment, I meant the via system coupledoption in fluent.nIs there any way that I can find the mesh location of the model where the energy starts diverging ?nFebruary 2, 2021 at 5:29 amvsjay3Subscriberyes it seems 44C everywhere but the max temperature shows 700K. I cant even see that 700K temperature anywhere. Sand top temperature is 55C and soil bottom is 30C. Coolant at inlet is 20C.nFebruary 2, 2021 at 9:50 amRobAnsys EmployeePut a slice through the mesh about on the pipe mid plane (horizontal) and then post a zoomed in image. Use the option to show full cells. Also look at cell quality. Depending on the aspect ratio of the pipe mesh and some of the gaps I suspect the mesh in the transition from pipe hex to clay tet is the problem. nThe surface between two solids no longer has to be a wall, so having an interior is OK. In older versions of the code that would have flagged as an error. nFebruary 2, 2021 at 10:16 amvsjay3Subscriberthank you very much for replying and noted on the interior regions between solids. Following is the mesh.nnnI was trying to keep the mesh count to 512K due to academic version. Should the total of both elements and nodes be 512K or is it 512K for elements and 512K for nodes separately? Also I kept the orthogonal quality and skewness at acceptable standards.nnFebruary 2, 2021 at 10:22 amRobAnsys EmployeeIgnore Element Quality and focus on skew, ortho and aspect ratio for fluids. I tend to use skew and aspect ratio for hex & tets and leave ortho for poly meshes:nothing too scientific, it's just I have a better idea of what I can get away with. nYou want under 512k elements, node is more for Mechanical as they have elements with extra nodes:CFD has 2nd order solvers.Mesh looks reasonable so next thing is to look for where the temperature is going wrong. Also review the boundary conditions. Very simply, we work through mesh, models, materials, bc's and results in about that order when trouble shooting models. nFebruary 2, 2021 at 10:29 amvsjay3SubscriberThanks . Just to clarify on 512K limit for fluent, you are saying I can go upto 512K for elements and ignore nodes number? For example if its:nElements : 500,000nNodes : 300000nFluent will still solve for the above?nAlso,I performed same modelling procedure for one loop of pipe and it worked which is why I did not bother about checking boundary conditons since it worked. That is why I was a bit confused why one loop works but not two loops.nIs there any option in fluent to check which region of cells in the model is causing the energy to diverge?.Thank you!nFebruary 2, 2021 at 10:36 amRobAnsys EmployeeFluent should solve for 500k elements. Just remember that some models may create virtual cells so you may gain a few when switching to Fluent. nHave a look at the adaption registers, iso surfaces and volume reports. nFebruary 2, 2021 at 3:30 pmvsjay3SubscriberThanks . I have read that aspect ratio requirements vary. So what is a good mesh aspect quality range according to your opinion?nThanks.nFebruary 2, 2021 at 3:34 pmDrAmineAnsys EmployeeIf you read that mesh into Fluent: can you then list the boundary conditions there. I am actually concerned about that outer wall: it has one free part and one which should be coupled to the sand domain (or to whatever green domain is referring to). It looks like the mesh is conformal but please double check what are the boundaries in Fluent. Better to check that under Adjacency Panel.nnnFebruary 2, 2021 at 4:15 pmvsjay3SubscriberHi Array thank you very much for your reply. Yes the green domain is sand layer nSand is the top green rectangle and soil is the brown bottom rectangle.nSo the boundary conditions are a lot to list individually and may confuse you, so to save your time I will bunch them up :nsand - right wall, left wall, front wall and back wall = zero heat flux conditionnsand top wall = constant temperature of 70Cnpipe wall (iron) which is outside the sand = zero heat flux conditionnpipe wall inside sand = thermally coupled condition with sandncoolant and pipe wall = thermally coupled conditionnsoil - right wall, left wall, front wall and back wall = zero heat flux conditionnsoil bottom wall = constant temperature of 30Cnsand and soil contact wall = thermally coupled conditionnAlso yes, I believe that the mesh is conformal since it is one part and 4 bodies.nAre you telling me the free part of the pipe wall and coolant outside the sand is creating the issue?nFebruary 2, 2021 at 5:39 pmDrAmineAnsys EmployeeOkay now regarding your solver settings: focus on the Fluent part and start using coupled pseudo transient solver. Heat flux report is also helpful for debugging. nFebruary 2, 2021 at 5:56 pmvsjay3Subscriberthank you for your comments, appreciate it. But I am doing steady state. Can I still use the transient solver though?nAlso how would the heat flux report help - will it show the location of the model where the energy diverges (sorry Im quite new to fluent) ?nThank you!nnFebruary 2, 2021 at 5:59 