Learning Forum

[SEANGHAI]

Hello! I have a 3D building with air flow inside the building with many rooms as well, So do I need to apply all the domains as the fluid domains in the mesh part? But where can I define all the building walls as the solid? Because when I want to define my domain as solid or fluid, I have to define all the whole domain, I could not assign it by part or face at all. In short, I want to apply the air(fluid) in each room and the wall as the solid. Thank You in advanced! You can see my building as the following:

[peteroznewman]

nRead some discussions on this topic.n

[SEANGHAI]

Thank you for your kind reply! I checked the discussion in the link already, so I am just curious that I have to make the enclosure of my whole building model or not, also I never know how to use share topology before, but after I saw your discussion, I think I need to use it because there are many rooms in the building of my model, however, I still do not know exactly how to use share topology for my model, which domain or which face should I do the share topology? I will need to watch some videos on Youtube to more comprehend about it! However can you detail me more about it? Thank You again! You can see my figure of the full domain as the following:nThere is Inlet for applying air to the buildingnAlso there is outlet for taking out the air to the outside of the buildingnthere is also another outlet for taking out the air to the outside of the building as wellnInside the building, there is inlet for supplying air from a room to the free space of the buildingnFinally, there is a volume inside the building to supply a chemical (Water Vapor)(I used source) to the whole building when the air is blowing to the inside of the buildingnThank You!n

[DrAmine]

Do you have the walls resolved in your Case? Or they are just zero thickness wall If they are resolved, they will appear in Fluent as separate solid zones. If not resolved the internal wall will appear as zero thickness two sided wall (wall/wall-shadow) if internal. If the wall is an external wall (only one side is connected to Fluid) you want have any shadow.nnAlso please update to most actual release. 15.0 is outdated. n

[DrAmine]

You don't need to make any enclosure of the building as you are interested in the flow inside the building: the building itself is then your enclosure.n

[SEANGHAI]

Thank You for your kind reply and Yes, the wall of my building is just the zero thickness wall! So I apply all the domains as the fluid zone, and I create name selection of the wall as the wall except inlet and outlet of the building, then when I go to set up part, the wall will be created automatically as the wall boundary condition, in this case, is it correct?

[SEANGHAI]

And is it possible for my case if I do not do the share topology?n

[peteroznewman]

nIt is best to use share topology for the entire building. With share topology, solution quantities are passed from one cell to the adjacent cells normally. Without share topology, the cells don't line up, the solver can't pass solution quantities to the neighboring cells. Contact must be defined in meshing and interpolation equations added to the model to pass solution quantities across the interface. So it is possible to not use Share Topology, but it is preferred. One example where it might be best to not use Share Topology is when the element quality gets much worse with Share Topology than without.n

[DrAmine]

Yes go as Peter wrote and yes just have an inlet and outlet and keep all other walls as they are. Share Topology to have a conform and good looking mesh. You can assign each wall afterwards a thickness if you want but start simple to end big!n

[SEANGHAI]

Thank you so much Arrayand Arrayfor your advices! However, there is one thing about the contact region, is it possible to delete the contact region? Because in the mesh part, the contact regions are automatically created by fluent, and when I go to set up, there are some warning messages written that Cannot Create Surface from sliding interface zone, Create empty surface, and all of these surfaces are the contact regions surfaces, so I go to delete all the contact regions in the mesh part, then there are no the warning messages appeared in the set up process anymore. Therefore, in this case, is there any problem if I delete all the contact regions?nThere is one more thing which I want some advices from both of you. In my building there are 1 source volume, 9 inlets (Using mass flow inlet), and 11 outlets (Using Mass flow Outlet), thus is it too complicated or not for ANSYS Fluent to calculate the solution? Because I tried one calculation and used pressure based solver, then gave 1000 iterations, but the solution is not converged at all! Is it because of having too many inlets and outlets?nI am looking forward for your advices! thank you!n

[peteroznewman]

nYes, delete all the automatically created contacts in Meshing. If you use Shared Topology, you don't need any Contact. Dr. Amine can answer your other question.n

[DrAmine]

Avoid the combination of mass flow inlet and mass flow outlet: More natural is to have a pressure boundary at inflow/outflow regions.nYou are trying to solve an ill-posed over-constrained problem. I assume at your building outlets you have known pressure which is the outside pressure.n

[SEANGHAI]

Thank again ! I will try to change some mass flow outlets to pressure outlets, then I will check the results, and if there are still some problems, I will come here again as soon as possible, and I continue to look forward to your advices and helps! Thank You in advanced!n

[DrAmine]

Alright!n

[SEANGHAI]

Hello! and Mr. I have done the share topology of the domain and also I change the boundary condition from mass flow inlet/Outlet to Pressure Inlet/outlet already and the calculation is still not converged even I assigned 2000 iterations. Now I have just changed the geometry and did the same thing and the solution is not converged as well. I tried many methods according to this forum's group, but still not converged. I do not have any idea to keep going on my trying now, so can you give me more advices? You can see my new geometry , mesh and boundary condition as the following figures:nGeometrynThis source (pool) is used for applying the air and water vapor in the volume of that pool by using mass source in the set up part!nWall boundaries are all the exterior surface of the building excluding the inlet 1,2, outlet 1,2,3.nI used Realizable K-epsilon Model, Standard Wall Function!nThank You very much! I keep looking forward for your helps! n

[Rob]

