Learning Forum

[Amruth]

Hello,

I am running a transient simulation on cluster and would like to monitor static pressure at a point on the wall of the fluid domain. It would be great if anyone can point me towards a resource for commands to set up surface definitions, reports files and plots for transient simulations. Thank you.

Amruth

[ai0013]

First get familiar with the TUI commands. It is pretty straightforward to navigate through it (Enter: list actual menu, q: go back, "," accept default setup, etc...). As per your request, I attach an extract of a journal file which defines a drag-force monitor sampled at various surfaces.

;REPORT-DEFINITIONS (DRAG-FORCES)

/solve/report-definitions/add dragForce_wall_body_tube_1 drag average-over 1 thread-names ("wall_body_tube_1") force-vector 1 0 0 scaled no q q q
/solve/report-definitions/add dragForce_wall_ogive drag average-over 1 thread-names ("wall_ogive") force-vector 1 0 0 scaled no q q q
/solve/report-definitions/add dragForce_wall_ogive_tip drag average-over 1 thread-names ("wall_ogive_tip") force-vector 1 0 0 scaled no q q q
/solve/report-definitions/add dragForce_wall_sustainer_front_coupler drag average-over 1 thread-names ("wall_sustainer_front_coupler") force-vector 1 0 0 scaled no q q q
/solve/report-definitions/add dragForce_wall_sustainer_rear_coupler drag average-over 1 thread-names ("wall_sustainer_rear_coupler") force-vector 1 0 0 scaled no q q q
/solve/report-definitions/add dragForce_wall_sustainer_body drag average-over 1 thread-names ("wall_sustainer_body") force-vector 1 0 0 scaled no q q q

;ADD_REPORT_DEFINITIONS_TO_REPORT_FILES

solve/report-files/add monitors_drag_Forces report-defs (dragForce_wall_body_tube_1 dragForce_wall_ogive dragForce_wall_ogive_tip dragForce_wall_sustainer_front_coupler dragForce_wall_sustainer_rear_coupler dragForce_wall_sustainer_body) frequency 1 frequency-of iteration file-name "myDirectory/monitors_drag_Forces.txt" q q

In your case, you'll need to define the montor point first, and then setup the properties of the report-defintion. Hope this helps
(Don't forget to add the report definitons to the report files)

[Amruth]

Thank you so much for the response. Based on your journal file, I shall try setting up mine and will see how it goes.

[Amruth]

Hello Alain If I already have a .cas and .dat file that contains the key parameters of the simulation ( surface point, time-step size, max iterations/time step, iterations within time-step, report files, report plots, animations of the Mach number contours) and if I would like to run this file on cluster, should I again specify separate commands to output the files for pressure and animations in the journal file?
I actually set-up the simulation on my personal desktop (windows) and have run it to a certain time-step. In this process, I autosaved the .cas and .dat files every 2 time steps with the above parameters. Ideally I want to just continue running the simulation from this point onwards on the cluster and want fluent to keep outputting the file containing the static pressure for the surface point and the animation files of the Mach number contours.
Thank you.
Amruth

[ai0013]

If you launch the simulation on cluster from the latest checkpoint (windows) then there should be no problem. Maintain the same .cas file which already contains the whole instructions and continue running. You don't need to re-define the export commands, as these will be included in the .cas file as well. Just be careful, modify the path directories accordingly.

[Amine Ben Hadj Ali]

thanks for being so helpful here.

[Amruth]

Thank you Alainislas and DrAmine for all the help.