# Water Hammer Simulation in CFX

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

 January 23, 2012, 17:31 Water Hammer Simulation in CFX #1 New Member   Dominic Bernard Join Date: Jan 2012 Posts: 6 Rep Power: 6 I am currently trying to reproduce the water hammer phenomenon using a FSI method with Ansys and CFX. To do so, I have used a power point presentation given by an Ansys tech. rep. Unfortunately, the simulation seems to be valid only for the case of a rapid gate closure. If I slow down the gate closure ( from 0.0008 s to 30 s) , the pressure drops below the static pressure which doesn't make any sense. Furthermore if I compare results between a 2 s or 30 s closure, they are the same. Does anyone have an idea of what could be the problem ! Thanks

 January 24, 2012, 09:11 #2 Senior Member   Join Date: Apr 2009 Posts: 532 Rep Power: 13 Did you use a compressible form of water (density as a function of pressure based on the bulk modulus of water)? What's your wave speed based Courant number (i.e. a Courant number calculated using the speed of sound in water, your mesh length scale in the streamwise direction and your timestep)?

 January 24, 2012, 10:57 #3 New Member   Dominic Bernard Join Date: Jan 2012 Posts: 6 Rep Power: 6 I am currently using water as fluid and the compressibility expression I use for it is : 998 [kg/m^3]*(1+4.5454E-10*pabs/1[Pa]) Characteristic of my half pipe model are: Length [ 60 m] Radius [ 0.5m] Thickness [0.015m] My elements have [2 m ] in the streamwise diraction and [ 0.157 m] in the circumferential direction Timestep is [ 0.001875 s] so the Courant Number is [ 1.21875 ] (According to a use of [ 1300 m/s] for the wave velocity) The reference pressure I use for my test is 7500 kPa

 January 24, 2012, 16:07 #4 Senior Member   Join Date: Apr 2009 Posts: 532 Rep Power: 13 Those settings sound OK. Are you using a mass flow outlet and a total pressure inlet? Could you provide more details on where the results are not making sense. Having the pressure drop below the reference pressure is normal after the gate has closed. You should get an initial high pressure wave moving upstream, then an expansion wave to equalize the pressure moving from the inlet back towards the outlet, then than expansion wave should reflect off the closed outlet and cause a large negative pressure. In the real world that might cause cavitation, but I assume you're not simulating that. If you have a partially closed gate, then I not too sure how the reflection of that expansion wave will behave. Also, are you solving the Total Energy equation - if not, turn that on.

 January 24, 2012, 16:38 #5 New Member   Dominic Bernard Join Date: Jan 2012 Posts: 6 Rep Power: 6 Hello Stumpy, Thank you for your quick answer ! Here are my parameters: Outlet: Mass Flow ( CEL function of the closure time and the initial speed) ( 1.8 [m/s]-0.06[m/s^2]*(t)) Opening: Opening press. and direction: 0 Pa Wall: Ansys Multifield Symmetry: ( I use half of the pipe to reduce the computation time *** All the mesh motion are unspecified I solve the Total Energy Equation I have a partial gate closure Results I get : As soon as I start reducing the mass flow at the outlet, the pressure drops abruptly.After few iterations, the wave motion starts.

 January 24, 2012, 17:34 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,831 Rep Power: 100 Can you post your CCL and some images of the geometry? Also it seems your fast opening case opens the gate entirely within one time step, but your slow opening case will open it over many time steps. This means the fast opening case does not have to deal with a partially open gate. Partially open cases can be tricky as you can get flow with high pressure through a small gap which can have compressibility effects and general difficulty in convergence.

January 25, 2012, 10:59
Data for the model
#7
New Member

Dominic Bernard
Join Date: Jan 2012
Posts: 6
Rep Power: 6
I posted the CCL for the transient and steady-state analysis.

You could also see an isometric and a section view of my model.

Finally, I posted the results I obtained when I plotted the pressure vs time at the outlet.

**** As you will see in the CCL, I analyzed a partial gate closure, but at the end of the analysis, the outlet opening was still large enough to not create small gaps.

