# [ICEM] Hybrid mesh for 2D boundary layer

 Register Blogs Members List Search Today's Posts Mark Forums Read

September 21, 2011, 08:06
Hybrid mesh for 2D boundary layer
#1
New Member

Andrea Bigliazzi
Join Date: Sep 2011
Location: Milano
Posts: 5
Rep Power: 16
Hy Guys,
I am trying to do an hybrid mesh around an airfoil to do a viscous analisys with fluent; I tried to do thta i some manner but everyone of this doesn't work well.
Solution 1: I scale my profile to do the boundary layer region and i mesh this space with an hexa mesh using the bocking startegy( blocking--> 2Dplanar) and the i mesh the external surface with an unstrucutured mesh, and this work but the problem is that when i export it into fluent the bpundary between the BLayer and the external surface is seen as a wall( this is i think because in the region between the airfoil and the boundary there is no surface, so i try to make a surface also in this region, but when i mesh the external surface with unstructured icem mesh also the internal surface)

Solution 2: I meke an unstructured mesh in all the field and i make the boundary layer using curve mesh stup--> height,ratio,layer and this work well but gave me problem at the trailing edge.

I post two images, i hope someone could help me, It's vey important.
Thanks
Andrea
Attached Images
 blayer.jpg (101.4 KB, 890 views) trailingedge.jpg (98.0 KB, 684 views)

 September 22, 2011, 09:00 Remove the line elements #2 Senior Member     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,663 Blog Entries: 1 Rep Power: 47 Lets fix your first approach since the offset method is really more for FEA users making bolt spiders... A wall just means you have line elements in 2D... These formed when you created the hexa mesh (when you associated the blocking to curves and then converted to unstructured mesh, you got line elements along those curves), which was good because the paving method used those line elements to make sure the new mesh fit to the previous mesh... You just need to do a couple more steps at the end to get what you want... 1) assuming this will be one fluid zone, you must put all the shells in the same part (such as FLUID). If you don't Fluent will expect you to have a wall between the zones and will give you an error if you remove the line elements... 2) Remove the line elements between the quads and tris... If you know the part name of your offset curve (and if this name is not used elsewhere) you can just Edit mesh => Delete mesh => Select by part. If the offset curve is in the same part as the airfoil curve (whose line elements you absolutely should not delete), then you could just turn off all the other element types except line elements and use the box select to delete the line elements of the offset curve. Remember, line elements are very important to Fluent. You must NOT delete the line elements around your perimeter. Fluent needs those for bocos and will give you a variety of errors (such as null pointer) if you delete any of those. Actually, I guess if your offset line elements were in a unique part between elements of the same part (FLUID), you could just turn it into an internal wall... But there are usually multiple solutions to any problem. metmet and Awsys like this. __________________ ----------------------------------------- Please help guide development at ANSYS by filling in these surveys Public ANSYS ICEM CFD Users Survey This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)... CFD Online Users Survey

September 26, 2011, 10:34
#3
New Member

Andrea Bigliazzi
Join Date: Sep 2011
Location: Milano
Posts: 5
Rep Power: 16
Hi Simon,
In reference with the last one ('hybrid mesh for 2D boundary layer') I did my job in another way, different from your.
I did an hexa mesh for the boundary layer with a 2D planar blocking, then I did my farfield and I made an overall surface into that. I cut the surface into the airfoil and i leave the surface between the airfoil and the boundary layer calling him 'stlim', the rest of the surface, betwen the boundary layer and the external domain is called fluido. Then i make some subregions for the refinement of the mesh and i create the unstructured all tri mesh with the 'respect line element' enabled, and the results is good. But the lines that delimitates the subregions are for me only construction line and they shouldn't have seen from fluent, so i export my mesh in fluent and i gave to these lines ( for examples the red line delimitating hexa and all tri mesh in the following picture) the 'interior Bounday Condition', do you think that this approach could be correct ?
Thanks a lot
Andrea
Attached Images
 total domain.jpg (68.6 KB, 454 views) airfoil.jpg (70.8 KB, 561 views) hexa and all tri mesh.jpg (56.8 KB, 481 views)

 October 3, 2011, 14:50 Delete the line elements. #4 Senior Member     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,663 Blog Entries: 1 Rep Power: 47 Yea, if you don't mind the work, this is a great example of the flexibly of a tool like ICEM CFD. Your only problem is that you still have line elements between your regions and Fluent is seeing these as walls. The fix is easy. 1) make sure your shell elements are all in the same part (aka zone in fluent), otherwise you will have trouble with the next step... 2) Delete all the line elements from the construction curves (and only from the construction curves since you need them elsewhere). You can do this by part if they were done with a unique part name, or you can just turn off all the other element types and select the lines manually with a box. Once these line elements are gone (assuming the parts on either side are the same) you shouldn't have any trouble. 3) another option is just to define the lines as "internal walls" for Fluent, but I would just delete them. Awsys likes this. __________________ ----------------------------------------- Please help guide development at ANSYS by filling in these surveys Public ANSYS ICEM CFD Users Survey This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)... CFD Online Users Survey

