Combustion model - Fluid Material
 

Hi,

I'm simulating combustion in an SI engine using BVM model. I tried using the 'Methane Air FLL STP and NO PDF' as the fluid mixture for all the boundaries of my model (inlet, outlet, cylinder). This fuel mixture is used in the combustion tutorials in CFX. However, I'm not getting the results I expected, like the pressure predicted is considerably less than my mathematical model results.

Is it advisable to use the predefined fluid mixutres in similar kind of simulation?

In my mathematical model I have an air-fuel ratio. Can I employ the same thing in CFX?

Do I need to develop my own mixture to simulate the gasoline engine combustion? Which could be a better material for the fuel?

Please help me with the above queries.

What is the fuel of engine you intend to model? Is the fuel methane or gasoline?

Hi,

I wish to use gasoline as the fuel for the CFD model. I do not know how to specify reactions then, and also the air-fuel ratio that I used in mathematical model.

In the case of 'Methane Air FLL STP and NO PDF' the reactions and fuel properties were predefined, and so it was easy to implement in the model. Unfortunately no much support is available from my Uni in this area as it is kind of new work here.

Hi,

Any one having experience in modeling combustion in gasoline engines, please help regarding specifying fluid material suitable for spark ignition model.

Can I use any default 'gas phase combustion model'?

Or do I need to introduce a new material? I just want to use normal gasoline as fuel.

I have an inlet port and an exhaust port. Do I need to specify air and fuel inputs to the domain separately as done in the combustor tutorial in CFX? If so, could you advice me how to do this in my case?

for engine simulations without coupling external kinetic code (for example chemkin) you will need to use reduced species but well defined fuel mixture for example isoctane and the chemistry involved depends on how many species you want to take into account. gasoline has hundreds of species and you cant sufficiently model it without some assumptions

I have not used the flamalet library so I cant comment if you can go towards that route

the only recommendation i can say to you is to start collecting/studying papers regarding IC engine simulations and look into if you will need to couple a kinetics code in your model.

perhaps the code from convergecfd is a better solution for you as its specifically created for IC engine simulations

Thanks George,

I'm not well experienced in this area as I have started the project recently only. I'm doing this work as a part of my masters thesis. I do not have access to any software package except Ansys CFX at the moment, and the computing facility available for me is very limited. We do not have any faculty with experience in similar area in this Uni for a discussion or guidance and so I have to depend on myself.

I'm not looking for a highly accurate and full fledged combustion simulation as it is beyond the scope of a maters thesis and the work has to fit withing my time frame. However, I will definitely try some more journal articles.

As I can use only Ansys CFX now, I cannot think of developing codes in external tools and coupling it with CFX. I may have to rely on CFX itself to do my job.

I know combustion simulation is tricky, but I want to crack it. Unfortunately only one tutorial simulation is there in the CFX help regarding combustion modeling and that too not discussing BVM model which I want to use here.

Please give your suggestions on this.

glenn might be a better person to ask for his opinion to be honest; I only performed 1D engine models as a part for my phd.
my concern is how it is possible to do a thesis without a supervisor that can help you on the subject. maybe you are trying to chew more than what you can eat ? :confused:

well my problem approach would be:
forget about gasoline but concentrate on isoctane; find the chemistry involved and the kinetic rates required for cfd.
learn how to use the ignition model in cfx.
learn how to use moving meshes
start with 2d and if physics are right then go to 3d
do a cold flow analysis first - do you have any data to compare? how will you validate your results?

perhaps contacting ansys and asking them for an example is the best way for you to get started if you dont have any other source of information

Thanks George<br><br>I have already successfully implemented moving mesh and BVM combustion model with ignition regardless of my limitations.<br><br>However, the problems now I'm facing are,<br><br>I used gas phase combustion as implemented in one of the tutorial in CFX help. I do not know if that's the right way to do it. <br><br>I used Methane Air FLL STP and NO PDF as the mixture, and the result obtained from simulation gave very low pressure predictions than I obtained from mathematical model I developed. I do not know if I have to modify the default mixture available in the flamelet library.<br><br>Expecting your comments on this.<br><br><br>

can you say that you can trust the mathematical model 100% how can you tell its more accurate than the CFD model?
do you have experimental data for cross checking?

swirl in the chamber and the turbulence model can have significant impact.

why you need to use the BVM combustion model? the only way you can use this model efficiently is if you have access to cfx rif or someone with access can make the particular fuel library for you.

Hi George,

I do not have experimental data for verifying my results, and its true that I cannot assure my mathematical model is accurate.

I preferred SST turbulence model over k-eps as the latter has problem with boundary flows and flows with separations. My supervisor also suggested to go for SST model.

I do not have access to CFX RIF. We do not have the license for RIF as the version we use in Uni is the education version of Ansys and my project is not funded to buy a license. Unfortunately this area of research is not even there in the research strength of the Uni. I took this project as a challenge.

I'm respecting your comments on my issue as rarely I get chance to speak to someone who has experience in similar area. Thank you for advising me on this.

do check the part in the manual which discusses which combustion model is more appropriate in solver modeling guide>combustion modeling> using combustion models

in this instance I'd think that you will use something in terms of the combined eddy/finite rate chemistry depending on your chemical reactions

let us know how you get on

Hi,

k-e has no problems with boundary layer flows. Yes, k-e has problems with separations but so does SST. 95% of engine simulations have been done with k-e so you will need a better reason than that to change. Use k-e until you have firm evidence it is inadequate.

