In the installation files, there is an exampel of a heat exchanger - hot air passing over a loop of cold water, as I remember from the training. The water pipe ends are closed off with lids, as are the airpipe ends.
Now: What if I want to make a closed circuit of the water? Say the water runs through a radiator and gets cooled down, and circulated back to the inlet?
Anyone having tried that?
//Bengt
Bengt,
While you can close the water loop and insert a "fan" as Jared suggested, the only result that you can obtain is that the water will approach the temperature of the air entering the "cooling coil" over time. I'm not sure if this will give you the information that you are looking for.
The tutorial is simplistic. While it will provide a result, that result may not resemble the real world because in the real world cooling air is done with enhanbced surface heat exchangers....ones that have fins to dissipate the heat. The water typically has a number of passes to provide sufficiently turbulent fow to obtain good heat transfer. Meshing such a heat exchanger is computationally very intense and you need a very fine mesh. When I have done this, I have to scale the problem to just one tube with an appropriate number of passes and rows of tube depth. In other words, a serpentine typically with the entering fluid entering the side of the heat exchanger where the air is leaving....counterflow.
And scaling this to one tube can take up to 48 hours processing time with 8 cores. However, I can solve this issue in a few seconds with a program from one of my suppliers of this type of enhanced heat exchange surface because their predicted performance is just scaled off actual test results. Maybe some day when Flow will support 1000 cores....................
Agreed. The fan is just to develop the closed circuit because it would be basically impossible to create a flow in on one side and pressure out on the otherside and connect them together so they act as a closed loop.
Regarding handling a dense heat exchanger. I would suggest handling it with a porous medium. Model a small part of it to get the porous medium curves and properties necessary. Then model the full system, replace the dense heat exchanger with the porous medium. You don't see the exact flow within that area, but at Hawk Ridge we've seen good overall system results with this method.
If either of you have a more detailed description of the system you're working with, feel free to PM me and I can give you an idea of how i'd approach it or if you're looking to have someone run the analysis or train you on running the analysis, we can do that through our consulting group here at Hawk Ridge.
Thanks, guys. Always good to get some input in areas you seldom handle.
I seem to recall from somewhere that there is a possibility to get data from the outlet - temp. of water for example - and feed it back into the inlet. Any of you done that sort of thing?
Bengt -
if you set a goal of the outlet temperature you can use this in an equation to define the inlet temperature.
Hi
Lets go back to phisics and energy equations (enthalpy)
Seems like you would like to reach steady state of this thermodynamic system. You should take energy of your cooling water in account! Not only temperature.
Steady state calculated by any cfd shall correspond to energy equations calculated for example by hand.
So you may consider boundary conditions with combination of energy values insted of temperature only.
... And your cooling water will reach steady temperature.... (If your simulation doesnt go into state of matter change because this is not what you can simulate within software that this forum is build for...check engineering database and material properties curves limits for more details)
Good luck
Radek
Have you tried this Chris? I think I tried this awhile back and there was a caveat. Most likely around having to pass the volume/mass flow rate from one side to another. Temperature is probably ok, pressure maybe, but I think the rest (enthalpy like Radoslaw suggest below) was a no go.
Good point here Radek. If this system involves phase change, then Flow Simulation will have some limitations.
Not recently, but I am fairly certain that I used this for a small water cooled environmental control. IIRC I used the outlet temperature and performance data for the radiator to define the inlet temperature. It was a low pressure room temperature cooling loop so nothing too complicated. If you've got compressibility and extreme temperature differences inlet to outlet it could quickly get more complicated.
Hi Chris, I made a straight tube with an inlet and outlet and tried using dependency to define the inlet temperature based on a goal for an outlet. I can't even get into the flow simulation tree to make a goal selection. Is there something that I'm missing? I know that you can set surface and volume sources dependent on goals but you do that by choosing the goal dependency option. Did you maybe fill in the dependency manually?
From the help:
Formula definition. Allows you to specify a formula dependency.
In the Dependency type list, select Formula Definition to define a formula dependency on x, y, z, r, phi, theta coordinates and time t (only for time-dependent analyses).
The log, sin, exp, cos, and tan argument must be in parentheses.
The "^" character is used to indicate the power to which the function is raised.
For example, to specify sin2x you must enter sin(x)^2. To specify sin x2 you type sin(x^2).
