9 Replies Latest reply on May 26, 2014 8:28 PM by Jared Conway

    problem with surface area

    Dan Hofstetter

      Hi,

       

      I have a simulation with an environmental pressure inlet with a surface area of 61.8 sq.ft. (7.415" x 100 ft long).  After running the simulation, I'm seeing results with a surface plot showing an inlet velocity of ~5 ft/s, when it should actually be closer to 10 ft/s.  Also, the surface parameter shows an area of 123.6 sq.ft., which is twice what it should show.  So, Flow Simulation is interpreting that surface to be twice as large as it really is, and the velocity is half as a result.  Any ideas what could cause this??

       

      Thanks,

       

      Dan

        • Re: problem with surface area
          Mark Keown

          Dan,

          Are you using a fan and fan curve? What is driving the flow?

          Is your inlet velocity an average velocity over the open area?

          This is a long narrow channel so friction forces will be greate and you more than likely have turubelent flow.

            • Re: problem with surface area
              Dan Hofstetter

              No, I'm using an outlet velocity on a face that draws air through three holes representing fan openings (I need to do it this way because I need a boundary condition that can be used even after a model has been changed by new design table entries).  The outlet velocity is 24.45 ft/s, which results in a flow rate of 60,000 cfm over three 50" diameter outlet holes.  I sized the inlet slots to be 7.415" high, and the total slot length in the building is 161.8 ft (along two walls), which gives a total inlet opening area of 100 sq.ft.  This should result in an inlet velocity of 10 ft/s (600 ft/min was the design inlet velocity I used with the 60,000 cfm flow rate to size the inlet openings).  I have attached my model if it helps.

               

              After solving the simulation, I inserted a cut plot across the centerline of the inlet openings.  The cut plot shows a velocity at the openings of only ~5 ft/s.  I also inserted surface parameters for one face of the longest inlet slot (which spans the entire length of the 100 ft-long building), and it shows an average velocity of ~ 5 ft/s with an area that is twice as large (no wonder the velocity is half of the correct value).

               

              Thanks,

               

              Dan

                • Re: problem with surface area
                  Mark Keown

                  I got it to solve properly but have SW 2014 which I think you have an older version.  Mass flow in = mass flow out (157.7 lb/s).

                  Increase the Computational Domain to include ALL geometry.
                  Suppressed Front Side wall Flow Box Outled lid.

                  Un-checked Hydrogen sulfide in the General Settings.Air Flow.jpg

                    • Re: problem with surface area
                      Dan Hofstetter

                      Mark,

                       

                      Thanks for running that!  Increasing the computational domain size to include all geometry certainly made the mesh look better - I was wondering why it didn't show very many solid cells.  Regarding this - flow simulation by default only creates a computational domain that extends a small distance into solid walls, so by default it doesn't include all geometry.  Is there a way to force flow simulation to include all geometry by default?  (maybe a setting somewhere)

                       

                      I was able to solve this before, it was just that the surface area reported by flow simulation for the inlet lid was wrong.  I've been working on this today, and by adding a local initial mesh on the inlet lid face with a fluid cell refinement level of 6, I can get the surface area to be reported as 63.5 sq.ft. (it should actually be 61.8).

                       

                      Here's what I don't understand:  That inlet lid is a rectangle, which is as simple as it gets when it comes to calculating area.  I understand that the surface area reported in flow simulation is calculated by integrating the mesh cell areas.  But, even a coarse mesh seemed to cover more than 95% of the inlet lid (the mesh and lid boundaries were nearly overlapping), so integrating the area of the mesh cells that were within the lid boundary should still give the same resulting area.  In other words, if you take a 100 sq.ft. rectangle and divide it into 100 pieces, then integrate the areas, you're going to get an area of 100 sq.ft.  If you divide it into 10 or 1,000 pieces, you're still going to get 100 sq.ft. when you integrate the areas as long as the boundaries are correct.  So why does flow simulation require so many small cells on that lid to report the correct area??  A mesh level of 3 did a great job of defining the rectangular inlet lid.

