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

How to calculate the average of torque in transient Ansys CFX Simulation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 3, 2013, 07:18
Default How to calculate the average of torque in transient Ansys CFX Simulation
  #1
New Member
 
Benjamin Stanke
Join Date: Sep 2011
Posts: 18
Rep Power: 5
xtphgu is on a distinguished road
Hi,

I am trying to calculate the power of a wind turbine in a transient simulation. My simulate of a rotor blade works well but as a result I need the torque of the blade as mean over many time steps. For my CFD simulation I am using Ansys CFX 14.5.
I can get the torque in CFD-Post ->Calculators -> Function Calculator -> Fuction:torque (Location). But just for the current time step I chose.

Those anyone know how I can get the torque Results over all my time steps? As a plot, a file or somehow else? Thanks ahead.
xtphgu is offline   Reply With Quote

Old   April 3, 2013, 07:28
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,959
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I would export the torque versus time history and do the averaging in another package like excel, matlab or whatever you wish. To get the full time history, make a monitor point set to torque_x/y/z()@location and then export this point in the solver manager.
ghorrocks is offline   Reply With Quote

Old   April 3, 2013, 08:07
Default
  #3
New Member
 
Benjamin Stanke
Join Date: Sep 2011
Posts: 18
Rep Power: 5
xtphgu is on a distinguished road
Thanks @ghorrocks. It works just perfect in this way!
xtphgu is offline   Reply With Quote

Old   April 4, 2013, 09:27
Default
  #4
Senior Member
 
Matthias Voß
Join Date: Mar 2009
Location: Berlin, Germany
Posts: 446
Rep Power: 11
mvoss is on a distinguished road
in case you did not set the monitor point before calculating, here is a little script which loops through each time step for a given res-file. start it from the cfx command line via cfx5perl. res-file needs to be next to the script (or viceversa).
Code:
>load filename=YOURRESFILE.res
! 	$Liste = getValue("DATA READER","Timestep List");
!	@TIMELIST = split(/,/,$Liste);
!	print "@TIMELIST \n";
!	open OUT, ">YOURDATA.dat";
!	print OUT "Time;Massflow Inlet;Massflow Düse;Massflow Mündung\n"; #HEADER
!	foreach $TS(@TIMELIST){
> 		load timestep = $TS
! 		print "calculating timestep $TS \n";
!		($time, $timeunits) = evaluate("Time");
! 		$pin=massFlow("INLET");
! 		$pduese=massFlow("Domain Interface 1 Side 2");
! 		$pmuendung=massFlow("Domain Interface 2 Side 1");
!		print 		"$time;$pin;$pduese;$pmuendung \n";
!		print OUT 	"$time;$pin;$pduese;$pmuendung\n";
!	};
!		close OUT;
> close
mvoss is offline   Reply With Quote

Old   March 13, 2014, 14:19
Default
  #5
New Member
 
Fernando Ruviaro
Join Date: Mar 2014
Posts: 9
Rep Power: 3
Fernando R. is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
I would export the torque versus time history and do the averaging in another package like excel, matlab or whatever you wish. To get the full time history, make a monitor point set to torque_x/y/z()@location and then export this point in the solver manager.
Hello. I can't set a torque monitor point. When I created it, torque wasn't in the output variable list. I've typed "torque_z()@pa" ("pa" was the name of the surface I've wanted to evaluate the torque around the z axis) in the box and it just goes empty again as I press "Apply". Is there any special way to do it?
Fernando R. is offline   Reply With Quote

Old   March 13, 2014, 14:36
Default
  #6
New Member
 
Benjamin Stanke
Join Date: Sep 2011
Posts: 18
Rep Power: 5
xtphgu is on a distinguished road
"torque_z()@pa" should actually work. Do you need torque over time or are you simulate 'steady state'?
xtphgu is offline   Reply With Quote

Old   March 13, 2014, 14:43
Default
  #7
New Member
 
Fernando Ruviaro
Join Date: Mar 2014
Posts: 9
Rep Power: 3
Fernando R. is on a distinguished road
Torque over time. I'm simulating a vertical axis wind turbine and I need in the torque vs angular position curve.
Fernando R. is offline   Reply With Quote

Old   March 13, 2014, 14:53
Default
  #8
New Member
 
Benjamin Stanke
Join Date: Sep 2011
Posts: 18
Rep Power: 5
xtphgu is on a distinguished road
If you create a output expression with "torque_z()@pa" in CFX-Setup you should get the curve as User Points in CFX-Solver.
xtphgu is offline   Reply With Quote

Old   March 13, 2014, 15:18
Default
  #9
New Member
 
Fernando Ruviaro
Join Date: Mar 2014
Posts: 9
Rep Power: 3
Fernando R. is on a distinguished road
I will try it.
Fernando R. is offline   Reply With Quote

Old   March 13, 2014, 16:16
Default
  #10
New Member
 
Fernando Ruviaro
Join Date: Mar 2014
Posts: 9
Rep Power: 3
Fernando R. is on a distinguished road
Is it what I should do? I type "torque_z()@pa", press enter and apply and the field doesn't go empty. But, if I press ok, then open again the monitor point, the output variable goes automatically to "Absolute Pressure".
Attached Images
File Type: jpg Capturar.JPG (67.7 KB, 109 views)
Fernando R. is offline   Reply With Quote