If you are specifying a dependency for a Surface Source or Volume Source, you may select a goal in the Dependent on goal list to add the goal to the formula. The temperature or amount of heat generated by the heat source will change during calculation in accordance with the formula.
Also from the KB, I was pretty sure that I had seen something before. Found this:
Solution Id: | S-038408 | Category: | FAQ | ||||||
Question: | My flow system is closed, so inlet temperature depends on outlet temperature. After one cycle, water from the inlet is warmer. Can I somehow add this dependence to my flow simulation? | Keyword: | |||||||
Visible to Customer: | Yes | ||||||||
Created On: | 6/2/2009 | ||||||||
Updated On: | 6/29/2012 | ||||||||
Answer: | The Internal Fan option allows the user to assign the outlet temperature as the inlet temperature. So as the outlet temperature increases so will the inlet temperature. The user can model the pump as a solid component and the inlet to the pump is treated as the outlet of the Internal Fan option. The outlet of the pump is the inlet of the Internal Fan option. The user will have to enter a curve for the flow rate vs pressure drop to make this work correctly. | ||||||||
Jared
How you want solver to know calculated outlet value before it is solved after first iteration? Impossible
thats what i'm thinking too. also the potential of perpetual flow generation. i think an internal fan is the only way to go. just like it would in the real system. (fan = pump)
Jared,
I have often used porous media to simulate the airflow across a water to air heat exchanger. In doing so, I am only able to simulate the air pressure drop across the porous media and determine if I have reasonable uniform flow across the face of the heat exchanger. I am not aware of any means that the porous media can create thermal effect on the fluids.
The example cited by Bengt was much the same as that in the heat exchange efficiency tutorial, except closing the loop. To make this tutorial more real world would require using much longer tube lengths, multiple passes through the fluid and the heat exchage tubing would be enhances on it's exterior with grooves spaced 26 to 40 per inch and on the interior with spiral turbulators to prevent laminar flow. This is often referred to as a Wolverine Turbo-Chill tube (www.wlv.com, products tab, evaporator tubes, Turbo-Chill or Turbo-B, etc.).
In my experience simulating four tube passes, each 10 feet long, with 26 fpi grooves, and with no internal tube spirals will take about 48 hours CPU time with 8 proicessors enabled. If the solver doesn't crash before that. Please let me know how you might simulate this type of tube with a porous media.
Hi David, just spitballing here.
First thing I'd do is see if we can get it to solve with a simple model. (Straight tubes) That should be do-able.
Then I would probably throw the spiral on there because I can't think of any way to handle that other than with modeling. This is obviously going to add some meshing and solving time. You'll probably have to do some testing here to figure out how much of a difference it makes to make sure it is necessary to include or to figure out how much mesh you need to get the basic behavior you're looking for from the spiral.
Now the fins on the outside, that is probably what is killing your computer and solve time. My first thought is to mesh it really coarsely and see what happens. My guess is, you're not going to get what you want. Even then, having all those fins modeled in SolidWorks is probably going to make the model really "heavy" to work with.
So that's where porous medium comes into play. You're going to have to work with a smaller section to get an idea of what kind of flow vs pressure drop curve it creates. You're also going to have to come up with a value for heat transfer coefficient within the medium that makes sense and also whether it behaves isotropically or ansiotropically. This is going to require some work and it won't be perfect, But I think it will get you close to what you're looking for. Check out S-050687 in the SolidWorks KB.
If that method doesn't work, you either you have to wait for the solution or break your problem up into smaller parts.
Jared,
Straight tubes solves very quickly. The finned surface on a heat exchange tube can increase the surface area of the tube 4-10x that of a straight tube, 30 minutes, let's say. With internal spirals in the tubing, the solve time increases to about 12 hours. Runnning with just the exterior fins requires about 48 hours. Running with both internal and external tube modifications crashes the system.
It is good thinking on your part to use a porous media to replicate the fins. but when you consider that porous media allows the fluid external to the tubes to flow through thte porous media, the result may not be even close. I envisioned minimizing the actual tube wall and encasing it in an annular porous media about as thick as the fins with a heat transfer coeficient 8 times that of the tube material. In effect making the heat transfer of the tube about 8 times what a straight tube would be. Probably make the porosity very high. Or just simulate the fins as a solid outer tube with a much higher heat transfer coeficient than the inner tube. I'll definitely try it when I get back to that issue.
But in any case modeling the actual heat transfer of a Turbo-B tube would seem to be a little beyond the realistic capability of Flow and 8 processing cores.
