CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   Siemens (https://www.cfd-online.com/Forums/siemens/)
-   -   EBU eddy break up unpremixed combustion for diesel (https://www.cfd-online.com/Forums/siemens/64105-ebu-eddy-break-up-unpremixed-combustion-diesel.html)

hkoten April 29, 2009 07:29

EBU eddy break up unpremixed combustion for diesel
 
hi
how do you use ebu for unpremixed model,
did you close cfm or ecfm models in esice
hkoten@hotmail.com

hkoten April 29, 2009 07:42

who use EBU combustion models for unpremixed....

Pauli April 29, 2009 11:18

You can use EBU for un-premixed diesel combustion. You do not need es-ice.

Define the reaction, define the ignition, define the spray, initialize the scalars & you should be done.

If it doesn't work, read the methodology and user manuals. Then post specific questions & details regarding what went wrong.

hkoten April 29, 2009 11:26

thank you pauli
I am studying in-cylinder diesel combustion modeling
I meshed in esice,
in prostar start of inj. 700CA end of inj 735CA
and ignation in 705CA,

but temperatures arent increasing~1000K

sthamit September 1, 2010 15:47

Pro-Star: Shell Modeling
 
Quote:

Originally Posted by Pauli (Post 214652)
You can use EBU for un-premixed diesel combustion. You do not need es-ice.

Define the reaction, define the ignition, define the spray, initialize the scalars & you should be done.

If it doesn't work, read the methodology and user manuals. Then post specific questions & details regarding what went wrong.


Hi, I have been trying so many different reaction models but all of them have failed. How do you know that un-premixed combustion with EBU standard is the best model for diesel combustion? Could you tell me what's the best combination reaction model and type for Diesel combustion simulation in Pro-Star?

Thank you in advance.

Amit

Pauli September 1, 2010 17:55

I never claimed EBU was the best model. ECFM-3Z should be superior. Flamelet models should be superior.

What do you mean by failed? Did it not "burn"? Or do you not match a measured pressure trace?

sthamit September 1, 2010 22:06

Quote:

Originally Posted by Pauli (Post 273659)
I never claimed EBU was the best model. ECFM-3Z should be superior. Flamelet models should be superior.

What do you mean by failed? Did it not "burn"? Or do you not match a measured pressure trace?

Hi. I am not saying that you are claiming. I am asking basically. First of all EBU and ECFM-3Z are two different things. ECFM-3Z is the combustion model that best suits the diesel combustion whereas EBU is a reaction type. I have been trying different combinations under ECFM-3Z like partially premixed scheme or unpremixed scheme with EBU standard and other options but all of them ended up with almost zero Ignition delay. this is what failed mean...meaning....failing to match the results with empirical ones.

If you have more idea about it, could you please help.

Thanks

Pauli September 3, 2010 11:20

What ignition model are you using? Have you tried to vary any of the parameters?

I was using EBU-LATC with 4-step ignition. I was able to make ignition delay & pre-mix phase vary significantly by changing the various parameters.

sthamit September 3, 2010 12:40

Quote:

Originally Posted by Pauli (Post 273925)
What ignition model are you using? Have you tried to vary any of the parameters?

I was using EBU-LATC with 4-step ignition. I was able to make ignition delay & pre-mix phase vary significantly by changing the various parameters.


Hi,

Until now, I have used Premixed with CFM, Unpremixed and Partially Premixed schemes with EBU STANDARD, LATCT and Modwall. Unpremixed and Partially Premixed seem to have no Ignition Delay. Premixed with CFM is mainly meant for HCCI and SI combustion. I really have to try something new now. What reaction scheme did you use?

Thanks

Pauli September 3, 2010 13:48

I am using Turbulent Unpremixed/Diffusion, EBU-LATC & 4-Step Auto-Ignition.

Are you trying to model a diesel engine? If so, why are you using unpremixed or partially premixed? That makes no sense.

How are you defining ignition delay? I compare start of injection to initial rise in the heat release rate curve. With that definition I have 3-4 degrees delay in both my test data & simulation.

sthamit September 3, 2010 14:14

Quote:

Originally Posted by Pauli (Post 273942)
I am using Turbulent Unpremixed/Diffusion, EBU-LATC & 4-Step Auto-Ignition.

