CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] ICE Mesh in ICEM - Block merge (http://www.cfd-online.com/Forums/ansys-meshing/130355-ice-mesh-icem-block-merge.html)

AA29 February 24, 2014 19:41

ICE Mesh in ICEM - Block merge
 
3 Attachment(s)
Hi everyone,

I am relatively new to ICEM, and I am trying to mesh an engine with two vertical valves in ICEM. Due to requirement of the solver , i need to have a sliding interface (2 surfaces at the same location overlapping each other but with a non -conformal interface after meshing) around the valves so as to allow for layer addition and removal. Hence i am trying to mesh two regions separately(green and orange in figure) i.e. make two separate blocks as i go and merge them as i need a non-conformal interface. The merge works fine, but when i recompute the mesh (using premesh) it looks like two surfaces can not co-exist and the mesh for one of the surfaces gets deleted, and the mesh also gets changed, as in more number of nodes on a particular edge.

My understanding is that when i merge the blocks, i get a common edge(associated with the interface surfaces) and hence a non-conformal interface will not be possible?

Moreover the same problem occurs when i try and merge the unstructured tetra mesh for the intake and exhaust ducts with the hexa mesh.

Is there a way to get around this ? Is my approach wrong or something

Thanks for your time. I would really appreciate the help.

AA29 February 25, 2014 11:57

Anybody who can help me out a bit. maybe with the approach to achieve such mesh?

diamondx February 25, 2014 13:45

Quote:

Hence i am trying to mesh two regions separately(green and orange in figure) i.e. make two separate blocks as i go and merge them as i need a non-conformal interface.
If you need two separate surfaces, why merging them. If I were you, I will totally block and mesh the orange part in a completly different project, do same for the other one. create their respective msh files. and load them separatly in Fluent

AA29 February 25, 2014 13:50

Thanks a lot Ali.

That makes sense . But can i combine both these meshes in Fluent into one .msh file?

My final objective is to use this mesh in OpenFoam.

Thanks again.

diamondx February 25, 2014 13:56

I don't know about Openfoam, in Fluent it is doable.
Moreover, if you want one msh do this:
-Mesh the orange part in a project, generate its unstructured mesh, call it orange-mesh.UNS
-Mesh the green mesh, generate its unstructured mesh, click files - open mesh and open the orange one, ICEM will ask you if you want to replace or merge, click merge. you will have the two unstructured mesh. then you can output it into on msh file, hope I was clear

AA29 February 25, 2014 14:03

Thanks for your prompt reply. This makes things a lot clear.

So what you are saying is rather than merging the blocking and then loading the mesh from blocks, i mesh them separately ,convert it to an unstructured mesh (i hope i will still get hex cells?) and then merge these two meshes as two unstructured ones.

Also, since you are saying it is doable in Fluent (as in fairly easily?) , it should be possible for me to open two .msh files and export a single .msh file from FLUENT. Then I can use it for OpenFoam. Hope i got that right !

Thanks.

diamondx February 25, 2014 14:28

Quote:

So what you are saying is rather than merging the blocking and then loading the mesh from blocks, i mesh them separately ,convert it to an unstructured mesh (i hope i will still get hex cells?) and then merge these two meshes as two unstructured ones.
YES

Quote:

(i hope i will still get hex cells?)
When you block your geometry, you still don't have a mesh, you a BLOCKING. that blocking needs to be converted to a mesh, unstructured does not mean your mesh will become unstructured, it just means that you will have a mesh that you can save as .UNS . (It is true that if you are beginer "convert to unstructured" leads to a confusion, folks at ansys should have came up with a different name)

In Fluent, you can load up two meshes separatly, but you cannot export a mesh. you will end up with a case file, that's it.
feel free to ask more questions...

AA29 February 25, 2014 14:49

Hi,

Then I would say Fluent is not an option ! I will try merging the "unstructured" mesh in ICEM then. I will try to do what you said and lets hope i dont have to ask any further questions !

Thanks a lot Ali. :)

bluebase February 26, 2014 12:34

It is possible to create those two interface meshes out of the blocking structure.

The key is to set up TWO Topologies. See the subnode "Topology" in the Blocking tree. It will probably show the key "root". With a right click you can create subtopologies and move your blocks in these sets.

To get the merged mesh with both interfaces do following. Have the interface surface Geometry in one part set.
# Activate just the first topology
# create Premesh with the first topology
# convert premesh to unstructured (for fluent), check if boundary mesh was created
# Deactivate the first topology and activate the next
# again create premesh (the first premesh zone shouldn't be included anymore)
# again convert premesh to unstructured

If you load a mesh like this into fluent, it will write a warning and divide the interface set into two sets.
This did the the job for me for a sliding mesh simulation in fluent.

Hope this helps.
Sebastian.

Mack March 1, 2014 17:54

Just one more tip for your mesh: use "o-grids" for the valves and the cylinder, otherwise you will end up with very bad quality elements. There is an example on ICEM (valve port or elbow) showing how to use this function.

Regards,
Mack

AA29 March 1, 2014 18:14

Thanks Sebastian and Mack for your suggestions.

Converting to unstructured mesh and then merging the mesh works right for me. What Sebastian suggests I think it will get me the same end result .
Right now I am trying to improve the "bad elements" as Mac suggested. I did use O grid the first time itself ,but I think I did not do it right. Anyways thanks again for your time, I will let you know when I hit a dead end again :D

AA29 March 25, 2014 14:11

1 Attachment(s)
Hello guys,

I have a question about projecting nodes on a surface/ curve in ICEM. I have a cylindrical sliding interface(the purple part in the picture) and i want to project all the points/nodes on to a perfect (analytical) cylinder. How do i ensure that? I have already used "project on surface" tool , but the surface itself is faceted. Also i am not sure if the surface is cylindrical , as I made that surface by extrusion of a curve which was obtained by a surface-surface intersection of the cylinder-head and intake duct.
So what does project on surface tool do? Does it project the nodes on the faceted surface (which is visible to us) or to a analytical surface?

Thank you for your time.

Mack March 27, 2014 17:39

Hi,

Actually you do not need to "project to surfaces", once ICEM looks for the closer surface and projects it automatically. However, sometimes when you want to project the mesh to a different surface, then you use this command. It also happens when you accidentally defines one edge to the geometry and latter one realizes it was wrong, so you remove the edge association but needs to project the surface, otherwise the mesh will shrink.
Regarding the faceted surface, it depends on the accuracy you used when imported the geometry. It also depends on the number of cells you have along the edge. You can increase it to have a more perfect circular face, but according to the picture it seems ok for me.
Just one hint, try to match the same cell size on both sides of the sliding interface. It will increase you convergence chances.

Regards,

Mack

AA29 March 27, 2014 18:16

Thanks Mack for the reply ! That was helpful.

I have one more question actually. Do you have any idea whether ICEM allows us to extract INTERIOR faces(surfaces) and export them as STL. We can export the entire geometry or the boundary faces of the mesh , but I need to export some internal faces of the mesh to use in OpenFOAM.

Thank you in advance.

Mack March 27, 2014 19:40

Yes, you can. Activate just the geometry you want to save, then go to File > Geometry > Save visible geometry as.
After that you can export the new geometry to *.stl, as you did before.

AA29 March 28, 2014 13:07

But that is for boundary faces. I am talking about internal faces in the volume mesh.

Thanks

Mack March 30, 2014 15:45

Well, this command (or "save visible mesh as") should do that.
Maybe you have not activated "interior walls" in the mesh setup window, so the meshing algorithm will not "see" the interior faces and will go through them.

Hope it helps.


All times are GMT -4. The time now is 23:50.