CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CD-adapco (http://www.cfd-online.com/Forums/cd-adapco/)
-   -   how to setting this boundary (http://www.cfd-online.com/Forums/cd-adapco/56415-how-setting-boundary.html)

tipakorn January 9, 2008 23:52

how to setting this boundary
 
I divide my model to 2 parts because it's very big and complex. Can I use part A's result be input to another part? And how to set it to part B. Thanks

DB January 10, 2008 16:00

Re: how to setting this boundary
 
I can give you an example:

Suppose you have a long pipe and instead of modeling as a whole you divide pipe into 2 parts such that outlet from one part is inlet to another. Run the first piece of model and write out the velocity,temperature etc at the outlet boundary in a tabular format [x,y,z,velocity/temperature] now this data will be input to second piece. Set the user option in inlet boundary in second piece to "user" and then in the user subroutine read the file to define the boundary values.


James January 11, 2008 09:24

Re: how to setting this boundary
 
I think you are looking for PMAP.

One way of doing this is to place a set of shells on the downstream model boundary and write them out. You read these into the upstream model, PMAP the data and write it out.

Then using the data files and the ORIGINAL shell file ( the data from the upstream model and the original shell file will be in the correct order and matched, it does not matter that the upstream shell numbers were different during mapping) you write some code that creates one region per face (it should require ~10 lines toi do this). You then ifile/BREAD the files into the downstream model and run it.

Overlapping the models rather than abutting them is preferred.

This process only works well if there is a good low gradient simple flow zone at which to map. Obviously you cannot have recirculation but you also have the issue that while you map the velocity field you do not map the pressure field or more specifically the pressure gradients that were driving the flow (or vice versa).

One check to see if the mapping is valid is to check the quantity (pressure/velocity) that you did not map between the two models. If they are close it's OK if not the mapping plane was not suitable.

I would suggest you map velocity for the highest chance of success.

tipakorn January 15, 2008 23:32

Re: how to setting this boundary
 
What is PMAP? I use Star CD V3.26?

James January 16, 2008 09:19

Re: how to setting this boundary
 
Did you try help PMAP ?

It maps volume data onto another set of cells, it is a bit like SMAP except you can do a part of a model and in addition you can map volume data onto shells for use with boundary mapping.


All times are GMT -4. The time now is 23:04.