[ansys_matt]

I didn't see this in the User Guide except that it says each solver needs different things specified for a successful run. For instance, icoFOAM needs only nu specified in transport properties and initial p and U, which I can tell by looking at the equations icoFOAM solves. Even still, just seeing nu in the equation doesn't mean I would know the correct symbol to use in the Transport Properties file -> nu, Nu, or NU, or KinemViscos or ? In this particular case I found it in the tutorials.

For other solvers, isn't there a list of the requirements for properties and files necessary to solve a problem?

I am using the User Guide from .org and not sure I can always rely on the material from .com.

Help?

[Yann]

Hi Matt,


In my opinion, the best way is to look at the tutorials corresponding to the solver you want to use. You will get a functional case and hence will be able to see the required parameters you need to set in order to use this solver.



Cheers,
Yann

[Ship Designer]

Hello Matt,

I agree with Yann, checking out how the solvers are used in the tutorials is a good starting point.

In addition, specifically for the required fields, every solver should have a source file called createFields.H. In there you will find the necessary fields that have to be supplied by the user as well as any fields that are generated by the solver. You'll have to figure out which are the ones you need to supply. There you'll also find the type of the fields e.g. volVectorField or volScalarField.

For other information you can execute the solver with any of these options or check which are available by typing <solver> -help in the command line:

-listFunctionObjects
-listFvOptions
-listMomentumTransportModels
-listRegisteredSwitches
-listScalarBCs
-listSwitches
-listUnsetSwitches
-listVectorBCs

e.g.
interFoam -listVectorBCs

Error messages are a good source of information if something is missing.

The settings in fvSolutions are another story I'm afraid. The tutorials don't always list all the possible settings for a particular solver, as default values are sometimes omitted from the dictionary. If you know the algorithm that is used, you can look up the source code of e.g. the PIMPLE algorithm. You should then find the source files called pimpleControl. In there you will find all possible settings and what their values are supposed to be, including default values at times. Be aware that sometimes additional settings might be defined in superclasses, so it might be necessary to work up the class inheritance chain.

For the fvSchemes, I stick with the tutorials and read the scheme descriptions, because I haven't found out how I can tell which schemes work with which field and with what solver.

So for details you won't get around looking at and studying the source code. I always keep a copy of the OF source code on my computer so that I can quickly browse through the source files and opening them with my favourite text editor. For searching and cross references, I find the extended code guides to work better.

I know that ideally there would be a complete manual for every solver and the source code is not a replacement for good documentation, but that's what's available at this time.

Have a nice weekend, Claudio