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

Force vs Time Plot

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

Like Tree6Likes
  • 1 Post By Hamidzoka
  • 2 Post By colinda1
  • 1 Post By Hamidzoka
  • 2 Post By colinda1

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 6, 2020, 11:04
Default Force vs Time Plot
  #1
Member
 
Ko Shine
Join Date: May 2018
Posts: 33
Rep Power: 6
Ko_Shine is on a distinguished road
Hello,

This might be a simple question. I would like to plot force or toque vs time from Unsteady or NLH simulations. How could I possibly export such data?

Thanks in advance.

Best regards,
Shine
Ko_Shine is offline   Reply With Quote

Old   January 9, 2020, 00:31
Default
  #2
Senior Member
 
Hamid Zoka
Join Date: Nov 2009
Posts: 277
Rep Power: 17
Hamidzoka is on a distinguished road
Hi,
you can easily select force (or torque) from the parameter selection in CFview. As you proceed in time steps, its value is updated. If you wold like to do it automatically, you had better to record this process once in CFview in .py format and later execute it.
I will be available for additional helps if needed.

regards
Hamidzoka is offline   Reply With Quote

Old   January 9, 2020, 09:53
Default
  #3
Member
 
Ko Shine
Join Date: May 2018
Posts: 33
Rep Power: 6
Ko_Shine is on a distinguished road
Hi Hamid,

Thanks for your help.

I selected scalar torque or force (from Mechanics group) and was able to plot a contour. Is there a way to export a single value (i.e. rotor torque, thrust, etc.) and plot it over time? I tried Representation > Cartesian Plot > Local Time Evolution but it didnt work though.

Im not sure about doing it automatically as you mentioned.

By the way, I forgot to mention that Ive been doing flutter simulations of wind turbine using both fully unsteady method and NLH method in FINE/Turbo.

Thanks,
Shine
Ko_Shine is offline   Reply With Quote

Old   January 12, 2020, 03:14
Default
  #4
Senior Member
 
Hamid Zoka
Join Date: Nov 2009
Posts: 277
Rep Power: 17
Hamidzoka is on a distinguished road
Hi;
It needs a code. Generally these sort of exports can be done using Python. The overall plot is simple: first you need to select boundaries on which the torque calculation is intended. Then calculate the force and then torque. Now go to the next timestep and repeat calculations. You can record all these in CFview through file>macro> record icon. When finished select save icon from the same address.
This will save whatever is done in Python. So the next time you can execute this code again from the same address.
Note that if you wish to make a plot with time, you need making some modifications in the recorded code. E.g. opening a text file and writing the torque values at each time scalethere. Or if you see volumeintegral() or something like that in the recorded file you have to change it to a=volumeintegral() to keep its value.
This is what exactly done in Design3d modulue in a fully seamless manner.
Professional users needs these skills to lower the time requirements for postprocessing.
I hope it helps.

Rdgards
Ko_Shine likes this.
Hamidzoka is offline   Reply With Quote

Old   January 14, 2020, 04:37
Default
  #5
Senior Member
 
Colinda
Join Date: May 2012
Location: Brussels
Posts: 144
Rep Power: 12
colinda1 is on a distinguished road
Some additional comments:
  • An NLH solution can only be post-processed in the same way as an unsteady computation if it is reconstructed in time. Otherwise, simply opening a NLH computation in CFView would show the time-averaged solution (just like a steady-state run).
  • The force and torque in CFView are per unit area. Therefore, one needs to perform a vector integral in order to obtain their total value (see the documentation).
  • It is known that force and torque calculations from CFView are not identical to the one given by the solver (due to different interpolations).
Hamidzoka and Ko_Shine like this.
colinda1 is offline   Reply With Quote

Old   January 15, 2020, 12:36
Default
  #6
Member
 
Ko Shine
Join Date: May 2018
Posts: 33
Rep Power: 6
Ko_Shine is on a distinguished road
Hi Colinda Thanks for your comments. I appreciate that. Im aware that time reconstruction is required for NLH solution which Ive done already. Ive also tried to compute force and torque using a vector or scalar integral as required.

Hi Hamid - Thanks for your help. They are indeed really helpful. To be honest with you, Im not familiar with Python but Ill surely give it a try. So basically, what the code does is calculating and recording force or torque values as the time step goes on. Would that be the same as those values computed from the vector integral as Colinda mentioned?

Thanks,
Shine
Ko_Shine is offline   Reply With Quote

Old   January 18, 2020, 00:42
Default
  #7
Senior Member
 
Hamid Zoka
Join Date: Nov 2009
Posts: 277
Rep Power: 17
Hamidzoka is on a distinguished road
Hi;
What Colinda mentioned explains the difference between what Cfview reports and Fineturbo "convergence history" window.
Automated post-processing using Python gives the same values seen in CFview and basically there is no difference.

Regards
Ko_Shine likes this.
Hamidzoka is offline   Reply With Quote

Old   January 20, 2020, 07:21
Default
  #8
Member
 
Ko Shine
Join Date: May 2018
Posts: 33
Rep Power: 6
Ko_Shine is on a distinguished road
Well understood! Thanks for that, Hamid!

Cheers,
Shine
Ko_Shine is offline   Reply With Quote

Old   August 13, 2020, 02:54
Default
  #9
Senior Member
 
Colinda
Join Date: May 2012
Location: Brussels
Posts: 144
Rep Power: 12
colinda1 is on a distinguished road
If you wish to get the information in a text file directly from the solver, it is also possible to use the expert parameter IUNSMF to allow Harmo2time to output a ".mf" file at each time step.
Hamidzoka and Ko_Shine like this.
colinda1 is offline   Reply With Quote

Old   August 27, 2020, 08:27
Default
  #10
Member
 
Ko Shine
Join Date: May 2018
Posts: 33
Rep Power: 6
Ko_Shine is on a distinguished road
Hi Colinda,

Sorry for getting back to you late. That's very convenient. I will try that one in my next simulation.

Many thanks,
Shine
Ko_Shine is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[solidMechanics] Support thread for "Solid Mechanics Solvers added to OpenFOAM Extend" bigphil OpenFOAM CC Toolkits for Fluid-Structure Interaction 685 August 31, 2022 13:34
Floating point exception error lpz_michele OpenFOAM Running, Solving & CFD 53 October 19, 2015 03:50
Star cd es-ice solver error ernarasimman STAR-CD 2 September 12, 2014 01:01
same geometry,structured and unstructured mesh,different behaviour. sharonyue OpenFOAM Running, Solving & CFD 13 January 2, 2013 23:40
Force can not converge colopolo CFX 13 October 4, 2011 23:03


All times are GMT -4. The time now is 18:06.