Mesh deformation test
 

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 ?????

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.

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

immage of domain

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.

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

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 :)

I will do so
:D
thankyou