Jump to content
Linux34

Oil Particels going trough Wall, Usage of SPH Method in SimLab

Recommended Posts

Hello Everyone!

 

I am using the nFX Tools in SimLab 2019.3 to create a simulation environment with SPH Particels. 

 

What i want to realise:

 

I just have a cup filled with Oil. It is open on both sides and surrounded by Air and i want the Oil to run out of the cup downwards. To close the system there is a cover around the air volume.

 

I have defined three Materials, the two Fluids Air and Oil, and a Wall Material. The Material specalizsations can be seen in the attachment.

 

I created the three different sorts of Particels in three steps. First i sealed the cup to create the Oil Particels inside the cup and the Air Particels. Then i opened the cup again and created the Container Particels as Wall. Finally i have put these three together.

 

To realise that the Oil runs out of the cup downwards i have created a Domain "Body Force".

 

The problem now is, that during the simulation with nanoFluidX some Oil particels are getting through the Wall Material of the Cup but i Have no idea why.  In the video attatched i have visualised the Velocity and the Oil (grey). The cup is not visualized there.  These particels are like shooted out of the cup.

 

Cup_SimulatinresultPNG.PNG.742b10b3357c6863eb9d07b88f1b9c57.PNG

I have also attatched an STL Model oft the cup and the cover. They are one model.

 

Does anyone have an idea what the problem is or what i am doing wrong?

 

Thanks a lot!:)


 

 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 

Materialdaten.PNG

Cup.stl

Share this post


Link to post
Share on other sites

Hi Linux34,

 

There could be many reasons why would this occur, but material definition is most likely not related to the problem.

 

For us to be able to provide better help, the log file of the simulation and the .cfg input file would be beneficial. Could you please share those here?

 

Thanks,

 

M

Share this post


Link to post
Share on other sites

So, looking at your log and .cfg - I cannot really see anything wrong. The only thing that strikes me is that your reference velocity (ref_vel) is 0.1 m/s, which could be a tad-bit too low, but I assume that a draining fluid could accelerate to faster than that under free fall. Try setting the speed to 0.5 m/s and see what happens.

 

Additionally to the above conservative measure, you can try to ramp up the gravity a bit more slowly by setting the:

 

t_damp_bodyforce_end             0.1     ; (instead of 0.01)

 

in the domain parameters. That might help stabilize things a bit. 

 

Finally, as a last resort, for these quasi-hydro-static type of problems, using the RIEMANN interaction scheme would probably be beneficial as it is more diffusive and would certainly smooth things out.

 

In order to do so, you need to set in the simulation parameters:

 

    adhesionmodel                    true

    freesurface                      true
    transportvelocity                false
    surften_model                    ADAMI
    energy_transport                 false
    viscTempCoupling                 false
    dt_factor                        1.0
    maxitsteps                       1000000000
    operationMode                    NORMAL
    interactionscheme                RIEMANN
    MLS_thres                        0.97
    APD_coeff                        0.001
    RM_freq_rho_reinit               20
    RM_rho_filtering                 INSTANT
    damping_type                     LINEAR
    

and in the phase parameters for oil/air:

 

phase
    {
        name                 Oil
        type                 FLUID
        rho_0                842.0
        dyn_visc             0.0463
        surf_ten             0.03
        print_info           true
        print_phase          true
        rho_compr            0.005
        rm_beta              3.0
        rm_rho_theta         1.e7
    }
    phase
    {
        name                 Air
        type                 FLUID
        rho_0                1.2
        dyn_visc             1.800000E-5
        surf_ten             0.03
        print_info           true
        print_phase          true
        rho_compr            0.005
        rm_beta              3.0
        rm_rho_theta         1.1
    }

 

The run will definitely be slower with these conservative settings, but you should get quality results, assuming sufficient resolution and no flaws on the geometry side.

 

Hope this helps.

Share this post


Link to post
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
You are posting as a guest. If you have an account, please sign in.
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.


×
×
  • Create New...