Are you trying to model a diesel engine? If so, why are you using unpremixed or partially premixed? That makes no sense.

How are you defining ignition delay? I compare start of injection to initial rise in the heat release rate curve. With that definition I have 3-4 degrees delay in both my test data & simulation.


Hi Pauli,

Partially Premixed doesn't make sense to me either. I was just trying to see what happens when I use that option. Other than that, Unpremixed is the one that I think I should be using either with Modwall or LATCT reaction type because of the one chemical reaction requirement of the 4-step Auto Ignition Model.

Now coming to defining Ignition Delay, the way you are doing is what even I or anybody would do. i.e. by counting the no. of CAD for ID for any given fuel in the RHR graph of the real test and putting that value on 4-step autoignition model to imitate the nature of the graph or ignition. But the problem arises when you would like to simulate a new fuel with new CN that has not gone through experimental test.

What I meant to say here is, I want to simulate a diesel combustion with fuel of known CN in Pro-star and come up with results that match the actual experimental test data. Is it something possible to do with Pro-star you think?

Thanks

sthamit September 3, 2010 16:02

Quote:

Originally Posted by sthamit (Post 273944)
Hi Pauli,

Partially Premixed doesn't make sense to me either. I was just trying to see what happens when I use that option. Other than that, Unpremixed is the one that I think I should be using either with Modwall or LATCT reaction type because of the one chemical reaction requirement of the 4-step Auto Ignition Model.

Now coming to defining Ignition Delay, the way you are doing is what even I or anybody would do. i.e. by counting the no. of CAD for ID for any given fuel in the RHR graph of the real test and putting that value on 4-step autoignition model to imitate the nature of the graph or ignition. But the problem arises when you would like to simulate a new fuel with new CN that has not gone through experimental test.

What I meant to say here is, I want to simulate a diesel combustion with fuel of known CN in Pro-star and come up with results that match the actual experimental test data. Is it something possible to do with Pro-star you think?

Thanks


Also, what do you do with Tgradient and Start and End time? How do you setup Ignition Delay on 4-step Auto Ignition?

Pauli September 3, 2010 19:23

Calibrating a combustion simulation involves tuning the spray, combustion and ignition sub-models. It's all coupled and very non-linear. So until you've seen your model predict well over a range of conditions, you can not be sure about just how well its calibrated. (You could have gotten lucky!)

The end results is that if you take test data with two different CN fuels, you might not see similar changes in your CFD results. My feeling is that It depends on how well your original calibration was. In other words, your spray model may have been off & you inadvertantly compensated with some combustion or ignition parameter. What changed in the fuel to give it a different CN? Did that also change something which would impact the spray characteristics? If so, then you'll need to update your spray model tuning.

sthamit September 3, 2010 21:30

Quote:

Originally Posted by Pauli (Post 273967)
Calibrating a combustion simulation involves tuning the spray, combustion and ignition sub-models. It's all coupled and very non-linear. So until you've seen your model predict well over a range of conditions, you can not be sure about just how well its calibrated. (You could have gotten lucky!)

The end results is that if you take test data with two different CN fuels, you might not see similar changes in your CFD results. My feeling is that It depends on how well your original calibration was. In other words, your spray model may have been off & you inadvertantly compensated with some combustion or ignition parameter. What changed in the fuel to give it a different CN? Did that also change something which would impact the spray characteristics? If so, then you'll need to update your spray model tuning.


Thanks Pauli,

It feels really great to share info when I come across somebody who is equally interested in the subject matter as I do.

What you are saying is right as spray modeling does play a very important role in combustion modeling. This afternoon I was trying to use 4-step auto ignition but I got confused with how to adjust the start and end time of ignition in terms of crank angle degrees as the option I see is in terms of time only. Could you guide me a bit please? Also, what ignition temperature/sec should I use? About spray modeling I will let you know what I have so that you will have an idea as well.

