CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > FloEFD, FloWorks & FloTHERM

Kv Value of a Valve

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 2 Post By Boris_M

LinkBack Thread Tools Search this Thread Display Modes
Old   October 3, 2016, 09:26
Default Kv Value of a Valve
New Member
Join Date: Sep 2014
Posts: 1
Rep Power: 0
chigyy is on a distinguished road
Hello all.

I am a student and new user of SWFS. As I know, interface of SWFS is same with FloEFD. Therefore, I post this new thread here. If it is in the wrong place, I am sorry.

As a part of my study, I should be able to validate my flow simulation with the experimental results. However, I encountered with a problem. My problem is about the calculation of Kv value of a ball valve. I know that there is a tutorial about it. Eventhough, I follow the steps in the tutorial, my calculation deviates much more than the experimental result.

For the experimental setup, I follow "ISA-75.01.01-2007 (60534-2-1 Mod): Flow Equations for Sizing Control Valves" standard. Results of the experiment is given below:
  • Volumetric Flow Rate (Q)=53.1 [m^3/h] with pressure difference (Delta p)=0.2 [bar]
  • Kv=118.8 [m^3/h] by using the formula Q=Kv*(Delta p / SG)^0.5 where SG represents the specific gravity which is equal to 1 for water.

On the other hand, the setup I have done in the SWFS is given below:

Initial Setup
  • 2*D (D=Diameter of valve inlet) pipe is assemblied to the upstream and 6*D pipe is assemblied to the downstream (as it is stated in the standard for pressure taps locations).
  • Analysis type: Internal. Exclude cavities without flow conditions is unchecked.
  • Fluid is water. Flow type is laminar and turbulent. Cavitation is unchecked.
  • Default wall thermal condition: Adiabatic valve.
  • Thermodynamic parameters: Pressure=1.01325 [bar] and temperature=293.2 [K].
  • Units are same with ISO except few differences which are: Pressure&stress=[bar], physical time=[h], volume flow rate=[m^3/h].

Boundary Conditions
  • Environment pressure=1.2 [bar] at the inlet
  • Static pressure=1 [bar] at the outlet

  • Surface Goal: Inlet Lid: Volume Flow Rate [m^3/h]
  • Equation Goal: Pressure Difference: {Environment Pressure 1:1.200e+000}-{Static Pressure 1:1.000e+000}
  • Equation Goal: Kv: {SG Volume Flow Rate 1}/({Pressure Difference}^0.5) [m^3/h]

  • Global Mesh
  • Level of initial mesh: 7
  • Advanced channel refinement is thicked
  • Refinement level: 3

According to this setup, obtained results are attached as a supplementary information (Project name in pictures is 90_Degree_1bar. Please do not consider the statement "1bar" in the project name). I know that I should make time step analysis and mesh independency analysis. Since the flow is steady state, time step analysis is omitted. For the mesh independency, I raised the level of initial mesh from 4 to 7 and refinement level from 1 to 3. However, I am not be able to get the volumetric flow rate equal to the 53.1 [m^3/h] with +- %1-%2 error.

Before I post here, I read many of the threads in this forum. However, I could not overcome this problem. If my post is too long I am sorry. I just wanted to give all details that can help you to resolve the problem. Thanks for reading/helping me.

Have a good days and good luck in your studies/works.
Attached Images
File Type: jpg Convergence.jpg (59.5 KB, 20 views)
File Type: jpg info.jpg (66.7 KB, 15 views)
File Type: jpg log.jpg (67.0 KB, 12 views)
File Type: jpg results.jpg (16.6 KB, 9 views)
chigyy is offline   Reply With Quote

Old   October 11, 2016, 06:56
Senior Member
Join Date: Jul 2009
Posts: 616
Rep Power: 22
Boris_M will become famous soon enough
Hi Chigyy,

What are you looking for KV = Flow Factor or Cv = Flow Coefficient?