                       

                      Another thing I'm not clear on is how flow simulation treats partial cells.  If one mesh cell does cross over the boundary of the inlet lid, doesn't flow simulation trim this into partial cells for the calculation?  If so, shouldn't it report the correct area every time, regardless of mesh level?  I can understand a circle not being perfect if the mesh is too coarse, but rectangles should be easy.

                       

                      Thanks,

                       

                      Dan

                        • Re: problem with surface area
                          Mark Keown

                          Dan,

                           

                          Others would need to help you with meshing details (area issues) or great information in the Help\ Flow Sim \ Tech Ref document. 

                          In Results \ Cut plots tick the mesh icon to show the mesh - so you can see what is up?

                          Try un-ticking the Automatic mesh setting and adding planes on each face of the opening - to force the mesh to fit OR

                          Insert \ Local mesh on each surface of the opening.

                           

                          Not sure why the default domain did not work.  Possibly it was the lids sticking out of the domain.

                           

                          In my opinion mesh level 3 should be used only to test to insure that everything is solving.  Higher levels of mesh are needed for results especially at low velocity / Reynolds number (Re < 1000).  How do you tell if you have enough mesh?  If you have 'enough' mesh then increasing the mesh level will not change your answer.

                           

                          I would suggest using mass-flow instead of velocity & volume.  As the gas pressure changes the density will change so the gas volume in and out will not be the same.  Conservation of mass not volume.

                           

                          In general the areas that the gas goes through should be increasing.  Each expansion and contract of the gas is a head-loss with resistance related to 1/Area^2.

                          Flow resistance are:

                          Expansion into the room

                          Flow across the room

                          Contraction into the vent

                           

                          Strongly suggest using a fan-curve.  A fan rated at 100 cfm will not deliver 100 cfm it will always be something less (and can be significantly less) due to system head loss.

                           

                            Cheers, Mark

                            • Re: problem with surface area
                              Dan Hofstetter

                              Mark,

                               

                              Thanks for all the suggestions!  I modified this model slightly by disabling that inlet lid so there would be a physical opening instead of just a surface, then adding a new environmental pressure lid over the entire outer face of the wall.  Flow simulation seems to like that better, since it correctly recognizes the opening, even with the default mesh level of 3 (I'm also using that low mesh level for testing).  I'm running the simulation right now to make sure it gives me correct flow velocities.

                               

                              I'd love to use a fan curve, but I need to be able to change the fan flow rate from a program outside of SolidWorks, and the Flow Simulation API doesn't allow that.  It does allow one to change velocity and flow rate for an inlet/outlet volume flow, though.  For this model, it is assumed that the flow rate through the outlets is the total flow rate at 0.10" S.P., which will account for much of the headloss through the building.

                               

                              Thanks,

                               

                              Dan

                                • Re: problem with surface area
                                  Jared Conway

                                  Getting here late. What is the status of the issue?

                                   

                                  It sounds like a mesh resolution issue but I haven't looked at the files.

                                   

                                  Outlet volume flow rates are also not recommended by the developers.

                                    • Re: problem with surface area
                                      Dan Hofstetter

                                      Better late than never   I need to look at the results from the latest simulation tomorrow morning, then I'll post an update.

                                       

                                      I've seen the "Outlet volume flow rates are also not recommended by the developers" comment before.  Why is that?  In this particular case, the actual physical system uses exhaust fans to draw air through the building.  Wouldn't the correct model for this be an outlet fan or outlet volume flow?

                                       

                                      I know the fan model is preferred because of the fan curve, but since the fan models can only be changed by a human at the keyboard I can't use them here.  I'm setting flow parameters from VBA code, and I already have 19 different configurations in my Flow project which can be activated via the API from my code.  Each configuration has a different fan selected to cover the selected range of possible pit fan flow rates.  The barn ventilation air flow rate could be anywhere from 35,000 to > 1,000,000 cfm depending on building size and number of animals, which would require too many additional model configurations, hence the outlet volume flow B.C.  I'm not modeling a specific fan, I'm modeling the overall system.  All I really need in this case is a simple fan model with ~10% loss in flow rate at 1" S.P., but with an API programmable flow rate.