March 15, 2021 at 11:24 pmpeteroznewmanSubscriber
@NathanielChong asked about how to create a mesh to make a CFD analysis of duct work that circulates air in a lecture theatre.March 16, 2021 at 5:11 amKeyur KanadeAnsys EmployeeFrom image it looks like solids. For this user needs to extract he fluid volume first. nUser can check following video for volume extract. nAfter that as Peter has suggested, please check if you can reduce problem size by using mirror. nUser can also check following for meshing. nPlease check following videosnnAnsys Meshing Sizing:n" target="blank">nRegards,nKeyurnHow to access Ansys Online Help DocumentnHow to show full resolution imagenGuidelines on the Student CommunitynHow to use Google to search within Ansys Student CommunitynMarch 16, 2021 at 2:48 pmNathanielChongSubscriberArrayThank you for responding to my question. If i may ask, how will i have to create the model of the ducting so that it would only show 1 surface not including the outlets. The ducting was drawn with a ton of mate function from solidworks, will that be a possible source of problem? As for the faces, will i have to individually indicate the outlets as i draw or only later when I am doing the preprocessing before meshing. Lastly, i found it very challenging to select the inlet and outlet surfaces when i was trying to indicate these surfaces before running the mesh. nRegards,nNathanielnMarch 16, 2021 at 2:53 pmNathanielChongSubscriberArrayThank you for your input. For the issue suggested, I modelled the ducts using only flat surfaces without any fancy curvature due to my limited skillset. With that mention will i have to carry out the extract fluid volume in this case?nRegards,nNathanielnMarch 16, 2021 at 6:09 pmpeteroznewmanSubscriberMarch 17, 2021 at 1:06 pmNathanielChongSubscriberThank you so much for this hands on guide. I have been static for a while now and finally have a direction to head towards. For the imprinting part, is there a specific technique that i can use to reproduce the diffusers or do i have to resketch it? Also if i made it to the meshing part, do i have to change the mesh sizing on the ducts?.Thanks and regards,nNathanielnnMarch 17, 2021 at 1:26 pmNathanielChongSubscriberIf i create the duct solid using the blend function, will the duct still be hollow? nMarch 17, 2021 at 2:32 pmpeteroznewmanSubscribernYou are not meshing the duct, you are meshing the air in the duct. That is why you want a solid. The air is a volume, the outside surfaces of the volume are the walls of the duct.nThe strategy for meshing solids in CFD is to put an inflation layer of elements on the walls of the duct to capture the boundary layer of the turbulent airflow.nAn ANSYS CFD expert might comment on if there is a way to handle the diffuser inside Fluent without drawing all the vanes inside the circle. nTry building a model with circular outlets. You can draw all the vanes in on a second more detailed model after you get the first simplified model up and running.nMarch 17, 2021 at 3:02 pmNathanielChongSubscriberI see. So my concept has been wrong for the whole time. So as I draw a new model, I wont have to go through the trouble of modelling a hollow structure? As for the outlets, I think I will just forfeit the idea of drawing a complex diffuser and sticking to a circular outlet.n Also, is there an easy way to draw a the theatre walls as drawing the walls were really challenging for me in this model?nMarch 17, 2021 at 3:19 pmpeteroznewmanSubscribernThe air in the theatre is just a rectangular solid minus the air in the duct. Construct the box and use a Boolean Subtract to subtract the two ducts from the air in the room, but keep the duct solids. Now you have three solids that have no interference and define the walls of the room and the walls of the duct. Take this into SpaceClaim and on the Workbench tab, use the Share button. This will cause the coincident surfaces to be shared, and eliminate any contact being created in Meshing.nThe faces at the diffuser are labeled using Named Selections in Meshing as Interior, meaning they are not walls, but simply a boundary between the air in the duct and the air in the room. You also need some faces on the walls of the theatre labeled as outlet for the outlet of air from the theatre. The rectangle at the base of the duct will be labeled as inlet have an Inlet BC of a specified mass flow rate. The outlet on the theatre wall will have a Pressure BC.nMarch 17, 2021 at 4:03 pmNathanielChongSubscribernShould I just start modelling the rectangular room in designmodeller and draw the solid ducts within the rectangular room and only bring it to spaceclaim for the subsequent steps? Is it feasible to draw within the inner surface of the rectangular room to model the ducts? Or do I model the ducts first then construct the hollow rectangular box?nThank you for your guidance as all this is very new to me.nnMarch 17, 2021 at 5:12 pmpeteroznewmanSubscribernIt is simpler to model one duct first, including imprinting the diffuser circles on the faces of the solid.nThen create a mirror image of that first solid using a Mirror function.nThen draw a rectangular box for the theatre room, then do the boolean subtract.nEach of these operations can be done in SolidWorks