I am trying to simulate flow in reciprocating internal combustion engines using a CFD package. This involves complete cycle analysis i.e air intake, fluid compression, gas phase combustion and expansion. I am right now struck in the initial phase of the problem. The problem is as follows - how should the valve motion simulated? (the valve motion being time dependent)- when the valve is completely/partially open there are grid cells present in the passage between valve seat and valve head, but as the valve approches to close all the grid cells merge. Can some condition be imposed? I have seen many publications on IC engines simulation, but it doesn't discuss any of these issues. Can someone provide me suggestion in this regard? Also can somebody worked on similar kind of problem earlier give me overall guidance ?

(1). When the valve is closed, there is no flow through the intake port ( or exhaust port), you don't need to mesh that region. (you don't have a gap at all).(2). When the valve is open, there is a gap there. Naturally, you have to put some mesh points there through the inlet port to let the mixture in. So, at time=t_valve_open + dt, your mesh will be different from the mesh used for the valve closed condition. (3). That is the nature of the moving mesh (changing boundary conditions). (4). One way you can do is to use the topology the open valve mesh, and squeez it to a very small gap to simulate the valve closed position.

Thanks for the message. Can you elaborate on the different kinds of combustion and fluid flow dynamics models available and which would be appropriate for different kinds of problems. Also which due you feel is the right one for IC engine kind of work. Thanks once again.

(1). I think the turbulent reacting flow modeling can be studied in a simple environment. In this way, a systematic approach can be used to validate the model. It doesn't have to be studied in the complex unsteady, moving boundary IC environment in the first place because this can only complicate the modeling process. (2). So the non-reacting flow should be the only goal in the use of the moving grid to resolve the fluid dynamic part of the problem, such as the flow through the valve at different crank angle positions, the effect due to the mass flow rate on the flow separation behavior through the valve, the control of the inlet manifold flow to achieve the desirable flow behavior in the cylinder, the valve open duration and its effect on the low rpm and high rpm flow field and mass flow, the control of swirl and tumble in the cylinder through inlet port design,...etc... (3). In other words, these must be resolved before the effect of combustion is included to avoid the unnessary complications. (4). Unfortunately, for those who are focused on the chemistry of the reacting flow, sometimes the reacting flow modeling has a higher priority in order to justify the study. (5). In this case, the handling of the moving mesh has to be accurately resolved first. Otherwise, the solution accuracy will be questionable because of poor handling of the mesh. The 3-D moving mesh problem is not a simple one. (6). After this is under the control, un-steady turbulent flow modeling will be the next one. This one is very tough because you are dealing with 3-D transient turbulent flow modeling with flow separation. The most complex fluid dynamic problem you can have. (7). Beyond that, the combustion modeling in the turbulent flow will be the next item. The effect of mixing, turbulence will be important factors there, in addition to the chemistry of combustion. (8). It can become easily a life time career. So, the most practical way to study is to isolate the coupling and make it a sequence of simpler problems. In this way, you will be able to learn how to control some of the geometric and fluid dynamic parameters to improve the design. (otherwise, at the end, all you can say is you have used a code to run IC engine simulation.)

Thanks a lot for your valuable advice. In fact my approach would be on similar lines. Can you suggest me some publications/books which would make me more familiar with the modelling work. I am asking this b'coz I shall be using a commercial cfx package for my work. It is more like a black box, i need to understand the working methodology prior to using this s/w.

(1). I think, there were some discussions posted here sometimes ago about the modeling of flow through inlet valve into the cylinder, and even the use of commercial codes and accuracy issues (2). It is a rather specialized field, but I am sure that you can find some conference papers in this area. I don't have any at hand right now.

Dear all,

I would like to contribute with some thoughts to the question raised by Mr. GSridhar. I use the finite element method to model biological structures in the human cardiovascular system. One problem I am facing right now concerns the modelling of the dynamics of the heart valves. For this type of problem one has the same type of difficulties described by Mr. GSridhar, which is the change of topology of the domain along its evolution. That change does not allow the moving domain (and therefore the mesh) to be continuously deformed during the closing and opening of the valves. In the case when the solid part of the structure is considered as made up of (possibly moving)rigid bodies, there is the alternative of using the fictitious domain method (e.g., Glowinski and colaborators). Finite volume or finite differences methods can also be applied to such strategy (e.g. Peskin and others). Simply speaking, it consists of modelling the solid and fluid domains as one domain where the cfd equations will be defined. Then, the modelling of the solid part is done separately with the equations for its evolution defined accordingly. In order to couple the two models, a restriction is defined to enforce the velocity of the fluid part to be equal to that of the solid part where the two domains overlap. Such restriction produces a Lagrange multiplier on the solid domain which is incorporated in the cfd equations.

However, care must be taken when the fluid is incompressible and the solid is not or when the fluid is compressible and the solid is not. In these cases modifications should be provided...

I hope I could help with something...

Best regards,

Felix C. G. Santos _____________________________________________ Computational Mechanics Group - CTG/UFPE Federal University of Pernambuco Brazil

Posted By: GSridhar <gsridhar@cgpl.iisc.ernet.in> Mon, 26 Jul 1999, 12:09 a.m.

I am trying to simulate flow in reciprocating internal combustion engines using a CFD package. This involves complete cycle analysis i.e air intake, fluid compression, gas phase combustion and expansion. I am right now struck in the initial phase of the problem. The problem is as follows - how should the valve motion simulated? (the valve motion being time dependent)- when the valve is completely/partially open there are grid cells present in the passage between valve seat and valve head, but as the valve approches to close all the grid cells merge. Can some condition be imposed? I have seen many publications on IC engines simulation, but it doesn't discuss any of these issues. Can someone provide me suggestion in this regard? Also can somebody worked on similar kind of problem earlier give me overall guidance ?

You may interested in taking a look at STAR-CD (www.cd.co.uk), which is widely used for in-cylinder transient analyses. For transient simulations, STAR-CD is capable of nodal movement, dynamic cell addition/removal, arbitrary sliding interfaces, and dynamic attachment/detachment. This allows deletion of the cell layers in the valve curtain when closing and a full flow shutoff through the dynamic detachment when the valve is fully closed. Likewise, cell layers can be added when desired during the valve opening. Hope this helps.

thorny problem! some fellas at INRIA (in france) solved this problem. they have an animation on one of their webpage of a cylinder with opening and closing valves. they used and upwind scheme and a multiblock mesh. portions of the mesh deform and others don't (the displaced volume deforms, the head and the squish areaas don't, and the valve area deforms). i guess you could inquire to them. unless your canned code has this kind of ability you may have a hard time, as it'll be difficult to construct a good single block deforming mesh for this problem. their problem was 2-d i think

STAR-CD does this problem automatically through use of a Pre-Processor termed Pro-Ice.

To all people responding to the original questions, I would be more than happy to mail you a documentation on this package.

As far a guidance on this problem: The transient in-cylinder problem involving valve and piston motion is not trivial. You need to convince yourself your mesh motion is accurate, you have included the correct combustion setup (i.e. active scalars) and that your spatial introduction of the fuel makes sense (i.e. port or cylinder injection). Also, many time leakage is important in predictiing peal pressure and temperatures.

Good luck in your work!