CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Mesh Motion (Piston valve)

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 10, 2009, 12:05
Question Mesh Motion (Piston valve)
  #1
New Member
 
Ali
Join Date: Oct 2009
Posts: 9
Rep Power: 7
AliAli is on a distinguished road
Hallo to all,

I am using CFX for simulating pressure wave propagation created by restricting flowrate by movement of piston (20 mm in 0.03 sec, linear relationship, piston speed is constant) inside pipe.The fluid water, taking into account the compressiblity by using Material group IAPWS IF97, turbulent model SST, mesh motion is specified location.

During the simulation, I do not get any error message and the piston moves also 20 mm without any negative volume. However, with smaller time step, I get unrealistic results. For example, for time step 0.01 sec, the maximum pressure rise is 0.2 bar which is corresponding maximum movement (20 mm),but for smaller time step for example (0.0005 sec or smaller), there is an unrealistic pressure increasment for the first few time step (for the first time step (0.0005 sec correspondes to 0.33 mm movement), pressure rise is 1 bar or even more with smaller time step). After 3 to 5 time steps, the pressure decreases again and then lineraly increases till 0.03 sec. Again, there is another fluctuation or oscillating in the pressure, when the piston moves back. I refined the mesh and using different turbulent models, but there was no improvement. Could someone help, any ideas or advice, thanks in advance.
AliAli is offline   Reply With Quote

Old   October 11, 2009, 06:13
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,716
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Before using IAPWS for this type of analysis I would use a simple bulk modulus approach, where density is a linear function of pressure. This gives quite good results and is much more robust than IAPWS. If you need the highest levels of accuracy then go to IAPWS but it is tricky to converge for things like pressure waves.
ghorrocks is offline   Reply With Quote

Old   October 12, 2009, 04:15
Post
  #3
New Member
 
Ali
Join Date: Oct 2009
Posts: 9
Rep Power: 7
AliAli is on a distinguished road
Hi,

I have used also linear relation for pressure, but it is still the same (no improvment).
AliAli is offline   Reply With Quote

Old   October 12, 2009, 07:16
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,716
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
What do you mean by "linear relation for pressure"?

I have done compression of hydraulic fluid in a high speed, high pressure system and successfully captured the acoustic waves using a bulk modulus approach. It even matched experimental results pretty well so I know I was on the right track - so it can be done.

Make sure you have a fine enough time step to resolve everything and second order time differencing helps (but second order time differencing is not generally a good idea if you are using a moving mesh model, stick with first order - or maybe this has been fixed in V12, not sure).
ghorrocks is offline   Reply With Quote

Old   October 12, 2009, 07:39
Post
  #5
New Member
 
Ali
Join Date: Oct 2009
Posts: 9
Rep Power: 7
AliAli is on a distinguished road
Hi,

Thanks. Linear relation between density of water and pressure, I took it from book, may be it is the reason why I am getting such unrealistic or oscillating in the results. Regarding the time step, and mesh refinement, I think that they are good, however, I could refine it more. Mesh size is 0.2 mm close to the piston and increases linearly to 20 mm far a way from the piston in the pipe.The pressure in the pipe is about 2 bar and velocity is almost 2 m/s inside the pipe.
Could please explain it or send me this bulk modulus approach equation?Thanks in advance
AliAli is offline   Reply With Quote

Old   October 12, 2009, 08:01
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,716
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
http://en.wikipedia.org/wiki/Bulk_modulus

Just read your initial post again. Did you say you used a time step of 0.01s? Then that is your problem, your time step is WAY too big. Reduce it such that you get 3-5 iterations per time step. Also don't forget that acoustic waves in water have a velocity of something like 1500m/s so base your time scales on this velocity, not the flow velocities.
ghorrocks is offline   Reply With Quote

Old   October 12, 2009, 08:33
Post
  #7
New Member
 
Ali
Join Date: Oct 2009
Posts: 9
Rep Power: 7
AliAli is on a distinguished road
Hi,

Well, with time step 0.01 sec (which is big), I got some how good results, but I am interested in using smaller time step (0.0005 sec or smaller) to see the wave and how it moves inside the pipe to reach other side. With smaller time step, I am getting this oscillating problem. Any how, I will use also smaller time step with the bulk modulus approach. One more question please, shall I define the densiyt as (let say) a function of bulk modulus and local speed of sound in the expression and then used it in the material properties? Shall I also use constant bulk modulus for water?

I got a problem in expression, that Local speed of sound is unavailabe variable. could you please tell me how do you define it in the expression in CFX?

Thanks in advance

Last edited by AliAli; October 12, 2009 at 10:41.
AliAli is offline   Reply With Quote

Old   October 12, 2009, 19:02
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,716
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
So what time step are you using? How many coefficient loops per time step does this end up with? Have you done a sensitivity analysis on your convergence critereon and time step size?
ghorrocks is offline   Reply With Quote

Old   October 13, 2009, 06:40
Post
  #9
New Member
 
Ali
Join Date: Oct 2009
Posts: 9
Rep Power: 7
AliAli is on a distinguished road
Hi,

The time step that I use is 0.0005 sec (also 0.0001 sec). For the first few time step, when the mesh movement starts, it takes about 20 iteration to get converged. After that it will take 4-5 iteration, although, the mesh is still moving.

Could you please tell me how did you define the bulk modulus approach in CFX? Is that right, I used bulk modulus as a function of pressure (table below), then I used an expression for calculating densiyt as a function of bulk modulus and constant speed of sound (1500 m/s)? or?? Table: bulk modulus versus pressure at 68 F degree

Pressure (Psi) Bulk modulus (Psi)
.................. ........................
15 ------------320,000
1,500 -------- 330,000
4,500 ---------348,000
15,000 --------410,000

But, from the slover, i saw the speed of sound is equal to (578) in the average scale information, that is not true. Could you please tell me whether you have also defined the bulk modulus approach also like this or in another way??? Thanks in advance.




Last edited by AliAli; October 15, 2009 at 03:56.
AliAli is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Define mesh motion in cylindrical CS rikio CFX 0 June 3, 2009 23:21
valve motion skarp CFX 2 April 29, 2008 19:51
Oscillatory mesh motion setup mesh flux ERROR jaswi OpenFOAM Running, Solving & CFD 5 August 23, 2007 05:41
Automatic Mesh Motion solver michele OpenFOAM Running, Solving & CFD 10 September 26, 2005 09:21
about preview mesh motion lingo FLUENT 1 July 8, 2004 13:13


All times are GMT -4. The time now is 01:55.