CFD Online Discussion Forums

CFD Online Discussion Forums (
-   STAR-CCM+ (
-   -   Moving piston inside cylinder (

Hope2010 November 10, 2013 03:16

Moving piston inside cylinder
Hi everyone,

Hope one of the expert help me and show me step by step how can i simulate a moving piston inside a cylinder using STAR CCM+. There is one inlet and an exit, the entering flow is oil which should push the piston.

Many thanks,


cwl November 10, 2013 16:37

While experts are away - i advice you to read about Overset Mesh; its around p. 2381 in User Guide.

Hope2010 November 11, 2013 00:14

Thanks cwl :),

Mark_89 November 11, 2013 19:05

The simulation of a moving piston in a cylinder can be very difficult in star ccm+ because the software has some problems when work with morphing mesh. However the diffiCulty is related to two variables: 1) the difficulty of the simulation is proportional to compression ratio:the higher the compression ratio, the greater the difficulty. 2)the difficulty increases also if you have to use valves movements, especially if you start from closed valves, open them and close again.
the process is:
1) you can prepare a region composed by intake valve, exhaust valve, piston crown and the other boundaries. Impose the physics (3 gradients, turbulent, constant density for your case, implicit unsteady, segregated flow ecc) and generate the mesh (basic size about 2 mm). Go to tools-motion and select morphing. One click to region and you change motion menu from stationary to morphing (you can find motion menu into physics condition folder relative to the region). Then For each mobile boundary (intake valve, exhaust valve and piston crown) go to physics condition and impose morpher-displacement. Go to tools tables and import three tables (time); each table contains the law motion of the moving boundaries (create three .csv files with 4 headers, named "column0", "column1", "column2", "time" have to insert respectively the x-y-z displacemet in metre and time in seconds). Go to each moving boundary- physics values-morpher-table (time)- specify its relative table. Remesh. Solvers-implicit unsteady-time step between 0.001 s and 0.00001 s (start from smaller time step). Run simulation.

while the simulation is running you can see that cells mesh are deforming and probably they will have negative volume. When this happens, go to representation, click to volume mesh and extract boundary surface, export surface. One right click to initial surface-replace surface with that you have just exported (choose metre m, and tick the link above between the two choices). Remesh (surface and volume). In some cases this technique is not sufficient, BUT there are other techniques to bypass the problem of the negative volume cells that i haven't explained here. For now Try this and tell me if you have need. I'm sorry for my horrible english!
G O O D L U C K :D

Hope2010 November 13, 2013 00:48

Thanks Mark :),

All times are GMT -4. The time now is 08:41.