[ghorrocks]

Hi,

It can't answer your combustion questions, it has been too long since I did that stuff to remember.

Using the cycle 1 results as a starting point for cycle 2 can be easily done using an initial guess file. What is the problem here - is there some reason this does not work for you?

I am pretty sure you can run CFX over ssh if you have to. Buried somewhere in the configuration files I remember seeing something to make CFX use ssh rather than rsh but can't remember where exactly. Have a look and try to find it.

Glenn Horrocks

[ckleanth]

Originally Posted by geothokar

In BVM model when I use a default fuel mixture I can initiate the combustion reaction with the help of spark ignition. I wonder how this is done in case of EDM. I'm using Methane Air WD1 NO PDF. (I know EDM is easier compared to BVM and is widely used for quite some time now)

I as I said I would simply use a volumetric energy source to represent ignition spark as a function of crankangle, not sure about the cluster question

[geothokar]

Hi,

I used a command in SSH, like initial=FILE_RES to edit in cfxQsub, and then I made modification in the cfxJOB to input the result file for initiating the cycle-2.

When I put it to run in the cluster the job won't even run for a step. It suddenly exits. I do not know if the way I used is specifically for inputting result file of a steady state simulation for initiating a transient simulation, or is there a different way to feed the result file of a transient simulation as the input for another transient simulation.

I tried to see if I can resolve it, but couldn't find a solution.

[geothokar]

Temperature - BVM.JPG

Pressure - BVM.JPG

Hi,

I'm attaching two pics of the result I obtained with BVM model.

First figure shows the temperature (global) plot at spark ignition point, and the second one shows the pressure plot at the same crank angle (local).

The problem I faced with BVM is: the ignition starts, but the combustion is not performed. The fluid material I used was Methane Air FLL STP NO PDF (FLL) as I mentioned in first post. The problem with the model might be an issue with the reacting material I used.

Please give your comments and suggestions about this.

[ghorrocks]

Originally Posted by geothokar

When I put it to run in the cluster the job won't even run for a step. It suddenly exits. I do not know if the way I used is specifically for inputting result file of a steady state simulation for initiating a transient simulation, or is there a different way to feed the result file of a transient simulation as the input for another transient simulation.

You need to set it up so that it does not ask for a password. If you set up rsh as described in the documentation you can login to another machine and it automatically takes the password and logs you in without askign for a password. The security implications of this are obvious and some issues are discussed in the manual - maybe if you showed the IT people the restrictions you can put on rsh (eg limit it to a single user account only) they might allow it. Otherwise you need to convince ssh to somehow automatically get a password from a config file somewhere. Good luck!

Glenn Horrocks

[geothokar]

The cluster problem seems quite complicated. I should ask the IT people to have a look into this issue and get this fixed asap.

I found that I can make use of some default fuels in CFX for combustion modeling (EDM)(for instance, Methane Air WD1 NO PDF). In the case of SI engine modeling which default fluid model will be more accurate to apply? (I think a trade-off will be needed as these are predefined models) As SI engines are premixed ignition models I think the fuel must be satisfying the conditions for premixed ignition. Which of the default available models are good for SI engine premixed combustion modeling? Is there any way to see how the chemistry and settings made for these models in CFX?

Even though the BVM model is for premixed combustion modeling the combustion tutorial in CFX uses seperate air inlets for oxidiser and fuel inlets for the fuel. Why is this?

[ckleanth]

referring to the burning velocity model have a look in the cfx manual in solver theory section.
when ansys refers to premixed combustion they mean that the global reaction process (fuel + oxidizer-> products) in the domain is modeled by a single progress variable however this doesn't not mean that we are constrained to use only one inlet with premixed fuel + oxidizer...

[geothokar]

I would like to further clarify a few doubts.

So, the fact is we can have multiple inlets, if needed, in case of premixed combustion in BVM model.

Based on the material I used for BVM model 'Methane Air FLL STP and NO PDF', do we need to have another oxidizer inlet? In my engine model I have a series of inlets which is all meant for air+fuel mixture entry. When I define the boundary I can either select fuel or oxidiser or mixture fraction. By default I chose fuel. Is that correct? I do not know how to specify mixture fraction.

In the inlet boundary I selected reaction progress as 'fresh gas'. I had another option to specify the value of reaction progress. Do I need to use the reaction progress rather than 'fresh gas'?

I have 3 domains for the entire model; an inlet, outlet, and a cylinder. When I initialized the inlet domain I set reaction progress as 0, for the outlet I chose 1, and for the cylinder domain where combustion happens I again select 0. Is that correct? I have other option to select mixture fraction and mixture fraction variance, both of them I set to automatic. Does it sounds okay?

I'm grateful for your help.

[ckleanth]

george, I have not used the flamelet libraries in my simulations therefore I cannot comment more than what I believe is accurate.

without having the model in front of me, and not knowing what the physical problem is I cannot suggest what is the "best option to use"

setting initial conditions other than t=0 is tricky as its very difficult to get proper velocity and turbulence levels to initialize the problem. my suggestion is set velocities to 0 and start everything from the start of the compression stroke

[geothokar]

Hi George,

I used to set the initial velocity values to 0, and I start simulation from compression stroke.

I used to put the reaction progress as 1 for inlet initially. I think that was a mistake which I understood when I went through the literature. I made few modifications and now running a new simulation. I'm waiting for the results now.

