|
[Sponsors] |
October 6, 2004, 04:57 |
initial value file question
|
#1 |
Guest
Posts: n/a
|
Hi all,
is it possible to start a simulation with using only some of the variables from initial value files. E.g. setting velocity to a new value (from initial guess of the definition file) and maybe temperature from a result file ? The mesh should be the same. ulf |
|
October 6, 2004, 18:14 |
Re: initial value file question
|
#2 |
Guest
Posts: n/a
|
Hi,
Yes, it is possible. Set the initial conditions for that variable in CFX-Pre either globally or for that domain to "Value", and it will always use the specified value for initial conditions even for restarts. The other main option is "Automatic with value", which means if there is no result set for that variable from a previous run use the specified value. Glenn Horrocks |
|
October 7, 2004, 04:32 |
Re: initial value file question
|
#3 |
Guest
Posts: n/a
|
This will have to be done through cfx5cmds in CFX5.7.
|
|
October 7, 2004, 09:26 |
Re: initial value file question
|
#4 |
Guest
Posts: n/a
|
The option Value can be set from CFX-Pre by using the Edit in Command Editor from the mouse right button. CFX-Pre will complain about invalid option, but the solver will run fine.
Another option is to use the Edit Definition File (Toolbar/Tools Menu) in the CFX5-Solver Manager. Of course, Jon's option is possible via cfx5cmds. Just a reminder, do not forget to reset it back to Automatic/Automatic with Value to continue with clean restart. Otherwise, the next run will be a repeat of the previous. You can do that from the Edit Current Results File (Toolbar/Tools Menu) in the CFX-5 Solver Manager.. Hope this helps, Juan Carlos |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
transsonic nozzle with rhoSimpleFoam | Unseen | OpenFOAM Running, Solving & CFD | 8 | July 1, 2022 06:54 |
Velocity blows up suddenly after 30,000+ iterations | lordvon | OpenFOAM Running, Solving & CFD | 15 | October 19, 2015 13:52 |
Upgraded from Karmic Koala 9.10 to Lucid Lynx10.04.3 | bookie56 | OpenFOAM Installation | 8 | August 13, 2011 04:03 |
Orifice Plate with a fully developed flow - Problems with convergence | jonmec | OpenFOAM Running, Solving & CFD | 3 | July 28, 2011 05:24 |
error while compiling the USER Sub routine | CFD user | CFX | 3 | November 25, 2002 15:16 |