or SpaceClaim or DesignModeler. Whatever you are best at. They have different names in different packages. In SC a boolean operation is called Combine, but you have to check the box to Keep Tools.nThe last step, creating Shared Topology, can only be done in DesignModeler or SpaceClaim. I provided instructions on what to do in SC.nMarch 18, 2021 at 7:15 amNathanielChongSubscribernDuly noted. Will start working on it. Again, thank you so much for the help.nRegards,nNathaniel nMarch 22, 2021 at 5:28 pmNathanielChongSubscribernDear Mr. Peter,nI have trouble trying to produce the cavity of the lecture theatre, I have tried using boolean subtract with the room being set as target and the ducts as tool structure but the result of the boolean subtract is not making any sense as it doesnt show the body of the ducts. I have also tried using fill feature to get the interior of the lecture theatre but it kept showing errors. What should i do?nAlso, at what stage should i define the walls of the ducts and the walls of the theatrennThank you.nMarch 26, 2021 at 3:24 ampeteroznewmanSubscribernYou did a good job on the ducts. You haven't quite got the concept of the room air being a solid. You created a hollow box for the theatre. You want a solid that is the shape of the theatre with the ducts subtracted from it. I have attached that solid. Look at it in wireframe and you will see this single solid has duct-shaped cavities in it. Add your two duct solids to this and that is the three solid body assembly I was talking about. Use Share Topology in SpaceClaim to share walls.nMarch 26, 2021 at 9:23 amNathanielChongSubscriberDearArray,nThank you so much for getting back to me. I have resolved this and have successfully created three solid (Set as fluid) (2 ducts and fluid in the lecture hall) with the respective walls labelled using named selection. I have also extruded the round diffusers and Outlets as they were causing me a lot of contact issues in meshing which after doing so solved the issue. However as i moved towards the setup stage, Missing new zones issue showed up and caused a lot of undefined surfaces to appear in the zone section.nI should also mentioned that I preserved the duct bodies when I Boolean Subtract it from the cavity of the lecture hall. What would most likely be the cause of this issue?nHope to hear from you soon.nThank you.nMarch 26, 2021 at 9:33 amNathanielChongSubscriberArraynUpon Further inspection in the Fluent setup, I noticed that majority of the undefined surfaces at Interface tab are duplicates of surfaces such as ductwall and diffusers (interior).nnMarch 26, 2021 at 11:34 ampeteroznewmanSubscribernI noticed your file had extra surfaces that defined outlets from the room. Did you delete all of those extra surfaces? You don't need them because there are faces on the room body where those surfaces used to be.nDid you use the Share button on the Wokrbench tab in SpaceClaim?nIn Meshing, did you see any contacts created under the Connections folder? Delete them.nLooking at your model, the element size is too large. Set the Element Size to a smaller number, don't leave it as Default. That should fix the meshing issues. nI don't understand how you extruded the round diffusers. Did you do that on both the Duct solids AND the Room Body? In one case adding material and in another case removing? This should not be necessary to get a good mesh.nIt's okay to have a wall and a shadow-wall because you have fluids on both sides of that wall. This allows Fluent to define a property of the wall for the air inside the duct separate from a property of the wall for air in the room.nMarch 26, 2021 at 12:27 pmNathanielChongSubscriberArraynAt the moment, I have four outlets extruded on the room body and it is all defined under one outlet named selection. nI did use the share button only to unshare the inlet surface from the room body based on the initial advice. Other than that I did not share any surfaces. Should I share any surfaces?nI saw 55 problematic surfaces, which were the diffusers and outlets. If I deleted the contacts, would it cause problem to the simulation? I was afraid to delete anything cause I didn't want to do anything that I couldn;t fix. I was stuck on the contact issue for 2 days b4 extruding it.nI extruded the sketch because I didn't know how to resolve the contact issue so I thought that extruding it would be able to eliminate the problem and still allowed me to select the surface as interior. nOh I see. But it showed warning messages when I opened the setup in the bottom right console window.nAlso what does interface boundary condition means?.March 26, 2021 at 2:18 pmpeteroznewmanSubscriberArraynWhen you say extruded what exactly are you doing to the solid body? I think you mean adding or removing from the solid volume, but maybe you are doing something that I would call imprinting. It is very important to start the project with clean geometry.nOnce you use the Share button in SpaceClaim, you don't need any contacts. Delete them all. It is better to start a fresh Fluent model, because the old Fluent model will remember that there were contacts and you will waste time cleaning up the old model. It is much better to start a fresh Fluent model with clean geometry