CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   Collect transient results CFD POST (

mortain November 15, 2012 12:33

Collect transient results CFD POST

I am relatively new to the forum and to CFD world.
I am designing a turbulence grid and I wanted to check that the place where the probe will be inserted is enough downstream compared to the grid in order to have an homogeneous flow at the probe.

I have simulated the grid, in a transient simulation with k-e model.

Why transient, well, I wanted to see the turbulence level which CFD was going to give to me.

I have the simulations and using CFD post I wanted to evaluate the velocity in a point of the domain, in order to calculate the velocity fluctuations.

I was trying to code with CEL language:

1) create the point
2) evaluate the velocity in Point 1
3) save the value in a table
4) save the table

but I don't know how to open all the transient results in order to get the velocity, does anyone have a suggestion, please? Do you think there's an easier manner?


cdegroot November 15, 2012 13:52

Probably the easiest thing to do is load the full run history. When you open the res file, select the last one and make sure "Load complete history" is selected.

mortain November 15, 2012 14:21


Originally Posted by cdegroot (Post 392322)
Probably the easiest thing to do is load the full run history. When you open the res file, select the last one and make sure "Load complete history" is selected.

if I do as you say, then how can I output the velocity history?

cdegroot November 15, 2012 14:24

You can make a time series chart and export the results as a csv file.

mortain November 15, 2012 15:10


Originally Posted by cdegroot (Post 392332)
You can make a time series chart and export the results as a csv file.

Cool, did not know there was chart for time history. It works perfectly. Thanks a lot for your help!
It takes a bit of time to open all the different files....but it;s better than coding!

cdegroot November 15, 2012 15:22

Great, glad to help. You are right, it does take a while to load, but it's a pretty easy solution once it does.

monkey1 November 19, 2012 08:49

Another (faster) way to get a time dependent variable value at fixed points:
Create a monitor (or several monitors) point in CFX Pre at the the location of your point1 and with in your case the velocity to be monitored.
In the CFX Solver you can now see the Monitor point plotted over the simulation time. There you are also able with a right click on the graph to export it as csv.
That way you just avoid opening all trn files in Post.

A second way is to use a perl/CEL Script wich writes you a csv file with all the information required.
If this is of interest for you just have a look at this thread. I posted an exampe file there.

sanjeetlimbu April 15, 2015 17:39

1 Attachment(s)
Dear sir

I am trying the temperature vs time plot but getting these errror

I created a point location and trying using the CFD post

ghorrocks April 15, 2015 18:22

The error message looks pretty clear to me - it cannot find transient data. Are you sure this is a transient simulation? Or does it only have a single time point in the results file?

sanjeetlimbu April 15, 2015 19:07

It is transient solution as I set the time steps 1e-5 s and its runs with flow time as autosave name

monkey1 April 16, 2015 01:41

Maybe a stupid have written out transient results with all the varaibles you need? If not...then he will hardly find a value to post process

sanjeetlimbu April 16, 2015 07:59

I have selected the variable like static temperature and pressuree absolute while prior to run- in the solutions - export CFD post compatible.

Since the error seem due to transient time step - is there any way to activate transient mode in CFD post also?

ghorrocks April 16, 2015 18:36

You do not need to activate transient mode in CFD-Post. When it loads a transient results file with multiple time step data it handles it automatically.

sanjeetlimbu April 16, 2015 22:57

2 Attachment(s)
Thanks !

I did that

1. If I wanna add the flow time in animation is there some way..
2. I had actually two zones - both separated by an interior boundary... so the contour images are discontinuous between those two zones. Can I avoid that ... mean making smooth as both are fluid - same . Actually the top part is clearance volume- made finer mesh with inflation

ghorrocks April 17, 2015 05:46

Time display - yes, add a text object.

CFD-Post shows the simulation results. If the simulation results are not smooth then why would you want to show them smooth.

Maybe you need photoshop, not CFD-Post. Then you can draw whatever results you like in.

brunoc April 17, 2015 08:29

Seems to me that you used Fluent for the simulation (hence the 'Export CFD-Post Compatible', 'zone', 'interior') but only exported the final result. If that is the case, what you should have done was create 'Automatic Exports' in the 'Calculation Activities' panel, or at least have saved several data files during the simulation.

If you didn't do either of those two then sorry, but you won't be able to extract transient data from the simulation.

All times are GMT -4. The time now is 17:44.