5 Replies Latest reply on Jun 23, 2017 4:09 PM by Bill McEachern

    How to set inlet flow as transition Reynolds number

    Ayman Kamal

      I have a flow simulation problem in a rectangular duct with heat transfer.

      Duct walls are isothermal at 200 C and the inlet flow is at 450 C

      I am simulating inlet velocities between 40 - 80 m/s where I will have Re between 2600 and 5600

       

      Under Boundary conditions, inlet velocity, I can select inlet flow velocity, mass flow rate ..etc

      I don't want to select fully developed because I want to study the entrance region effects and where the flow will be fully developed

      But my question, I can only select boundary layer to be either laminar or turbulent and or input turbulence parameters

      What if my flow is going to be in transition region, how to input that to SW?

       

      What triggered me is that I am using 254 long duct (2.2 wide x 25.4 high) and I am splitting the duct into two parts in length

      And I am calculating the heat transfer rate at the second part (towards the outlet) so that the flow is more fully developed

      And I am back calculating heat transfer coefficient and comparing it to analytical prediction. What I am getting from SW with the current settings, a higher h values that seem to be for a turbulent flow not a transition flow. I want to make sure that I am selecting the right parameters for the inlet flow

       

      Thanks

      Ayman

        • Re: How to set inlet flow as transition Reynolds number
          Bill McEachern

          What I would do is extend the duct inlet, set it to laminar and let the flow develop to whatever state you want at the "start" of the section of interest. Run some tests on duct length to get what you are looking for and stick that in front of your model or something similar.

            • Re: How to set inlet flow as transition Reynolds number
              Ayman Kamal

              Thanks Bill for your reply.

              So what I was doing is extruding my channel extra 5-10 inches depending on inlet velocity and Re, I input inlet velocity as uniform without fully developed check box selected. And I am doing my analysis only towards the end region of the model (I split surfaces...etc)

               

              My issue that I am getting inconsistent heat transfer coefficients with theoretical prediction. My question is even with this extended part of the pipe, is there a certain procedure to specify inlet flow to SW that it is a transition case.. I see I can select laminar BL or Turbulent and set some Turbulent %

              But I don't see if there is an option to tell SW that this is a flow with transition Re

              Is there such thing? or in other words am I supposed to specify this to SW or it is implicitly taken care of

               

              Thanks

              Ayman

                • Re: How to set inlet flow as transition Reynolds number
                  Bill McEachern

                  My understanding of "transition" is a range of R'numbers form ~2000 to ~4000 for pipe flow. This is where the bulk flow in the pipe goes from strongly laminar (R'number <2000 - parabolic velocity distribution across the pipe diameter ) to strongly turbulent (R'number>4000 - more or less uniform velocity across the diameter - with well defined velocity gradient across the B'layer). Where in the range do you want to be exactly? You can just pick a velocity to get whatever R'number you want. The wall roughness and/or any other disturbance can get the flow to trip to turbulent in the range. I really don't get what you are after given my understanding of the phenomena involved. Maybe you are after something completely different.

                    • Re: How to set inlet flow as transition Reynolds number
                      Ayman Kamal

                      Hi,

                       

                      According to SW flow simulation technical reference. the entry length until the flow become fully developed is: (page 2-18 SW 2015 flow sim tech reference):

                      L entry to full developed = 100.d for Re=2500-6000

                      L entry = 40 d for Re>6000

                       

                      I agree completely of your description for transition region. My question is about operating and setting up SW

                      If I have a flow that I know will be in the transition region, are there any setting that I a missing that I should add while I am specifying inlet velocity or inlet mass flow rate boundary condition?

                      What I see is that I can select laminar boundary layer if my flow is laminar. I also can select an option for % turbulence...etc

                      But if my flow in transition (my Re is about 3000 for this run) I don't know if I should be specifying somewhere for SW that the flow is in transition region or not. Or does SW take that into account (i.e. automatically get Re and if it is within 2500-6000, it will apply transition region parameters to get the right entry length, the right Nu, the correct heat transfer coefficient?

                       

                      What triggered me is that I calculated the heat transfer coeff "h" for the surfaces downstream where (I assume fully developed flow exist) and analytically it was about 100 W/m2-K, but SW gave me about 196 (that will be if the heat transfer calculations were to be done using turbulent fully turbulent flow). So I am not sure is SW is considering this flow in transition regime or not.

                        • Re: How to set inlet flow as transition Reynolds number
                          Bill McEachern

                          You can plot the velocity profiles as cross section deformed surfaced plots. - that is to say a topographic representation of the velocity. I would plot those at intervals along the length and see how the flow transitions from laminar to turbulent - or whether or not it even happens for a given R'number. You are into some very fine details about how a RANS code does transition from laminar to turbulent. It uses a K-e model for closure and a wall model to keep the mesh size reasonable. This sounds like a problem well suited to a DNS solve and this would not be the code for that. Try open foam. Do you know any codes that pull this off with ease? I don't but then again I haven't looked. I would think you need to dig deep to find out how it handles the transition by doing numerical experiments and seeing how it makes the transition and over what length of pipe. My guess is that it would be more sudden than what would happen in an experiment and any experiment that said it was a reliable indication of heat transfer would need to have very high repeatability due to the tendency to want to go to turbulent with it being so susceptible to imperfections.  I would think in an experimental set up you would need a very well defined surface description to make this is any way repeatable in a different set up. It might work for an aerodynamically smooth pipe but hey I don't do this exact thing for a living and have not tried to find any papers on the subject but you might want to do that - I doubt it is simple though. Turbulence is not really well figured out in terms of simulation and transition and separation are in particular difficult aspects as far as I am aware. Good luck. It would be interesting to hear what you find. The first question I would examine though is exploring how transition manifests itself in flow simulation as you very the R'number through the transition and compare the transition lengths to some experimental work if it exists in the literature.

                          On the other hand if you know what velocity profile you want you can specify that as an input - however I think you are into a binary choice the initial B'layer. You can also change the free stream turbulence parameters if you know what you need.