Hexa + Tetra meshing (Hybrid) in ICEM
I have to monitor flow over a cylinder.....My domain is pretty simple.....Its just a square domain with a cylinder around it......I need a hexa mesh around the cylinder and tetra mesh filling the rest of the domain ........ I did not find any tutorial related to it........!!!!!!!! Can someone help me out ???
As a variant to mix tet and hex one can do:
1.hex mesh of a solid/fluid attached to the surface, where you need later to have a connection with tetras.
2.saving a surface mesh of a contact surface
3.loading the surf. mesh to a new file and changing QUADs to TRI
4.making tet using the existing mesh (without smoothing - to prevent changes in the "interface")
5.smooth tet excluding the connection face
6.loading hexa and tetra in one file and merging
I did not get any of it !!!!!!!!
Is there any PDF that I may refer to ???
I think you just need to block the domain, and then change the block you want to unstruct (Edit block -> convert block type -> Type free).
Ogrid in a box...
This is a very simple topology, so we don't have a tutorial for it explicitly, but the SphereCube tutorial is a very similar idea (Sphere in a Box), and explains how to use Ogrids..
I guess this is what you are looking for...
To get it, I start with my initial 3D Block around the box, split twice in across each end to "block" out my cylinder. Then I run an Ogrid thru the central block with faces on the ends. Then I associate the edges with the curves (actually, I used the auto associate button and did everything at once). Then I deleted the central block (inside the pipe) since it was not part of my flow domain. Then I set up my edge distributions and took the picture... I also attached the files.
Or perhaps you were looking for a swept block like this...
TO get it, I made sure that I built topology on the model (it connects the geometry). Then I created 2D surface blocking (automatic), with the sweep option. I selected both ends and the source faces. THen I did the 2D to 3D MultiZone Fill with the sweep option. (This model was so simple, I guess I could have just blocked the one side and done a 2D to 3D translate).
But I guess you want boundary layers around the pipe;
so I went back and put an Ogrid around that (at the blocking level), setup edge params and output the mesh again. I also saved this version of the model.
note: I didn't select both sides for this later Ogrid, so it came out the sides of the model (boundary layer across the back...)
Oops, here are the files...
blocked and swept with Ogrid... You can sweep it differently to get the ogrid from end to end... Or just turn on the option for boundary layers around the pipe during the 2D to 3D sweep step...
Thanks a lot Simon.
Hi. I want to do meshing around a cylindrical body in cube domain with ICEM like this video:
I am new to ICEM . I want to simulate vortex shedding behind the pipe.
I read the above mentioned tutorial but I couldn't perform the meshing. I used the geometry was built in ansys workbench . can any one help me?
If you already have the geometry, is it 2D or 3D...?
I would just use 2D and shell mesh it, but if you use 3D, the steps are similar, but you should sweep it and then do the shell controls on the source face...
What you want to do is use the default ANSYS Mesher (shell or sweep), but right click on the body to insert an inflation method into the body (the surface for 2D or the sweep source for 3D) using the circular curve. Set a number of layers and an initial height appropriate to capture the viscous boundary layer.
Then setup named selections for boundaries, etc.
That is it...
a circle in a rectangle is pretty easy, try some tutorials if you just need to get some basic skills first.
Hi, thank you for the reply. I used the default ansys mesher with 20 inflation layers, but the processing time was too much because the default meshing was not appropriate for this case I think. . I want to know if I could use structural meshing from ICEM, like the video linked in my last post,will the problem be less time consuming?
I have problems in associating the split lines to vertices on cylinder. I don't know how to create vertex on cylindrical part of the fluid.
also, I don't know whether I should import both the cylinder and fluid parts in ICEM, or just the the fluid.
I forgot to tell you. it is a FSI problem. vortex induced vibrations for the circular cylinder.
Unless you want to model the solid, you only need the fluid parts. And you don't need to associate the verts at all.
You could just associate the edges to the curve...
The blocking is just a very few steps...
Most of the fluid is an HGrid, but then split out a box around the hole (some distance away), put an Ogrid in the box with faces on the ends of the cylinders. Then delete the hgrid at the center of the OGrid. Associate the inner edge of the Ogrid with the curves. Associate the outer edges of the Farfield with the box. Associated verts with points if they are handy. You should have points on all sharp intersections (such as corners) but they are not really necessary for smooth connections like around a circle.
thanks for really useful answer, Simon. I created the Hmesh and Ogrid, but I still have problems in refining issues (I need refined edges in my case). I guess I should describe my meshing steps:
1. importing the geometry, creating 2 parts and creating body (LIVE as in tutorial)
2. blocking the geom, splitting around the cylinder
3. creating Ogrid around the cylinder and Association the corresponding edges to the cylinder curves. deleting block in the ogrid
4.using Blocking>Pre-mesh params>refinement for ogrid with leval 5
5. using Mesh>Surface mesh setup and defining the values like the case without refinement
6.using mesh>Curve mesh setup and defining the params like the case without refinement
7.using Mesh>compute mesh with Hexadominent, all boundary and inherited.
I did the above mentioned steps many time with various values as input, but no change was appeared in meshing. I guess this method is not appropriate for Hmesh. It would be great if you can help me out
2 to 1
I don't know of any solver that supports 5 to 1 refinement. perhaps that is where your work broke down...
Try 2 to 1 for fluent or 3 to 1 for CFX (but you will need to Edit Mesh => Merge Meshes => Resolve Refinements since CFX doesn't actually support hanging nodes at all.)
If you post images, I may be able to help more.
|All times are GMT -4. The time now is 05:50.|