[John222]

I'm trying to mesh a U-bend in ANSYS for later FLUENT simulations.

I can't think of a proper mesh to adopt in this case (180 degrees pipe).

I would believe a C-grid is the most reasonable. But I lake the expertise to do such complex grid using ANSYS MESH.

Anyone have good tutorial or idea of how to mesh this complex geometry, would be much appreciated?

[John222]

Originally Posted by John222

I'm trying to mesh a U-bend in ANSYS for later FLUENT simulations.

I can't think of a proper mesh to adopt in this case (180 degrees pipe).

I would believe a C-grid is the most reasonable. But I lake the expertise to do such complex grid using ANSYS MESH.

Anyone have good tutorial or idea of how to mesh this complex geometry, would be much appreciated?

Will I get an answer. Or just wasting my time here?

[jsm]

Hi,
If I understood your question clearly, here is my comments.

For simple geometries, you can use sweep or multizone mesh method to get full hexa mesh. For complex geometries, multizone method with "ICEM CFD interactive option enabled" is the best way. You can move the block edges to get good quality meshes.

If you post image of geometry, you will get better comments and solution quickly.

with regards,
Subramanian

[diamondx]

would you mind sharing your geometry ?

[abhiprayj]

http://www.youtube.com/watch?v=tYrbScUH9RE

Part 1 2 and 3

Hope it helps and gives some idea.

[John222]

Originally Posted by diamondx

would you mind sharing your geometry ?

[John222]

I want to mesh the geometry using ANSYS WORKBENCH MESH not GAMBIT or anything else.

[diamondx]

i'm not an ansys meshing expert (i really need to start playing with it a little bit). but i can mesh it with icem cfd. I'm sure that somebody with an expertise in ansys meshing will help you with this geometry.

[John222]

Originally Posted by diamondx

i'm not an ansys meshing expert (i really need to start playing with it a little bit). but i can mesh it with icem cfd. I'm sure that somebody with an expertise in ansys meshing will help you with this geometry.

If I do the mesh in ICEM CFD. Can I then save the case so I can run ANSYS FLUENT using the mesh done in ICEM CFD, or it has to be done in ANSYS WORKBENCH MESH?

[diamondx]

of course you can use with fluent. you can export you mesh and specify as output parameters FLUENT. it doesn't have to be workbench

[Gweher]

Can you please add your .agdb, I'll have a look with Ansys Meshing

[John222]

Originally Posted by Gweher

Can you please add your .agdb, I'll have a look with Ansys Meshing

Please check mail. I have sent you the geometry please note it's a 2D model and mesh must be done in 2D and in ANSYS MESH.

[Gweher]

I had a quick look at your geometry. Well basically if you want a C-grid then the quickest way is to split your geometry. I sliced the U bend into 5 sub-surfaces within DesignModeler, then select all the 5 sub-surfaces and right click >form new part.

After updating inside Ansys Meshing you can assign different element controls in order to get the mesh you want. As I didn't know exactly what you are trying to model I just generate a mesh and added a boundary layer just to show you how to play around with Ansys Meshing. There is not only one unique method to generate a C-grid, and there are lot of different ways to create your boundary layer like adding inflation layers, I did it this way but use the method that better suits you.

As I didn't know if I could upload the .agdb file I attach images of the splitting and the mesh and send you a private message with the .zip file.

[John222]

Originally Posted by Gweher

I had a quick look at your geometry. Well basically if you want a C-grid then the quickest way is to split your geometry. I sliced the U bend into 5 sub-surfaces within DesignModeler, then select all the 5 sub-surfaces and right click >form new part.

After updating inside Ansys Meshing you can assign different element controls in order to get the mesh you want. As I didn't know exactly what you are trying to model I just generate a mesh and added a boundary layer just to show you how to play around with Ansys Meshing. There is not only one unique method to generate a C-grid, and there are lot of different ways to create your boundary layer like adding inflation layers, I did it this way but use the method that better suits you.

As I didn't know if I could upload the .agdb file I attach images of the splitting and the mesh and send you a private message with the .zip file.

Hi

I have ANSYS WB V13 not V14. What are the exact steps to do this kind of mesh?

[Gweher]

Well you can either use slice material by plane and create several planes to cut your surface into sub-surfaces or create several sketches and use them with extrude by selecting the option "slice" within the extrude menu.

