August 8, 2017 at 6:19 amsmallfrog99Subscriber
I was trying to run simulation on surface detail mechanism by adding CHEMKIN format file and comparing simulation results with my experiment from CH4 reaction on platinum surface. I did not consider gas phase combustion because the temperature was no more than 1500K. I tried to prevent gas phase combustion to occur in my experiment as well.
My questions are:
1. Is there any possibility that makes the reaction so tiny?
2. Can I leave the gas phase reaction as a blank file?
3. I have all constants (A and Ea) but I don’t know how to make them to the right format. Could you give me correct CHEMKIN formats for ‘surface CHEMKIN Mechanism file’ and ‘surface Thermodynamic Database File’?
I added the mechanism file by these following steps
1. ‘File > Import > CHEMKIN Mechanism…’ then a new window shows up.
2. I added ‘Gas-Phase CHEMKIN Mechanism File’ with a blank file that had no reactions but there were elements and species in that file as:
H O C N
CH4 CO CO2 H H2 H2O O O2 OH N2 C3H6
3. I left ‘Gas-Phase Thermodynamic Database File’ as default
4. I selected ‘Import surface CHEMKIN Mechanism’
5. I used the surface CHEMKIN Mechanism that Deutschmann has proposed on his website.
6. I put the site density to be 2.72e-8 [kgmol/m2]
The simulation result did not make sense, because there was tiny amount of CO2 and H2O coming out from the surface in the order of 10e-8. I am expecting amount of CO2 and H2O up to the order of 10e-2
March 29, 2018 at 2:44 pmWeiqiang LiuSubscriber
Can I have your contact email? I am also doing the same simulation. I've also tried to leave gas phase reaction blank like what you did. however, my simulation can not start to calculate normally with error like' received a fatal signal (segmentation fault)'
By the way, I use the same surface mechanism as you do.
would you share some experience with me ?
Thanks a lot!
April 3, 2018 at 1:45 pmWeiqiang LiuSubscriber
Can anybody help me with it? or is it possible to send me a case file.
May 2, 2018 at 1:31 amsmallfrog99Subscriber
Sorry for answering your question so late. I was so busy and forgot to reply your message.
Now, I can figure out how to run the surface reaction. Many times I got that error, fatal signal, because I didn't set the cell zone conditions accurately.
What I recommend you to start with is to setup the geometry as this paper, 'Extinction Limits of Catalytic Combustion in Microchannels' by Prof.Maruta in 2002. It is only a straight tube, 1-mm diameter and 10-mm long.
P.S. Fluent 16 works. Other than this version, they don't work. I don't know why.
Let me know if you still have the same problem.
May 2, 2018 at 8:28 pmWeiqiang LiuSubscriber
I have figured out this problem. I included both gas phase and surface reactions in my model. Seems like it is because the limitation of the number of gas species. In Fluent manual, the number of UDS can not be more than 50. I guess the gas phase species in chemkin format are treated as UDS in Fluent. When I reduced the number of gas phase species from above 50 down to below 50 step by step, the error did not occur until the number of gas phase species is under 50 and reasonable results were obtained.
However, the technical staff of Fluent told me gas phase species in chemkin format are not treated as UDS in Fluent which confuses me a lot. Besides, I read the above-mentioned paper before. I tried Fluent 15 ,16 and 17 and every version works by decreasing the number of gas phase species down to 50.
PS: would you mind sharing your contact email? So I can consult some questions about Fluent simulation considering your expertise.
January 30, 2019 at 3:54 amWeiqiang LiuSubscriber
are you there? I almost reproduced the results of the literature you recommended. Now I have some questions regarding to the simulation. Could I reach you?
Thanks very much!
January 30, 2019 at 4:08 amsmallfrog99Subscriber
Thank you for reaching me again. I was so overwhelmed when you tried to reach me last time (7 months ago) and I forgot to reply. Sorry about that.
Please feel free to ask me on this webboard that everyone can take benefits from our discussion.
Now I found ANSYS 16.0 doesn't have any problem with detail mechanism.
January 30, 2019 at 3:25 pmWeiqiang LiuSubscriber
Yes, I almost gave up on this project. I read the literature you recommended and tried to reproduce his results. Majorities of the literature results can be reproduced. However I met some difficulties.
I am using Ansys Fluent 17. Just like the author did, I ignored the gas phase reactions and all the gas phase thermo and transport data are left blank in fluent. I guess fluent will use the default thermo and transport data in its data base.
With the above settings, I can get converged and comparable results. However, when I imported my own transport and thermo data, iteration diverges very quickly.
I am reaching you to consult:
1. Did you also ignore gas phase reactions?
2.Did you use the default thermodynamic and transport data in fluent database or import those data with chemkin file?
3.Did you do any special procedures to help with convergence?
4. How do you usually ignite the mixture numerically? Normally, I would give a initial high temperature to the whole computation domain to 'ignite' the mixture.
Thanks very much!