There is a difference as you can see and can depend on the units. I'm not an expert in the valve application when it comes to these coefficients but it makes a difference of course if you use US gallons per minute or m^3/s. The same goes for the pressure. Make sure the units match. FloEFD doesn't convert them, it only calculates with the values and puts the unit that you select for the equation goal at the end of the equation goal value. If you have to convert the units then you have to put the conversion factors in yourself or use the converted units directly by setting the unit already in the settings to the right unit.

As for your other settings:

Initial setup:
- You can use exclude cavities in the simulation as it will only ignore any hollow chambers where there is no flow happening as there are no boundary conditions applied. Everything that is connected to the boundary condition is resolved.
So if you have a tiny hollow area where there is no flow, it will simply ignore it. Saves CPU time and cells if there is nothing happening.
- You don't need to set the unit for the physical time if you don't do a transient simulation where that unit might make it easier in the post processing of a simulation that is running for 24 hours or longer and you want to see the results in hours rather than in seconds in any post processing feature.

Boundary Conditions:
- Be aware that Environment pressure is defined automatically as Total Pressure if it is an inlet (flow coming in) or as static pressure if it is an outlet (flow going out).

- For the pressure drop equation goal it is wise to specify a pressure goal for the inlet and outlet if you need a specific pressure. So if you want to know the total pressure loss then use a total pressure bulk average goal for inlet and outlet.
Right now you "might" get the total inlet pressure minus the static outlet pressure. Which is not a typical pressure loss definition. Better be clear what pressure you want to use to calculate the pressure drop.

- I highly recommend not to use only global mesh and simply use the highest level and adaptive refinement. This is a somewhat lazy setup and will cause often a very fine mesh with high CPU times to solve and a better mesh can be created manually in a more smarter way.
By manually I mean deactivate the automatic settings and set some specific mesh settings manually and maybe a local mesh around the valve body, the ball in case of a ball valve. You can still use the adaptive refinement to resolve the gradients but the global settings and full level is not giving a perfect mesh but rather a oversized mesh. Especially if you want to also show best meshing practice for high accuracy in the thesis rather than saying at the end the simulation took for ever and FloEFD or SWFS is too slow. A good mesh is usually built somewhat more smart rather than lazy. I usually start with a level 3 automatic to see how it turns out in a first mesh run and then go from there manually but in the latest versions you often can do that already nicely with the new features such as the refinement preview in order to judge the level you need. Only for larger complex models it is hard to look in every edge of the model and it is easier to simply create the mesh once with the settings you thing should work well and then sweep a cut plot with the mesh preview through the model and find areas which should be improved either by making them finer or coarser.

If you want a specific flow rate, then why don't you specify that and you will see what the pressures will be. You can specify surface goals of total and static pressure for the inlet and outlet and see which values you get. A 90 setting for the valve will have some larger deviations as it is basically a straight pipe with not much disturbance mostly. So the deviation for the pressure loss can be for example 1Pa from a 5Pa pressure loss in the experiment. That would give a 80% error but considering that 5Pa is basically nothing make the error not really relevant.
So if you expect a specific flow rate then simply apply it to see the pressure difference. Otherwise make sure you use the right pressure for the inlet and outlet (static or total).

I hope this helps,
Stevie_1200 and Manolis like this.
Boris_M is offline   Reply With Quote


ball valve, floefd, flow coefficient, swfs

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
udf for valve closing a pipe using dynamic mesh chem engineer Fluent UDF and Scheme Programming 2 May 13, 2017 10:39
Modelling an initially closed valve which a fluid opens siw CFX 1 April 26, 2014 07:32
Gate valve flow simulations... nikesh FloEFD, FloWorks & FloTHERM 5 January 28, 2014 02:31
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 10:11
Valve Forces in CFdesign Mike Clapp Main CFD Forum 3 March 8, 2001 15:09

All times are GMT -4. The time now is 17:21.