Thanks

sthamit September 7, 2010 12:46

Quote:

Originally Posted by Pauli (Post 273967)
Calibrating a combustion simulation involves tuning the spray, combustion and ignition sub-models. It's all coupled and very non-linear. So until you've seen your model predict well over a range of conditions, you can not be sure about just how well its calibrated. (You could have gotten lucky!)

The end results is that if you take test data with two different CN fuels, you might not see similar changes in your CFD results. My feeling is that It depends on how well your original calibration was. In other words, your spray model may have been off & you inadvertantly compensated with some combustion or ignition parameter. What changed in the fuel to give it a different CN? Did that also change something which would impact the spray characteristics? If so, then you'll need to update your spray model tuning.

Hi,

Although I have been trying, I still don't have an idea on how to set Tgradient in 4-step Shell Autoignition. Also, how to set start and end time of the ignition in terms of crank angle degrees rather than in seconds.

I would appreciate your help.

Thanks in advance

sthamit September 7, 2010 14:08

Quote:

Originally Posted by Pauli (Post 273942)
I am using Turbulent Unpremixed/Diffusion, EBU-LATC & 4-Step Auto-Ignition.

Are you trying to model a diesel engine? If so, why are you using unpremixed or partially premixed? That makes no sense.

How are you defining ignition delay? I compare start of injection to initial rise in the heat release rate curve. With that definition I have 3-4 degrees delay in both my test data & simulation.


Hey Pauli,

If I am modeling a diesel engine, what should I use? Premixed or Unpremixed or what?

Please help. Thanks

Pauli September 8, 2010 11:12

To enter values in crank angle, you need to tell prostar to use crank angle. That is done with the trelation command. Or in the Nav Center, it is under the first entry: Select Analysis Features -> Time Relationships. Note: The time relationships sub-panel is not active until you switch to transient mode.

Diesel engine is unpremixed.

sthamit September 8, 2010 12:47

Quote:

Originally Posted by Pauli (Post 274469)
To enter values in crank angle, you need to tell prostar to use crank angle. That is done with the trelation command. Or in the Nav Center, it is under the first entry: Select Analysis Features -> Time Relationships. Note: The time relationships sub-panel is not active until you switch to transient mode.

Diesel engine is unpremixed.


Thank you very much man.
In my case, I have been using time relationship in angle with transient mode fortunately but the problem is it is not firing.
Okay, if I am running a case for which SOI is at 718 CAD (in prostar or 1 CAD before TDC in real engine), and the RHR trace obtained from the real test shows that the combustion starts 4 CAD after TDC. In such situation, what value should I enter in the start and the end boxes?
In addition to this, the other problem I am facing is the TGRADIENT (K/s). Currently I am using the default value of 1.0e+06. I wonder if this is the right number to be entered in the TGRADIENT box !!
Most importantly, if we are specifying the start of combustion using the start and the end boxes then it means that we are defining the Ignition delay. In such case how will the cetane number plays its role as this is what determines the delay.

I have been trying different values but it is misfiring every time. I would appreciate your guidelines deeply.

Thanks a lot.

Pauli September 8, 2010 13:51

The start & end of ignition boxes only tell the code when to activate the ignition sub-model. They have nothing to do with ignition delay. Set start of ignition crank angle to something just before start of injection. Set end of ignition to the end of your simulation or end of injection. Limiting the time the ignition sub-model is active is done to minimize computational overhead (no point checking for ignition when it can't/shouldn't occur).

The effect of cetane number is decribed in the methodology manual. See the section for the ignition model (equation 11-85 in the Star 3.26 manual).

The default Tgradient value should work fine for initial runs. You can tune it later.

sthamit September 8, 2010 13:56

Quote:

Originally Posted by Pauli (Post 274489)
The start & end of ignition boxes only tell the code when to activate the ignition sub-model. They have nothing to do with ignition delay. Set start of ignition crank angle to something just before start of injection. Set end of ignition to the end of your simulation or end of injection. Limiting the time the ignition sub-model is active is done to minimize computational overhead (no point checking for ignition when it can't/shouldn't occur).

