CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   STAR-CCM+ (http://www.cfd-online.com/Forums/star-ccm/)
-   -   Initialisation and transient data output in Star CCM+ (http://www.cfd-online.com/Forums/star-ccm/82947-initialisation-transient-data-output-star-ccm.html)

gmach December 9, 2010 13:07

Initialisation and transient data output in Star CCM+
 
I have two questions -

1) I am trying to initialise my transient run from a solution of a different run? Is that at all possible with STAR-CCM+? Any help would be most appreciated.

2) For transient data output in STAR-CCM+, is the autosave option correct? If so - does the final result have an automatic link to all the other transient files (like other software like CFX have)?

Any quick help would be greatly appreciated!

Georgios

abdul099 January 7, 2011 22:36

Hi Georgios,

first the second part: No, ccm+ will NOT link to the other files from the transient run - at least not in the current versions. There will be an enhancement, but I don't know in which version it will be released. So just be patient.

for the first question, yes, it's possible, but there are several ways and it takes a lot of memory.

One way is to export the mesh of the transient run. Import it to the sim-file (for safety, safe the sim-file under a new name) of the simulation where you want the initialization from. There will be a new region (or several region when your transient run includes more than one), and now you can right-click on the old region and choose "Replace region", choose the new one in the opening window and depending on your precision requirements, "use higher order stencil for interpolation" (take care, it will need a lot of memory. I estimate, at least 2 - 2.5 GB / 1 million cells). It will take some time.

The other way is to export the mesh and solution data (at least velocity (as a vector) and pressure and tke and tdr as scalar data. Hold Ctrl while selecting several scalars in the export window) of your old file.
Then open your new sim-file and import the mesh (the old solution will be imported as well).
Then go to Tools -> Data Mappers, right-click -> new
Choose source and target volumes (regions, source is the imported one), select the scalar and vector data to map and other options you may want.
The right-click on this data mapper and choose "Map Data".
After the mapping is completed, go in the physics continuum to the folder "Initial Condition" and set field functions as initial values and choose the appropriate field functions, e.g. "Mapped Pressure" as field function for pressure, "Mapped Turbulent Kinetic Energy".....

And enjoy the hopefully faster convergence of the simulation ;-)


All times are GMT -4. The time now is 07:55.