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] beautiful o-grid (http://www.cfd-online.com/Forums/ansys-meshing/112123-beautiful-o-grid.html)

diamondx January 22, 2013 13:07

beautiful o-grid
 
dear Icemers ,

i have a problem, please refer to the picture below

https://dl.dropbox.com/u/35161486/as...on_circles.png

when i need to make a blocking for a circle, and after doing the splits, the associations always come up with this kind of grid. How can i obtain straight and neat square inside the circle since it plays very much on the quality later. Is there a way for doing that ??

Thanks a lot

diamondx January 22, 2013 17:48

ok problem solved never mind...

Far January 22, 2013 18:07

how?...........

diamondx January 22, 2013 18:36

sorry for giving fake hope. but i solved the problem but changing my blocking strategy...

diamondx January 22, 2013 19:25

Let me share what i have done so far. my initial geometry was a cylinder, with a series of holes around it. blocking is doable, but you have to be very careful to the location of vertex etc... another way of doing this is to block a portion of the cylinder and rotate the mesh. as the picture shows, i took just a small portion of the cylinder and meshed it:

http://dl.dropbox.com/u/35161486/holes_cylinder.png

quality is good enough, min angle too, but i just don't like the stretched element near the edge, what do you guys think of this blocking , i can share the project if you want.

energy382 January 23, 2013 05:57

Quote:

Originally Posted by diamondx (Post 403443)
Let me share what i have done so far. my initial geometry was a cylinder, with a series of holes around it. blocking is doable, but you have to be very careful to the location of vertex etc... another way of doing this is to block a portion of the cylinder and rotate the mesh. as the picture shows, i took just a small portion of the cylinder and meshed it:

http://dl.dropbox.com/u/35161486/holes_cylinder.png

quality is good enough, min angle too, but i just don't like the stretched element near the edge, what do you guys think of this blocking , i can share the project if you want.

That's ok. I recently had a centrifugal pump simulation with a heavy curved blade, so my inflow/inlet looks similar (or to be precise: much more curved).
Look at your min. ortho, max. dehedral and your volume change. These paramters are much more important than deter. or angle in my experience.

I often had meshes with a lower angle, but good ortho and they achieved better and faster solution than good angles and bad ortho.

BrolY January 23, 2013 06:32

From my point of view, you reached the limit of structured mesh done with blocking ;) Some areas are over-refined, but you can't avoid it.

About the quality values, it would depend a lot on your solver. For some of them, min angle is very important, and for others, it's not a top priority criterion.

About your blocking, I think you could move some vertices to improve the nodes repartition and maybe add some elements to have a better volume change. Otherwise, your strategy looks good !

diamondx February 7, 2013 15:27

i'm back dear friend,

I have a question about these criterion: max dihedral and volume change. from your experience what is the range of acceptable values. what i found so far is that it should be 10<x<170 for the max dihedral. i couldn't find any for the volume change...

thanks a lot

energy382 February 7, 2013 17:23

Quote:

Originally Posted by diamondx (Post 406597)
i'm back dear friend,

I have a question about these criterion: max dihedral and volume change. from your experience what is the range of acceptable values. what i found so far is that it should be 10<x<170 for the max dihedral. i couldn't find any for the volume change...

thanks a lot

You've to be carefull about the volume change. Once, I made a mesh study (turbine blade) and had just one block, were I've forgotten to adjust spacing 1 (and therefore had volume change of 170).
The mesh achvied a very good convergence (max Res <10E-4), but produced physically invalid results!
A good value is <5, but <10 is also acceptable.

Just make a best practice with three meshes (global scale factor arround 0.7 and 1.4). and create some monitor points (e.g. pressure difference...). These values should either fall constantly from coarse to fine (mesh) or go up. If so, your mesh is fine. If not, you've to look about your volume change, orthogonality etc...

diamondx February 8, 2013 14:25

christoph, thanks a lot for you answer.
there was a major change in the geometry, and it turns out i had to use a quarter of the cylinder because more holes were added
However, as shown below, the holes gave me hard time to block. i spent the hole day yesterday trying to get a descent blocking.

https://dl.dropbox.com/u/35161486/difficult_1.png


having to add an o-grid for all the holes, and because it's cylindrical, the move vertices can't be applied as i can't fix the x or y or z.
i just don't know how to deal with them, is there some kind of automatic arrangement to deal with these o-grid ?? i'm asking for too much

https://dl.dropbox.com/u/35161486/difficult_2.png

thanks a lot

Far February 8, 2013 14:45

Quote:

Originally Posted by diamondx (Post 406779)

having to add an o-grid for all the holes, and because it's cylindrical, the move vertices can't be applied as i can't fix the x or y or z.

thats why I asked for this feature
http://www.cfd-online.com/Forums/ans...-required.html

diamondx February 8, 2013 14:54

i voted for it :D

I started to hate perforated cylinders like these, i guess i should go unstructured...

Far February 9, 2013 07:36

Quote:

Originally Posted by energy382 (Post 406609)
You've to be carefull about the volume change. Once, I made a mesh study (turbine blade) and had just one block, were I've forgotten to adjust spacing 1 (and therefore had volume change of 170).
The mesh achvied a very good convergence (max Res <10E-4), but produced physically invalid results!
A good value is <5, but <10 is also acceptable.

Just make a best practice with three meshes (global scale factor arround 0.7 and 1.4). and create some monitor points (e.g. pressure difference...). These values should either fall constantly from coarse to fine (mesh) or go up. If so, your mesh is fine. If not, you've to look about your volume change, orthogonality etc...

Good info. This may be important and manageable in internal flows but impossible to keep in external aero CFD. When downstream domain extent may be stream-wise : 15 upstream and 20-30 downstream. Transverse may be up to 15-20 lengths.

More it is important in the critical flow areas (external flows) near wall or it is necessary to keep the volume change <10 in farfield?

Can we use the global scale factor for Hexa? when combined with part mesh setup and update all option we can use it but how to define the local spacing and growth ratio? Manually?

BrolY February 11, 2013 03:54

You can move vertices by fixing a direction, which is very useful for o-grid. It requires times, but at the end, you can place the vertice wherever you want.
Otherwise, align vertices in line tool is very useful too.

About the volume change, I would say the first limit is your number of elements. For industrial cases, and especially when dealing with hexa, you can't increase too much the number of elements .. Anyway, I think < 20 is ok, and < 10 is good !


All times are GMT -4. The time now is 09:41.