The effect of cetane number is decribed in the methodology manual. See the section for the ignition model (equation 11-85 in the Star 3.26 manual).

The default Tgradient value should work fine for initial runs. You can tune it later.


Thank you man.

Let me try what you said and will get back to you very soon.

Thank you once again.

sthamit September 8, 2010 15:05

Hi Pauli,

For SOI of 718 on prostar, I am using the following scheme

1. Unpremixed/Diffusion
2. EBU LATCT
3. 4-step Autoignition
4. CN: 45
5. Tgradient: 1.0e+06
6. Ignition Reaction Based: N-Heptane
7. Interval (degCA) - Time (sec), Start Box: 700 and End Box: 875

Result: Misfiring.

Any suggestions

Thanks

Pauli September 8, 2010 18:57

At SOI (718 deg), do you have the correct pressure and temperature? Are they sufficient to produce auto-ignition? Do you have oxygen and fuel vapor present? If the answer to all these is yes, then the settings you quoted should work.

sthamit September 8, 2010 22:35

Quote:

Originally Posted by Pauli (Post 274528)
At SOI (718 deg), do you have the correct pressure and temperature? Are they sufficient to produce auto-ignition? Do you have oxygen and fuel vapor present? If the answer to all these is yes, then the settings you quoted should work.

Hi,

How do you set temperature? Is it the injection temperature? What about pressure?

Presence of Fuel vapor is assured by selecting scalar 1 for fuel properties I think but not sure to be true.

Could you tell me where to find all these info. What manual to read?

Thanks

Pauli September 9, 2010 14:01

My question was about the temperature & pressure calculated within the computational domain (i.e. the engine cylinder). Did you check these to make sure the solution is computing reasonable values?

Injection temperature should be set to fuel supply temperature.

Yes the fuel vapor usually goes to scalar 1. But I don't think it has to be that way.

You should all ready have read the methodology and user manual spray and combustion sections. :) Clicking on the help button in each of the Nav Center panels can sometimes provide information not in those manuals.

What do you mean by misfire? What are you observing?

How are you doing your mesh motion?

sthamit September 9, 2010 14:18

Quote:

Originally Posted by Pauli (Post 274658)
My question was about the temperature & pressure calculated within the computational domain (i.e. the engine cylinder). Did you check these to make sure the solution is computing reasonable values?

Injection temperature should be set to fuel supply temperature.

Yes the fuel vapor usually goes to scalar 1. But I don't think it has to be that way.

You should all ready have read the methodology and user manual spray and combustion sections. :) Clicking on the help button in each of the Nav Center panels can sometimes provide information not in those manuals.

What do you mean by misfire? What are you observing?

How are you doing your mesh motion?


Pauli,

The engine cylinder pressure and temperature values were 25 bar and 850K respectively. Oxygen content is 23%. With these conditions, still it is not firing i.e. No combustion at all. Now I am running a case with 950K and advancing the injection timing at 716 degrees bTDC and see what happens.

In the mean time, let me study the nature of pressure trace without combustion.

Thanks. Will get back to you once the case run completes.

sthamit September 10, 2010 09:17

[QUOTE=sthamit;274659]Pauli,


Hi,

Need help.

I tried couple of other combination of temperatures and pressures but combustion didn't take place at all.

I have no idea on what to do now? Could you provide some guidelines please.

Thanks

Pauli September 10, 2010 11:11

Hard to say. It could be plenty of things.

You never answered if you have fuel vapor present?

You have sufficient temperature & oxygen. So if you also have fuel vapor present, then something is configured incorrectly.

You should consider asking CD-adapco support folks to look at your model.

sthamit September 10, 2010 11:59

Quote:

Originally Posted by Pauli (Post 274765)
Hard to say. It could be plenty of things.

You never answered if you have fuel vapor present?

You have sufficient temperature & oxygen. So if you also have fuel vapor present, then something is configured incorrectly.

You should consider asking CD-adapco support folks to look at your model.



