Hello. I work with FLUENT in some alike simulations with dynamic mesh, and I guess CFX must be pretty much the same, so maybe some of what I got might help you. I configure the dynamic mesh with mesh methods of Smoothing and Remeshing (they are probably available in CFX too), but I set the motion of the movable element through a User Defined Function, say, a C++ code interpreted and compiled inside FLUENT framework. No matter how simple the motion is, I always use the UDF option. That way the motion is always under control during the simulation. I hope that could give you some additional clue.

Thank you. I make piston move by giving displacement as a boundary condition and I given total time and time steps.

OK, that's fine. Then you might want to check the dynamic mesh methods applied into your model (smoothing, remeshing, layering, etc…).

CFX does not have any of that methods (smoothing, remeshing, layering,..)

But maybe It should allow you to program a specific routine for a given boundary…

I used ideal gas to compress the air inside the cylinder. I am getting about 75 bar but calculated value is 35 bar. Pressure value is more than the calculated value inside the cylinder. What should be done to get required pressure..?

Considering the fact that your calculations are OK, then you might want to check (I don't know it it is possible in CFX) parameters such as mole number (or gas mass inside the cylinder), working temperature and if equations for energy exchange are implemented in your model. Also some attention should be paid to the conditions in terms of system isolation, because that might affect the temperature balance, hence the final pressure achieved

Hi, dynamics meshes there 3 options, none as default, specified by means a expression through CCL  no coding) and often used,  or controlled by a  junction box routine in FORTRAN in some exceptional complex cases. 

The mesh is entire deformed. No remeshing or layering is  permitted, because at each one an interpolation must be done in the new volumes, and the flux conservation can be broken. This is the philosophy of CFX. But regarding  to smoothing there are a similiar thing: 

The displacement is limited by diffusion displacement model, div(Gamma.grad(delta))=0

gamma is the stiffness of the mesh, and delta the displacement. This will retain the mesh refinement proportional  after a displacement. Refined regions will continue refined after a displacement cycle. The same to coarse regions. Very similar to  laplace smoothing technique. 

The stiffness can be a constant value variable  through the mesh. High values  means that the nodes will have a little relative displacement, moving almost together. 

Some options can be set: Increase Near Small Volumes - which preserves  little elements and let to bigger elements to absorb almost all displacement. This is good to preserve mesh quality but depends on the initial mesh resolution, what is not always desired . Increase Near Boundaries -  which considers that the boundary elements are less susceptible to deformation than interior elements. It does not depend on the initial mesh resolution. And Value - defined as a number or a function with CCL (CFX command language) which can depend on any variable that you define and available during solution as temperature, or pressure, or force, or time...

Yo must specify  the Mesh Options, or in few words, how and which boundaries  move. Some boundaries not move other moves but there are a flux as a inlet or outlet...

Stationary - fixed, Unspecified - determined by the global setting and  neighbors elements displacement, Specified - CEL function. The components cartesian or cylindrical  and reference frame can be  provided.

There are other, but these are  the most common.

Warning: The time step must  provide a smooth displacement that does not extrapolates the  faces or edges of the element, that is, to distort and invert a element. This is a common error that results in divergence because generate negative volumes and degenerated volumes at least. 

Sorry by the longer answer. But I think will hope you to work  with your problem.

I CANT GUESS HOW ARE YOU IMPLEMENTING MESH MOTION. HAVE YOU SET ''REGIONS OF MOTION SPECIFIED '' OPTION IN DOMAIN SETUP. IT SEEMS FROM YOUR QUESTION THAT YOUR SOLID AND FLUID MESHES ARE NOT INTERACTING. YOU SHOULD MAKE A SINGLE PART OF FLUID AND SOLID REGIONS IN DESIGNMODELER AND THEN FLUID SOLID INTERFACE WILL BE CREATED AFTER WHICH YOU CAN SPECIFY DISPLACEMENT TO PISTON AND THIS MOTION OF PISTON SHOULD COMPRESS OR DEFORM FLUID MESH.