January 30, 2019 at 5:33 pmWeiqiang LiuSubscriber
By the way, I am currently in Canada. I don't know if we have jet lag.
February 2, 2019 at 8:13 amsmallfrog99Subscriber
1. I left the gas phase reaction blank, like the one in the my first post. I am really sure that there is no gas phase combustion in my setup, because the temperature is only about 1000K, lower than the ignition temperature of the fuel.
2. Yes, I used the default thermo data and transport data from Fluent database.
3. I didn't do any special procedure.
4. What I usually do is to start with cold flow (supply only fuel-air mixture). Then set the platinum surface to around 800 K, run it for 100 iterations. And then set the platinum surface to "coupled". The combustion will sustain on its own.
Have you included radiation in your calculation? Otherwise, the temperature on the platinum surface will higher than it should be.
I'm just curious, why do you need to include your own thermo and transport data?
I am a PhD student at USC, Los Angeles.
Sorry for my late response, I will try to check ANSYS Forum more often.
February 2, 2019 at 2:19 pmWeiqiang LiuSubscriber
Thanks for replying.
1. I want to use my own thermo and transport data because a lot of literature just claim that they use external subroutines to calculate thermodynamic and transport instead of fluent database. Therefore, if I want to reproduce their results exactly, all the setups should be the same, right? Besides, I can get similar results of the literature you recommended with default thermodynamic and transport data from fluent database. However, I can not ignite the mixture when thermo and transport data are imported by chemkin files. I don't know why.
2.You said you set the platinum surface to 'coupled'. So you have solid wall computation domain in your model? As far as I am concerned, there is no solid geometry in the literature model you recommended.
3. I don't activate any radiation part in my model.
4. How do you define the mixture viscosity and conductivity in material panel of fluent. If I use default value of thermo and transport in fluent data base and do not do any modification to the material panel, viscosity and conductivity in material panel are constant value by default. However, if I change the calculating method to ideal gas mixing law or mass weighted average, The calculated results would be very different with the literature or can not even be ignited.
5. Have you reproduced the results of the literature you recommended to me exactly the same?
6. I also read some literature which claim that gas phase reactions are very important and can not be ignored. However, when I include gas phase mechanism like GRI3.0 in my model, convergence becomes very hard to achieve and mixture can not be ignited. Besides, iteration speed becomes much slower. Logically, results should have no difference with and without gas phase mechanism if gas phase reactions are not important. I know if I include gas phase mechanism, much more transport equations and reaction schemes must be solved by fluent, which causes slower iteration speed. But how can not I even ignite the mixture with gas phase mechanism.
7. I know Prof. Hai Wang has a combustion group in USC. Do you know him?
Thanks very much for sharing your experience.
February 2, 2019 at 6:18 pmsmallfrog99Subscriber
1. If you want you can also overwrite the Fluent data file in ANSYS Incv160fluentfluent16.0.0cpropepdata > thermo.db , but to me thermo data and transport data should be similar, no matter what the source is.
2. Yes, I made an arbitrary wall that is set to coupled. If you don't have a solid wall, you might set it to 'Convection' or 'Mixed' and put heat transfer coefficient in the setup. That should work too.
3. It is important. Try radiation and your result will be close to reality.
4. I used ideal gas mixing law. It should give you more accurate result.
5. I would recommend you not to reproduce everything exactly the same with the literature. It is not necessary. We are not using the same solver with Prof.Maruta. Even you and me, I used Fluent 16 and you are using Fluent 17. To me I would compare my simulation with the experiment instead of the literature.
6. For the gas phase, it depends on the temperature. In my real setup, there is no gas phase at all, just pure surface combustion. I still recommend you to compare your simulation with your experiment instead of literature. If you get somewhat similar result with the literature, that should be enough.
7. Yes, I know him (but he doesn't know me). He moved to Stanford 5 years ago.
Hope this help.
February 2, 2019 at 6:57 pmWeiqiang LiuSubscriber
Thanks very much for your answer. Unfortunately, I am not doing any experiments. Are you still doing the same project, methane catalytic combustion?
Your suggetions are very useful. I’ll try to get radiation involved.
Thanks very much!
February 4, 2019 at 4:02 pmWeiqiang LiuSubscriber
I found an interesting phenomenon. That is either external imported gas thermodynamic or transport data is used, the methane and air mixture can not be ignited. Only if I use both gas thermodynamic and transport data in fluent database, I can get similar results in literature though with some local discrepancies.
I've verified this for many times. I am wondering have you ever met this before since you mentioned thermodynamic and transport data has no difference between fluent database and external imported data.
By the way, do you make the leading edge of the channel inert just like the literature does.
- You must be logged in to reply to this topic.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Suppress Fluent to open with GUI while performing in journal file
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Getting graph and tabular data from result in workbench mechanical
- The solver failed with a non-zero exit code of : 2
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
© 2023 Copyright ANSYS, Inc. All rights reserved.