I have recently done a fairly dense HX with 3 nested helical tubes. the tubes were smooth luckily for me. Took a fair amount of resources. The long path length, in my case at any rate, of the tubes needed a lot of iterations for the initial temperatures to transition to steady state.
On the non smooth wall approach using porous media with heat transfer: I would bet it would dramatically reduce the resource requirements however some complications may arise. I have used this capability extensively to model high intensity heat sinks in electronics cooling apps. For this it works very well as the flow properteis in different directions can be handled with good fidelity. I think with a helical tube coated inside and out with a porous mdeia volume would have to be approximated with an isotropic porous media in terms of flow properties (of course it depends on how the fluid is moving - you may get away with directional properties if say the flow is along the axis of the helix which it might very well be on the outside at any rate). On the heat transfer side managing directions could be tougher as well but the energy only has one place to go and that is into the tube (or out of it) so it might work out. I would run a nice simple model and tune the porous media to get the best approximation against a geometric high fidelity computational model.
turbo-b looks pretty crazy, but i think the method that Bill and I describe can still work. You're right that it might have some complications to get absolute answers but i'm pretty confident that it will help you generalize the system performance and help you determine trends. it comes down to what you're trying to accomplish and learn. if you want to tune the pattern on the tubes, this method isn't going to work, if you want to understand the system, it should help.
Regarding implementation, it sounds like you've got a handle on it. Like you said, it won't act exactly like the fins but high density and appropriate porosity will help make things act as close as you can. You can tune the model through some initial simple setups.
Keep us updated on how it goes, sounds really a really interesting problem. We're going to have something on our blog at blog.hawkridgesys.com about the basic method shortly. (in the blog, we talk about going from a modeled perforated panel to porous medium using design studies in Flow 2013)
Jared,
Your ideas are appreciated. The application is the field of refrigeration where the primary heat exchange is between a refrigerant and air or waster, or many other types of fluids and vapors including other refrigerants. Secondary heat exchange is between water and air as is the basis of this post. All heat exchange between a refrigerant and another fluid is inherently two phase. Thuse the complexity of the outer surface of the Turbo-B tubes. They are designed to maximize the wetting of a boiling surface tube. Flow will not resolve these problems, and I am not sure that is realistically done with any simulation program.
Water to fluid should be attainable, though because there is no change of state. Your idea of using a porous media may allow for sufficient calibration to get a result, but it is certainly not straight forward in flow. Just a work around. If Flow is to provide a credible solution in this application will will require much more processing capability, either with more cores or compatibility with GPU processing. Unfortunately, SW is making very slow progress in harnessing thhe power of multi-core and GPU processing. I have seen CFD programs that do and can actually resolve airflow over a car in real time.
Hey Dave,
Don't you think you are asking a bit much for a program that is pretty much the lowest cost credible CFD program around? For starters I know very few programs for any amount of money that are going to pull off full geometric representation with suitable mesh density for a hgih fidelity analysis with any sort of reasonable cost compute resources. Yeah maybe you could get Fluent, CFX, STAR-CD or some other code that supports DMP to mesh and solve this type of geoemtry but the mesh will be unstructured and the number of iterations to get the thing to converge will be staggering due to the numerical diffusion inherent in such schemes. How many cells would it be? 50 million? Maybe double, triple or even way more than that? The only practical way to do this is with a model for the fins both inside and out. The cost to get some large number of processors involved through these vendors is completely non-trivial at like $2k per core -some more, some less and I am sure volume discounts would apply once you get into the hundreds of thousands of dollars range. What about the memory to hold the array?
The only way to get this done in any practical way will be an approximation of some sort and the methods available in in FLOW Sim I would bet could be made to provide at least a decent approximation sufficient for engineering purposes without some staggering amount of work. However, you would have to try it and tune the model against, numerical sub scale high fidelity anaysis and full scale test data. Yeah it might be a work around compred to brute force and ignorance methods but those approaches will have there challenges as well. It might not be so bad even with the limitations on coordinate systems in Flow. If flow allowed for continuopusly variable coordinate systems so that the radial, axial and circumferential directions could be slaved to the helix then you could do as good a model as could be expected for the general case.I am not sure this would be all that easy to pull off in any code. You could do this in Flow Sim if you were prepared to do the work by splitting the porous media bodies into sufficiently small chunks and putting in a coordinate systems for each one and then taking the time to assign them - I don't think this would be a work around. It would just be work. I think the "slow progress" remark is a bit unfair and not based on a realistic assement of what is availble in the market place. Flow Sim doesn't even charge for additional cores. Yeah OK they only go to say reasonable performance upto say 12 or so but still that could cost you $24k per year on Fluent. Would you be willig to allocate more $$$ to get these capabilites in Flow Sim? I am sure if enough people stood up and said there was a market and they would be willing to pay reasonable dough for it they might actually get it done.
