Please provide your Test case as well as the empirical equation and the limits of the equation.
|
You should avoid excesive cell volume jumps close to the wall. In my experience introducing some rounding at the edges of the contraction reduces the pressure loss. What are realistic radii achieved in the production?
|
1 Attachment(s)
Hello
my files are here. I've tried many different grids and schemes but all seems to reproduce roughly the same result. It could be I should try a small rounding of the transition and corners to make the geometry more realistic. Attachment 65952 The empirical relation comes from the book Pipe Flow - A practical and Comprehensive guide by Rennels and Hudson. It is given by where is the velocity in the small part of the pipe. is the loss constant, which for a diameter ratio of 0.5 is roughly 0.5. This formula also agrees well with this webpage calculator: http://www.pressure-drop.mobi/0303.html I've estimated k and epsilon from the following page http://ichrome.com/blogs/archives/342 and also tried other formulas. I've also tried running the simulation without wall functions and used the zero gradient boundary condition. |
Well, after your equation it is clear that you can satisfy your results based on Bernoulli. However, I will check the case today in the evening and will report back.
Edit. The geometry is missing. |
Here is a link to all the files:
https://drive.google.com/file/d/11-w...ew?usp=sharing My problem is that K_2 should be around 0.5, but my simulation corresponds to more like K_2 = 1.5. I really appreciate you taking your time to help |
Hi all,
I should do other things than investigating in that case:). However, I made it, and the result is as follow:
Also, we can take the Bernoulli equation that states: We know:
This is equal to 98125 Pa. The difference is 1875 Pa (= 18.75 mbar). In that calculation, we do not have any dissipation effects caused by vortexes/turbulences. Thus, as we already know that the Reynolds number is high, dissipation effects take place, and the pressure drop will rise. Therefore, the should be higher than 18 mbar and not lower. I changed your mesh completely and made the simulation with almost 80% fewer cells. Based on the high Reynolds number, the steady-state simulation cannot be reached (fluctuations). In your fine mesh, it has to be much worse. However, the average value of the pressure at the outlet is: Code:
Executing functionObjects Assuming the pipe to be very smooth, we might use the simple formulation of Blasius: The following calculation is related to the case attached. Pipe #1 (from the inlet to compression)
The pressure lose within the first pipe section is: Pipe #2 (from compression to outlet)
The pressure loose within the second pipe section is: Thus, the pressure loose based on the roughness inside the pipe is around 480 Pa. The 480 Pa are based on the pipe system and its length. As already stated, based on Bernoulli we will get an automatic pressure drop which is around 1875 Pa.So we end up in total with 23 mbar pressure loose. I guess - but I am not sure - that the K value, respectively the value takes care of turbulence dissipation inside the pipe too (becasue the Reynolds number is included). So as you can see from the K values calculated based on Blasius, we get complete different ranges for the pressure drop in the two pipe sections. I would trust that the pressure drop is around 30 mbar here. I already spend 3 hours for that topic now and to make it a fundamental work, you should:
Keep in mind that the pressure drop in the CFD simulation is more complicated as one might think at the beginning. Friction at the pipe wall (nut wall function), dissipation due to turbulence and recirculation, and bla blub :) even though this example is very simple, it demonstrates the complexity of fluid dynamics and the knowledge one should have to be really good within that topic. Hopefully your question is solved now. By the way. As you might realize, that the mesh sizes are entirely different (mine has around 20.000 cells) the results are more or less in the same area ~ 30 mbar. There would be other things I would like to say, such as the turbulence resolution, RANS, ... but well - I go to bed now. By the way, I got 30 mbar pressure drop via laminar calculation too. Case Download OpenFOAM Foundation 6.x |
Hi,
first of all, thank you for the kind words and your feedback & recap. Based on my lack of knowledge and almost rusty fluid dynamics lecture, I remember some equation you mention (Bernoulli + dp), but I cannot find my material right now. However, a short search gave me the following link (http://www.thermopedia.com/content/659/) where a comparison/equation is provided to calculate the pressure drop (it seems to be a bit different to yours) for cases we are looking at. One thing is clear at all: The sudden jump in terms of the pipe diameter should give a pressure drop based on viscous shearing/friction . Summing up. I refreshed my knowledge of the topic and might do some further investigations with the roughness of a pipe, respectively the nut wall functions - roughness (if there is any time). However, as I realized, there are still plenty of knowledge gaps I should reconsider to investigate some day. To your question of CFD information. I read a few books such as Bird et al. (Transport Phenomena), Wilcox (Turbulence), Ferziger et al. (Numerical ...), Moukalled et al., the Ph.D. thesis of Jasak Hrvjoe or Philipp Cardiff and many more. Personally, some literature was harder to read, others more straightforward. A summary of different books/papers/thesis is given in my book (still free on research gate). However, considering my book, there are still a lot of things to improve, and it might be somehow written in a 'different' way - I donīt know. The good thing nowadays is, that there is plenty of information out for CFD in general and OpenFOAM. E.g., the wiki.openfoam.com site or the courses of Chalmers :) As I am not intelligent and smart as other genius people out there, I always have to derive the equations on my own. After that, commonly I get the point - but not always :), and in some cases, I struggle to figure it out at all. Therefore, picking up your statement 'I am an idiot' does not hold and is disproved. To get an overview of the influence of numerical schemes you can check out my voluntary part of my website voluntary.holzmann-cfd.de. However, this is just an overview :) |
thanks for the reply.
I think the equation you linked to are the same as mine, rewritting for mass flow instead of velocity, and expressing v_1 through v_2 using the area ratios (constant volume flow). |
Okay, I was not sure because of the more complex formulation. As you said, K is around 0.5, I expected it is the S value of the equation, and thus, the C value is somehow missing. However, a simple calculation of the formula will give the answer.
|
I actually think they write that S is the area ratio of the two pipe section. C is K or at least closely related to it.
|
All times are GMT -4. The time now is 10:55. |