 December 31, 2012, 11:31 Boundary layer zone creation for an airfoil #5 New Member   Manuel Martínez Castro Join Date: Dec 2012 Posts: 1 Rep Power: 0 Hi Andrea, How did you manage to create the region of the boundary layer by scaling the airfoil in icem? I have tried geometry/transform geometry/scale but the created curve is not satisfactory, it does not create a "parallel" airfoil with constant distance from the original airfoil. Thanks, Manuel

 March 15, 2013, 20:34 #6 Senior Member   Jie Join Date: Jan 2010 Location: Australia Posts: 134 Rep Power: 16 Hi Bigio and PSYMN I am trying to build a simple hybrid mesh of a circular flow domain with wall around it as I am trying to simulate a stationary vortex (an inner circle-vortex core + an outer circle around the core). I meshed the vortex core which is unstructured (orange region). Then, I meshed the outer region, which is structured. Then, I load both meshes together and merge them by icemcfd. However, when I load it into OpenFOAM, the interface between the two meshes become undefined surface with type wall. I tried to delete the interface in icemcfd, but I got some unclosed the surface error. I just wonder how should I merge the two mesh properly so that I would not have these undefined surface at the interface? I will try to attached the picture shortly. Thank you. jiejie

 March 16, 2013, 08:46 #7 Senior Member     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,663 Blog Entries: 1 Rep Power: 47 If the two volumes are different materials it will expect a wall between them. You can handle that in the solver (just call it an internal wall), or you can put all the volume elements into the same volume part and remove the wall (assuming the nodes are merged). Awsys likes this. __________________ ----------------------------------------- Please help guide development at ANSYS by filling in these surveys Public ANSYS ICEM CFD Users Survey This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)... CFD Online Users Survey

March 16, 2013, 17:16
#8
Senior Member

Jie
Join Date: Jan 2010
Location: Australia
Posts: 134
Rep Power: 16
Quote:
 Originally Posted by PSYMN If the two volumes are different materials it will expect a wall between them. You can handle that in the solver (just call it an internal wall), or you can put all the volume elements into the same volume part and remove the wall (assuming the nodes are merged).
Hi PSYMN

Thanks for the quick reply. When I created two meshes, I define both flow domain as FLUID.

I tried to remove the "interface" wall, but it cause open cells in this case. As I am doing a 2d mesh, there is no volume element in this case.

I have attached the mesh here: the orange is the vortex core region and pink is the outer region. I created them separately. After I merged them, the interface between the two meshes become a wall.

Thanks

jiejie
Attached Images
 circularMesh.jpg (97.1 KB, 242 views)

Last edited by jiejie; March 17, 2013 at 00:09.

 March 17, 2013, 12:43 #9 Senior Member     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,663 Blog Entries: 1 Rep Power: 47 The same rule applies with one dimension less. You can't have a zone like "Core", adjacent to another zone, without something between them to apply the boundary condition to. This is just a basic need of the solver. If the core and the surrounding quad mesh are node for node conformal mesh and your only problem is boundary between them, just put all the shell elements in the same part. For instance, put it all in CORE, or create a new Part called FLUID and put all the shell elements in that. Don't put the line elements or point elements in that FLUID part, they need to be in separate parts so you can apply boundary conditions. __________________ ----------------------------------------- Please help guide development at ANSYS by filling in these surveys Public ANSYS ICEM CFD Users Survey This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)... CFD Online Users Survey

 March 17, 2013, 18:05 #10 Senior Member   Jie Join Date: Jan 2010 Location: Australia Posts: 134 Rep Power: 16 Hi PSYMN Unfortunately, the core and surrounding nodes at the interface are not conformal. What should I do in this case? or what should be the correct procedure to produce such a mesh in this case? Thanks a lot. jiejie

 March 17, 2013, 20:43 #11 Senior Member     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,663 Blog Entries: 1 Rep Power: 47 You could go with a non conformal interface. Or you could use the edit mesh => Repair mesh command to sew the meshes together... If it were me, I would probably have generated the core mesh after the hexa mesh and would have just started from the perimeter so it would have been generated conformally. It is mostly just a matter of doing things in the right order. How did you generate the core mesh? jiejie likes this. __________________ ----------------------------------------- Please help guide development at ANSYS by filling in these surveys Public ANSYS ICEM CFD Users Survey This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)... CFD Online Users Survey