Is that the mesh you're running CFD on? n

[SEANGHAI]

! Thank for your reply and Yes ! this is the mesh which I ran in the mesh part of ANSYS FLUENT (ANSYS ICEM CFD). Is there anything wrong with the mesh? Is the size of the mesh too big or not? I read many discussions, the problem that the solution is not converged because of the mesh, but I do not know whether my mesh is appropriate or not, I just made the size of the mesh is big enough to be easy to run quickly and make sure the meshes have not skew. n

[DrAmine]

Can you please check check the quality of the mesh in Fluent? I know you want to deal with large building but is a bit coarse and there are some other things which I hope are only due to the resolution of the picture. You created the mesh in ICEM CFD?n

[SEANGHAI]

! Yes! I created the mesh in ICEM CFD. Now I have just successfully done the calculation with the convergent solution by changing the mesh from tetrahedron to hexahedron mesh and doing the coarse mesh in stead of the medium mesh (I enlarge the size of the mesh). Thank You so much! Now the solution is converged at 1250 iterations. nHowever now there is another problem after I checked the results, I realized that there are wall boundaries of the pool inside the building, so the source cannot come out from that pool volume to the domain of the building. I did not create name selection of the wall of that pool, but fluent created the wall of that pool automatically in the set up. My goal is to create one source pool inside the building in order to apply source of air and water vapor in that volume of pool(source), but I do not want to create the wall at all. I want the air flow in the building blow the source in the pool and bring the water vapor to the whole building and some will go outside the building by passing through the outlets. So can you give me more advices to solve this problem? Thank You in advanced! The pool is inside the building as the following figure:nnn

[DrAmine]

Can you show the Fluent Cell Zones?n

[SEANGHAI]

! Yes! Sir! You can see the following figures. There are two cell zones, one is the pool for applying the mass source and another one is the cell zone inside the building except the pool. nEven its name is solid, but its type is fluid and the source pool cell zone is the cell zone for applying mass source(Water Vapor and Air). nIs this what you want to see? Am I right? Or do you want to see the other figures? Thank you again!n

[Rob]

Do you have a wall & wall:shadow pair between the pool source volume and the rest of the building? n

[SEANGHAI]

! Thank You very much for keeping in touch with my problem! Now I have done the calculation successfully! The problem which I mentioned above is because I did not form a new part to combine the source pool domain and the building domain together, so now when I form a new part in the modeling and when I go to set up, fluent does not create the wall of the pool anymore, and the solution is also converged at 2730 iterations! The iterations seem too big, but in reality, the calculation is very fast! It took only 1 and half minutes to complete the calculation at 2730 iterations! nI will check all the results and if there are more problems, I will come to get the advices from you again! Thank you so much! you help me a lot!n

[SEANGHAI]

! Thank you! Sir! and Yes! there are overlapping walls at the bottom face of the pool between face of the pool and face of the building in the set up! So I go back to mesh part and in the name selection of the wall, I unselected the bottom face of the building which is a bottom face part of the pool! then when I go to set up and in the boundary condition, there are two kinds of wall, one is wall of the building and another one is the bottom wall of the pool(created by fluent automatically, but it does not impact the flow calculation) which is connected to the wall of the building, and this time there are no overlapping wall anymore in the set up! so am I doing correctly? I always appreciate to get all your guide and advice!n

[Rob]

That's fine. If the wall & wall shadow pair you got were unique to that face you can also change the boundary type to interior in Fluent. n

[SEANGHAI]

Yes!Sir! Thank You very much for your advice!?! I will come here again if there is any problem that I cannot comprehend after checking my results! n

[SEANGHAI]

Hello! and ! Now I do not understand one thing! It is velocity result! I applied the same mass flow inlet 2 and mass flow outlet 2, but the results of velocity at inlet 2 and outlet 2 are totally different. I applied mass flow inlet 2=mass flow outlet 2= 1.51kg/s, and according to my calculation the results of velocity at inlet 2 and outlet 2= 1.64 m/s, but the velocity vector shown in Fluent appeared that velocity at inlet 2=1.64 m/s to 1.72 m/s (this one is quite correct), but the at the outlet 2 , the velocity is only 0.094m/s. According to the same amount of mass flow rate that I applied at the inlet 2 and outlet 2, so it is correct or not that we should get the same amount of velocity at the inlet 2 and outlet 2? Or because of the flow behavior that make the velocity at the outlet 2 become too small? I also realized that the velocity at the outlet 2 is not normal to the surface of the outlet2 at all, maybe this is the reason, but I am still not sure! You can see the boundary of inlet 2 and outlet 2 as the following figures:nAnd here is the results of velocity:nThank you again for your helps and great advices for me!n

[Rob]

You shouldn't have mass in and mass out unless there is a way for the solver to add/remove material to balance the boundaries. How does the mass balance in the domain look, and how good is the convergence? n

[SEANGHAI]

Thank again for your reply! Sir! Honestly, I do not know how to check the mass balance, how can I check it? Is it the contour of mass imbalance? I never check about it! Can you guide me something? And the solution is converged at 2730 iterations! I saw a problem in the velocity vector, the vectors at the inlet 2 are too big because of the amount of mass flow rate is big! You can see the velocity vector as the following:nI am looking forward for your help!nn

[Rob]

Look in Results - Fluxes. Please go through the tutorials as they cover most of the basics. n

[SEANGHAI]

Thank You! Sir! I will look at it!n