10 Replies Latest reply on Feb 4, 2011 7:36 AM by Chris Michalski

    Flow Simulation mass balance

    Chris Michalski

      Okay, anybody got any hints on an easy way to determine where Flow is losing mass?

       

      I've got a furnace process modeled.  Long muffle furnace so I put a 1atm pressure BC on the open ends of a segment of it.  Process gas is injected and exhausted (both defined as mass flow rates) in the center of this segment.  I get vortex warnings routinely so I tried switching one open end to a defined flow out (50% of (injected - exhausted)).  I left the 2nd side as a pressure just in case....

       

      Well, when the pressure end still has vortex warnings (oh well, I'll live with a bit of resolution error there).  But when I query the Surface Parameters that end is nowhere near the other end for mass flow rate.  Somewhere my model is consuming gas.

       

      I know it's a closed model because I've got fluid assemblies that show the interior and exterior are separated so unless someone changed the rules Flow should only allow gas to enter or exit the model at BC's correct?!?!?

       

      IDEAS?!?!?!

        • Re: Flow Simulation mass balance
          Dan Cook

          Are you sure the solution is converged? I'm not a SW expert but I've been doing CFD for 20 years but you may need to tighten up your convergence criteria over the default.

            • Re: Flow Simulation mass balance
              Chris Michalski

              Dan -

               

              Thanks, I hadn't considered that.  It was such a nice round difference (the mass lost was equal to some of my inlet/outlet flows) that I immediately assumed it had simply lost something, not that the pressure BC hadn't fully converged.  I've found enough points where the VAR submits a request and SW responds that I've found an unusual anomaly that by default I jump to blaming the software instead of the operator.

               

              Defining convergence criteria has never been my strong point.  I'm always afraid I'll under define - I've got 3 computers with 2 dedicated to simulation so a few extra hours doesn't kill my productivity.

                • Re: Flow Simulation mass balance
                  Dan Cook

                  I've done CFD work with Fidap, Fluent, Star3d and Comsol besides having written some very basic modeling code myself. I think every software support engineer has reminded me to tighten up the convergence criteria when I would come to them with the same question... 8) I'm not so smart but I have worked with some very smart people.

                   

                  In all of those codes, the convergence criteria was based on residuals falling below 0.001 or thereabouts, which still allows pretty hefty errors in localized parts of the solution domain.

              • Re: Flow Simulation mass balance
                Bill McEachern

                I have been working with this code pretty hard for 12 years on all kinds of different problems and I don't think I have had one analysis where it did not produce a converged mass balance pretty quick - but hey I haven't seen your problem or the set up so you may have something different going on. To properly check the mass balance go to surface parameters and pick all (three?) inlet/outlets and ask for the mass flow rate. If that is producing significant non-zero amounts, then you have an issue. If you have re-circulations then the temp of the fluid coming back from outside the domain might lead to errors if the recircs are significant fractions (see error msg as they occur to get the ratio of in flow to out flow) and the temp specified is significantly different than what is being discharged. If that is the case extend the domain to avoid the recircs at the boundary well at least till they become less significant - say less than 5% or so.

                  • Re: Flow Simulation mass balance
                    Chris Michalski

                    Bill -

                     

                    I typically don't look at the mass balance to verify it's not an issue (I just assume it gets the basics right).  But there was so much vortex and non-uniform flow at the 2 ends of the system that I just couldn't believe it would be that asymmetric.  I've got 7 years of FloWorks under my belt (most of it with similar process equipment) so this was a surprise to say the least.

                     

                    If you look at the attached PDF of the feature tree:

                    1) First is the major process gas inlet (mass flow written in pen is verified from Surface Parameters)

                    2) upstream process ambient - ideally 1 atm but in this iteration I set it as 1/2 of the input to try to keep it symmetric instead of letting it go askew

                    3) downstream abient - I left this side as ambient to avoid overconstraining the model

                    4 & 5) define mass flow inputs of barrier gas flows

                    6-17) define pairs of individual flow paths - don't communicate with each other or the rest of the system

                    18 & 19) defined exhaust flow

                     

                    So 1 + 4 + 5 = 2 + 3 + 18 + 19 (input = output) but this is not the case.  As I said, 4, 5, 18, 19 are each 50SLPM so the fact that my model was missing 100SLPM immediately struck me as it simply lost some of those, but when I look at flow trajectories they are all reasonable, except the downstream that I left it to solve the mass flow.

                     

                    I am left to assume that because I left one end as a pressure it takes time for it to resolve the flow based on iterating using the pressure as the driving force.  I would think it would take into account a mass balance to speed up convergence but this might complicate other parts of the calculations.  I suppose in the future I'll simply constrain the flow rates or look into setting an initial velocity condition on those ends to have a balanced mass flow from the beginning but leave it constrained as a pressure opening BC.

                      • Re: Flow Simulation mass balance
                        Bill McEachern

                        At the risk if embarrassing myself, what are SLPM? Is that standard liters per minute or is it some unit of mass?

                          • Re: Flow Simulation mass balance
                            Chris Michalski

                            Yes, SLPM is standard liters per minute - for our process mix 1slpm = .00002085kg/sec

                              • Re: Flow Simulation mass balance
                                Dan Cook

                                I was going to try to come up with something humorous but wasn't quick enough...

                                • Re: Flow Simulation mass balance
                                  Bill McEachern

                                  At the openings with recirc's what is/are the in out fractions and what is the average fluid temp upstream of the recirc eddies and what is the temp setting in the BC specification under thermodynamics parameters? Maybe you have a colder temp on the BC so more dense gas in coming in via the recircs and resulting in a upset mass balance - though you would think it would sort it out. extend the outlets and get rid of the recircs - see if it help.

                                    • Re: Flow Simulation mass balance
                                      Chris Michalski

                                      The temperatures are a bit off, I guessed at 200C but they're working out closer to 300C - they are cooling loops so I don't have data back yet from production on the exhaust temperatures.

                                       

                                      As for the recriculation, when it ended the calculation it was getting .09-.12 for the inlet/outlet.  These are non-critical cooling loop flows and things are streamlined by the time it gets to any point of significance so I'm not overly concerned.

                                       

                                      BUT.... it says inlet/outlet is at most .12 - then why when I look at the surface parameters for one of those do I see:

                                      Mass flux [kg/(s*m^2)] minimum: -5.99  maximum: 1.97  Avg: -2.05  Bulk Avg: -3.44

                                       

                                      If it says in/out is ~10% then why is it really more like -6 to +2  So I have 6 masses leaving for every 2 recirculating back in - in my math that's 2/6 = .33 not .12

                                       

                                      I'm entirely self-taught in FloWorks so my understanding of the physics is better than the interface so how exactly it defines some terms is debatable, but inlet/outlet seems like a pretty straightforward concept.