I'm also trying the EDM model. I tried introducing the energy source through the domain and also using source point to resemble the spark ignition. However, both didn't work for me. The simulation finished without error, but no combustion. Over the entire cycle I set the energy (10J) to be sent in for 2 crank degrees with piston position 10 degrees before TDC. (Methane Air WD1)

I used to let CFX calculate the HTC till the last simulation I did.(by specifying a fixed wall temp) This time I explicitly specified it to save computation time. I think it won't affect my results significantly.

[ckleanth]

the source point allocates the spesifed energy in one volumetric element, where as if you use a volumetric energy source to represent ignition spark you need to define by ccl an assumed sphere volume that the energy is dissipated into.

a useful ccl routine to spesify the transition of a quantiy search for "smeared volume" in the cfx manual; pehraps it will be useful to you. if still having problems let me know

I'd look again that 10J energy value if I were you.

heat transfer and cocoling through the cylinder walls is quite important, pehraps a thermal transfer coefficient and outside temp is a better assumption

[geothokar]

I can apply the energy to the default domain boundary.I hope that is what you mentioned as volumetric energy source.Could you tell me how to specify this by ccl and why it is needed to dissipate energy to a sphere volume.

Is the 10J energy value I specified seems insufficient?I specified this amount as 'total source' in default boundary.I specified the HTC values explicitly and also the outside temperature.

[ckleanth]

Originally Posted by geothokar

I hope that is what you mentioned as volumetric energy source.Could you tell me how to specify this by ccl and why it is needed to dissipate energy to a sphere volume.

Source = EnergySource
Source Coefficient = -EnergySourceCoefficient

EnergySourceCoefficient = (watt/sphere volume) [W/(m^3 K)] *SphereDispersion * step((5000. [K] - T)/1. [K])
EnergySource = EnergySourceCoefficient * (5000. [K] - T)

where with SphereDispersion is an equation that uses maths from the "smeared volume" example in the cfx manual to specify the location of the spark in the domain, the size of the spark and a "smoothing" transition relation.

the reason I use the energy source over the surce point is that with the source point you apply the energy to the nearest volumetric element in which you are never 100% sure if the said energy is added to the system where you wanted it to be. secondary with the source point you can make your simulation unstable.

why a sphere volume? an assumption that the sparking event is much faster than the fluid timescales and takes the shape of an energy sphere

Originally Posted by geothokar

Is the 10J energy value I specified seems insufficient?

http://en.wikipedia.org/wiki/Spark_plug
I dont intent to work out for you what sparking energy you should use however you'd need at least the activation energy of the fuel to initiate combustion.

Originally Posted by geothokar

I specified the HTC values explicitly and also the outside temperature.

i dont quite understand your statement - or is it a question? anyway its farly easy to to calculate a thermal conductivity and use outside wall temperature

[geothokar]

Hi George,

Thank you for replying. That was a fairly good explanation on how to perform the EDM ignition. I should try it tomorrow in the Uni cluster and I will let you know the outcomes.

About 'HTC' in my post; that was not a question. I was saying I used HTC values and wall temperature to specify the heat transfer.

[geothokar]

Hi George,

Could you advise me on what activation energy would be sensible in case of a methane-air combustion modeling? What all factors the activation energy depend on? How to find the activation energy of different fuel mixtures available in CFX?

[ckleanth]

the activation energy is used in the Arrhenius rates so either you should have all kinetics and rates in advance to setup your reaction or as in this case you can easily look at the activation energy in the particular methane oxygen reaction setup in cfx.

however...

sparking is achieved because the gas between the spark gap is ionized due to the high voltage. P=V^2/R and lets assume a spark voltage is 30 KV, unfortunately I cant tell you what resistance the air has because its a mixture of gases. you will need to assume something or find a better value. try 2 KW /volume sphere of 3 mm diameter [m^3] i might be able to suggest a value tomorrow if I dig my stuff at work.

[geothokar]

Thank you George. I'm grateful if you can help me with that.

I think it is necessary to have CFX-RIF to setup or modify or view the predefined fuel mixture characteristics (especially flamelet models), which unfortunately we do not have in Uni.

[ckleanth]

I have only values for argon and electric conductivity [S/m] which is 1/resistivity [1/ ohm/m]

forget about CFX-RIF, just put a value to start the combustion maybe a small 2d test model can help you find a good value

[geothokar]

I was trying something in BVM model over the weekend, and came across few doubts. (still reluctant to give up BVM for EDM, though trying EDM as well)

In my model I have one inlet and an exit port. Since BVM with spark ignition, only flamelet library can be used. (have no CFX-RIF) I used default Methane Air FLL STP NO PDF as fuel. Since 'inlet port' is the boundary for flow into the cylinder I have to define my mixture to flow through that boundary. The problem is, the 'mixture' option in the boundary definition let you choose any one of these: 'fuel', or 'oxidiser', or 'mixture fraction', or 'mixture fraction mean and variance'. In IC engine model we need fuel air mixture. So, if I choose 'fuel' will that be okay? Or, do I need to have another oxidiser boundary as described in combustor tutorial. (which is impossible in my case as I have only 1 input port for the model) How to make use of 'mixture fraction' option here?

Please give your suggestions to tackle this problem.

[ckleanth]

Originally Posted by geothokar

..'inlet port' is the boundary for flow into the cylinder...

besides that you need to assume a mixture of fuel and air (not that difficult thing to do really - not sure why you ask how to do it) I think you are loosing a lot of flow information and bring a lot of uncertainty to your simulation and in addition this is not physical thing to model. the only way i know of simulating ic combustion chamber is to actually model the intake/exhaust ports together with the valve and piston movements. however prior to cfx 12 versions this meant you need to manually stop and restart the simulation at various points when for instance the valve is about to close and you need to remesh.