 March 17, 2013, 20:46 #12 Senior Member   Jie Join Date: Jan 2010 Location: Australia Posts: 134 Rep Power: 16 Hi PSYMN I generated the core mesh and outer mesh separately as in two separate icem project, then I load the two mesh into a new project and try to merge them together. For the core mesh, I create a 2d circle with surface and then mesh it with the unstructured tri-elements. I think my problem is how to mesh the two region. In my case, I can mesh the outer region with the proper block topology and I define a material point in the out region as "FLUID". Then, the problem appears as I move on to mesh the core region. If I tried to mesh the core region with unstructured mesh by "Mesh" -> "Part mesh setup" -> "Computer mesh", icemcfd will remesh the outer region as well as the outer region was in the "Part mesh setup" as well. Or should I define a different material point in the core region? I think my problem is no matter which part I mesh first, this part will be overridden by the second part of the mesh. jiejie Last edited by jiejie; March 17, 2013 at 22:16.

 March 17, 2013, 23:22 #13 Senior Member   Jie Join Date: Jan 2010 Location: Australia Posts: 134 Rep Power: 16 Hi PSYMN I think I fixed the problem I had previously by trying a coarse two region mesh and I will try a properly built one. Now I can mesh both region together by shifting the body (material point) from the one region to the other. In my case, I mesh the outer region then the core region. Thank you very much for your time and help. jiejie

 March 18, 2013, 07:25 #14 Senior Member     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,663 Blog Entries: 1 Rep Power: 47 In 2D meshing, the body (material Point) is irrelevant. But if you load your quad mesh and mesh the core region afterward with the option to "respect line elements", the mesh in the middle will be generated conformal with the pre-existing mesh. __________________ ----------------------------------------- Please help guide development at ANSYS by filling in these surveys Public ANSYS ICEM CFD Users Survey This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)... CFD Online Users Survey

 March 20, 2013, 00:42 #15 Senior Member   Jie Join Date: Jan 2010 Location: Australia Posts: 134 Rep Power: 16 Hi PSYMN The material point is irrelevant for 2D mesh (almost forgot it after a lot of 3D meshes) as I managed to create the mesh without moving the material point. I am also curious about the merging mesh you mentioned. I load the core region mesh. Then load the outer region mesh. After I chose the 2nd mesh (outer region), icem asks whether I want to merge them together. However, I could not find the option to "respect line elements"? Thanks jiejie

June 28, 2013, 11:42
#16
Senior Member

Sijal
Join Date: Mar 2009
Posts: 4,553
Blog Entries: 6
Rep Power: 54
Quote:
 Originally Posted by PSYMN Yea, if you don't mind the work, this is a great example of the flexibly of a tool like ICEM CFD. Your only problem is that you still have line elements between your regions and Fluent is seeing these as walls. The fix is easy. 1) make sure your shell elements are all in the same part (aka zone in fluent), otherwise you will have trouble with the next step... 2) Delete all the line elements from the construction curves (and only from the construction curves since you need them elsewhere). You can do this by part if they were done with a unique part name, or you can just turn off all the other element types and select the lines manually with a box. Once these line elements are gone (assuming the parts on either side are the same) you shouldn't have any trouble. 3) another option is just to define the lines as "internal walls" for Fluent, but I would just delete them.
Hi Simon.

Greeting. I found both solutions useful and making a tutorial on it. 4

I have one question, is it possible to add density in tetra mesh ?

 June 28, 2013, 12:23 question #17 Member     sadjad Join Date: Jan 2012 Posts: 72 Rep Power: 14 hi ahmed, you mean "tri"? __________________ ICEM, CFX and Fluent expert

 June 28, 2013, 12:30 #18 Senior Member   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,553 Blog Entries: 6 Rep Power: 54 yes and tetra (patch dependent)

 June 28, 2013, 13:05 Answer #19 Member     sadjad Join Date: Jan 2012 Posts: 72 Rep Power: 14 i tried it already and my experience says that: Density boxes are just for 3D. For getting smaller mesh in particular regions in 2D, separate those regions in other surfaces and mesh them separately with smaller mesh size. It seems that absence of Gambit Size function is sensible, particularly in 2D cases. __________________ ICEM, CFX and Fluent expert

 June 28, 2013, 13:09 #20 Senior Member   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,553 Blog Entries: 6 Rep Power: 54 yeah, I am also missing gambit size function speically in 2d