Collect transient results CFD POST

mortain · November 15, 2012, 12:33

Hello,

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?

Cheers,
Antonio

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

Quote:

Originally Posted by cdegroot

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

Quote:

Originally Posted by cdegroot

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.
http://www.cfd-online.com/Forums/cfx...tml#post385850

sanjeetlimbu · April 15, 2015, 18:39

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, 19:22

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, 20:07

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, 02:41

Maybe a stupid question...but...do 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, 08:59

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, 19:36

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, 23:57

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, 06:46

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, 09:29

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.

November 15, 2012, 12:33	Collect transient results CFD POST	#1
mortain New Member Antonio Join Date: Sep 2009 Posts: 12 Rep Power: 17	Hello, 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? Cheers, Antonio

November 15, 2012, 13:52		#2
cdegroot Senior Member Chris DeGroot Join Date: Nov 2011 Location: Canada Posts: 414 Rep Power: 18	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. Cecilia Zhang likes this.

November 15, 2012, 14:24		#4
cdegroot Senior Member Chris DeGroot Join Date: Nov 2011 Location: Canada Posts: 414 Rep Power: 18	You can make a time series chart and export the results as a csv file. mortain likes this.

November 19, 2012, 08:49		#7
monkey1 Senior Member Join Date: Jul 2011 Location: Berlin, Germany Posts: 173 Rep Power: 15	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. http://www.cfd-online.com/Forums/cfx...tml#post385850 hwangpo likes this. Last edited by monkey1; November 19, 2012 at 08:51. Reason: Forgot to include a link

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Future CFD Research	Jas	Main CFD Forum	10	March 30, 2013 13:26
Matching CFD results and wind tunnel testing	huskerwong	Main CFD Forum	0	July 16, 2009 15:24
CFD vs Experimetal Results for Aerofoil	aceofharts414	Main CFD Forum	0	April 22, 2009 08:14
Using Transient Statistics results for tracer exp.	houman	CFX	11	August 15, 2005 04:46
Minimal transient result lokks like full in Post	Korsh Mik	CFX	14	July 19, 2005 03:45

November 15, 2012, 15:22		#6
cdegroot Senior Member Chris DeGroot Join Date: Nov 2011 Location: Canada Posts: 414 Rep Power: 18	Great, glad to help. You are right, it does take a while to load, but it's a pretty easy solution once it does.

April 15, 2015, 19:22		#9
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,854 Rep Power: 144	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?

April 15, 2015, 20:07		#10
sanjeetlimbu Member sanjeet Limbu Join Date: Mar 2015 Posts: 91 Rep Power: 11	It is transient solution as I set the time steps 1e-5 s and its runs with flow time as autosave name

April 16, 2015, 02:41		#11
monkey1 Senior Member Join Date: Jul 2011 Location: Berlin, Germany Posts: 173 Rep Power: 15	Maybe a stupid question...but...do have written out transient results with all the varaibles you need? If not...then he will hardly find a value to post process

April 16, 2015, 08:59		#12
sanjeetlimbu Member sanjeet Limbu Join Date: Mar 2015 Posts: 91 Rep Power: 11	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?

April 16, 2015, 19:36		#13
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,854 Rep Power: 144	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.

April 17, 2015, 06:46		#15
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,854 Rep Power: 144	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.

April 17, 2015, 09:29		#16
brunoc Senior Member Bruno Join Date: Mar 2009 Location: Brazil Posts: 277 Rep Power: 21	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.