I have no idea about the fuel vapor but yes according to what I see in the es-ice input file, here are the details:
1. Fuel = 0
2. Oxygen = 0.22
3. N2 = 0.78
4. Temperature = 850 K (also tried with 950 K but didn't work)
5. Pressure = 26 bar

Now I am assuming Fuel to be fuel vapor and therefore using the following details I am running a case.
1. Fuel = 0.01
2. Oxygen = .21
3. N2 = 0.78
4. Temperature and Pressure same as above

Will get back to post more comments once the case gets over.

Thanks.

sthamit September 10, 2010 12:51

Quote:

Originally Posted by sthamit (Post 274772)
I have no idea about the fuel vapor but yes according to what I see in the es-ice input file, here are the details:
1. Fuel = 0
2. Oxygen = 0.22
3. N2 = 0.78
4. Temperature = 850 K (also tried with 950 K but didn't work)
5. Pressure = 26 bar

Now I am assuming Fuel to be fuel vapor and therefore using the following details I am running a case.
1. Fuel = 0.01
2. Oxygen = .21
3. N2 = 0.78
4. Temperature and Pressure same as above

Will get back to post more comments once the case gets over.

Thanks.


Nope...didn't work.

Pauli September 10, 2010 13:51

So this is what you are using to intialize the computational domain? If so, I don't understand what you are doing. That is pretty hight temperature and pressure for domain intialization. And you do not initialize the reaction's fuel scalar with a non-zero value.

You indicate these values are from an es-ice input file. This affirms my assumption that you are doing a moving mesh, spray and combustion simulation for a diesel engine. Correct? What version of the software are you using?

If you want to figure out what is going wrong, you need to be looking at what is coming out of the solutions - i.e. the transient result file, and the info file. You still have not answered my question regarding if you are getting fuel vapor. You should go to the transient results file, load a time step after spray and ignition start, load the fuel vapor scalar and see if the value makes sense. Are your fuel spray droplets evaporating and going into the correct scalar? If not, you will never get a reaction.

sthamit September 10, 2010 14:02

Quote:

Originally Posted by Pauli (Post 274783)
So this is what you are using to intialize the computational domain? If so, I don't understand what you are doing. That is pretty hight temperature and pressure for domain intialization. And you do not initialize the reaction's fuel scalar with a non-zero value.

You indicate these values are from an es-ice input file. This affirms my assumption that you are doing a moving mesh, spray and combustion simulation for a diesel engine. Correct? What version of the software are you using?

If you want to figure out what is going wrong, you need to be looking at what is coming out of the solutions - i.e. the transient result file, and the info file. You still have not answered my question regarding if you are getting fuel vapor. You should go to the transient results file, load a time step after spray and ignition start, load the fuel vapor scalar and see if the value makes sense. Are your fuel spray droplets evaporating and going into the correct scalar? If not, you will never get a reaction.


I am using 4.12.038 version of star-CD.
Yes you are right. I am doing a moving mesh, spray and combustion simulation for a diesel engine.

Let me check my transient results file and check what is happening?

sthamit September 10, 2010 14:33

In the info file I can see that fuel is being injected but I just can't find fuel vapor. Also I am not able to find this results transient file. Could you guide me a bit further?

Thanks

sthamit September 10, 2010 14:38

Quote:

Originally Posted by sthamit (Post 274789)
In the info file I can see that fuel is being injected but I just can't find fuel vapor. Also I am not able to find this results transient file. Could you guide me a bit further?

Thanks


Okay in the shell.info file, I found that mass of fuel evaporated from liquid film is zero all the time. May be this is the problem. Any idea what to do now?

sthamit September 13, 2010 14:05

Quote:

Originally Posted by Pauli (Post 274783)
So this is what you are using to intialize the computational domain? If so, I don't understand what you are doing. That is pretty hight temperature and pressure for domain intialization. And you do not initialize the reaction's fuel scalar with a non-zero value.

You indicate these values are from an es-ice input file. This affirms my assumption that you are doing a moving mesh, spray and combustion simulation for a diesel engine. Correct? What version of the software are you using?

If you want to figure out what is going wrong, you need to be looking at what is coming out of the solutions - i.e. the transient result file, and the info file. You still have not answered my question regarding if you are getting fuel vapor. You should go to the transient results file, load a time step after spray and ignition start, load the fuel vapor scalar and see if the value makes sense. Are your fuel spray droplets evaporating and going into the correct scalar? If not, you will never get a reaction.



