catalytic combustion of methane in micro-channel

  • 45 Views
  • Last Post 5 days ago
  • Topic Is Solved
Weiqiang Liu posted this 3 weeks ago

Hi all,

I've posted a few threads about this topic. For now, I can model methane combustion with surface mechanism only successfully. I am trying to include both gas phase and surface mechanism. I followed exactly the same setting in literature except I did not include radiation since divergence problem. The residuals show that the case is converging as shown below:

The temperature of the out wall is set as constant 773 K. In order to ignite the mixture, I tried two methods. One is by setting a high enough temperature to the catalytic wall firstly and calculate for hundreds of iterations. Then reset the thermal boundary condition to coupled. The other method is to patch a high temperature to the whole computation domain. My problem is no matter what I do, maximum temperature in the domain keeps decreasing until to the out wall temperature 773 K. Namely, all reactions do not happen. I put the temperature contour as below. The maximum temperature should be 1800 K according to literature.

another aspect that confuses me is the contour of methane model fraction. I set the mole fraction of methane of inlet to 0.105. However, the contour shows that the mole fraction of methane near inlet is 0.0864 which is smaller than the value 0.105. This does not make any sense.

Can anybody help me to check my model?

Best regards.

Weiqiang

Order By: Standard | Newest | Votes
Weiqiang Liu posted this 3 weeks ago

anyone please help.

abenhadj posted this 3 weeks ago

It is hard to comment without looking into the case. Check all reaction mechanism, boundaries. Moreover why bulk reaction are not included. The contour plot of methane tells me that the case is not converged.

Best regards,

Amine

Weiqiang Liu posted this 2 weeks ago

Hi Amine,

I believe the mechanism has no problem. I checked line by line with the mechanisms the author listed in the paper. All the boundary conditions are consistent with those in literature. Even the mesh number is the same with literature. 

Yes, the case is not converged. 

I wrote emails to the author however got no respond. I am wondering are there any special strategies to ignite or something is wrong with my model?

Best.

Weiqiang.

abenhadj posted this 2 weeks ago

Either a spark or a continuous heat input. Try patching the cell layer to the wall and the wall itself with high temperature. I have already mentioned that several times already.

Please check if there is error messages in the chemkin out files.

If still not working please get in touch with ASC and he will check with local support if possible.

Best regards,

Amine

ansysuser posted this 2 weeks ago

You can ignite the mixture by putting a heat flux.  Try a value of 5E5 on a small segment of the surface.  I did the video in the gif link below using a small segment of the bottom wall with such a flux.  About 1/4 of the way through, the flux is turned off.  The mesh shows where the heat flux is located.  I used the default 2-step mechanism.

 Link to the solution video gif:

https://i.imgur.com/Nj462uQ.gif

 

And here is where the mesh shows the small part of the surface that has a heat flux to ignite the mixture. The inlet is on the left and the outlet is on the right.

 

 

  • Liked by
  • Weiqiang Liu
  • Goenitz
Weiqiang Liu posted this 2 weeks ago

Hi,

Do you also have gas phase and surface mechanism in your model? By giving a heat flux to a segmentation of the wall, do you mean I have to redraw the mesh and separate the wall with and without heat flux. Then set the small segmentation of the wall to 5E5 to calculate for hundreds of iterations and switch back to boundary condition I want?

Best regards.

 

Weiqiang

ansysuser posted this 2 weeks ago

Hello,

 

I only used the gas phase in that simple model.  Yes, in DesignModeler I split the lower wall into 3 parts so that I could put a flux on only a small section.  You can put the igniting flux wherever you need it.  You can avoid stopping the simulation by using the "Execute Commands" found in "Calculation Activities".  Simply enter the command to switch the boundary condition to zero flux or whatever at the appropriate time step.

 

 

Weiqiang Liu posted this 2 weeks ago

Hi,

My case is steady-state. I read some literature and found those authors often ignite the mixture by patching a high temperature to the whole computation domain. It's really interesting to give a heat flux initially to ignite the mixture. How do you find this? Have you tried to ignite the mixture by patching the whole domain high temperature? 

Since my case is steady state, can I just give an initial heat flux and then turn it off? 

Best.

Weiqiang

abenhadj posted this 2 weeks ago

You can use an expression to restrict the heat input to certain part if the wall.

Best regards,

Amine

abenhadj posted this 2 weeks ago

Mesh manipulation or UDF are not required with 2019R1

Best regards,

Amine

Weiqiang Liu posted this 2 weeks ago

but I am using Ansys fluent 17.0 . Can I use expression to restrict heat input with this version?

Weiqiang.

Weiqiang Liu posted this 2 weeks ago

Hi Amine,

I just get ignited results by calculating more iterations with high catalytic wall temperature. I calculated 300 iterations before I switched the thermal boundary condition to back to coupled. Then I tried to calculate 600 iterations with high catalytic wall temperature. What is amazing is mixture get ignited!

Best.

Weiqiang

Goenitz posted this 6 days ago

Good day Sir,

I am using ANSYS CFX 18. I want to simulate methane combustion on hot wall not in bulk gas by using Arrhenius eq. Though I set all inltet/outlet/wall temperature to be 300K and hot wall 600K but activation temperature 3000K yet reaction occurs.

The second problem is I want reaction to occur only on hot surface but idk how to set it. In paper they have assigned chemical kinetic equation (by using FORTRAN code) I guess i can use same by assigning some source or flux to heat or momentum (specie transport) equation. is that so? 

Goenitz posted this 6 days ago

Weiqiang Liu posted this 5 days ago

Hi , Goenitz,

I am sorry. I don't use CFX. You can post a thread separately in this forum.

Best. 

 

Close