11 Replies Latest reply on Oct 18, 2010 2:58 PM by Igor Isayev

    Temperature input settings at Pressure Boundary Condition

    Igor Isayev

      I’ve ran CFD transient study for an application with (2) volumetric heat sources and a cooling fin between them. Cooling fin has Inlet and Outlet ports as well as a flow field for the coolant to pass through it and to pick up the heat from those (2) hot bodies. Inlet Volumetric Flow has initial temp. (20C) and has a complex flow cycle (5 min. pump off, 30 sec. on). Heat source rate is also time dependent (it does not matter for the case).
      When the maximum fluid temperature at the Outlet port was plotted for the first 1000 sec., I’ve noticed that the maximum outlet temperature starts rising from initial 20C up to 30C and has no change after 30C that did not have much sense to me (see attached JPEG). The minimum and average temperature values showed all values between 20C & 30C though.  Analyzing the nature of the temperature 30C as the potential upper temperature limit, I realized that this temperature was initially setup at the Outlet where I applied Static pressure condition.
      Currently, the pressure condition requires the temperature input in Flow Simulation Dialogue box.

      I wonder whether the pre-set temperature at Pressure BC has any effect to the actual temperature of the flow. If yes, how to eliminate this effect and get the actual temperature data of the outlet flow? 

      Thank you.

       

      2010-10-14_170703.jpg.
       

        • Re: Temperature input settings at Pressure Boundary Condition
          Bill McEachern

          the outlet temperature as I understand it is  used in case of re-circulations at the outlet. If you have a vortex crossing the boundary the temp set for the outlet temperature is the temp of the incoming fluid. It should have no effect on the fluid coming from within the flow domain. It doesn't look like your geometry would  produce such a vortex but it is hard to tell from the picture supplied. I would draw a sketch through the flow path and then plot the temp along the path and see what you get. I can imagine situations where would see higher temps than 30 in this plot so it may or may not be a definitive plot. Since you know the heat input and the flow rate and obviously the heat capacity of the fluid what does that calculate out to be for the average temp of the fluid?

            • Re: Temperature input settings at Pressure Boundary Condition
              Igor Isayev

              Thank you, Bill for the quick response. Frankly speaking, I’m dreaming about having VAR like you.  For the last 4 days, I’m still waiting for any response from my VAR….

               

              When you mentioned about a vortex crossing the boundary, I’ve realized some things.  First of all, I’ve seen the warning in Flow Simulation monitor regarding “A vortex crossing….ratio Inlet/Outlet =1 (or 0.99999962)” that showed up when pump was off (5 min.). After 5 min., the warning disappeared and did not show up during the 30 sec. when pump was On. Initially, it did not make any sense because there was no flow condition with pump OFF so it should not be any vortexes. However, there was a very low velocity shown in the corresponding plot (see attached JPEG) so I’m guessing it might be the natural convection flow type. Second, if I have flow cycle with pump ON-OFF, probably I should not have setup just (1) CFD study having “Heat Conduction in solids “option enabled.

               

              I guess I had to generate multiple CFD studies for each cycle period and enable “heat conduction in solids” option when a pump is ON and “heat conduction in solids only” when pump is OFF. Additionally, I have to transfer all results from one CFD study to another to get the complete data in 1 hour for this transient study. I expect to see 11 CFD projects if I use this strategy and my assumption is correct.

               

               

              2010-10-15_094829.jpg

                • Re: Temperature input settings at Pressure Boundary Condition
                  David Arthur

                  Igor,

                  One option here may be to create an offset surface off of the outlet port and use the new surface to define the outlet goals. You can use offset surface command to generate a surface and then just disable it using component control. You can then use the offset surface to define the outlet goals instead of using the outlet BC face. You won't need to change the location of the BC. Just change the surface the goal is referencing. This may help stabilize the results.

                   

                  David Arthur

                  • Re: Temperature input settings at Pressure Boundary Condition
                    Bill McEachern

                    Hi Igor,

                     

                    If the vortex is happening when the pump is off it is probably inconsequential. I wouldn't worry about it - as you implied it might be either noise or natural flow if gravity is turned on. I am not sure I fully get what you are trying to capture but I would think you can do the whole thing as a single transient study with heat conduction though it may take a while to compute. As the next poster, David Arthur, alluded to you may just have an "instrumentation problem". His approach may have a problem though. Flow Sim at least as far as I am aware will not recognize a "surface", though it might in this particular case (i haven't tried it) but generally not a good idea to involve surfaces. I would suggest putting in a solid body just upstream of outlet and then disabling it and picking one of the surfaces to use as a goal. Feel free to extend the outlet further downstream if you need to get the measurements at that plane. Moving the outlet further downstream will avoid any "contamination" near the sensor.

