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

Sloshing simulation using ansys cfx vof method

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 26, 2018, 09:01
Default Sloshing simulation using ansys cfx vof method
  #1
Member
 
Aashi
Join Date: Dec 2018
Posts: 40
Rep Power: 3
Aashi171185 is on a distinguished road
hello everyone i am doing sloshing simulation of ground supported tanks using ansys cfx which is 80 % filled with water but i came across pressure values of min -8172 pa and max 1891 pa and when i import pressure values to calculate stresses on the tank shell it only shows stress on the top head which is not right plz help me out my ref pressure is 1 atm and tank geometry is 1m dia and 1 m height
Aashi171185 is offline   Reply With Quote

Old   December 27, 2018, 05:24
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,050
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

Why do you think the pressures you report are wrong?

Your other comments suggest you are not doing the FSI correctly. Have you done the tutorial examples to see how FSI simulations are performed?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   December 27, 2018, 07:22
Unhappy Sloshing result comparison
  #3
Member
 
Aashi
Join Date: Dec 2018
Posts: 40
Rep Power: 3
Aashi171185 is on a distinguished road
Thanks for reply sir yes i have done FSI simulations both one way and two way actually i have performed the simulation couple of weeks back with the tank of same geometry which is half filled and i have got pressure values min -3.03 pa and maximum value 5482.7 pa and when the pressure is imported using one way coupling it shows stresses on the wall i.e. where the water is impacting against the wall which seems to be reasonable but when i perform the same analysis using exactly same settings in cfx ansys v 19.2 the results changes drastically with min -4447.o3 and max 1103.27 and resulting in stresses on the top of roof not showing any stress where the water is impacting (at the side wall) it creates kind of vacuum near top roof resulting in inward and outward movement of roof top
sir thats why i am saying my results are going wrong please sir help me out as every setting is same but results are very different is it bug or something going wrong in cfx solver or software issues???
Aashi171185 is offline   Reply With Quote

Old   December 27, 2018, 18:21
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,050
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Check the geometry of the CFD and FEA models match up properly. Have a look at the diagnostics in the output file and ANSYS file to check that the surface pressure is mapped across properly.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   January 1, 2019, 14:42
Unhappy Sloshing results seems to be inverted
  #5
Member
 
Aashi
Join Date: Dec 2018
Posts: 40
Rep Power: 3
Aashi171185 is on a distinguished road
sir i have tried every thing and checked about my model both in cfd and fea thay are one and the same but my results seems to be inverted i have done it last night with same settings and results are correct that it shows pressure in right areas and corresponding stresses but when i done it again it shows inverted results sir can you please guide me about this phenomenon is it software fault or and malware?
Aashi171185 is offline   Reply With Quote

Old   January 2, 2019, 06:31
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,050
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
CFX and ANSYS are professional level software, written by experts and tested extensively. It is unlikely you have found a bug in basic functions like what you are doing.

Look in the CFX and ANSYS output text files for information about the FSI coupling. There is also debug levels to have a look at for more information.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   January 2, 2019, 14:56
Unhappy
  #7
Member
 
Aashi
Join Date: Dec 2018
Posts: 40
Rep Power: 3
Aashi171185 is on a distinguished road
thanks sir for your kind concern sir can you please guide me that is it possible to have negative pressures like -8760 [pa] during sloshing problem where as 1800 [pa] is max pressure in the fluid domain it think where the fluid slammed the wall pressure should be more profound over there instead it shows differently where it slams 1800[pa] and where air is present it is -8760[pa] which is not justified
sir please help me out i need your guidance
Aashi171185 is offline   Reply With Quote

Old   January 2, 2019, 15:23
Default Sloshing result comparison
  #8
Member
 
Aashi
Join Date: Dec 2018
Posts: 40
Rep Power: 3
Aashi171185 is on a distinguished road
sir i have done analysis recently with exactly same settings i.e. 80 percent filled tank and i came across different results i have done these one after another on the same day after proper shutdown of my laptop so that ram may not override previous results sir please look at them and guide me what is happening with the pressures
the pressure values in the cfx correct.png are seems to be right and shows corresponding stresses on the wall whereas cfx wrong.png shows negative pressures and shows corresponding stress on the roof of tank which is wrong please sir help me out i m very upset with these variations of results from the same settings
Attached Images
File Type: png CFX correct.png (62.9 KB, 15 views)
File Type: png CFX wrong.png (65.6 KB, 16 views)
Aashi171185 is offline   Reply With Quote

Old   January 2, 2019, 23:20
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,050
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Please upload your output file.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   January 3, 2019, 06:18
Default Sloshing result comparison
  #10
Member
 
Aashi
Join Date: Dec 2018
Posts: 40
Rep Power: 3
Aashi171185 is on a distinguished road
sir the output files are attached here with the only difference between them is analysis time correct one run for 6 sec whereas output file with poor results run for 3 sec remaining setting is same sir please guide me i need your help thanks in advance

Last edited by Aashi171185; January 3, 2019 at 13:14.
Aashi171185 is offline   Reply With Quote

Old   January 3, 2019, 06:38
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,050
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Don't worry about comparing these simulations. There are many fundamental errors in your setup which will make the results grossly in error, so comparing results with gross errors is meaningless.

