Torque on rotating blades
I'm doing a simulation of rotating Savonius rotor
How to get the torques on blades in unsteady simulation?
The torques should be different at every time step
then what does the moment by "Report->Forces->Moment " mean?
I also did that Solve->Monitor->Force->Moment
that can write a Cm at every time step
but what does the Cm mean?
Report->Forces->Moment reports the actual torque value. You can select your blades and report the torque at specific time intervals, which is what you need to do for an unsteady simulation. You could then use these values and determine the average torque for a single rotation of the wind turbine.
Solve->Monitor->Force->Moment reports the moment coefficient (Cm) and requires that your reference values are set up correctly to compute the non dimensional moment coefficient.
thank you for your reply
If I want to read the torques at the last 360 time steps of 1440 time steps (I set one time step for one degree), what is the convenient way to do this?
what i only want to get are just the torques
if i set autosave at every time step, the file may be too large.
The best way to do this is Report->Forces->Moment at every time step. This will print the torque for every time step to the screen.
Run the simulation in batch mode (NO GUI) and pipe the output to a file like FLUENT.out or something like that, you'll need to look up how to do this if you're unfamiliar, it's all over the internet. Because the torque will be recorded every time step, you can write a script to parse through the output file and save all the torque values to another file for analysis.
After exploring different options, this was the best way I found to do this. It prevents you from having to autosave the case file at every time step and go back to extract the torque from the .dat files, which like you said takes up way too much memory. It's much more efficient to save the data you need to a text file.
If you want visualizations, you'll need to save .dat files for later, or you could just save images at each time step, once again saving yourself from wasting memory on .cas/.dat files.
Hope this helps.
At first I thought Cm is moment coefficient too but the value looks more like moment/torque. Shouldn't moment coefficient be between 1 and -1? Some people told me it's "convergence history of moment". However, if so, why is it different from the value in Report->Forces->Moment? It's been bothering me, don't know which value I should take.
Thank you Travis! I've been stocked in this problem for couple of days. Although in the end I choose a little different method as yours, it was you that inspired me at all. Just want to say thank you.
It won't be necessary to run Fluent in Batch mode, instead, This is how I did it:
"Calculation Activities" -> "Execute Commands (Create/Edit)" -> Define Macro...
after you name the macro, just press OK and it will start to record your moves.
Rather than using GUI, here I choose TUI to input my command.
Therefore I type in the command window:
XXX.out ; your output file name
yes ; Create this .out first, so you could tell Fluent to append data to it in this step.
End the macro and define how often will you need this. Then it is done.
I did a few test and it seems to work! Thank you guys~
Hi, I have few little questions. Aren't we trying to calculate torque? Should we type in the command "wall-moments" instead of wall-forces?
Also, I checked the output file but couldn't tell the time step. And how do you calculate the average torque during a period? Or plot it?
Hey folks, I've figured out another method to output your force data so you can easily plot it with time (based on inspiration by f0208secretx) which uses a macro, and then some extra editing afterward.
i'm running Fluent 12.1.4 and doing transient modeling fyi.
1. Reports -> Forces -> Setup (and setup the force or moment as you like)
*notice, if you print/write here, you get the whole list of forces and you may not want that
2. Reports -> click Parameters -> select the output parameter you want to print -> drop down menu "More" and select "Write" -> name file and save
3. Calculation Activities -> under Execute Command click Create/Edit -> define Macro: name your macro and click OK to start recording the macro
while recording the macro:
4. Repeat steps 1 and 2, but this time when writing the file, make sure you save it as the same name and click the YES when it asks " ...already exists. Do you want to append output parameter data to it?"
This avoid the trouble of having to click YES while running the calculation.
If you don't get this, then make sure you save some data in that file and then record the macro again.
5. Click End Macro, and go back to the Execute command screen. make define commands to 1 (up top) and write in the macro name in Command. You can set it up to write the data how ever many interations/time steps you want.
Ok, now you have the data file, time to make it easy to plot
6. open the data file in Excel. It opens as one column of data, and you want to convert it to separate the numbers into it's own column. Select everything, and go to the Data Tab (Excel 2007 and later) and click Text to Columns.
7. select Delimited -> select the delimited as space only, and uncheck the box where it says "treat consecutive delimiters as one". -> Finish
and tada! you have a column with only your moment values. now to get rid of the spaces.
8. select the column with the numbers -> Home tab and click Find & Select, click Go to Special -> select the Blanks and OK -> right click and delete the blank cells, and shift cells up.
