Pressure drop not correctly predicted
I'm modeling an experiment with a flow obstruction and predicting the pressure drop that was measured in that test section. However, my prediction is about 26% underpredicted from the experimental results. This struck me as odd. I thought that pressure drop would be predicted better than experimental velocity, but experimental velocities are predicted to within 10%. What could I change in my simulation to improve my prediction of the pressure drop. I tried refining the mesh by doubling the number of cells, but that didn't cause any improvements in pressure drop prediction (but did improve the velocity prediction).

If velocities and flow topology are predicted correctly, my bet would be on skin friction. Check that the y+ requirements of your turbulence model are fulfilled. Good luck!

Well, the accuracy of the flow velocity prediction is within about + 10% for like 80% of the measurement points. I don't know if this should be considered good or not. I was using the realizable kepsilon model with twolayer all y+ wall treatment. What kind of y+ values should I be targeting? My y+ values are between ~0.1 and 40. I thought that small and large y+ values were okay for all y+ wall treatment.
Another problem I just picked up on is my wall temperature calculations are about 30 Celsius off from experimental results, which seems like an awful lot to me. The surface area average temperature of the flow area matches up to experimental values within 1 Celsius, though, so it looks to me that the heat transfer coefficient at the wall is being badly predicted in addition to the skin friction coefficient, which again makes me think there's something wrong with the wall treatment. Any suggestions on how to improve that problem? 
What's your Mach number and what is the blockage ratio? And is your flow incompressible? If it is incompressible, average velocity coming in has to equal average velocity going out, assuming constant area. Conservation of mass. And the delta p is related to total loses. So how well are you predicting the drag on the obstruction and the WT walls? It is not surprising your velocity is better predicted than pressure loss. Also, how do you define pressure loss? Is it the average pressure loss upstream and downstream over the entire cross section area?

Quote:

Mach number, I don't know... it's incompressible and the Reynolds number is about 100,000. Blockage ratio, I think, was about 30%, but I'll have to get back to you on that if that's important. I'll tell you what I did notice about the velocity predictions, though. In areas of the flow region where there is a higher ratio of wall to open flow area, the velocities are more severely underpredicted compared to the regions where there is a higher ratio of open flow area to wall, which is almost predicted perfectly. It seems like it's the shear at the wall that isn't being predicted right. Mass flow rate is conserved, I checked on that already.
The experiment had pressure drop measurements taken over several sections of the flow area  each section having the same type of flow blockage in it (a grid of complicated geometry). I'm calculating pressure drops over those same sections. Interesting that you say it isn't surprising that pressure drop is poorly calculated compared to velocity. Why is that exactly? What of the poor heat transfer between the wall and the fluid, resulting in the severe overprediction of wall temperature? Can that problem not be related to the poor pressure drop prediction by a bad modeling of the wall effects in the turbulence model? I don't think I'm going to be able to post a pic of this, as you requested, but think of metal straps with their thin sides oriented with the direction of the flow. 
Quote:
However, pressure is sensitive and is a reflection of the loss across the blockage (grid of complicated geometry) So by saying that you are not capturing the pressure you are also saying that you are not capturing the drag on your blockage. Yes, there are possibly wall temperature affects, but if you can not get the drag on the blockage you have no hope of getting the pressure drop. Not sure of what your blockage is, but it sounds like some sort of radiator. What is your Reynolds number length based on? If you are incompressible, it does not sound like your Reynolds number is based on the fins of the radiator (i.e. grid). What is your y+ on the radiator fins/metal straps? Sorry, your y+=1 for your metal straps must be based on a representative length of the metal straps. If I understand this correctly, you are going to have a lot of small cells. Ouch. 
That all makes sense.
My Reynolds number is based on the hydraulic diameter of my flow channel. Should I be aiming for a certain y+ value on the straps in order to better predict the wall drag? Is there a problem with having lots of small cells (aside from the computational demand)? Could that be the cause of my inability to correctly capture the wall shear? 
Quote:
Quote:
Quote:
Another part is the equation of state. I deal with air and it sounds like you deal with a fluid (water?). It sounds like your blockage is significant in terms of creating entropy. For air, I would recommend using the compressible equations. I don't have a suggestion for a liquid. It sounds like your problem, in air, would cause a significant pressure drop and some sort of temperature rise. By the equation of state (perfect gas law), the density ratio of upstream and downstream would be affected noticeably, i.e. (rho1/rho2)=(p1/p2)*(T2/T1). Both the pressure drop and temperature rise push the density down. This then feeds back into the the other equations. I'm not sure what your equation of state is. But, for example, if your equation of state is equally sensitive to everything, like the perfect gas law, you need to use the full set of compressible equations. If density is not sensitive to pressure or temperature changes then you need to use the full set of incompressible N.S. equations. By this I mean that you need to include the energy equation and link it to the others by the equation of state. I assume you've done this since you have mentioned temperature. Sometimes the energy equation is dropped by neglecting temperature. And, finally, if temperature is not sensitive to pressure or density changes then the energy equation becomes decoupled from the other equations. In short, you need to use the right set of equations. Turbulence modeling. And I'm referring to turbulence modeling around the obstruction, i.e. wake/eddy modeling. It will determine the drag on the obstruction. It will also determine how your pressure loss and entropy loss mix in with the rest of the flow. But, how important that second part is depends on where your measurements are taken. It sounds like your Re number is low. So, around the obstruction you may not have much choice in regards to turbulence modeling. Or I should say wake/eddy modeling. You will need to go with unsteady laminar (i.e. not LES or RANS) flow and do the best you can with the resources you have. All of which is maybe what you are doing now. Oh, and at this point, all of my suggestions are just my opinions. It seems the physics you are modeling are complex due to significant interactions. 
BTW, you mentioned flow channel. Does this mean something like a water channel with the top surface exposed to air?
If so, there is a lot going on. Much more than I thought when this thread started! 
Ooops, I should be clear. Assuming adiabatic wall conditions, the only ingredient added by the obstruction is entropy.

