I am trying to develop a 2d model for a piston ring blow-by case. At the moment I am concentrating on a particular steady state scenario at a certain point in the engine cycle.

I am having convergence problems and was wondering if there is any previous experience out there with this type of simulation?

Thanks in advance. James.

Need more details on physics, mesh and geometry.

Exported a 2d x-y mesh with just under 500 000 cells. I know its alot but there are some very small gaps so I thought it best to increase the number of cells.

I have modelled 1/4 of the piston so just to concentrate on ring pack area. Size is about 40mm x 30mm.

The case is taken at 10 deg ATDC so high cylinder pressure. On that basis I have fixed the rings as faces against the bottom edges of the grooves thus not allowing any flow through the back of the rings. I have therefore given the rings a specified gap between the bore and the ring to allow a flow condition.

Boundary conditions are Pressure inlet and pressure outlet inlet obviously higher than outlet and the case is initialised from all zones.

The problems seem to be in convergence, as yet I have not achieved any level of convergence. Due to the high number of cells I have been running many interations (10000+) but all variations in the case either end in failure or run without convergence. have tried changing the convergence criteria.

Solving it as steady state?

The leakage jets are probably inherently transient once they get a opertunity to expand into a quiescent region.

Post a pic of the grid near the smallest gap.

Turbulence model?

New to this forum and haven't worked out how post pictures here yet. My email addy is abracabratby@yahoo.com email me and I will reply with an image.

I initially wanted to achieve a steady state model before moving to a transient, is this not possible? I was also trying to achieve a convergence using a Laminar model before proceeding to a K-E model.

I am however still quite new to Fluent and self teaching.

Posting images http://www.cfd-online.com/Wiki/Ansys...ible_answer.3F

Thanks, Here's the entire grid.

http://img504.imageshack.us/my.php?image=griduq9.jpg

And here is a close up view around the gap between the bore and the 1st compression ring.

http://img515.imageshack.us/my.php?i...idclosegq7.jpg

You can see the mesh is very fine, maybe even too fine. Using a coupled and explicit solver with the laminar model and an Ideal gas it seems the resuiduals graph doesn't wish to converge. The current solution is at around 100000 iterations and seems to heve settled at a fairly constant graph. But the values of the residuals look too high, the strange thing here is that for the first time the results look somewhere near what I might expect, despite the residuals looking wrong.

Why are you modelling the fluid deep within the ring-recesses on the cylinder? I cant see how that fluid is going to influence blow-by? Unless you need it for some other reason e.g. thermal calcs I would suggest excluding that from the geometry.

As regards the reason for the lack of convergence, it is almost certainly related to the jet flow formed downstream of the rings suddenly expanding into a larger domain. This is particularly likely at the third ring. These jet flows will be inherently unstable physically and your fine grid will capture this instability. There is a simple way to test this in your case: Create an animation of velocity in the region shown in your second image. This animation should be updated oncer per iteration, not once per timestep. You will likely see jet instability.

Two options:

(a) If your ultimate objective is to get transient results then simply stop trying to get a ss solution and proceed to a transient analysis. If you still experience convergence issues with a well configured transient solution then the problem may lie elsewhere.

(b) If you insist on trying to get a ss solution, counter intuitively, coarsen the grid downstream of the ring jets. This will tend to force grid resolved instability into the turbulence model (which you dont use at the moment). Check the jet Re numbers first though before using a turb model. If you do use a turb model make sure you select a wall treatment compatible with your fine grid.

Thanks for the answer, it has given me some avenues to follow.

In reality the blow-by would be a transient issue influenced by factors far wider ranging than this investigation. What I am particularly interested in here is the pressure between the compression rings (ring land 2). Hence I have created a ring-bore gap (that may not exisit in reality) in order to allow a blow-by into these regions.

Modelling the cavities behind the rings shows me if I have modelled a realistic gap since the pressure in the cavity behind the first ring should be higher than that bewteen the rings (at the point in time of question). Is this an incorrect assumption?

Would introduing another outlet (such as the oil hole behind the oil scraper) reduce this jet flow after the bottom oil ring?

"Modelling the cavities behind the rings shows me if I have modelled a realistic gap since the pressure in the cavity behind the first ring should be higher than that bewteen the rings (at the point in time of question). Is this an incorrect assumption?"

It could be in a transient analysis i.e. if the pocket inside ring 1 takes a long time to pressurise. The pressure drop (when there is flow) will be dependant on the width and length of the channel. Ring 1 - Bore gap is larger and much shorter than that above ring1.

"Would introduing another outlet (such as the oil hole behind the oil scraper) reduce this jet flow after the bottom oil ring?"

No.