All done! now you can add the time steps to another column and plot. Worked for me so far, let me know if this helps :D
ear frnds plz tell me hoe to calculate torque in fluent i am working on vertical axis wind trubine h shaped daarruis type so for that concern ia m doing 2d simulations unsteday for that i am giving cl ,cd cm moniters on blades so will plz tell me how to find out direct torque in flunt or how to co relate it 2 moment ia m aatching paper and some images of my mesh so it will clear u piture of problem
plz tell me it needs udf to find torue on blades :confused: :confused: :confused: :confused: :confused: :mad:
how do you specify the direction/center of force/moment?
man you are a life saver
some doubts plz reply if any body know
dear frends i am validating one paper entiled "Proposal of a Means for Reducing the Torque Variation on a Vertical-AxisWater Turbine by Increasing the Blade Number" in that they mentioned that "physical time step equal to the lapse of time the rotor takes to make a 1° rotation." can any body know what is mean by the Lapse of time of rotor ....?
sorry to asking you but what i understand that the time taken by
rotor to move 1 degree of rotations ....
so from that i am trying to find out time step size as follow for TSR =0.5,
TSR= RW/ Vin .....so W=1.94 , Where R = radius of rotor ,W =
angular velocity ,V in = inlet velocity =2 m/s you have taken so for
1 degree rotation .....
FOR TSR 0.5,
TIME STEP =1×π⁄180×1⁄1.94
is it right ?
2.So from that i know that for 1complet rotation of turbine (means
360 degree ) i got time =0.00893×36 °=0.32148 sec ...sir i read one
article where mentioned that to conversed soln rotor will need at
lest 10 complete rotation of turbine is right ? if from that i
concluded that 0.32148 ×10=3.2148s means in mesh motion i am setting
Times step size =0.00893 and NUMBER OF TIME STEP =360 is right ? If
not what is right ? . what is the value you people have have taken ?
3 And another one doubt that frnds When i am iterating ---iterate
--fluent take time step which i set in mesh motions that is 0.00893
here Number of time step = ? can i set here value which i set in
mesh motion, which is 360 .
4 . Another one when finding out torque ....in fluent i used
----report ---forces ---moments ---here sir by default moment centre
--- X(m)=1 Y (M)=0 , Is it right ?
what is mean bye X(M)=1 here can i take it default ? or set it to
X=0,and Y =0.... AND frnds it gives total moments in n-m so sir can i
take this moments that torque in formula in papper have given Ct=T/(1/2
ρAR_rotor V∞^( 2)) OR can we adopt another procedure is that
---solve --force monitor ---moments coefficient ---..
5 .Dear frnds i am asking you so much doubt because i was never done
unsteady simulations ...so i got such doubts .... dear frnds how much
time is needed for simulation of one case such TSR =0.5 ...I have
computer of 8 GB ram and i 5 processor is it sufficient for this case
6. ia musing silding mesh techquine one thing when giving mesh motion for case of 3 blades and TSR 0.5 i am setting up boundary conditions my mesh is same as in paper i have made rotor sub grid area as papers and 3 circle around 3 blades and created fluid zone in gambit and name them inner circle 1, inner circle 2 inner circle 3 and also reaming portions of rotor sub grid
area ....so my question is that while using mesh motions options
1 st Thing i am define boundary conditions ---- inner circle 1
--motions type --moving mesh and Rotational velocity =1.94 same has
been done for all circle and reaming portion of rotor sub-grid area
and for DOMAIN SUB Grid AREA - ---motions type --moving mesh and
Rotational velocity =0 because it is fixed .....after that i am
initailze soln --- mesh motions ----time step size =0.00893 and number
of time step 360 ...is it right ?
6 last thing to ask you people that i have seting coversion cratirea 1 e-5 but soln not getting conversed its shows " Turbulent viscocity is limeted to viscocity ratio 1.000000e+005 in 51249 cells " WHAT IS EXACTLY MENA BY THAT ?
i have attached some images with these POST for you understanding .........
plz see my frist post above bcz of limed file attachemnt my mesh is above images i post same no change
After I set up these steps and run the calculation, there is only the initial data in my torque output file. The torque was not recorded in the output file as the calculation time goes by. I have been tried many times and stuck in a couple of days. Could anyone help me out with this problem? Thank you.
I couldnt find anything on the internet about saving torque and forces through batch scripts.
Periodic boundary condition vs torque calculation
I have to simulate a internal flow in a cylindrical case having both end stator blades and in middle there are rotor blades.There is no outlet and inlet.Atmospheric pressure is maintained initially.I have to calculate torque at different rpm.SO i have cut the whole geometry by 45 degree.and applied periodic boundary condition and used sliding mesh Technic to simulate the physics of flow.
I need to know that what is the torque value.Is the torque value = 1/8 of full model value(actual value).As number of rotor blades are 9 and stator blades are 8.
Thanks in advance
simulation of rotating tool
I want to simulate a milling tool with inner canalisations.
In those canalisations i will simulate a mixture of fluids (air and oil) for the lubrication. and I want to see the direction and the projection of the flow when it comes to the exit of the canalisations. so I am simulating all of this with three composants: the first for canlisations as a fluid, the second for the mill as a solid, and the third for the extern air as a fluid.
-first question I want to khnow if I have to specify the walls and the interfaces or does the logiciel recognize them.
-second question: to simulate the rotation, I activate the frame motion and I road that it uses the MRF approach.
In th help, in this approach with the exemple of one rotating impeller, the zone of the rotating frame in bigger than the rotating impeller, i think that is done with this manner to take into account the rotating air around the impeller, but how can we define the thikness of this rotating frame. is there a formula, because I am thinking to do the same with my canalizations.
Thank you in advance
|All times are GMT -4. The time now is 01:59.|