Dominic
Attached Images
 Pipe Section.jpg (28.8 KB, 184 views) Pipe Model.jpg (27.4 KB, 182 views)
Attached Files
 Transient File.txt (10.6 KB, 169 views) Steady State File.txt (10.5 KB, 118 views) Pressure vs time at Outlet.doc (73.0 KB, 167 views)

 January 26, 2012, 07:17 #8 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,831 Rep Power: 100 What has the steady state analysis got to do with this? Why is this an FSI analysis? What is moving? Your transient CCL file suggests the mass flow transition happens at 50s, but the simulation only runs for about 21s. Have you run it long enough? I note in your pressure versus time graph the pressure goes way beyond absolute zero. In reality this would be a massive cavitation bubble and not go lower in pressure than approximately the vapour pressure of water.

 January 26, 2012, 10:08 #9 New Member   Dominic Bernard Join Date: Jan 2012 Posts: 6 Rep Power: 6 What has the steady state analysis got to do with this? To initiate a transient analysis, a SS analysis is mandatory or else the pipe of the wall will have a sudden acceleration due to the large force causing the solver to fail. Why is this an FSI analysis? What is moving? The pipe's wall is moving. CFX transmits the forces produced by the pressure to Ansys through the wall. Ansys transmits the total mesh displacement to CFX . They then iterate until the convergence of both variables. Your transient CCL file suggests the mass flow transition happens at 50s, but the simulation only runs for about 21s. Have you run it long enough? The transient analysis starts at 20s due to the 20 iterations in the SS analysis. It runs until about 21s. The mass flow transition starts at 20s and could run until 50s but it stops at 21s due the end of the run. The 50s in the CEL function is necessary to create the slow mass flow transition. ( It reproduce a gate that would close in 30 seconds......1.8 (m/s)/30 s =0.06 (m/s^2)) The 50 s is the addition of the initial 20 s plus the 30 s closure time. I note in your pressure versus time graph the pressure goes way beyond absolute zero. In reality this would be a massive cavitation bubble and not go lower in pressure than approximately the vapour pressure of water. The reference pressure is 7500 kPa so 0 kPa on the graph is a relative pressure. My problem with this simulation is the initial drop. Theory tells us that the pressure should slowly increase and act as a sinusoidal wave.

 January 26, 2012, 15:44 #10 Senior Member   Join Date: Apr 2009 Posts: 532 Rep Power: 13 I see... so the pressure drops rather than increases when you start to close the gate. I would add a monitor point for mass flow at the outlet, then compare that to the value specified in the steady state run, just to make sure the mass flow really is decreasing at the start of the transient run (the expressions looked OK to me). On the structural side how did you run the steady state case? Was it a static analysis, or a transient with time integration off? Did you generate and edit an ANSYS.mf file to switch this back to transient? I would also look at the transient results after a couple of timesteps. What's the mass flow? Compare the total mesh displacements on the pipe walls near the outlet - did the walls expand compared to the steady state results? If so, look at the forces passed to ANSYS.

 January 26, 2012, 17:36 #11 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,831 Rep Power: 100 In addition to stumpy's comments, I would get this simulation running correctly with no FSI, then add the FSI component. FSI is adding another possible source of error which makes debugging harder. And I do not know why you say the wave should be sinusoidal. You are not closing the gate sinusoidally, and you have FSI in there which will add another non-linear effect, so why would it be sinusoidal?

 November 21, 2012, 00:02 Cavitation in Francis Turbine #13 New Member     Mausam Shresha Join Date: Aug 2012 Posts: 13 Rep Power: 6 Can get any ideas on to perform cavitation in Francis Turbine with CFX

 November 21, 2012, 00:07 Cavitation in Francis Turbine #14 New Member     Mausam Shresha Join Date: Aug 2012 Posts: 13 Rep Power: 6 Can get any ideas on to perform cavitation in Francis Turbine with CFX

 October 27, 2014, 10:51 compressible or not? #15 New Member   Giovanni Bettega Join Date: Sep 2014 Posts: 1 Rep Power: 0 Hello, in the attached ccl file both at the inlet, and both at the outlet the flow regime has been defined as SUBSONIC. How to obtain wave propagation with these settings? Regards Giovanni

 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 BalanceChen CFX 28 September 28, 2016 02:11 maryliz CFX 6 November 1, 2011 00:26 micpage18 CFX 10 January 5, 2011 06:16 park Main CFD Forum 0 September 28, 2008 01:43 adma CFX 6 February 3, 2006 12:17

All times are GMT -4. The time now is 03:37.