Old   March 13, 2014, 17:00
Default
  #11
New Member
 
Benjamin Stanke
Join Date: Sep 2011
Posts: 18
Rep Power: 5
xtphgu is on a distinguished road
Ok you have to change the Option drop down menu from "Cartesian Coordinates" to "Expression" then CFX will accept the torque-espresssion. God luck
xtphgu is offline   Reply With Quote

Old   March 14, 2014, 13:35
Default
  #12
New Member
 
Fernando Ruviaro
Join Date: Mar 2014
Posts: 9
Rep Power: 3
Fernando R. is on a distinguished road
It works now. Thank you very much
The unit of the torque measured is relative to the solution units, right?
Fernando R. is offline   Reply With Quote

Old   March 14, 2014, 16:56
Default
  #13
New Member
 
Fernando Ruviaro
Join Date: Mar 2014
Posts: 9
Rep Power: 3
Fernando R. is on a distinguished road
I was testing the results with this method and noticed that the value of torque obtained with the monitor point differed a bit from the value acquired by using the 'Function Calculator' (in Calculators) in a given timestep.

So, to have an idea of this difference I've made a simple simulation of a rotating "square" in an air flux, first with it still, to have the inicial values, and then with it moving, and a monitor point measuring the force in the x direction in the sides of the square (defined as "paredes").

After, I've compared the data exported from the monitor point and the force in the x direction evaluated at each timestep using the 'Function Calculator'. The data is shown in the third image (in the table, data refers to "exported data", and manual to data obtained with the function calculator).

It seems that the x axis using the monitor point is refers to a frame of reference fixed in the rotating domain. I've tried marking the "Coord Frame" box and selectinig the "Coord 0" (the only one that appear), but the result is the same.

How can I export the data referred to the global coordinate system?
Attached Images
File Type: jpg Capturar.JPG (51.5 KB, 50 views)
File Type: jpg Capturar2.JPG (94.6 KB, 64 views)
File Type: jpg Capturar3.JPG (81.9 KB, 85 views)
Fernando R. is offline   Reply With Quote

Old   April 24, 2014, 11:13
Default Average Temperature
  #14
Banned
 
Join Date: Feb 2013
Posts: 16
Rep Power: 0
anon_f is on a distinguished road
Hello,
The subject treated here is very interesting.
I would like to ask a question in my turn. My simulation on CFX is on heating a large block into contact with a combustion chamber. A heat flow is transmitted to the block and the temperature of the block varies with time.
So I get for each time step the temperature profiles of tho block. When I want to see the transient variation of the block temperature with XY - transient or sequence in Chart I can do it for points only (not all the domain).
Does anyone can tell me, please, how to plot the average temperature of all my block function of time? Or how to export at each timestep the average temperature of my block.
Thank you in advance for your help.
anon_f is offline   Reply With Quote

Old   April 24, 2014, 12:29
Default
  #15
Senior Member
 
Matthias Voß
Join Date: Mar 2009
Location: Berlin, Germany
Posts: 446
Rep Power: 11
mvoss is on a distinguished road
You can create an expession like volumeAve(T)@block And use it instread of the Point in the Chart schematic.
For the export via script see #4 above.
mvoss is offline   Reply With Quote

Old   April 24, 2014, 14:08
Default
  #16
Banned
 
Join Date: Feb 2013
Posts: 16
Rep Power: 0
anon_f is on a distinguished road
Thank you so much.
anon_f is offline   Reply With Quote

Old   May 16, 2014, 07:00
Default
  #17
New Member
 
Walter
Join Date: May 2014
Posts: 2
Rep Power: 0
walter.vahlbruch is on a distinguished road
Thank you so much for all of this information!
I would like to monitor the pressure of a moving wall.

Unfortunately it doesn't work like that: "pressure()@MOVING_WALL"
Ansys doesn't know the word "pressure". What can I do?
walter.vahlbruch is offline   Reply With Quote

Old   May 16, 2014, 09:22
Default
  #18
Senior Member
 
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 500
Rep Power: 11
singer1812 is on a distinguished road
The variable goes into the parenthesis. The first part is how you want to evaluate the variable. In your case for example:

areaAve(Pressure)@moving_wall
maxVal(Pressure)@moving_wall
minVal(Pressure)@moving_wall

can give you the area average, the max value and min value. Please look up CEL in the help.
singer1812 is offline   Reply With Quote

Old   May 16, 2014, 10:40
Default
  #19
New Member
 
Walter
Join Date: May 2014
Posts: 2
Rep Power: 0
walter.vahlbruch is on a distinguished road
Thank you very much! I'm new in CFX. I will look up CEL.
Saved me a lot of hours!
Thank you!
walter.vahlbruch is offline   Reply With Quote

Reply

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
Reaction with CFX (transient simulation) ameen0602 CFX 2 May 4, 2012 16:11
Verifying results for a wind turbine blade simulation in ANSYS CFX Joystix CFX 3 April 27, 2012 17:52
Boundary condition setting regarding turbine simulation using CFX Lacerlacer CFX 11 March 12, 2012 10:32
Ansys FSI and CFX (valve simulation) farianka ANSYS 0 April 17, 2011 16:20
MFX: weired force transfer from cfx to ansys zyf CFX 3 October 7, 2006 03:08


All times are GMT -4. The time now is 20:18.