You may also like to have a look at my prehistoric PhD thesis. It used CFX4 to model the aerodynamics of an IC engine. No combustion modelling, just the air flows. That was more than enough for a CFD model 10 years ago. http://hdl.handle.net/2100/248

From memory (it has been a long time since I looked at combustion in IC engines) the most common approach is using eddy breakup models. These models can account for swirl and tumble which, as ckleanth says is vital for model IC engines.

Glenn Horrocks

Hi Glenn,

I have tried using k-eps model couple of times, and my simulation finished with error at times. Later I shifted to SST to give a try, and my simulation went well. So, I assumed SST has a hand over k-eps. May be that was an early judgment; I would have given more trials with k-eps. In most of the journals also I found k-eps is most widely used from a long time.

Thank you for referring your thesis. In fact I had gone through it several times (even now) and it helped me to understand IC engine modeling, especially gas flow through valves and swirl motion inside cylinder.

I would try the eddy break up models. I was clinging to BVM model since a long time as it had a spark ignition option coming with the model. May be its time for me to think about my modeling problem in a different way. I think CFX is quite rarely used for IC engine combustion modeling.

Thanks Glenn and George, for your valuable suggestions.

Hi,

Star-CD is by far the market leader in IC engine modelling. Fluent also does quite a bit and AVL's FIRE used to be common but is not so common now. Just about nobody in IC engines use CFX. Except me and ckleanth I guess.

But in recent releases of CFX, especially V12, there is lots of stuff specifically aimed at IC engine modelling. I think CFX has made a big effort to close the gap in IC engine modelling with the V12 release.

The result of this is that you should get your school to put V12 on. No point working with an out-of-date tool, you will just do months of work for no reason.

Glenn

Hi Glenn,

If you have already experienced V12,

does it have a new combustion model for handling IC engine combustion problems? (like BVM introduced in V11)

does it have more tutorials on combustion (especially on IC engines) modeling?(V11 had only 1 tutorial)

Would you recommend me to go on with BVM? Do you know if anyone tried it successfully?

I heard my Dept. is planning to buy V12, but don't know when this is going to happen. I have hardly 1 month to finish my work, and I know its not going to be a cakewalk for me.

Hi,

I have not done IC engine modelling in V12. My PhD was in CFX4 and afterwards I continued doing related IC aerodynamics work in CFX5 but never combustion modelling. So I can't really comment about the combustion models.

If you only have 1 month to model IC engine combustion and you are new to CFD then you either are a genius or have taken on an impossible task. I recommend you simplify your topic to something which will actually be possible.

Glenn Horrocks

Hi,

I have started this project in Spring '08, and so it is almost 1 year.

However, no experienced person is available in the area of CFD based IC engine modeling in my Uni for guiding me and no good computing facilities available. So I was doing self learning right from modeling engine geometry using Ansys DM, meshing using ICEM, and simulation using CFX. These works consumed my 1 year.

Once I implemented BVM model I thought its done. Now I understand it is not even the beginning!!!

As you suggested I may should think about stripping down complexities in my model to make it work in 1 month time.

I hope you have one more month for modeling and not writing up

in this instance forget isoctane, do methane or butane combustion - these reaction rates are already available in the library, if you cant use the combustion/ignition model use an energy source to represent ignition

what I'm concerned about is the data you have to compare the cfd results with. back your assumptions up and be proud of what you have achieved as cfx (especially v11) is the worst software to have in regards to required user input for IC simulations

Hi George,

I have already done some part of my writeup. To move further I need results from CFD analysis. So I can invest (I have to) some time for trying simulation in CFX.

Since I do not have experimental results I have to rely on the mathematical model results I obtained. I generated this model in spreadsheet. (I know this result may not be accurate, but for the time being I do not have anything else to compare)

I have already modeled some simulations with moving boundaries with another concept which I call domain source, where I use air ideal gas and explicitly supply energy to the domain. This model worked fine and I got results. (However, it is not combustion)

I'm planning to compare results in terms of P-V plots, T-crankangle plots, Velocity and turbulence plots. I'm not worried about combustion after-burn products and other similar complicated things.

By energy source, I assume you are referring to use source point to supply energy. I think I would try EDM or FRC now, not BVM.

Hi,

I have started shifting to EDM for combustion modeling. I have a few doubts if you could help me to clarify.

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)

Another doubt, not specific to the topic, but would like to hear your comment - I am modeling air-standard cycle as well for this particular engine model. I wish to run 2 cycles of numerical simulation instead of just 1 (I think the same is done by Glenn in his thesis). I'm running my simulation in cluster. I want to take the cycle-1 end-result as the initial assumption for cycle-2. Can anyone help me how to do this in cluster environment (do not have parallel license for CFX, SSH secure shell)

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

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

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.

BVM - Sample results
 

Attachment 725

Attachment 726

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.

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

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?

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...

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.

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

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.

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

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.

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

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.

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

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.

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?

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.

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.

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

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.

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.