                      • Re: Temperature input settings at Pressure Boundary Condition
                        Igor Isayev

                        Bill,

                        You’re right - the gravity was ON so as a possible step to fix the problem is to disable it. In this case, I would know that there is no natural convection hence the velocity is 0 within a flow domain when a pump is OFF.  I think it will be the best bet for now rather than generate 21 sequent CFD studies as I initially thought (previously I counted the number of separate CFD studies incorrectly). You’re also absolutely right saying that the study will take a while. From my records, it took about 91 hours to calculate 1096 sec.( having 8 processors running simultaneously).

                        Regarding David’s suggestion, I could extend the outlet port as a typical solution in a case when there was a warning “A vortex crosses the pressure opening”. The fact is that I used that model more 200 times solving CFD studies under various BC’s with no warnings so I don’t think that the port extension will fix the Temperature Issue I had.

                          • Re: Temperature input settings at Pressure Boundary Condition
                            Bill McEachern

                            Hi Igor,

                            There is a switch for a function called flow freezing which may have the potential to substantially speed up your computation. However, it would be a bit tricky to manage but not all that difficult. The flow freezing holds the convective terms constant while allowing the diffusive processes like conduction with slower response time time to sort of catch up without having to compute the convective transport terms. So, that means that when the pump is starting and stopping you do not want to be holding the convective terms constant as that would be a bad approximation. However in the middle sections when the pump is running, once its through its start up transient to just before it shuts down, it would be a good approximation. What I would suggest is tor run 1 cycle with the automatic time stepping and no flow freezing to get a base line - you may have it already. Then experiment with the flow freezing to speed up the calc and hopefully land at the same result or close enough for your purposes. 91 hours seems like a long time to wait. And another thing: there is not much to be gained by throwing 8 processors at a problem. You might as well throw 4 at it and start up another session of swx and Flow sim and work on something else - just can't be the same files (if you want the same files do a batch run and allocate  the resources so they are evenly split amongst the jobs for best scaling or if you still want to fire up another session of swx use just 1 processor per job and use whats left over to run another session).

                              • Re: Temperature input settings at Pressure Boundary Condition
                                Igor Isayev

                                Bill,

                                Thanks for all good recommendations. I’m familiar with freezing option to speed up some applications especially having Conjugate Heat Transfer.

                                If I have just one cycle (like my pump is ON permanently), it’s very convenient to freeze all convective conditions and push CFD tool to be focused on calculating the conductive processes. However, in case of the transient study with the specific Pump cycle, I don’t know how to use Freezing option:

                                1. Flow condition changes every 5 min. and it is active the 30 sec.  In order to apply flow freezing option, there is either periodic or permanent option to be used. If you look at this cycle from periodic or permanent stand point, you’ll realize the difficulty I’m having. For example, the pump will be on at 300 sec., and be stopped at 330 sec.  The next flow cycle will be in a time range of 630-660 sec. and so on. I would try to use this option if there is a tabular option for physical time or iterations. However, this option does not exist. Neither of the existing options won’t let me to freeze the flow at the right moment(s) during 1 hour ( see the flow cycle in JPEG) .
                                2. Another thing – how to define the possibility to apply the flow freezing option in the transient study if the flow condition in the application is very short. Will 20-30 sec. be enough to stabilize the flow parameters in order to “stop” it and direct CFD tool towards heat conduction in solids? 

                                Thanks.Pump ON-OFF cycle.jpg

                                  • Re: Temperature input settings at Pressure Boundary Condition
                                    Bill McEachern

                                    Well that is the tricky bit I mentioned. Essentially you have to manually do it and hence baby sit the calc. You just use the calculation control options to turn it on and off as required. Essentially you can let it run a sufficient number of iterations at pump turn on to get the flow more of less steady, then turn on the flow freezing option, it will rapidly advance in time, when it get close to pump shut off, turn it off and let it calculate the new flow or lack of it. Once that settles down you can re enable the freezing option and then repeat till the pump is about to go back on and then repeat for the process. Chances are that the flow will stabilize is some fraction or low numbers of seconds - which it terms of iterations could be more than a few -= like 40 or more (that is just a wild guess). It would be nice if you could put in a table to control freezing. It would be a nice enhancement.