and no contacts.nHere is an idea to make getting started a bit easier. Do only the airflow in the room, not the room and ducts together. That means each diffuser is an Inlet and you will define the flow rate for each diffuser and it will flow straight into the room and out the outlets.nBut first, in a separate model, simulate just the flow of air inside one duct. Again, this will be a single solid simulation. The diffusers are Outlets in this model and the rectangular end at the root of the duct tree is the Inlet where you define the flow into the duct tree. The results of this model will be the flow rate out of each individual diffuser. You can then enter those values into the Room model for Inlet flow rate at each diffuser and this will be a good approximation of the combined flow model, but you will have two smaller models that are easier to mesh and faster to solve.nWhen meshing one duct, use an element size of 50 mm and use Inflation to capture the boundary layer. That will result in a mesh of 453k elements, which is under the 500k Student license limit. That element size will be too large for the Room, which has a much bigger volume to fill.nDrag and drop a Fluent analysis onto the Mesh cell and it will create a fresh Fluent model that should run. I set the Smoothing to High and the Quality on the Mesh Metric of Skewness has a Max value of 0.84 which is good enough to get some initial results.nGood luck! nMarch 26, 2021 at 2:34 pmpeteroznewmanSubscribernMarch 26, 2021 at 4:44 pmpeteroznewmanSubscriberMarch 26, 2021 at 7:04 pmpeteroznewmanSubscriberHorizontal Slice through the Duct TreennVertical Slices through each duct, diffusers are pointing up.nIn Meshing, I named each diffuser outlet individually. Here is the Surface Integral Report on Mass Flow Rate: nFlow RatenVelocity Magnitude (m/s)(kg/s)n-------------------------------- --------------------ninlet 0.55125noutlet-a1 -0.033792286noutlet-a2 -0.049290673noutlet-a3 -0.064988827noutlet-a4 -0.075592129noutlet-b1 -0.023795012noutlet-b2 -0.039852063noutlet-b3 -0.065017148noutlet-b4 -0.084580287noutlet-c1 -0.060169858noutlet-c2 -0.080808306noutlet-d -0.039081787nwall-oneduct-px_duct-px 0n---------------- --------------------nNet -0.065718376nnNotice that there is a 12% mass flow rate imbalance since the Net value should be zero.nThis is because the Continuity Residual has not gone down sufficiently.nI ran this for 1000 iterations and it didn't go down much further.nCFD experts, what is needed to get the Net Mass Flow smaller?nMarch 26, 2021 at 8:13 pmpeteroznewmanSubscriberMarch 27, 2021 at 2:32 pmNathanielChongSubscribernThose are great tips doing them separately. But forgive my stubbornness because I feel like I am close to producing what I wanted. nI just realized that i did not click on the share button in workbench and once i did, Ansys was able to set the boundary condition according to what I named them as. But I am now facing one new issue that is the interior showing up as a wall boundary condition while also showing up as interior boundary condition. That's the remaining issue before I could successfully run the simulation.nWhat might be the cause of this problem sir? Also I am not using student version so I will clean up the mesh to a finer setting once I can run the simulation. nI know I am pushing here but the zip file is attached below if needed. THANK YOU!!!nnMarch 30, 2021 at 2:26 pmNathanielChongSubscriberArraynGood day Mr. Peter Newman,nI have done some reading on multiple sites to find out how i would be able to set the diffusers as interior BC properly. To summaries what I have found, It was said that If i Mesh both sides of the diffuser surfaces (Room and Inside the duct), I should be able to get the diffuser to be an Interior BC. There was also one that said that I should Separate faces from the mesh which would trigger the need to create a new BC. Which of this advices would be the better approach according to your experience?nThe reason that I am so adamant about running the airflow simulation both inside the duct and out into the room simultaneously is because I have to also simulate airflow distribution for a different kind of duct (Fabric Duct) within the same room which would involve a ton of small diffusers which would prove to be really tedious if I were to run the simulation separately to determine the airflow velocity at each small diffusers.nnNote the large amount of small diffusers that spread across each ducts.nHope to hear from you soon. Thank you.nMarch 30, 2021 at 4:42 pmpeteroznewmanSubscribernI didn't know how to answer your March 27 question so I didn't reply, hoping some CFD expert would reply. Unfortunately, they didn't. nMy understanding is that if you put the room solid that has duct shaped cavities and the duct solids into a single part, you use the Share button in SpaceClaim and the face on the room solid that represents a diffuser and the coincident face on the duct solid that represents a diffuser are recognized by SpaceClaim to be coincident faces with the same exact boundary edge, and that gets sent to Meshing as a single face. That face is selected and named using the Named Selection function in Mechanical. The name of the selection is Interior. Once those two things are