CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   I want to restore Adapted mesh.. (http://www.cfd-online.com/Forums/fluent/107409-i-want-restore-adapted-mesh.html)

cartman September 26, 2012 10:08

I want to restore Adapted mesh..
 
Hi all :D

These day, I use fluent to analysis supersonic CD nozzle flow,

and I used 'adapt mesh' in order to identify Mach disk

Mesh around the Mach disk was refined as i wished,

the problem is that, Mach disk was Moved :eek:

so I want to refine another place and restore refined mesh to original one


The question is "Can I restore adapted mesh as original mesh??"


thanks for your kind attention, and wait for your reply

NormalVector September 26, 2012 21:01

No, I was under the impression that you cannot restore to the initial mesh after adaptation. I think the Fluent manual even says to be sure to save an instance of the original mesh in case adaptation goes sour. Do you have a saved case of your pre-adaption mesh?

cartman September 27, 2012 08:04

thanks, NormalVector

so .. what can I do is...

----------------------------------

save case before adaption ->

adapt the mesh ->

calculate with adapted mesh ->

read the case ->

adapt again ->

iterate

----------------------------------

again, I appreciate your kind answer

Jinglz September 28, 2012 11:49

The movement of the mach disk is supposed to happen because as you adapt your mesh your solution becomes "less mesh dependent" (more physically accurate). If you try the procedure you list, your solution validity will most likely suffer. If you try to impose the "correct" solution on a mesh that is not "correct" all kinds of strange things can happen. The correct way to go about this is to both refine and coarsen using adaptive meshing.

For instance, in your adaptive mesh option interface, you select to adapt based on the *NORMALIZED GRADIENT* of static pressure (*hint hint Ive done at least 40-50 adaptive mesh rocket nozzle/plume simlulations at a professional level) to a refinement tolerance of 0.7 (since normalization makes everything between 0-1). You should also set the coarsen tolerance to a value of 0.3. That way your range of 0.3-0.7 dictates that if there is a static pressure gradient steeper than 70%+ of all of the gradients calculated in the field, refine this area. As your mach disk moves, the coarsen threshold implies that if there is an area of the field with static pressure gradients in the weakest 30%, coarsen these. This technique is one that I use for near all high speed combustion flows. It is especially helpful with transient simulations where your flame front is continuously moving. Hope this clears things up.

Let me know what you think,
-J

NormalVector September 28, 2012 12:27

Quote:

Originally Posted by Jinglz (Post 384087)
The movement of the mach disk is supposed to happen because as you adapt your mesh your solution becomes "less mesh dependent" (more physically accurate). If you try the procedure you list, your solution validity will most likely suffer. If you try to impose the "correct" solution on a mesh that is not "correct" all kinds of strange things can happen. The correct way to go about this is to both refine and coarsen using adaptive meshing.

For instance, in your adaptive mesh option interface, you select to adapt based on the *NORMALIZED GRADIENT* of static pressure (*hint hint Ive done at least 40-50 adaptive mesh rocket nozzle/plume simlulations at a professional level) to a refinement tolerance of 0.7 (since normalization makes everything between 0-1). You should also set the coarsen tolerance to a value of 0.3. That way your range of 0.3-0.7 dictates that if there is a static pressure gradient steeper than 70%+ of all of the gradients calculated in the field, refine this area. As your mach disk moves, the coarsen threshold implies that if there is an area of the field with static pressure gradients in the weakest 30%, coarsen these. This technique is one that I use for near all high speed combustion flows. It is especially helpful with transient simulations where your flame front is continuously moving. Hope this clears things up.

Let me know what you think,
-J

I think this will be very helpful for me as well, I'm doing some rocket related CFD as well. Thanks Jinglz! You have any other tips? :D


All times are GMT -4. The time now is 11:01.