# Gate valve flow simulations...

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 January 12, 2014, 22:03 Gate valve flow simulations... #1 Member   Nikesh Bhattarai Join Date: Nov 2011 Location: Sacheon, South Korea Posts: 82 Rep Power: 6 Hi all, I have been working on valve flow simulation project in my company recently and this is probably my third or fourth post in this forum here. "Boris", mostly has been very helpful in sorting my problems out from time to time. And I really thank you for sharing your precious time and knowledge with everyone in this forum. Anyways, let me describe briefly again what I am doing. I need to simulate for ball valve and gate valve flows while they are opening from a fully closed position (0%) to fully open position (100%). I am running steady state simulations for all the cases in a stepwise manner with an interval of 10%, which means I have 10 individual simulations to run for Ball valve flows and 10 more for gate valve flows. With the results, I need to compute and compare mass flow rate, i.e. the total amount of fluid (water, in kg) coming out through the valve in each of the two cases. So far I have pretty much managed to complete ball valve flows and now I have moved on to gate valve flows. While working on it, I have encountered few problems, few doubts I should say that has been confusing me. Fig 1 shows the 3D sketch of my gate valve and the pipe with the boundary conditions that I have imposed at the inlet and outlet lids. I started my simulations with 100% valve position. There seems to be no problem. I also compared the pressure drop with the "pipe only" flow, with the same BCs and the total length of pipe. The "delP" is again compared with the analytical result using "pressure drop online calculator" in the internet. Here are the results: delP-analytical = 0.25 bar delP-pipeOnly = 0.234 bar delP-100%Valve = 0.248 bar mass flow rate at inflow-analytical = 629.55 kg/s mass flow rate at inflow-pipeOnly = 627.755 kg/s mass flow rate at inflow-100%Valve = 626.599 kg/s In my understanding, these results made sense, so I then carried on with my further simulations, for valve position at 90% and so on. Pipe roughness and heat transfer effects are not considered. Here in Fig2, I would like to discuss some of the results and would like to hear from the experts here whether or not its looking alright 1. As the valve is closing, 100%-90%-80%-...and so on, delP is increasing-which is desirable BUT Why is the total pressure at inlet increasing despite the inlet velocity is fixed as a BC for all the cases? If my results make sense, I'm looking for an explanation for this. 2. Or should not the velocity at outlet change as well? Mass flow rate through the inlet and outlet are the same for each of the cases. I was expecting mass flow rates through the outlet to decrease from 100-90-80%....valve positions. Mass flow rate is the final result that I need. I need to plot "mass flow rate-vs-valve position", which should increase almost linearly with increase in valve opening area (valve position). With this observation I am most likely to obtain the same mass flow rate even at exactly the valve position, (rho*OpeningArea*avgVelocity), is it so? 3. To answer this question, I even tried obtaining the mass flow rate at the valve position but could not succeed to do so. Could anyone as well instruct me if there's a way to effectively extract those results in SW Flow simulation? GateValveFig.jpg 2-Results.jpg

 January 13, 2014, 06:04 #2 Senior Member   Boris Marovic Join Date: Jul 2009 Posts: 468 Rep Power: 15 Hi Nikesh, Your error is in the physics and your boundary condition definition. First let's consider the physics: There are some fundamental laws such as Mass and Energy balance. They are always valid and basically say what is put into a system will come out of the system again. m_in = m_out with m = roh * v * A and A beeing the aera and v the velocity Also if you look at the basic Bernulli you'll see that the total pressure is the sum of all kind of pressures: P_total = P_static + P_dynamic + P_potential dyamic pressure (1/2 * roh * v^2) is basically the pressure that can be built up on a flat plate in the find like the pressure you feel on your chest when driving a motor cylce. The potential pressure (rho * g * h) is due to hight difference. You can write this also as: P_total = P_static + 1/2 * roh * v^2 + rho * g * h Here you can also put the mass flow rate into the bernulli equation if you have an unknown parameter by for example using m = rho * v * A as v = m / (rho * A) and give you: P_total = P_static + 1/2 * m^2 / (rho * A^2) + rho * g * h Ok, now let's consider your case: In your case you can ignore the potential pressure. And since you are dictating the velocity, it will not change at the inlet and with the area of the inlet fix only the density could change but it won't for water in the pressure range you are condsidering (water can be considered as incompressible). That will automatically lead to a fixed mass flow rate and since the mass balance is law you will always get the same mass flow rate no matter what the valve does. For the pressure at the outlet you defined the static pressure and with that only the dynamic pressure could vary but since you fixed the inlet velocity the mass flow rate is fixed and with that at the outlet the velocity is fixed too. That leads to a fully fixed total pressure at the outlet since neither the static pressure, nor the density and velocity of the dynamic pressure changes. The changes you see at the outlet are probably in case you have used "average total pressure" as a goal instead "bulk average total pressure". The difference is av will use the surface averaged value and bulk av will use the mass flow averaged value and therefore also consider variations in the velocity distribution over the outlet surface. That leaves only the static pressure variation at the inlet as a free parameter that can be changed and since that is part of the total pressure you will see a total pressure change at the inlet. If you want to see a mass flow rate-vs-valve position diagram then you should not define the mass flow rate but the pressure. I think I suggested you to use rather total pressure at the inlet and static pressure at the outlet. So please try using total pressure at inlet and static at the outlet and you will get better results. If you want to have an initial mass flow rate at 100% valve opening which you might know from measurements then use it as an initial calculation with a fixed flow rate to find the total pressure to define at the inlet and use this for your next calculations. If you talk to your measurement team how they do such measurements, check with them if their pump regulates the flow rate or the pressure at the inlet. This should make it clear how it is done in reality. Regards, Boris manojkv and priyant like this.

