CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Help Urgent about changing boundary condition (http://www.cfd-online.com/Forums/fluent/41993-help-urgent-about-changing-boundary-condition.html)

Anjum Naveed August 10, 2006 18:45

Help Urgent about changing boundary condition
 
hi all i want to know that how can i change a boundary condition in fluent i have given the boundary condition of wall when i was meshing in gambit and then run my simulation in fluent now i want to run DPM model on the pre developed flow field. but there are only three option for particle when they strike with wal reflect absorb or split. now my prob is that i want to reflect particles from some area of wall and absorb in some area but fluent consider the whole area as on wall as i had given the boundary condition in first. my question is can i change this one wall into two or three walls in fluent or i have to construct geometry again and there give boundary condition of wall at differnt areas and run simulation again. please help me out thanx Anjum

Raj Kiran Grandhi August 11, 2006 03:18

Re: Help Urgent about changing boundary condition
 
Look into Grid->Separate->Faces and Grid->Separate->Cells

Also see the FLUENT user manual on these topics.

Jason August 11, 2006 07:17

Re: Help Urgent about changing boundary condition
 
Instead of running the whole simulation from scratch, you could also do file->interpolate and write the solution (make sure to write ALL of the variables) of the current setup. Then re-create the geometry in Gambit (this will give you more control of the walls you want to change) and interpolate the old solution onto the current mesh (file->interpolate). Re-iterate a little (depending on how similar your mesh is it could be a couple dozen or a few hundred) to make sure the solution took onto the new mesh.

Hope this helps, and good luck, Jason

ANJUM NAVEED August 12, 2006 11:01

Re: Help Urgent about changing boundary condition
 
thanks for your help


ANJUM NAVEED August 12, 2006 13:03

Re: Help Urgent about changing boundary condition
 
hi i am anjum. thanks for ur advice but can u give some detail how to impliment interpoaltion function because i tried first save file than with new mesh i set every thing and instead of initializing i read interpolation file that i stored before and than start iteration but it did not work. Also separate face did not work Anjum

Jason August 14, 2006 07:50

Re: Help Urgent about changing boundary condition
 
About the separate face... what do you mean it didn't work? Are you talking about you redid the geometry in Gambit and didn't get an extra face? Then you didn't define your wall BCs in Gambit, you didn't build your geometry correctly, or you didn't read the correct mesh back into Fluent. What exactly did you do (what steps did you perform), and what were the results (were there any errors).

About interpolating the data... what do you mean it didn't work? What happened when you tried interpolating the data?

Jason

ANJUM NAVEED August 14, 2006 12:13

Re: Help Urgent about changing boundary condition
 
hi sorry i mixed it up in my previous mail. separate>face did not work was message for raj kiran. and for interpoaltion i saved my interpolation file . created a new mesh in gambit as i desired. than give all the BC and model to the new mesh but i did not inialize it rather i read my interpolated file at this time. my simualtion (i think) was inialized with this file automatically after ward when i start iteration it gave the message invalid argument[2]: wrong type [not a number] and stopped. any suggestions thanks Anjum

Jason August 14, 2006 12:25

Re: Help Urgent about changing boundary condition
 
Well, as for splitting the surface, you have to mark the cells first(Adapt->Region... don't Adapt, instead select "Mark" to mark the cells). Mark the cells in the area you want to split, then you can separate by "mark".

As for the interpolation problem, it could be different things. I forgot to mention to make sure your geometry is in about the same XYZ location and is the same scale. Fluent interpolates the values from the original XYZ locations to the current XYZ locations, and if you've shifted your geometry, then you could be interpolating to completely different areas (if you shift an airfoil forward, all of a sudden the LE stagnation point is at the TE of the airfoil, and the TE stagnation point is out in space). Also, before you read in the interpolation file go to Solve->Initialize and set your initialization values. Make sure you click "Apply" to store the values. You don't have to actually initialize though. What happens is that Fluent will interpolate the old solution onto the new geometry and then any variables that are missing will be filled in using the values you stored in the initialize panel. If you didn't set these values then it could've set the default pressure (0pa) which would've causes a NaN for compressible flow.

Also, make sure you set all the variables in the original interpolation file (Fluent will list each variable as it's being written to or read from an interpolation file).

Another thing that could be a problem is if there's a big difference between the setups you've done. If you make a large change on the BCs for example, this could cause a problem.

Hope this helps, and good luck, Jason


All times are GMT -4. The time now is 16:02.