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

Mesh deformation test

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 3, 2013, 13:02
Unhappy Mesh deformation test
  #1
Member
 
Marco
Join Date: Jul 2013
Location: Italy
Posts: 36
Rep Power: 4
bertozzi_marco is on a distinguished road
Hallo Everybody
I'm trying to do a silmple simulation of a compression camber, follow the
description of the model:
Geometry: simple cylinder
CFX pre: air ideal gas
in the domain turn on region of motion specified
one of the two face of the cylinder has mesh motion, specified displacement with cos function
the cylindric surface of the bonduary has mesh motion unspecified
transien analisys

When I see the results of the solutions I can see clearly the defomation of the cilinder mesh but if I try to plot the pressure contour there are no variation......

can anyone help me to understand why the pressune doesn't vary ?????
bertozzi_marco is offline   Reply With Quote

Old   August 4, 2013, 07:14
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,959
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I have done this type of analysis many times and accurately reproduced adiabatic compression of an ideal gas. I regard this as an important benchmark simulation to complete accurately before doing compressible gas/moving mesh simulations.

Can you post your CCL and an image of your domain? There is going to be an error with it, this type of simulation is straight forward to set up and run.
ghorrocks is offline   Reply With Quote

Old   August 4, 2013, 07:38
Default
  #3
Member
 
Marco
Join Date: Jul 2013
Location: Italy
Posts: 36
Rep Power: 4
bertozzi_marco is on a distinguished road
thank you for your help,
you will find 2 files .ccl

motore.ccl
motrore_ideal_gas.ccl

the file motore.ccl obtain the solution but the fluid is constant density so
has no meaning,
the second file use air ideal gas but the solution get an error

thanks again for your help
Attached Files
File Type: zip _Ansys_14.zip (6.9 KB, 8 views)
bertozzi_marco is offline   Reply With Quote

Old   August 4, 2013, 07:42
Default
  #4
Member
 
Marco
Join Date: Jul 2013
Location: Italy
Posts: 36
Rep Power: 4
bertozzi_marco is on a distinguished road
immage of domain
Attached Images
File Type: jpg untitled.jpg (93.7 KB, 11 views)
bertozzi_marco is offline   Reply With Quote

Old   August 4, 2013, 07:54
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,959
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You have the heat transfer model set to "Isothermal". This makes the fluid incompressible. You want this to be "Total Energy" to model an compressible fluid. Also your fluid is "Air at 25C" this fluid does not have density as a function of pressure or temperature. This will need to be "Air ideal gas".

A minor point: I would remove the mesh stiffness parameter. You should not need it here.

Don't forget the sin function generating your motion is in radians. So your time steps of 0.1s are far too big. I recommend using adaptive time steps homing in on 3-5 coeff loops per iteration.
ghorrocks is offline   Reply With Quote

Old   August 4, 2013, 08:28
Default
  #6
Member
 
Marco
Join Date: Jul 2013
Location: Italy
Posts: 36
Rep Power: 4
bertozzi_marco is on a distinguished road
Hallo Ghorrocks

Now it's work perfect thankyou, but I've a question:
the times step of 0.1 make the domain move of one millimiter per step.
Why this condition is too big ?
Using adaptive as your advice, make the solution working but the domain move
very little so I need to run a lot of time steps.
Is there the possibility to make the time steps bigger ???

thankyou
bertozzi_marco is offline   Reply With Quote

Old   August 4, 2013, 08:47
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,959
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Rather than asking why is 0.1s time step too big, why not ask what time step size do I need to run to get an accurate solution? So I suggest you run some trial simulations with different time step sizes and see what happens when you compare against a nice benchmark like adiabatic compression of an ideal gas.

Then you will see for yourself why I recommend the adaptive time stepping method
ghorrocks is offline   Reply With Quote

Old   August 4, 2013, 08:53
Default
  #8
Member
 
Marco
Join Date: Jul 2013
Location: Italy
Posts: 36
Rep Power: 4
bertozzi_marco is on a distinguished road
I will do so

thankyou
bertozzi_marco is offline   Reply With Quote

Reply

Tags
cfx, compression, mesh deformation

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
how to set periodic boundary conditions Ganesh FLUENT 13 January 22, 2014 05:11
CFX interpolating to a mesh with deformation martindg CFX 5 October 17, 2012 05:52
mesh deformation - mesh stiffness alfonsojurado CFX 6 October 2, 2012 07:15
Mesh deformation, negative volume! Turbomachine CFX 12 June 9, 2011 08:05
Convergence moving mesh lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 15:09


All times are GMT -4. The time now is 21:24.