Sloshing forces
 

I have modelled a tank sloshing with gravity change.
I can see the free surface by making an isosurface of watr.volume.fraction.
I want the forces on the wall, I want to know how much force is being inserted on the walls due to the water sloshing and elevation. How can I calculate this?

Regards;

In post processing, use the function calculator to give force_x()@Wall assuming x is the direction you want.

Or during a run make a monitor point with a CEL expression force_x()@Wall or whatever, then you can see the time history of it as the flow evolves.

Thanks Glenn. another question if you cuold please help me.
How can a define reference pressure in the air portion of my tank?

This sounds very close to what I would like to do. I have a wind turbine simulation (3 blades) and I would like to have the forces/torques on the blades output on every timestep, whereas I only need full pressure/flow field every 10 steps or so.

It would be nice if I could use expressions ( for example torque_z()@blade1 ) to easily extract the forces/torques from all the timesteps and have them output to a chart or spreadsheet or even a text file. It seems like I can do this afterwards in CFX post, but all the transient results files have to be accessed which takes quite a bit of time. If I could get these values calculated/written during the simulation, I wouldn't have to wait for Post to read all the large trn results files, plus it will reduce my data storage and transfer needs.

In CFX-Pre, I tried adding force_x()@blade1 to the monitor list, and it shows up in the monitor, however, the values are not automatically exported as far as I can tell (by looking at the written files). This is where my problem lies, since I will not be running the case with a graphical interface, I'm sending it to a cluster, and I will not be able to manually export the data (right click > export).

Any suggestions on what I should do?

Regards,
Shawn

This is straight forward. Use a monitor point to output the expression you want, then you have the full history of every time step. You get the values out of the Solver Manager. You can also manually get it out with cfx5mondata (I think that is the command line).

Hi Glenn,

Thanks for the input on this. Do you now what file the monitor point(s) will be written into?

Alternately, do you know how I would reconstruct/rebuild my case to view the results in Solver Manager if I have to load my case onto a remote cluster instead of running it locally on my desktop? Is it just as simple as copying the necessary files back to my local system and opening the project in Workbench (or -Pre/Solver Man./-Post)?

On a side note, any experience running a case created in the Windows environment on a Linux system? I seem to remember something about the file coding being a little different, such that I would have to create all my files within Linux for solving on Linux.

(Oh the joys of having access to a whack of processor to "speed up" my job. Feels like its just slowing me down ... :( )

Regards, and many thanks,
Shawn

The monitor data gets written to a temporary file during running and becomes part of the results file at completion. But do not access the file directly, use the solver manager or cfx5mondata to access it.

If you have problems loading the run in solver manager just use the cfx5mondata command.

There should be no problems with running a simulation set up on linux on windows or vice versa. You might need to sort out file paths, but that's about all.

OK, I think I understand. I should be able to open the results (.res) file for my case directly in CFX using the Solver Manager, at which point all of my monitor points/expressions will be available and I can export from there to a .csv format. Seems simple enough.

As for the file paths, I currently have things stored on C:\folder\folder\folder\workbench\default\folder\s tructure and once I transfer the files to my cluster my structure is /work/username.

For example, my cmdb mesh files is:
C:\Folder\Folder\Folder\Folder\CUBE_files\dp0\CFX\ CFX\CFX.cmdb
Once I transfer it to my cluster, it becomes:
/work/username/CUBE_files/dp0/CFX/CFX/CFX.cmdb

I see that the paths and filenames appear a couple places in the .cfx and .def files. Would it be suffucient to change, for example in my .def file:

Assembly File Path = C:\Folder\Folder\Folder\Folder\CUBE_files\dp0\CFX\ MECH\CFX.cmdb File Type = Mesh

to:

Assembly File Path = /work/username/CUBE_files/dp0/CFX/CFX/CFX.cmdb File Type = Mesh

Or will things be a little more complicated than that?

Hmmm....

So I tried a few things to see what the outcome would be. I deleted my .cmdb mesh files and CFX-Pre and Solver Manager still ran without a problem.

I moved my .cfx and .def files to a different location and both pre and solver ran.

I renamed my .cfx and .def files...and everything still ran ok, solution and all.

This leads me to believe that the mesh data is already included in the .cfx and .def files. I'll try to transfer over just a .def file and see if I can run it on the cluster.

I rarely run CFX inside the WB environment because it just complicates things. When you run CFX stand-alone things are much more controllable.

Yes, the def and cfx files contain the mesh. So does the results file by default.