 January 14, 2014, 01:11 #3 Member   Nikesh Bhattarai Join Date: Nov 2011 Location: Sacheon, South Korea Posts: 82 Rep Power: 6 Boris, Thank you very much for your swift reply. This is exactly the kind of explanation that I was looking for and I've been trying to hack into these for quite some time now. Ok, let me now put it the way I've understood so far in general sense. We have mass conservation equation, m_in = m_out and Energy equation (Bernoulli's equation) p_total, in = p_total, out to be satisfied for any flow, where p_total = p_static + p_dynamic + p_potential; In this case p_potential can be neglected which leaves us with: p_total = p_static + p_dynamic And incompressible flow condition. Case1-BC 1: My previous case where V_in and p_static,out were fixed and imposed as BC. Firstly, Continuity equation will always be satisfied leading to V_out = V_in. Secondly, p_static,out is fixed and from continuity equation V_out is obtained and is fixed too so is p_dynamic,out, hence p_total,out = fixed valve. I see some p_total,out values changed in my result, this is because I've used "average total pressure" as goals instead of "bulk average total pressure". Ques 1: Is "Bulk average total pressure" what I should use for goals??? Now, in the inlet, p_dynamic,in has been fixed too, hence, leaving only p_static,in to be free which changes (increases) leading to increase in p_total,in too. This increase in static pressure is because the flow has to move from inlet towards downstream since velocity has been imparted at inlet. Then, p_total,in > p_total,out leading to NOT satisfying the energy (Bernoulli's) equation, exactly the problem with my setup in the first case. Ques 2: Did I get it right here? Ques 3: Could this also be the reason why I was getting negative pressure values near the wake of the valves at 60%, 50%, 40% and so on? Furthermore, in each of these cases, pressure seemed to be increasing further downstream until the outlet which was fixed at 1 atm. These did not seem very physical to me, yet I wasn't able to figure out the source of this problem. There was no sign of negative pressure for 100%, 90%, 80% and 70% valve position cases. I forgot to mention this behavior earlier before. Case2-BC 2: As you suggested, p_total,in and p_static,out are fixed and imposed as BC. V_in and V_out are not known, hence calculation moves to the energy equation. Since, p_total,in = (p_total,in + 1/2*rho*V_in^2) = (p_static,out + 1/2*rho*V_out^2) = fixed valve, V_out is obtained. The solver then iterates to obtain optimal V_in and p_static,in values based on above equations and values. BUT then my question again: Ques 4: Since continuity equation has to be satisfied, which, for incompressible flow leads to: V_in = V_out, as inlet and outlet areas are the same. From energy equation, this again leads to p_static,in to be the free variable that can change and increase perhaps. This goes back to the same problem as in Case 1. This is not making sense to me again. These are few things that have been baffling me at the moment. I'm sure there're some misconceptions in my understanding or something that I might have missed. A little bit of more insight into it is highly appreciated, Boris. Thanks, Nikesh. bhushanvelis likes this. Last edited by nikesh; January 14, 2014 at 03:56.

January 14, 2014, 02:59
#4
Member

Nikesh Bhattarai
Join Date: Nov 2011
Location: Sacheon, South Korea
Posts: 82
Rep Power: 6
The reason why I didn't (couldn't) use pressure as inlet condition as you suggested earlier is because I do not have enough initial data to proceed with it. Figure 1 shows all the condition that's available to me at present. So based on the height of the reservoir, I have used Torcelli's equation to calculate velocity at the the bottom of the reservoir (the inflow position);
V = sqrt(2*g*h) = 12.82 m/s

As the measurements and experiments have not be carried out yet, we are at the moment, unsure of what the flow rate is at the inlet.

Like your suggestion in this post, I could perhaps use this velocity calculated in above equation, or mass flow rate for valve at 100% position (or pipe-only flow) to obtain the total pressure at inlet. This inlet total pressure value can then be defined as the inlet boundary condition for the flows with valve at various other positions. Will it make sense?

Also, while setting goals, I need to use 'Bulk average values' rather than simply 'average values'.

Does that sound reasonable?

Thanks,
Nikesh
Attached Images
 EntirePicture.jpg (50.3 KB, 70 views)

Last edited by nikesh; January 14, 2014 at 04:08.

 January 28, 2014, 02:31 #6 Member   Nikesh Bhattarai Join Date: Nov 2011 Location: Sacheon, South Korea Posts: 82 Rep Power: 6 Thanks a lot Boris! You solved all my problems with such precise and detailed explanation. However, it did take me a couple of simulations until I could completely grasp few ideas. Yet, now its all crystal clear and I have managed to complete all my simulations. I just need to wait for the experimental results and see how it goes. It might be couple of months more. Talking about Bernouli's equation as the energy equation was rubbish from my side, I don't know how it came into my mind Its the Navier-Stokes equation that govern the flow. Anyways, thank you very much Boris. Sincerely, Nikesh.

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post siw ANSYS Meshing & Geometry 13 November 27, 2012 13:07 dott.ing FloEFD, FloWorks & FloTHERM 6 May 4, 2012 16:52 steamerandy Main CFD Forum 0 October 31, 2011 22:08 safikhani_hamed CFX 1 August 9, 2011 06:46 TOM FLUENT 0 November 5, 2001 11:42

All times are GMT -4. The time now is 23:28.

 Contact Us - CFD Online - Top