pmDrAmineAnsys EmployeePseudo transient is steady state using flash time stepping under relaxation nFebruary 2, 2021 at 6:01 pmDrAmineAnsys EmployeeFlux report will tell if there is an issue in heat crossing the coupled walls. First use the couples solver and also ensure that you issues mesh check in Fluent. You better want do some tutorials to get familiar with all that.nFebruary 2, 2021 at 6:08 pmvsjay3SubscriberThank you very much for you kind advice . I will try coupled pseudo transient solver and yes, I normally do mesh quality check before simulation.nThank you!nFebruary 3, 2021 at 10:15 amvsjay3Subscriberand I tried modeling without the pipe wall part sticking outside the sand region and it seemed to work. But I have a few doubts that would be great if I can have clarified:n- I kept the top of sand region at constant 70C . But after the solution was calculated, the top of the sand was 67.9C. Is this normal or does it mean the results are wrong?nn- Also, the residuals started rising a bit midway around 200-250 iterations but then started dropping again. Is this fine or is it also a problem?nnYour advice is much appreciated!nnFebruary 3, 2021 at 10:22 amvsjay3Subscriberand I tried modelling the design without the pipe parts that stick outside the sand region and it seemed to give reasonable results. But I have a few doubts that would be great if clarified:n- I set the top of sand region (very top horizontal edge in design) to constant 70C but after modelling, the results show maximum temperature at top as 67.9C. Does this mean the results are not correct or is there a way to improve it?nn- Also I noticed that the residuals rise midway suddenly at around 200-250 iteration range but then drop down. Is this a problem or is it normal for residuals to rise up a bit midway or should I be worried? nnYour advice is greatly appreciated!nFebruary 3, 2021 at 10:39 amRobAnsys EmployeeYou'll be showing the effect of conduction and near wall cell. Display temperature on the top wall only with node values off: that'll be the wall temperature. The boundary value is assigned to the boundary, but the contour will be showing the near wall cell value by default.nThe residuals are a function of the sum of the errors. It's common for them to not drop cleanly throughout the solution as the solver alters cell values as a result of the iterative process. nI'm a little surprised that removing the pipe stubs had that much of an effect. But, if that's improved the mesh and/or boundary settings it could easily explain it.February 3, 2021 at 10:58 amvsjay3Subscriberthank you very much for replying. Noted on the wall temperature. I am still not sure if it is the removing of the pipe studs itself that did the trick but I kept the boundary conditions the same. So i guess it is not the boundary conditions that fixed it. Anyways, I will try modelling with pipe studs again and see. nAlso noted on the residuals. But if the residuals start rising significantly then there is definitely a problem yes? Like below in the first time I modelled - that rise is too much and I should realize there is a problem right?nnFebruary 3, 2021 at 11:31 amRobAnsys EmployeeYou can have a rise like that and all is well in the model: it's a significant change in a flow feature such as a jet attaching. In your case the fact that the residual doesn't then fall is a problem. nWhat did you set as the pipe boundary for the stubs? nFebruary 3, 2021 at 12:17 pmvsjay3Subscriberthank you very much. As for your question - I set the boundary condition as zero heat flux for the stubs. Since I took off the stubs I was granted more allowance for the mesh number of elements and was able to make the mesh a bit finer for the model - maybe that worked. Yet to check exactly what is happening.nRegarding residuals - Generally is there a threshhold below which the residuals should fall....like for energy I read somewhere it is better if it falls below -10^6?nAlso, one more small thing - I plotted certain xy charts in cfd post along an inserted line. The graph plots well but I want to export it to excel. May I please know if cfd post supports the exporting of xy data along an inserted line at a particular location?nThank you very much!nFebruary 3, 2021 at 1:30 pmDrAmineAnsys EmployeeYes it does support: You can export to CSV (Button Export in the Chart Panel: you cannot overlook it..)nFebruary 3, 2021 at 1:41 pmvsjay3Subscribermy apologies, must have missed the export option. Thank you very much for the support!nViewing 33 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.Trending discussions
- Suppress Fluent to open with GUI while performing in journal file
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Getting graph and tabular data from result in workbench mechanical
- The solver failed with a non-zero exit code of : 2
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error: Received signal SIGSEGV
Top Rated Tags
© 2023 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.