Geometry preparation for CFD

peteroznewmanpeteroznewman Member Posts: 97

@NathanielChong asked about how to create a mesh to make a CFD analysis of duct work that circulates air in a lecture theatre.

Nathaniel, you provided an IGES file that has 5,029 individual surfaces.

Instead, create three solids. One for each duct tree and one for the room. You can make just one solid for the duct tree because the other one is a mirror image. The duct tree solid should have faces to indicate inlet and outlet of air.

«1

Comments

  • kkanadekkanade Posts: 3,319Forum Coordinator

    From image it looks like solids. For this user needs to extract he fluid volume first.

    User can check following video for volume extract.

    After that as Peter has suggested, please check if you can reduce problem size by using mirror.

    User can also check following for meshing.

    Please check following videos


    Ansys Meshing Sizing:

    https://www.youtube.com/watch?v=w4q6q8nKF3U

    Regards,

    Keyur

    How to access Ansys Online Help Document

    How to show full resolution image

    Guidelines on the Student Community

    How to use Google to search within Ansys Student Community

  • NathanielChongNathanielChong Posts: 23Member

    @peteroznewman Thank 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.

    Regards,

    Nathaniel

  • NathanielChongNathanielChong Posts: 23Member

    @kkanade Thank 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?

    Regards,

    Nathaniel

  • peteroznewmanpeteroznewman Posts: 11,404Member

    @NathanielChong

    You need to create a solid from the duct. I used SpaceClaim and the Blend tool to make a solid between the opposite surfaces of the duct.

    Here are hundreds of surfaces.

    Here is a single Solid body that is the start of the duct tree. I used a Sketch to imprint the outlet face onto the duct solid.

    Attached is a zip file that contains a Parasolid file that you can open in SolidWorks to get the idea.

  • NathanielChongNathanielChong Posts: 23Member

    @peteroznewman Thank 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,

    Nathaniel

  • NathanielChongNathanielChong Posts: 23Member

    @peteroznewman If i create the duct solid using the blend function, will the duct still be hollow?

  • peteroznewmanpeteroznewman Posts: 11,404Member
    edited March 17

    @NathanielChong

    You 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.

    The 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.

    An 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.

    Try 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.

  • NathanielChongNathanielChong Posts: 23Member

    I 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.

    Also, is there an easy way to draw a the theatre walls as drawing the walls were really challenging for me in this model?

  • peteroznewmanpeteroznewman Posts: 11,404Member
    edited March 17

    @NathanielChong

    The 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.

    The 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.

  • NathanielChongNathanielChong Posts: 23Member

    @peteroznewman

    Should 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?

    Thank you for your guidance as all this is very new to me.

  • peteroznewmanpeteroznewman Posts: 11,404Member
    edited March 17

    @NathanielChong

    It is simpler to model one duct first, including imprinting the diffuser circles on the faces of the solid.

    Then create a mirror image of that first solid using a Mirror function.

    Then draw a rectangular box for the theatre room, then do the boolean subtract.

    Each 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.

    The last step, creating Shared Topology, can only be done in DesignModeler or SpaceClaim. I provided instructions on what to do in SC.

  • NathanielChongNathanielChong Posts: 23Member

    @peteroznewman

    Duly noted. Will start working on it. Again, thank you so much for the help.

    Regards,

    Nathaniel

  • NathanielChongNathanielChong Posts: 23Member

    @peteroznewman

    Dear Mr. Peter,

    I 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?

    Also, at what stage should i define the walls of the ducts and the walls of the theatre


    Thank you.

  • peteroznewmanpeteroznewman Posts: 11,404Member

    @NathanielChong

    You 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.

  • NathanielChongNathanielChong Posts: 23Member

    Dear @peteroznewman,

    Thank 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.

    I 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?

    Hope to hear from you soon.

    Thank you.

  • NathanielChongNathanielChong Posts: 23Member

    @peteroznewman

    Upon 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).


  • peteroznewmanpeteroznewman Posts: 11,404Member
    edited March 26

    @NathanielChong

    I 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.

    Did you use the Share button on the Wokrbench tab in SpaceClaim?

    In Meshing, did you see any contacts created under the Connections folder? Delete them.

    Looking 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.

    I 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.

    It'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.

  • NathanielChongNathanielChong Posts: 23Member

    @peteroznewman

    At the moment, I have four outlets extruded on the room body and it is all defined under one outlet named selection.

    I 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?

    I 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.

    I 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.

    Oh I see. But it showed warning messages when I opened the setup in the bottom right console window.

    Also what does "interface" boundary condition means?

  • peteroznewmanpeteroznewman Posts: 11,404Member
    edited March 26

    @NathanielChong

    When 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.

    Once 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.

    Here 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.

    But 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.

    When 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.

    Drag 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.

    Good luck!

Sign In or Register to comment.