Quote:
As for temperature, I should clarify, I'm running several cases. Some are heated and temperature is important. Some are unheated and temperature change is insignificant. The flow is incompressible (water). For the case where I'm comparing the pressure to the experimental values, the case is not heated and so I don't include the energy equation, just continuity and momentum. I don't think my Re is low (100,000), well into the turbulent region. I used kepsilon first, but I think I'm going to try out komega and see what difference that makes. There is no air above the vertically oriented channel, it's totally filled with water. It is a flow loop. 
To me, it sounds like you have TWO things you are trying to model. You are trying to model the obstruction and you are trying to model the channel. The obstruction just happens to be in the channel. The Reynolds number of 100,000 is for the channel since it is based on the hydraulic diameter of the flow channel. That will give you the y+ and turbulence model requirements for the CHANNEL WALLS. However, 100,000 is NOT the Reynolds number for the obstruction. The Reynolds number for the obstruction MUST be based on a representative characteristic of the OBSTRUCTION. For example, the maximum width of your metal staps. Or another way to think about it is this. How would you model the obstruction if it was not in the channel?
BTW, I goofed on the entropy statement. The obstruction is adding entropy and enthalpy because of work done by viscosity. I was thinking Euler equations. 
Have you tried comparing to an experiment without the obstruction?

Yes, I'm sorry I was not clear about that before. I'm trying to model the entire experimental test section, which includes both the obstructions and the bare flow region. You are correct that Re is based off of the hydraulic diameter of the bare region. However, I thought since the velocity increases in the vicinity of the obstruction and since there is a small drop in the hydraulic diameter, then the Re doesn't drop much or at all. Certainly, I'm sure the flow is not laminar in that region of the obstruction. The obstruction acts to increase mixing of the fluid in its vicinity. But I guess what it comes down to is what should my y+ values be for the bare region and the obstruction region? Or how could I find that out? Is it possible that my y+ values of <1 are actually too small?
As for your question about the behavior outside of the obstruction (in the bare region), my calculated wall temperatures for the heated walls are consistently off by about 30 degree celsius, even far away from the obstructions (>15 L/D). For all I know, the obstruction modeling might not even be a problem, or a very small one. It might mainly be wall shear and wall heat transfer being incorrectly modeled in the bare region (which is much larger than the region of the obstruction). 
It is my opinion that on the wall of the channel in the region of the obstruction (assuming the obstruction goes all the way to the wall) and on the obstruction itself you can not use wall functions. Therefore the y+ must be less than 1.

as far as i know ur y+ values should be between 0 5 then only u will get satisfactory results. The reason for this may be the mesh so i thnik u have to refine ur mesh.
Regards, Anil 
I've seen other posts where ppl said y+ should be above 30 always, however, I think that's if you're using a high y+ wall treatment. I'll check how the y+ differs between the obstructions and the wall of the test section.
The obstruction does touch the wall, but the obstruction is less than 10 mm long whereas the bare section of the flow area is over 200 mm long. I'm running a case using komega. I'll see how that works out and report back; however, I'm still using the same wall treatment. I'll also toy with my prism layers and see what that does. Thanks for all the suggestions. I'll report back with what happens. 
I'm assuming your obstruction is a grid of metal straps with the wide flat side facing the flow vector, this is used for mixing, and you mentioned that the obstruction is 30%.
The Cd for a flat plate, with the flat side facing into the flow vector is 1.98 based on its surface area. The Cd based on a reference area of your cross section is basically 0.6 (i.e. 0.3*1.98). This corresponds to a Cp loss of 0.6. This value is also about the same as the head loss of a thin plate orifice with a beta of 0.5 (i.e. sqrt of 30%) From the Moody Chart, assuming smooth walls and an Re of 100,000 based on diameter, the friction factor is 0.018. Therefore it takes 33.3 L/Ds (0.6/0.018) before the head loss from the channel walls is equal to the head loss from the obstruction. I guess I don't understand why your focus is on the walls. Head losses through orifices, and that is what your grid of straps sounds like, is huge. So, I guess I totally misunderstand your geometry and/or what you are measuring. Here is another way to look at it. Compare the drag due friction on your channel walls to the drag of your obstruction. This may help direct your focus. 
I'm going to be straight forward and I am sorry if I misunderstand things. And, I know I don't understand the big picture. But it sounds like you believe that only the wall friction contributes to the head loss. This is not true. Separation from the obstruction also contributes. And it could contribute a lot.

All times are GMT 4. The time now is 11:20. 