remove backflow

frankefranke Member

Hello,

I am modelling a body in a 3d mutliphase domain, of water at the bottom and air on top, I am interested in the drag forces on the body which is partially submerged. my velocity inlet is 2 times the length away from the body and the outlet is 4 times length away, I am getting a lot of back flow and the mass flux is very highly positive. I am using symmetry through my body and all other boundaries are over 1L away from the body

Any suggestions on ways to reduce the backflow? Ideally zero backflow but that is not always possible, I have attempted to use both outflow and pressure-outlet. I am using the student software more or less to capacity on the number of nodes so very restrained on adding any additional length to the domain.

Thanks in advance!

«1

Comments

  • RobRob UKForum Coordinator
    edited April 1

    Do NOT use the outflow condition. It's not intended for multiphase, and is obsolete for pretty much everything else. 

    Have a look at open channel boundary conditions, that should help. Note, you can stop back flow in single phase, but it's not yet ready for multiphase. 

  • frankefranke Member
    edited April 1

    Hi,

    could you provide any more help on this? I've been trying to use the pressure outlet but the final mass flux it's recording is still very high. I've tried to look it up but had not much luck with what I can practically do, I have the operating pressure set as 101325Pa

  • frankefranke Member
    edited April 1

    I am also getting drag results with much higher magnitude than would be expected, coefficient of around 1.7 and force around 25000N any suggestions for this? I have all reference values and everything set? If there is any further info you need please let me know.

    The domain is rectangular with the upper and lower bounds sset as wall. Should the upper and lower walls be set as moving? it is a constant velocity through the flow 

  • DrAmineDrAmine GermanyForum Coordinator
    edited April 1

    Upfornt 2 object length is a minimum. Downflow 5 is a minimum. Better is to have more distance upwards and downwards. You can keep the top boundary as symmetry if it is far away from the free surface. I would say more than 0.5 of wave length if you are modeling open channel waves better to have more. Using pressure outlet at top boundary not really far away will result in affecting the overall free surface behavior. Same with symmetry which is actually wrong if you keep it near the free surface.

  • frankefranke Member
    edited April 1

    hi,

    Please find my current domain and conditions attached, I am modelling open flow but with zero wave condition. I originally had the upper and lower walls as symmetry but it was suggested to me that this could be affecting a previous error I was experiencing. would you suggest these be wall or symmetry conditions? my values have just significantly decreased as I discovered i had not set the operating density correctly but still possibility of change further.

    Thanks for taking an interest

  • frankefranke Member
    edited April 1

    any help on this, mass flux is currently around 6200000.... and it is suggesting that all the flow is being reversed... when i check the flux both inlet and outlet are positive...

  • DrAmineDrAmine GermanyForum Coordinator
    edited April 1
    you can use symmetry or free slip wall at top. St the bottom if it correspond to real condition use no slip wall.
  • frankefranke Member
    edited April 1

    Hi,

    Do you have a reference on these values for distances to boundary conditions? Thanks

  • DrAmineDrAmine GermanyForum Coordinator
    edited April 2
    based on internal investigation we made and recent work I did. Some can be found on customer portal as solution.
  • frankefranke Member
    edited April 2

    Ok thank you, 

    would you say a velocity inlet is acceptable for this simulation? I have seen evidence of it being sucessfully used however it is not suggested by ansys as a recommended condition for multiphase vof with open channel/wave bc

  • DrAmineDrAmine GermanyForum Coordinator
    edited April 2

    Nothing against using velocity inlet here. I used with open channel wave bc.

  • frankefranke Member
    edited April 2

    Hi, great thanks

    do you have any suggestion for the reversed flow? I am currently experiencing purely positive mass flux from both inlet and outlet...

    If i use pressure inlet then for the mass flux the inlet is negative and the outlet positive...

  • frankefranke Member
    edited April 2

    Should I be using a UDf for the outlet?

    thanks so much

  • DrAmineDrAmine GermanyForum Coordinator
    edited April 2

    You need to provide pressure profile at the outlet. For that reason I recommend working with open-channel /wave bc or you input your profile there.

  • DrAmineDrAmine GermanyForum Coordinator
    edited April 2

    And you will always get some reversal flow.

  • frankefranke Member
    edited April 2

    I have been using both open channel flow and wave bc however still experiencing flux issues. have also set pressure inlet

    I have specified the operating density as 1.225 (air) and the operating pressure as 101325Pa, . the boundary is now 5L downstream of the body. do these seem acceptable values for you

    I read the operating density should be of the lightest fluid however i am using water density for my reference.

    I have nt altered the default turbulent kinetc=ic energy or dissipation rates could this be a problem? I am only interested in the drag force and coefficient

    thanks so much

  • DrAmineDrAmine GermanyForum Coordinator
    edited April 2

    Please use the density of the lighter phase. To reduce backflow you can check if you can enlarge the domain or add a sort of modification downwards (venturi like or even a weir) this should not affect the main flow.

  • frankefranke Member
    edited April 4

    Hi,

    I have been doing these simulations as a transient simulation but would you find it acceptable as steady state? 

    I am interested in the drag results and not the time to reach it, key principles of the flow are k-epsilon turbulence, incompressible air and water

    I am somewhat limited for time to run these also

  • DrAmineDrAmine GermanyForum Coordinator
    edited April 6

    You can try Coupled plus pseudo-transient steady state solver. But I am sure the whole flow phenomenon is unsteady even it does not move at all. (motion of the body)-. We have done series of flow past ship hull using steady state solver

  • frankefranke Member
    edited April 6

    Yeh, 

    I also think it needs to be transient, even though I am running this my resuidulas are not converging to very high orders would you have any suggestions?

    I am also wondering if one of my issues could be through the wall function of the turbulence model, it is affected by the mesh size correct? My main mesh is of 10m size, the waterline is 1m and around the body is 0.5, the body is meshed at 0.1m

Sign In or Register to comment.