[desert_1250]

tnx Linnemann, your suggestion is the best you are right

[ebah6]

Hello Niels,

I am trying to use this forces function to extract moment. But the output is all the time zero. would you have an idea of what I am doing wrong?
Here is a sample output:
-----------------------
forces output:
forces(pressure, viscous)((0 0 0) (0 0 0))
moment(pressure, viscous)((0 0 0) (0 0 0))
--------------------
Basically what I am trying to do is to get the moment and calculate the rpm such that the next iteration has this rpm.

Thank you for your time.

Best regards.

[ebah6]

Hello Niels and anyone reading this post and the previous one,

Please, disregard the fact about the outputs being all zeros.
I made a stupid mistake by not mis-spelling on of my patches.

Yet if one has a lead on the second part, any suggestion is welcome.

My best regards.

[ebah6]

Dear all,

Is there a way to choose the output format.
For instance, in file forces/0/forces.dat, every thing is output in one line for each time step.
How should proceed to have this output in column.
e.g.,
Fpx = ....
Fpy = ....
Fpz = ....
etc.

I want to do this because I need to read some of the components and do some calculations the result od which I feed to the next iteration.

Thank you all for your time.

[protarius]

Hi

There is a Python script in this thread:

http://www.cfd-online.com/Forums/ope...-brackets.html

Regards

[ebah6]

Thanks Gabriele for answering,

I wrote a dummy script of my own.

Best regards.

[prasanth]

Hello All,

Can any body face the issue with torque value in OpenFOAM? Currently I am using OpenFOAM-2.1.1. Torque value is not matching with any of the other commercial packages like CCM+ or fluent etc. In CCM+ there is option called wall rotation set to zero for some patches. Is it same as non rotating Patches in OpenFOAM. If I am giving patch names under non rotating patches, velocity is showing zero on those patches. According to settings, it is correct only. But There is a Rotating Zone. So, there should be some relative velocity on those patches. I am thinking, this may be the reason, why OF torque value is not matching. May be my thinking can be wrong.

Can any body help me on this.

[prasanth]

Hello All,

Can any body face the issue with torque value in OpenFOAM? Currently I am using OpenFOAM-2.1.1. Torque value is not matching with any of the other commercial packages like CCM+ or fluent etc. In CCM+ there is option called wall rotation set to zero for some patches. Is it same as non rotating Patches in OpenFOAM. If I am giving patch names under non rotating patches, velocity is showing zero on those patches. According to settings, it is correct only. But There is a Rotating Zone. So, there should be some relative velocity on those patches. I am thinking, this may be the reason, why OF torque value is not matching. May be my thinking can be wrong.

Can any body help me on this.

[pechwang]

Hi Linnemann,

I want to know the torques on two patches. So I added two names. However, OpenFOAM only gives me the sum of the two torques. Can you help me with this? Thank you very much.

Pengchuan

Originally Posted by linnemann

Just a question.

Why dont you just use the forces library already present in OF?

put this in the end of the controlDict.

functions
(
    forces
    {
        type forces;
        functionObjectLibs ("libforces.so");
        outputControl timeStep;
        outputInterval 1;
        patches (wallBlade);
//        pname p;
//        Uname U;
        rhoName rhoInf;
        log true;
        rhoInf 1.205;
        CofR (0 0 0);
    }
);

This will output the forces/torque in x,y,z direction.

The output to the terminal will look like this.

    forces(pressure, viscous)((2162.2 -313.192 35.8823) (12.5865 3.1166 3.97532))
    moment(pressure, viscous)((1162.4 6862.37 100.944) (-12.5067 35.4299 -50.9462))

Then you can always make your own script to add the pressure torque with the viscous torque or just calculate them by hand.

[olivierG]

hello,

I guess you already have find the solution, but just in case :

functions
(
forces_patch1
   {
   type forces;
   ...
   patches (patch1);
   ...
   }
forces_patch2
   {
   type forces;
   ...
   patches(patch2);
   ...
   }
)

regards,
olivier

[pechwang]

Hi Olivier，

Thank you very much. It helps me a lot. I have another question. Do you know how to calculate the flow rate on one surface. It seems that it is very complex to do that. Is that right？Thank you again.

Pengchuan

[olivierG]

Hello Pengchuan,

If you are using OF version <= 2.0, take a look at http://openfoamwiki.net/index.php/Contrib_simpleFunctionObjects.
If this is not the case, take a look at swak4foam.

regards,
olivier

[pechwang]

Hi Olivier,

Now I use SRFSimplefoam to do some simulations. In SRFsimpleFoam, there is no U file, only Urel. I modify the code to Pname P; Uname Urel. Unfortunately, it didn't work. Can you give me a hand on this?

[neiht]

I think just waiting for some writing steps and modify controdict with Uabs.

[MadsR]

Hi guys,

I use Urel (this is the only one that works) in the force section of controlDict but I get very wrong torque. Any suggestions here? Or anyone having issues with SRFSimpleFoam and torque/forces.

Mads

[Tobias Adam]

I have the same problem as Pengchuan. I use SRFSimpleFoam and don´t get the right name for U. I even tried Urel but it didn´t work!

 forces
    {
        type forces;
        functionObjectLibs ("libforces.so");
        outputControl timeStep;
        outputInterval 20;
        patches (BLADE);
        pname p;
        Uname Uabs;   // or Urel, or U, nothing worked...
        rhoName rhoInf;
        log true;
        rhoInf 1.205;
        CofR (0 0 0);
        liftDir (0 0 1);
        dragDir (1 0 0);

I get the following error message:

  FOAM Warning : 
    From function void forces::read(const dictionary&)
    in file forces/forces.C at line 449
    Could not find U, p in database.
    De-activating forces.

I don´t understand why Urel does not work.
I use a second Run-time Post-processing library called Probes which works perfectly with Urel.

probes
     {
        type probes;
        functionObjectLibs ("libsampling.so");
        probeLocations ((0 0 -0.7) (1 0 -0.1) (1 0 0.1)  (1.55 0 0));
        fields ( Urel p );

Thank you very much for your help.

Best regards
Tobias

[Aurelien Thinat]

Hi Tobias,

I have never used SRFSimpleFoam, but there are some similar problem other solvers.

If there is no file U in your solver : it's possible that the force calculating utility use a hard coded name of the velocity file. If you can compile on your machine, you can juste create a field U defined by U = Uabs. And then use the force function with this new field. It should work.

You may have to do the same with the pressure if there is no "p" field.

[immortality]

Hi dear Tobias,
I haven't worked with this solver,what are the fields it uses?

[Tobias Adam]

Thank you very much for your help!

The problem is resolved as I changed

Uname Urel; to
UName Urel;

I found the problem, after trying all different controll dict entries listed in the different threads for this problem (also on other websites).
Many posts include this error that only leads to problems if your velocity-field is not named "U".

@ Aurelien: This seems to be easier than craeting the new U field ;-). Nevertheless thank you very much for your help

@ Eshan: As far as I understood the question, it uses Urel for the data output in the output-file from the backround process and from this it generates the Folder Urel and Uabs in the time directory.
The rest is similar to SimpleFoam :-)

best regards
Tobias :-)

[ozes]

Hi Friends, Somebody can compilate the files of calculateTorque?