[w784370882]

Hello, everyone. Here is the situation that I want to calculate the same model with outlet mass flow changing from 5kg/s to 15kg/s. I add 1kg/s every time so that is 10 results finally. I don't want to change the outlet boundary condition manually. Is there some way to realize it? I've already searched question on the internet but no detailed introduction was found. Thanks

[urosgrivc]

Use parameters:

if you set your outlet as an expression you are able to set it as a parameter and then you are able to set up 10 simulations from workbench and run them one after the other automaticaly, without even opening cfxpre in the proces.
just be sure to export all the needed data by that I mean output parameters (easily set in cfx post before you start your 10 simulations) that you observe and you need to be sure that the simulation is correctly solved before it goes to the next one.

this process has great capabilities like genetic optimisation, response surface, etc.

To make your outlet as an expression you can do this:
Make an expression named, let us say;
OutletMassFlow
you then set this expression as;
5 [kg s^-1]
this unit will be used when the expression is used in cfx
and rightclick on the expresion and select (use as a workbench input parameter)
This will make it visible as a parameter in the workbench automatically
Than in the settings for outlet you call in this expression OutletMassFlow instead of writing in fixed walue

[Opaque]

What version of ANSYS CFX are you using?

If you check version R19.2 or later for the "operating maps" feature. You can set a variable to be changed during the simulation. You will obtain as many results file as variations you included in the setup.

Say, you select mass flow from 1->5 kg/s in 10 increments. The software will start with 1 kg/s, once converged, it will start another simulation with 2 kg/s and so on until it finishes. In the future, we should be able to run the 10 simulations at the same time (assuming parallel licenses and resources available).

The ANSYS Solver Manager monitor all the simulations for you automatically and give you a status which simulation failed, converged, etc.

[w784370882]

many thanks!!! I've tried this method just now and it's stilling running. Now I'm going back to sleep and check it out tomorrow morning. Wish you have a good day! ( ^_^ )

[ghorrocks]

An alternative approach is to generate a series of CCL files with the different flow rates defined and then run them in a batch file. This method allows you to do this sort of thing outside Workbench, if that is of interest.

[Opaque]

The operating maps functionality is a stand-alone feature independent of Workbench, not to be confused with design parameters.

[w784370882]

Originally Posted by ghorrocks

An alternative approach is to generate a series of CCL files with the different flow rates defined and then run them in a batch file. This method allows you to do this sort of thing outside Workbench, if that is of interest.

ghorrocks, thank u very much! I used to write .bat file for fluent calculating. Now I learned how to write it in CFX format, it's also useful in situations when calculation needs lots of operation points.

[w784370882]

Originally Posted by Opaque

The operating maps functionality is a stand-alone feature independent of Workbench, not to be confused with design parameters.

My ansys version is 19.1 so I will check this method after I install a new version. Thank you for your advice!

[Gert-Jan]

If you have a def file called case.def, you can simply create a batch file containing commands like:

cfx5solve -def case.def -ccl 1kgs.ccl -name 1kgs
cfx5solve -def case.def -ccl 2kgs.ccl -name 2kgs

This will give you result files:

1kgs_001.res
2kgs_001.res

where your ccl-file 1kgs.ccl only contains:

FLOW: Flow Analysis 1
DOMAIN: domain1
BOUNDARY: inlet
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Mass Flow Rate = 1 [kg s^-1]
END
END
END
END
END

So you only need a small part of the ccl-tree.

[Gert-Jan]

When starting a case in the solver manager, you can also add these commands in the Solver-tab/Solver Arguments.

So, if you run case.def and add arguments "-ccl 1kgs.ccl -name 1kgs" then the result will be the same. But only 1 file at a time, manually.,,,,,

[w784370882]

Originally Posted by Gert-Jan

If you have a def file called case.def, you can simply create a batch file containing commands like:

cfx5solve -def case.def -ccl 1kgs.ccl -name 1kgs
cfx5solve -def case.def -ccl 2kgs.ccl -name 2kgs

This will give you result files:

1kgs_001.res
2kgs_001.res

where your ccl-file 1kgs.ccl only contains:

FLOW: Flow Analysis 1
DOMAIN: domain1
BOUNDARY: inlet
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Mass Flow Rate = 1 [kg s^-1]
END
END
END
END
END

So you only need a small part of the ccl-tree.

It's a good idea! Now I start to get the hand of these situations. Thanks!

[Opaque]

If this is a one-time effort, it does not matter much which approach you take.

However, if you expect to repeat this approach multiple times you are better off learning a feature which takes care of the nuisances of simulation management, file management, monitoring multiple runs, post-processing, etc.

In either case, you are at the start of the learning curve.

My 2 cents.