The errors are (most important first):
* You have the time step at 0.1s. Have you checked that this is correct using a sensitivity analysis? While you are at it, check your mesh and convergence tolerance as well. These are basic checks which should be done for all simulations.
* You are generating the horizontal motion by putting an X component in the gravity vector. This is an approximation of the correct motion which is to define the displacement of the body and use a moving mesh. So you are using a simplification which may or may not be applicable in your case.
* You have the surface tension model turned on. This is a VERY expensive model to use properly and will enormously slow your simulation down. So unless surface tension is important turn this option off.
* You do not appear to be using the hydrostatic pressure correctly in your initial condition. In models with a gravity vector defined the variable p (pressure) includes the hydrostatic component. You do not need to add it.
* You have the viscous work option turned on. Unless it is needed, turn it off.
* Why is this a total energy simulation? What heat transfer occurs? If no significant heat transfer then turn the total energy option off.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   January 3, 2019, 07:06
Default Sloshing result comparison
  #12
Member
 
Aashi
Join Date: Dec 2018
Posts: 40
Rep Power: 3
Aashi171185 is on a distinguished road
Thanks for your kind concerned Sir i will follow your instructions and then let you know thank you very much
Aashi171185 is offline   Reply With Quote

Old   January 4, 2019, 08:36
Default Sloshing results
  #13
Member
 
Aashi
Join Date: Dec 2018
Posts: 40
Rep Power: 3
Aashi171185 is on a distinguished road
Hello sir first of all i would like to thank you for such a good response from your side sir i have done the analysis as per your directions by.
* Improving mesh size
* Remove hydro pressure term from expression as you guided me by defining g in gravity vector there is no need to enter the hydro
term in expression.
* Exclude the heat transfer and viscous work term
* Exclude the surface tension model
but my results still doing in the same way as before as i attached the snap of pressure results showing the same results
now the tank is 50 percent filled and acted upon by acceleration of 3 m/s^2
sir i dont understand what is going on please help me i need your help and kindness.
Attached Images
File Type: png CFX.png (62.5 KB, 7 views)
Aashi171185 is offline   Reply With Quote

Old   January 4, 2019, 09:20
Default Sloshing results
  #14
Member
 
Aashi
Join Date: Dec 2018
Posts: 40
Rep Power: 3
Aashi171185 is on a distinguished road
sir i also attached the output file please guide me. i'll be thankful to you Sir
Attached Files
File Type: zip file.zip (23.8 KB, 0 views)
Aashi171185 is offline   Reply With Quote

Old   January 5, 2019, 06:27
Default
  #15
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,050
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
You have made no comment about the two most important points - have you done a sensitivity check on your time step size, and what about the fact you are using a major simplification of the true motion by making the gravity vector move rather than displacing the tank.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   January 5, 2019, 16:06
Default Sloshing result comparison
  #16
Member
 
Aashi
Join Date: Dec 2018
Posts: 40
Rep Power: 3
Aashi171185 is on a distinguished road
actually sir i dont know the difference between defining acceleration in gravity vector instead of converting it into displacement. can you please provide some theoretical reference to understand what you have mentioned. and secondly sir how can i check sensitivity on time step. thank you so much sir for guiding me and responding to this thread Thank you sir
Aashi171185 is offline   Reply With Quote

Old   January 5, 2019, 18:06
Default
  #17
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,050
Rep Power: 123
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Moving gravity vector: Do a simulation which compares moving the acceleration vector as you have done to moving the vessel horizontally with moving mesh. Then you can see if the results are comparable.

Time step size: Do a simulation with half the time step size and compare results to your current simulation. If they are the same to within a tolerance you are happy with then your time step size is OK. If there is a significant difference then you need to keep halving the time step size until the results do converge. The same principle should be applied to convergence criteria and mesh size.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   January 5, 2019, 20:45
Default Thanks sir
  #18
Member
 
Aashi
Join Date: Dec 2018
Posts: 40
Rep Power: 3
Aashi171185 is on a distinguished road
can you please reply to my other thread titled "sloshing pressure level settings"
ok sir i will perform whatever you said THannnnks
Aashi171185 is offline   Reply With Quote

Reply

Tags
cfx

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
Ansys cfx multi-field simulation Ahmed osman CFX 0 February 12, 2018 10:22
Ansys SIG$ILL error loth ANSYS 3 December 24, 2015 06:31
Verifying results for a wind turbine blade simulation in ANSYS CFX Joystix CFX 3 April 27, 2012 18:52
2D Simulation ANSYS CFX antonello CFX 2 December 20, 2007 04:12
Exporting results from CFX to ANSYS ?? sohail ahmed CFX 1 December 20, 2007 02:10


All times are GMT -4. The time now is 19:05.