Yes I am getting fuel vapor which is very less as compared to the fuel mass, and it's going to the right scalar which is 1 for the fuel I am using C7H16 (L).

sthamit September 13, 2010 15:49

Quote:

Originally Posted by sthamit (Post 275019)
Yes I am getting fuel vapor which is very less as compared to the fuel mass, and it's going to the right scalar which is 1 for the fuel I am using C7H16 (L).


Okay fuel vapor is about 90% of the total mass injected. Any suggestions !!

sthamit September 15, 2010 14:30

Quote:

Originally Posted by Pauli (Post 274783)
So this is what you are using to intialize the computational domain? If so, I don't understand what you are doing. That is pretty hight temperature and pressure for domain intialization. And you do not initialize the reaction's fuel scalar with a non-zero value.

You indicate these values are from an es-ice input file. This affirms my assumption that you are doing a moving mesh, spray and combustion simulation for a diesel engine. Correct? What version of the software are you using?

If you want to figure out what is going wrong, you need to be looking at what is coming out of the solutions - i.e. the transient result file, and the info file. You still have not answered my question regarding if you are getting fuel vapor. You should go to the transient results file, load a time step after spray and ignition start, load the fuel vapor scalar and see if the value makes sense. Are your fuel spray droplets evaporating and going into the correct scalar? If not, you will never get a reaction.


Important:

Hey Pauli, I found out what the problem was. Finally, combustion took place but with CN 60. No combustion occurred for CN < 60. Did it happened to you too? Please suggest.

Thanks

sthamit September 17, 2010 12:56

Does anybody know what to change in 4-step autoignition under Unpremixed EBU LATCT model to make Ignition delay vary with respect to different cetane numbers used. I tried different values starting from 1e6 to 0 for Tgradients but nothing seems to be happening as far as the ignition delay is concerned for one or varying cetane numbers. Any help would be highly appreciated.

Thanks in advance

sthamit September 17, 2010 13:07

Quote:

Originally Posted by Pauli (Post 273925)
What ignition model are you using? Have you tried to vary any of the parameters?

I was using EBU-LATC with 4-step ignition. I was able to make ignition delay & pre-mix phase vary significantly by changing the various parameters.


Hi Pauli, How are you doing man?

I am just tired of randomly trying different things in 4-step ignition. I was reading this post of yours and thought this is what I need to consult with you in order to control/change ignition delay and premix phase significantly. I have been trying changing Tgradient and cetane numbers but nothing seems to be happening as far as delay is concerned and the temperature rise is just shooting up in the order of 1500 K.

I am doing diesel with moving mesh, unpremixed and EBU LATCT.

Please help.

behzadniknam September 20, 2010 07:15

how i can solve this error in fluent heat vulometric source
 
i would like to modell fire in tunnel .i write this udf but fluet show this erorr how i can solve this erorr or how i can modell fire with 5*5*2.5 dimention and 20 mw size with .5m cells pls help me my yahoo id behzadniknam@yahoo.com
#include "udf.h"
#include "defines.h"
#define Q 20000000
#define H 5// flame hight above floor
#define D .5//cell size
#define DX D
#define DY D
#define DZ D
DEFINE_SOURCE(heat_source, c, t, dS, eqn)
{
real x[ND_ND];
real V=DX*DY*DZ;
C_CENTROID(x,c,t);
if (fabs(x[0])<DX/2 && fabs(x[2])<DZ/2 && fabs(x[1]+DY)<H){
return Q/V;
}
else {
return 0.0;
}
}
************************************************** **
*************************************************
error
************************************************** *******
chip-exec: heat_source: wrong return type: void udf function expected
Error:
FLUENT received fatal signal (ACCESS_VIOLATION)
1. Note exact events leading to error.
2. Save case/data under new name.
3. Exit program and restart to continue.
4. Report error to your distributor.
Error Object: ()


All times are GMT -4. The time now is 15:03.