done in SpaceClaim and Meshing, when Fluent gets the mesh, it knows there is a surface named interior, not outlet, not inlet and not wall so an Interior Boundary Condition is automatically created for that surface.nnMarch 30, 2021 at 5:48 pmNathanielChongSubscribernOh I see. Thank you for your guidance so far as I have learnt a great deal from you. Really appreciate it. nWhat should I do now sir? Should i keep waiting for experts to reply?nMarch 30, 2021 at 6:44 pmpeteroznewmanSubscribernIf you followed the directions I gave above, you should not get different boundary conditions on the same surface. Try building the model with a freshly made copy of the geometry that you know has Share Topology done perfectly, and the Named Selections done perfectly.nMarch 31, 2021 at 3:47 amNathanielChongSubscriberNoted. Will do that. Ill try removing the extruded diffusers to see if it makes any difference.nApril 2, 2021 at 10:10 amNathanielChongSubscribernGood day Mr Peter Newman,nI have done as you have told and all the boundary conditions were correct with the right amount of shadow BC. I was able to run the simulation. However, when i go into the solution and clicked on the streamline to show the movement of the air, I saw nothing came out at all even after I have clicked apply. I have even switched the flow equation to laminar to try to see the difference.nThis is what the scaled residuals looked like when the simulation was running.nCould it be because of the flow direction of the inlet that is causing this issue? nInlets Velocity and temperature: 8.22 m/s, 280 KnOutlet: 0 pressurenCould you have a look at my simulation file please. I have tried all i can to do this.nThank you.nnApril 3, 2021 at 5:23 pmpeteroznewmanSubscribernThis is the mesh you did the computation on. The elements are too large by at least a factor of 10! That is the reason for the poor convergence. Below are the outlets, which have 2 element faces.nThere are also only 2 element faces on the inlets into the duct tree.nContrast that with the inlet to the duct tree I provided in my example.nThe Element Size I used was 50 mm but I also applied Inflation to get 5 layers of thin elements on the surface to capture some of the boundary layer effect.nBest practice is to get the flow working well with Energy turned off, ignoring temperature, and once the flow is acceptable, turn Energy on.nApril 4, 2021 at 8:31 amNathanielChongSubscribernThank you again for your Input sir. I have reduced the element size of the mesh to 250 mm and by doing so i was able to get some improvement in the result. nnI have also turned off the energy equation but the velocity streamlines did not diffuse into the room for some reason. They did not even make it fully into the branches of the duct.nIt showed that the velocity reaches 0 magnitude before leaving the duct so i have even increased the magnitude of the inlet velocity to an absurd magnitude. It still returned me a similar result. I also tried running the simulation up to 1500 iterations and not much had changed. Should i try reducing the mesh element size and run the simulation again? Could i only further reduce the mesh size on the duct to better capture the flow?.April 4, 2021 at 9:30 amNathanielChongSubscribernI rechecked the Named selection and saw that when I selected the duct wall surface, I accidentally selected the diffuser surfaces too. After I corrected the my mistake, I was able to get some velocity streamline out into the room. Thank you for your Help Mr Peter. Thank you so so much. Now i can try to include the energy equation and run more iterations.nnApril 4, 2021 at 11:12 amNathanielChongSubscriberI have ran the simulation for a few times now with some adjustments. This is the result so far.nNote the flat energy equation line.nThis is the problem that i am facing. Notice that the temperature contour is constant throughout the room. I have tried increasing and decreasing the magnitude of the temperature but nothing changed. Did I set up the simulation wrongly? Convergence warning also showed up when i ran the initialisation.nHow do I get a more acceptable temperature contour? I just need something to analyse for the report. Thank younApril 4, 2021 at 1:57 pmpeteroznewmanSubscribernPlease show the Boundary Condition for the Inlet.nWhat temperature are you initializing the domain to?nApril 4, 2021 at 3:15 pmApril 4, 2021 at 4:22 pmpeteroznewmanSubscribernIf you run a Steady State simulation, then the domain will end up at the inlet temperature of 273 K.nIf you switch to Transient and change the inlet temperature to 280 K, then you can see the hot air come into the duct and then the room over time.nViewing 37 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
- how to improve the inflation quality at sharp corners?
- ANSYS Workbench Measuring within Design
- check element type
- The mesh file exporter could not resolve cyclic dependencies in overlapping contact regions error
- How to resolve Mesh Failure
- Meshing Error
- Error in meshing
- Conformal vs Non-Conformal Mesh
- execution error inside the mesher. The process suffered an unhandled exception or ran out of memory
- inflation created stairstep mesh at some location
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.