CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Collect transient results CFD POST

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By cdegroot

Reply
 
LinkBack Thread Tools Display Modes
Old   November 15, 2012, 12:33
Default Collect transient results CFD POST
  #1
New Member
 
Antonio
Join Date: Sep 2009
Posts: 12
Rep Power: 7
mortain is on a distinguished road
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
mortain is offline   Reply With Quote

Old   November 15, 2012, 13:52
Default
  #2
Senior Member
 
Chris DeGroot
Join Date: Nov 2011
Location: Canada
Posts: 387
Rep Power: 6
cdegroot is on a distinguished road
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.
cdegroot is offline   Reply With Quote

Old   November 15, 2012, 14:21
Default
  #3
New Member
 
Antonio
Join Date: Sep 2009
Posts: 12
Rep Power: 7
mortain is on a distinguished road
Quote:
Originally Posted by cdegroot View Post
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?
mortain is offline   Reply With Quote

Old   November 15, 2012, 14:24
Default
  #4
Senior Member
 
Chris DeGroot
Join Date: Nov 2011
Location: Canada
Posts: 387
Rep Power: 6
cdegroot is on a distinguished road
You can make a time series chart and export the results as a csv file.
mortain likes this.
cdegroot is offline   Reply With Quote

Old   November 15, 2012, 15:10
Default
  #5
New Member
 
Antonio
Join Date: Sep 2009
Posts: 12
Rep Power: 7
mortain is on a distinguished road
Quote:
Originally Posted by cdegroot View Post
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!
mortain is offline   Reply With Quote

Old   November 15, 2012, 15:22
Default
  #6
Senior Member
 
Chris DeGroot
Join Date: Nov 2011
Location: Canada
Posts: 387
Rep Power: 6
cdegroot is on a distinguished road
Great, glad to help. You are right, it does take a while to load, but it's a pretty easy solution once it does.
cdegroot is offline   Reply With Quote

Old   November 19, 2012, 08:49
Default
  #7
Senior Member
 
Join Date: Jul 2011
Location: Berlin, Germany
Posts: 120
Rep Power: 5
monkey1 is on a distinguished road
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.
export scalars from a surface

Last edited by monkey1; November 19, 2012 at 08:51. Reason: Forgot to include a link
monkey1 is offline   Reply With Quote

Old   April 15, 2015, 17:39
Default
  #8
Member
 
sanjeet Limbu
Join Date: Mar 2015
Posts: 91
Rep Power: 2
sanjeetlimbu is on a distinguished road
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
Attached Images
File Type: jpg CFD post error fot Temp vs time plot.jpg (50.3 KB, 19 views)
sanjeetlimbu is offline   Reply With Quote

Old   April 15, 2015, 18:22
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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?
ghorrocks is offline   Reply With Quote

Old   April 15, 2015, 19:07
Default
  #10
Member
 
sanjeet Limbu
Join Date: Mar 2015
Posts: 91
Rep Power: 2
sanjeetlimbu is on a distinguished road
It is transient solution as I set the time steps 1e-5 s and its runs with flow time as autosave name
sanjeetlimbu is offline   Reply With Quote

Old   April 16, 2015, 01:41
Default
  #11
Senior Member
 
Join Date: Jul 2011
Location: Berlin, Germany
Posts: 120
Rep Power: 5
monkey1 is on a distinguished road
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
monkey1 is offline   Reply With Quote

Old   April 16, 2015, 07:59
Default
  #12
Member
 
sanjeet Limbu
Join Date: Mar 2015
Posts: 91
Rep Power: 2
sanjeetlimbu is on a distinguished road
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?
sanjeetlimbu is offline   Reply With Quote

Old   April 16, 2015, 18:36
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   April 16, 2015, 22:57
Default
  #14
Member
 
sanjeet Limbu
Join Date: Mar 2015
Posts: 91
Rep Power: 2
sanjeetlimbu is on a distinguished road
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
Attached Images
File Type: jpg pressure contour ani2.jpg (8.3 KB, 7 views)
File Type: jpg pressure contour ani.jpg (8.2 KB, 8 views)
sanjeetlimbu is offline   Reply With Quote

Old   April 17, 2015, 05:46
Default
  #15
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   April 17, 2015, 08:29
Default
  #16
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 236
Rep Power: 12
brunoc is on a distinguished road
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.
brunoc is offline   Reply With Quote

Reply

Tags
cfd post, transient

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


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 14:24
CFD vs Experimetal Results for Aerofoil aceofharts414 Main CFD Forum 0 April 22, 2009 07:14
Using Transient Statistics results for tracer exp. houman CFX 11 August 15, 2005 03:46
Minimal transient result lokks like full in Post Korsh Mik CFX 14 July 19, 2005 02:45


All times are GMT -4. The time now is 16:39.