Reduce Mesh Skewness for an isolated generic building

    • I am doing a project where I need to simulate natural ventilation for an isolated generic building. When it comes to meshing, The skewnes is very high that is 0.9999+. 

      And this is the meshing.

      I used the hex dominant method as my supervisor said it will be much better for a cube shape building. However, i cannot reduce the skewness of the mesh. I am very new to this software, and I am trying to learn it in any possible way. Thank you in advance.


    • peteroznewman

       Skewness can be improved by editing the geometry in two ways:

      1) Remove small details from the geometry that are unimportant to the simulation. This will allow the mesher to use larger elements.

      2) Slice the geometry into pieces that are easier to mesh. The pieces have to be put into a Multibody part so the mesh reconnects the pieces.

      There are some mesh settings that allow mesh quality to be improved. One is the Mesh Defeaturing setting. That is like #1 above, but without doing any actual work on the geometry. That is found under Mesh Details. The mesher chooses to ignore small features and bridges elements right over them.

      There is a feature called Virtual Topology that can be applied that automatically selects multiple small faces of the solid and replaces them with one larger face. Right click on Model and Insert Virtual Topology.

      It will be easier to recommend a specific approach if you attach your Project Archive .wbpz file to a reply and say which version of ANSYS you are using.

    • Thank you for your reply. I'll try to do the solution as you mentioned above first. Here is the file of my project. If my file is wrong, please tell me so as I am very new to ANSYS. I am currently using ANSYS version 15.0.0.

    • peteroznewman

      The Attach button allows file extensions of .zip and .wbpz   Follow these instructions to create a .wpbz file from your project.  The file size must be less than 120 MB. If your .wbpz file is larger than that, you must right click on Mesh and Clear Generated Data, then save your project, then create the .wbpz archive file. It will be much smaller after the mesh has been cleared.


    • I did as what you said but the size after that is 1.43gb. I still cannot upload the file.

    • peteroznewman

      Do you use Gmail?

      Large attachments on Gmail are put on Google Drive and a link is created to send as the email content with no attachment.

      There are similar tools on other email systems. There are also services like Dropbox for sharing large files.

      Please reply with a Google Drive link.

    • https://drive.google.com/open?id=1ESCq9yLSceK22-NByxsFDYCncWMAn_Xw


      Here is the link to the project. Sorry for the trouble.

    • peteroznewman

      I have the file. It was so large because you did not Clear Generated Data on the mesh.

      I have 15.0 on another computer, but I made these snapshots on a newer version. I can redo this on 15.0 if you need more help.

      I suggest you idealize and simplify the problem somewhat and use a zero thickness surface for the "building". That is as simple as adding a MidSurface feature on the solid building.  I also suppressed the extrusions that make up the block of air and the cut body operation.  Instead I use an Enclosure. The solid and surface body are put into the same part using Form New Part.

      Then you will have one solid with a zero thickness walled building to mesh.

      The next thing I did was to create 5 planes, one on each face of the midsufaced building, and Slice the air up using those 5 planes. Select all the solid pieces and Form New Part to have the mesher connect them together. These solids are all put in a Multizone control to be meshed with hex elements. Here is the skewness report.

      I have not added any mesh refinement yet, that still needs to be done to get many elements around the windows and over the building.

      For other members, I attach an ANSYS 18.2 version of your file here, which you can't open. But if you want a 15.0 version, let me know.

    • Thanks for lending your time to help me. Well, for my project, I need to follow the building specification as the previous simulation and the building itself has thickness. My objective is to get the effect of different between each turbulence models and evaluate the performance of each turbulence model. May I ask if the enclosure's can be change or not as I need to use that block of air that you suppressed as my domain. Do you have any suggestion on how can I do without removing the thickness of the building. 1 more thing, what type of method is the best for generic building? Is it tetrahedrons or hex dominant?

      Thank you in advance.      

    • Also, can I ask for the 15.0 version? I want to look at how you create the geometry. Thanks

    • peteroznewman

      You can keep the building thickness by using 10 planes to slice the air up at the inside face and the outside face of each wall and the roof. I could do that to your existing solids, so the dimensions of the air will not change.

      I need more time to do this in ANSYS 15 so will post another reply later.