Was thinking about this a bit more last night. Another set of "workarounds" would be to idealize the additional fins as heat removal through a negative heat rate or convection coefficient or i think you could even do a reverse thermal resistance or modifying the properties of the tube conductivity. All of these would need to be tested for validity but like Bill says, I think they all have potential vs the time it would take to setup in another program and the cost for the licensing and computing.
I do agree that it would be nice to have GPU or cluster computing but in the long run, there are only so many things that you can parallelize. We see in Flow that around 6 CPUs we start getting diminishing returns. I don't think the developers want to limit us there but they are also spending time on a great interface so I think the balance is good. Also, for most of the consulting projects that we do here at Hawk Ridge, we can get away with 8GB of RAM, SSDs, quad or 6 cores and solve the problem in a reasonable amount of time. That being said, it doesn't hurt to submit the enhancement requests through the customer portal. The more people that are interested, the better chance we have of getting the functionality. Here is one:
| SPR 648538: Support the Nvidia Tesla GPU so that solve times for Flow Simulation can be reduced |
| Source: SPRs |
I just submit a general one: 1-3570343571, feel free to submit one and reference mine so that you're added to the same one.
Hi Bill,
I'm not so sure that Flow is the lowest cost CFD program around. OpenFOAM is free and may support up to 1000 cores..
http://www.openfoam.com/features/parallel-computing.php
I am still on Flow 2009. It seems to run on up to about 8 cores, which is what I have. But how much has improved since 2009? And if I had upgraded every year,, what would the maintenance cost have been, almost $15,000? For a lot much less money than that I can bujild a new computer with a Tesla or Fermi GPU and run FOAM.
I fully realize that complex geometry needs to be scaled to obtain a result in a reasonable or even possible amount of time. And then you need to move from a micro to a macro simulation. Jared's idea of using a porous media to simulate the outer fins is definitely in the right direction. But ultimately when designing a shell and tube heat exchanger I have to be concerned about the gas liquid separation in the vessel sheel with 200-500 or more tubes. But now without the ability to simulate two phase flow, I really have no means to determine if liquid refrigerant will be carried out of the vessel. I could inject air as a particle, but the particle is post process and cannot effect the liquid. Flow is probably just not the right tool for the job.
I do appreciate your insight into Flow and do value your opinion. What I would really appreciate though is "What's New" in Flow from 2009 to 2013. I can't seem to find that on SW web site.
there have been some pretty big strides in CPU usage and meshing since 2009. I'd highly recommend checking out 2013. If you really need the what's new, I can take a look for it, but I don't think you're going to get what you're lookign for. It mostly has general comments. Actually trying it out might be best. Who is your VAR? They may be able to hook you up with an eval or demo or some presentations that go over the faetures.
I'm also looking forward to seeing what you can do with OpenFOAM. I've looked at it and it has some great features/functionality but I don't think the interface is as easy to use as Flow and I think you need to rely fully on forum/community support. Both of which may take more time than what you can do with a VAR for a supported software. I'm also curious to see what the solve time is with the super computing they can use.
On 2 phase flow, you're right, we can't handle that. The closest I've seen people get is modifying the fluid properties. Not exact, but gets you close.
Jared,
I posted the results of your suggested use of a porous media to simulate tube heat exchange fins on anew post. Thanks for the suggestion, It does help.
I fully know that OpenFOAM is a much more difficult interface than Flow. But it does open up the opportunity to contract the work to either pre doctoral students that use it or professors in accademia. Flow is great to use. But BIG opportunities in product development may require a more parallel solver, like a Kepler GPU. I'm going to try it myself\. I used to keep a C++ programming manual to read when I couldn't go to sleep. But there are probably people out there that don't get sleepy usning C++ or Fortran.....
Good luck on open foam. Pm me with your findings.
Regarding flow and gpu, you never know what a future version will hold.
It can be done. Just like a rad system, you need an internal fan to drive the fluid motion.