7 Replies Latest reply on Jan 28, 2011 9:32 AM by Loic Ancian

    How to add the boundary condition

    Devi Prasad Samal

      Hi all,


      I have a storage tank, in which i have to simulate the water storage and it's effect on the tank. as i have to apply the water as a boundary condition in the vessel which has a density of 1000kg/m3. i am little bit confused how to apply the water in the storage tank.


      please help how to do it?



      devi samal

        • Re: How to add the boundary condition
          Tomasz Wroblewski

          Hi Devi

          If  is just only storage tank  try first floXpress , outletCondition and inletCondition, this is a Buondary Condition.
          SW  Help (F1) Find in contents Solidworks FloXpress. After that you can pass data to Flow Simulation, without problem. Sometimes floXpress is enough

            • Re: How to add the boundary condition
              Devi Prasad Samal

              Hi Tomasz,


              May be my posting did not clear what i want?


              actually i want to apply the weight of water in the storage tank. and with non uniform distribution... but how to do it?


              if my density of water is 100kg/m3, then how much pressure i have to aplly in the surface of storage tank.


              and what equation should i use to apply non-uniform pressure across the storage tank

                • Re: How to add the boundary condition
                  Ahmad Bakir

                  Hi Devi

                  The pressure distribution with liquid as we know is linear like th form:
                  P = 9.81 * density * H (if the tank is opened to atm pressure).
                  so you can easily find out the pressure value at the base of tank by using the equation above.


                  • But why you need to load the Tank with nonlinear pressure?
                  • Do you need to simulate other material like soil or wheat maybe?
                    • Re: How to add the boundary condition
                      Tomasz Wroblewski



                      If I understand good, to check the tank (for deformation by the pressure and weight of water) you have to use SW Simulation with different types of simulations - Static
                      Nonlinear or Outher and finally all these simulation or combinations thereof can be added to pressure vessel design simulation

                        • Re: How to add the boundary condition
                          Devi Prasad Samal

                          Thanks for all of your suggestion...


                          Besides tomasz i think you understand my problem...i have to go for all the studies which u mentioned.


                          but before that i want to know how to add a non uniform pressure distribution to the tank....my tank is not cylinder is a jug like shape.


                          My question is for applying a non uniform distri bution of water we required a equation & a co-ordinate .


                          So ijust want to know how to define a water's pressure distribution over a tank.


                          if u can uploaded a model with proper load distribution, it really helps



                            • Re: How to add the boundary condition
                              Jacob Kuruvilla Thomas

                              The pressure distribution inside a vessel / tank will be uniformly distributed with 0 at the top and maximum at the bottom. teh pressure at any intermediate point is pressure = density * gravity * height. the procedure to apply the pressure is as follows. Model the vessel / tank and create a new co-ordinate system at the top most point where the liquid will be filled.  The X axis of the co-ordinate system should be pointing vertically downwards.The equation for a straight line is y = m*x. This is the same as the pressure at any point is equal to the density * gravity * height. i.e. y is the pressure, m is the product of density * gravity and x is the height at any point. Go to SolidWorks Simulation and create a new static analysis study. Give all the input conditions. Now for the loading part, go to pressure load. Select the areas for applying the pressure load. Enter the value of (density * gravity) in the pressure field.Select the check box for non-uniform distribution.  Select the newly created co-ordinate system in the co-ordinate system box.  Enter “0” in the constant field and “1” in the X field. Enter “0” in all other fields. The pressure will be  applied as a variable pressure load with 0 at the top and max at the bottom. All the loads are applied. Now mesh and run the analysis. Hope this helps.

                              • Re: How to add the boundary condition
                                Loic Ancian

                                Recommended procedure to define an hydrostatic pressure:

                                1. When defining hydrostatic pressure, the pressure direction should be Normal to selected faces.

                                2. The location and orientation of the Coordinate system used to define the  variable pressure is important. The best practice it to have the XZ plane lying on the surface of the fluid and  to have the Y axis pointing downward  (same direction as the gravity).

                                3. Select SI as the unit system, and make  sure the pressure unit is N/m² and not MPa.

                                4. If the above conditions are met, then simply enter 1 for the coefficient of Y and 0  for all 5 others. In the Pressure value  field, enter  the  product of the fluid's mass density. For water at sea level, you should enter  9810 (1000 kg/m^3 for water and 9.81m/s^2  at sea level on earth for gravity).