    • peteroznewman

      After the slicing as shown in the video is done in DesignModeler, open Meshing and assign all solids a Multizone mesh control and you should have a a low skew mesh.

    • Thank you so much for the video. It was really helpful. I'll try to follow your instruction and proceed to mesh if I can. Here is the archive file for the mesh only. My question is can I proceed to do mesh without making the parts into 1? As I was told by my senior that I need to make it into 1 part, 1 body first, only then I can proceed with the meshing.    

    • peteroznewman

      In DesignModeler, when you select all solid bodies and Form New Part, that puts all the bodies into a single part that has Shared Topology. That means nodes on coincident faces will be shared.  That means when meshed, it will be as if it was one body, but the slicing helped the mesher to conform to your problem and make nice shaped elements.

      Do you know about inflation layers?  That is important in meshing near walls in Fluent models.

    • Ok. Thank you for the explanation.  I'll try to do it later. I know a little bit about the theory of the inflation layers. However, I dont exactly know how to do it. I remembered my senior said to me that my project is not that difficult but I am stuck at mesh already. There was once I tried to proceed even the skewness is high and as the result, my simulation turned out to be the opposite as the previous simulation done by other researchers.

    • peteroznewman

      I was able to open your Mesh Only file. You can add a Fluent system by dragging and dropping it on Mesh and it will look like this:

      You can build your Fluent model, and if you want to send me the mesh to edit in 15.0 and send back to you, all you have to do is delete the Fluent system and Save As a new file name, File, Archive and send that to me.

      Please make the 10 planes and 10 slices, the reply with a new mesh only archive attached and I will make a video on inflation layers for you.


    • I did 10 planes and 10 slices like you said. After that, I proceed with the mesh by using hex dominant method. Please correct me if I'm wrong. I tried to named the surface like inlet, outlet, walls and the building. However, when I tried to create named selection for the building, I can't seem to select the outer surface of the building. Here is the new mesh only archive attached. 

    • peteroznewman

      Here is a video on how to select the faces of the building walls. I forgot to mention to suppress the contacts in the Connections folder. In another video I will cover inflation.


      ANSYS 15.0 archive is attached

    • Thank you Peter for the video. I never knew about the box select. Really come handy when selecting the building. Thanks a lot. I'll wait for your next video. One more time, thank you.

    • peteroznewman

      Hi fox3ss~,

      I spent some time on your model last night.  That file has 60 solids after being cut by 10 planes, while my file with 5 planes to slice a zero thickness building out of the air only has 18 solids.  Since you are learning how to build a CFD model, I recommend you first get the zero thickness version working, then move on to the building with thick walls, which is 3 times more challenging to get a good hex mesh compared with the zero thickness building. The wall thickness in the image below is the cross shape, and you can see the inflation layers around that corner of the building. The air that is before and after the building wall probably should have 10 elements across the thickness.

      I plan to record a video to demonstrate creating inflation layers on the 5-plane sliced geometry and expect I will post a reply in the next four hours. Hex meshing takes a lot more time and effort to create than the tet element methods.

      If you go with tet elements instead of hex, there is a simple way to turn on automatic inflation for every surface that belongs to a named selection. You might look into that.


      Other members are welcome to suggest other approaches.

    • Thank you. I'll make sure to try take a look into that. I guess I will try from zero thickness first then.

    • peteroznewman

      These two videos show the automatic inflation capability of meshing. The video is in two parts.



      With a lot more work, it is possible to control the mesh more manually and improve the few elements with high skewness.

    • Thank you for the video. I will definitely take a look at the video. For now, I am a little bit busy with my schedule. I really appreciated with your help. Thanks

    • ahmadzaki



      Thank you for your tutorials and detailed answer. I tried this method and succeeded in generating a structured mesh that worked fine in FLUENT. However when I implemented the same mesh to CFX it didn't work?!!

      you can see the problem here: https://studentcommunity.ansys.com/thread/error-in-importing-mesh-to-cfx/

      Thank you for your support

    • Manuela1398

      Suddenly someone has a tutorial on the design of a one-story house that you can provide, please


Viewing 24 reply threads
  • You must be logged in to reply to this topic.