Hi!

In CFX-4 there is possible to monitor values in specified points, or patces, planes etc... during the transient. Is this possible by CFX-5? I did not find it.

I calculate fully developed flow with periodic boundary condition. It would be very useful, if I would be able monitor the average velocity in a certain patch during the iteration steps. Is it possible? I can monitor only the min and max values of some variables by the expert parameters.

You can monitor values in a specific point. Unfortunately there isn't a USRTRN subroutine to calculate average values in patches. To monitor the desired variable(s) you must edit your definition file. Major details how to do this you can easily find on the manual.
Reference Manual -> Master Index -> M -> Monitor Points.
Good luck, cfd guy

Hey Lego, the monitor points in CFX5 are real simple to set up, try appending a CCL script to the definition file when running from the comand line. If you do need to extract more complex information then the next step is to get into the user fortran. This can be tricky but you can get what ever you want out of the code with this, it just may need a little help from the guys at CFX, but they are very willing and able to help ! Dave

It is quite easy indeed. It is available within CFX offices and is taught in intro courses I believe. Ask CFX support.

Actually, you can monitor average values.

Create an additional scalar and define the value of the scalar as an algebraic expression. For the expression, just put a dummy value in for now (build will not allow you to use the expression you need, so make it equal to 1 for now and you can add the expression by editing your CCL).

After you have written out your def file, open it in the CCL editor and change your expression to equal:

areaAve(Variable Name)@Region Name

The syntax is exactly equal to the CFX-Post expressions and any of these may be used (Area Average, Volume Average, etc.).

Now if you create a monitor point and monitor the additional variable, you will ge what you want.

Regards, Robin

P.S.: These expressions can also be used in boundary conditions, making one boundary a function of another!

Do you mean average values in planes (an analogy to USER2D patches in CFX-4) ? I have several common faces between two subdomains (like a interface block boundary). How can I post-process these faces? CFX-BUILD doesn't export it to POST. Thanks in advance, cfd guy

Lego,

What you want to monitor during the solving process is the flow through an inlet, outlet, periodic boundary or what so ever. This is easy to do....

1) In the solver manager you have to define a new plot monitor. Then with your right mouse button click on the window, select flows and then in your case click on the name of the periodic boundary. This will show you the development of the flow during the iteration process.

2) alternatively you can add the keyword 'monitor totals' in the 'expert parameter section' of the ccl. This will provide the data in numbers, not in a plot.

Astrid

Hi Robin, Is there any way that you can stop a simultion automatically based upon a value at a monitoring point ? Bob

Hi Bob,

You can do this through user fortran, but it is not straightforward.

I have seen this question come up before. Why would you want to do this?

Robin

Hi Astrid, one are that I've seen has been looking at say a drag on an explicitly modelled porous plate. I was monitoring the residuals, and they were all very nicely converged, but the drag on the plate was still changing. Not greatly, but it hadn't evened off. A collegue of mine said that where he worked before, in the aerospace sector, they very rarely looked at the residuals for an indicator as to when to stop the run, they always looked at life and drag. And something we have to do occasionally is to look at residance times of air or gases in an enclosure. Often the simulation is run transiently using the fortran to inform us when say the gas concentration drops below a certain level. As you said, this is not easy to do in the fortran, but is do able. However I'm always looking to try and simplify methods, and from what Robin was saying, there may be a way of monitoring the maximum value of a scalar that we could possibly then use as a stopping parameter for our simulation once a certain criteria had been achieved. Sorry for going on. Bob

Hi Bob,

I agree that the residuals may be sufficiently low before some quantities are settled, particularly if you are looking at RMS residuals (really, you should always converge to MAX residuals).

In such cases, you should add a conservation target as an additional convergence criteria. Thus, if the MAX residual is met, but the conservation target is not, the solver will continue to run. If these quantities are still changing, then the global conservation will not be met. A conservation target of 0.0001 (1/100 of 1%) should suffice.

In every case though, you should ensure that the residuals have been reduced enough. Residuals are a necessary, but not ultimate judge of convergence.

Regards, Robin