I'll explain the first method as you have a simple geometry (but both are basically the same in a way).

1) Starting with your geometry, >tool>freeze (or under your SurfaceSk1 choose "add frozen" instead of "add material"). This will permit to use the slice option (see first attachment - "TreeOutlinePlaneSlice").

2) Create the 2 planes, >create>New Plane, in the options select YZPlane, under transform 1 choose "Rotate about Global Z", and enter 45, >generate. Repeat the procedure 2) for the second plane changing 45 to 135.

3) Now that you have defined the 2 new plane hit >create>slice, under Slice Type select "Slice by Plane" (default) and select the YZ plane, click >generate. This will slice your U bend into 3 parts (see second attachment - "FirstSliceOperation").

4) Repeat point 3) changing the plane YZ to one of the 2 plane you created in point 2) AND change "All bodies" under Slice Targets to "Selected Bodies" and select only the small U bend sub-surface created in point 3) (in order to keep the other sub-surfaces as rectangles).

5) Repeat point 4) by selecting the last plane and only the sub-Ubend surface that needs to be sliced (see third attachment -"SecondAndThirdSliceOperations").

-> You will end with the 5 sub-surfaces you are looking for

6) Under Parts you will now have 5 parts, select them all, right click and >Form New Part, this is important for the next meshing step if you want to have a single mesh and no interfaces between the 5 sub-domains.

-> Now you can easily play with the meshing tool of Ansys Meshing.

[John222]

Originally Posted by Gweher

Well you can either use slice material by plane and create several planes to cut your surface into sub-surfaces or create several sketches and use them with extrude by selecting the option "slice" within the extrude menu.

I'll explain the first method as you have a simple geometry (but both are basically the same in a way).

1) Starting with your geometry, >tool>freeze (or under your SurfaceSk1 choose "add frozen" instead of "add material"). This will permit to use the slice option (see first attachment - "TreeOutlinePlaneSlice").

2) Create the 2 planes, >create>New Plane, in the options select YZPlane, under transform 1 choose "Rotate about Global Z", and enter 45, >generate. Repeat the procedure 2) for the second plane changing 45 to 135.

3) Now that you have defined the 2 new plane hit >create>slice, under Slice Type select "Slice by Plane" (default) and select the YZ plane, click >generate. This will slice your U bend into 3 parts (see second attachment - "FirstSliceOperation").

4) Repeat point 3) changing the plane YZ to one of the 2 plane you created in point 2) AND change "All bodies" under Slice Targets to "Selected Bodies" and select only the small U bend sub-surface created in point 3) (in order to keep the other sub-surfaces as rectangles).

5) Repeat point 4) by selecting the last plane and only the sub-Ubend surface that needs to be sliced (see third attachment -"SecondAndThirdSliceOperations").

-> You will end with the 5 sub-surfaces you are looking for

6) Under Parts you will now have 5 parts, select them all, right click and >Form New Part, this is important for the next meshing step if you want to have a single mesh and no interfaces between the 5 sub-domains.

-> Now you can easily play with the meshing tool of Ansys Meshing.

I can't thank you enough. This is very helpful.

I'm trying to mesh the model and I tried doing a structured mesh the same one you made. But I keep getting non-uniformed mesh for some reason (see attached).



Would you be able to print screen your mesh tree outline so I can have an idea of what you have done to the mesh. Thanks!!

[Gweher]

You just need to add a mapped face (I think it uses pave by default if you don't specify anything), so right click on mesh, >insert>mapped face mesh, and then select all the faces. This should fix your problem.

I've also added a print screen of the mesh tree outline (as I told before I didn't know what you are trying to model so I just added several sizing in order to have more control in each sub-surface domain).

[John222]

Originally Posted by Gweher

You just need to add a mapped face (I think it uses pave by default if you don't specify anything), so right click on mesh, >insert>mapped face mesh, and then select all the faces. This should fix your problem.

I've also added a print screen of the mesh tree outline (as I told before I didn't know what you are trying to model so I just added several sizing in order to have more control in each sub-surface domain).

Thank you! I believe I know the basics now and will continue refining the mesh to meet my needs for later simulation.

Please check your mail box

[Far]

Good information. Learned new things about AM.

[John222]

how can I generate a contour plots that looks like this;