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/)
-   -   [GAMBIT] is it possible to create this type of grid? (http://www.cfd-online.com/Forums/ansys-meshing/95832-possible-create-type-grid.html)

ghost82 January 4, 2012 12:55

is it possible to create this type of grid?
 
1 Attachment(s)
Hi all,
is it possible in Gambit to create this type of grid (attached picture)?If yes, how?

Thank you,

Daniele

Far January 4, 2012 13:23

yes it can be done in gambit. but you need to make them in steps and then import into fluent and then create the interfaces. However this can be easily done in icem cfd by refining the domains by the factor of 2 and you have two nodes corresponding to one node to other side.

BigBen January 4, 2012 19:12

I confirm, it can be easliy done in Gambit but as said, you need to disconnect faces where the mesh is not conformed in Gambit and create interface in Fluent.

I may have another possibility. I would rather do everythng in Fluent using the Adapt/Region/refine in 3 steps.
Firts of all, create your mesh in gambit with the coarser mesh and import in Fluent.
In Fluent
1-adapt/region select by coordinates or by mouse button all the region which is refined (all the upper rectangular even the more refined). Press "refine" it will multiply by two the mesh in this region.
2-3 do it again for the small square on the upper left and upper right.

Hope it will help :)

Far January 4, 2012 22:28

Yeah it is much better and easier method and does not require interfaces :)

ghost82 January 5, 2012 11:07

Quote:

Originally Posted by BigBen (Post 337918)
I confirm, it can be easliy done in Gambit but as said, you need to disconnect faces where the mesh is not conformed in Gambit and create interface in Fluent.

I may have another possibility. I would rather do everythng in Fluent using the Adapt/Region/refine in 3 steps.
Firts of all, create your mesh in gambit with the coarser mesh and import in Fluent.
In Fluent
1-adapt/region select by coordinates or by mouse button all the region which is refined (all the upper rectangular even the more refined). Press "refine" it will multiply by two the mesh in this region.
2-3 do it again for the small square on the upper left and upper right.

Hope it will help :)

Thank you Bigben,
I knew that this could be done in fluent; however I was curious to know if that grid could be done directly in gambit.
Thank you all for replies.

Daniele

themeska February 3, 2012 05:55

Hi everybody! :)

I think this is the thread i've been looking for...as you all said a local refinement is possible and even easier in Fluent, by using the Adapt panel...anyway, this wouldn't be the easiest way for my geometry, since it consists of buildings with different heights...
Everytime i try to vertically sweep the outer region (which is to time as coarse as the inner one), Gambit says it cannot sweep it...i think it's because of the different number of intervals between the inner and outer region...and maybe Gambit is not able to connect them, am i saying something wrong? :confused:
can anyone explain to me how to do that?

What i'd like to do is to impose in Fluent different BCs for the inlet flow (i mean, different roughness heights), using different values for the inner and outer region...

Far February 3, 2012 11:03

Quote:

Everytime i try to vertically sweep the outer region (which is to time as coarse as the inner one), Gambit says it cannot sweep it...i think it's because of the different number of intervals between the inner and outer region...and maybe Gambit is not able to connect them, am i saying something wrong?
In mapping you cannot just change the nodes on one edge, you should change the no of nodes on parallel edges, but if you to make the mesh shown in 1st post, then you need to create different regions and save in different files and keep the region which you want to mesh and delete all other. Then export the mesh from all these files and read them in Fluent with append command. Got it?

themeska February 3, 2012 11:10

So, basically, what you're saying is that i should create as many meshes as the regions with different cells' sizes and then "put" them together in Fluent? :confused:
Thanks a lot for your fast reply, helped a lot!
Regards

Far February 3, 2012 11:22

yes and at the common boundaries specify interface as boundary condition.

You muest read first mesh and for other meshes you must use the append command.


All times are GMT -4. The time now is 02:29.