CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   FLUENT (https://www.cfd-online.com/Forums/fluent/)
-   -   Oblique detonation issue with reaction initiation (https://www.cfd-online.com/Forums/fluent/225268-oblique-detonation-issue-reaction-initiation.html)

nick1234 March 20, 2020 17:54

Oblique detonation issue with reaction initiation
 
1 Attachment(s)
Hello everyone,

I've been looking to create an fluent simulation of detonation over a wedge. I've described the problem below.

Geometry: 23deg wedge. 10cm by 8.3cm size.
Mesh: 2.5mm grid.
Model: Density based, species transport, Chemkin imported h2-air mechanism, finite rate/no TCI, chemkin-CFD solver, implicit, courant=1, density is calculated from idea-gas (not incompressible ideal gas).
Boundary Conditions:
- Top, left and right sides are pressure far-field with a flow of Mach 8, pressure of 1atm, species molar concentrations of H2:O2/2:1.
- Bottom right is wedge (wall)
- Horizontal bottom is symmetry.

Below shows my reaction temperature contour. You can see the oblique shock formed, and my post-shock temperature should be high enough to initiate reaction (3000K+). Unfortunately, I have been having trouble getting the reaction to not only initiate, but also to converge (residuals oscillate at 1). I'm aware of the patching process that can be done begin reaction, but every time I do so, the solution diverges. And if I patch too far downstream, the reaction cannot propagate upstream as the post-shock mach number is greater than 1.

My question is, is there a way to patch geometry without affecting mesh? If not, is there a way for me to initiate reaction without patching?

Also any other recommendations you may have would be greatly appreciated :)

Roh March 21, 2020 01:48

I'm working on the Detonation and ODW. Tell me about your reaction mechanism. Is it a multi-step mechanism? how many step? How did you create your Chemkin file(I mean tell us about your calculations)? what's the source of the mechanism? Are you sure that your mechanism works correctly(I mean did you validate the mechanism?)

nick1234 March 21, 2020 02:58

The mechanism file came from Lawrence Livermore National lab. Here's the link:
https://combustion.llnl.gov/archived...nisms/hydrogen

This mechanism has 5 elements, 10 species and 21 reactions. Do you mind telling me more about your ODW simulation? How have you approached your problem? What mechanisms have you chosen?

vinerm March 21, 2020 06:10

Clarity
 
I am afraid I could not understand what you mean by is there a way to patch geometry without affecting mesh?. Fluent does not have a geometry (it only has mesh) and patching never affects mesh. May be you wish to convey something else.

Secondly, far-field bc is never supposed to be touching any walls, which appears to be the case in your simulation. So, you should create a larger domain wherein the wedge is in the air and far-field covers everything from front to aft.

As far as reaction is concerned, it appears that you already have quite high temperature and as far as thermal condition is concerned, reaction should take place. Since you are using finite-rate mechanism, is there enough residence time for species within the domain to react? Else, try using FR with EDM.

nick1234 March 21, 2020 12:39

Vinerm, thanks for the response! I should have prefaced this by I am new with Fluent and this forum, and just now learning the ropes through trial and error.

By patch geometry, I meant this. In the meshing tool from workbench I would use virtual topology to separate a face from my domain to patch. More specifically, I used the split edge at +, hard vertex at + and split face at vertices to create a named selection. In doing so, the updated mesh became disrupted and caused divergence in the fluent calculation.

Is there a way for me to patch an area directly within fluent? For example create a new interior zone without having a named selection already created from the mesh tool?

Second, the pressure far field assumption was used in this tutorial for supersonic flow over a wedge:
https://confluence.cornell.edu/displ...w+Over+a+Wedge.
The tutorial uses pressure far-field as the boundary conditions, although I can try pressure outlet if you believe that would be better.

Lastly, I am now trying to introduce turbulence in my flow field. We'll see if that initiates reaction.

vinerm March 22, 2020 04:06

Patching and BC
 
I suppose you are using OpenFOAM terminology when you mention patch. Anyway, you can certainly separate a face within Fluent as well, however, it is not always easy to find a parameter with which to separate. The procedure is to mark the cells using any option under Adapt menu. There are multiple options that can be used, such as, boundary, region, iso-value, etc. You can use one or multiple of these to mark cells that identify the boundary patch you wish to separate. Do NOT click on Adapt. Just click on Patch once you have identified which method you want to use and provided the values to Fluent. E.g., if you want to separate a boundary into two along y-coordinate, then you go to Adapt > Iso-Value. Select Mesh and then y-coordinate. Click on Compute. This will show minimum and maximum of your domain. Now, you provide some minimum and maximum value for y-coordinate and click on Mark. Do NOT click on Adapt. This will mark all the cells within the min-y and max-y you provided. Marking is same as selection; now a particular subset of mesh is selected. Fluent shows the number of cells selected. Now, go to Mesh > Separate > Faces. Select the boundary to which your required patch currently belongs. Select By Register and then select the register that was created using Mark. Click on Separate. Do note that Iso-Value under Adapt is available only after initialization. You can initialize with any arbitrary values. Similarly, you can use any other method for marking.

As far as this is to be done in Meshing, better to do it at CAD level and not at meshing using Virtual Topology. That will give you better mesh as well.


All times are GMT -4. The time now is 02:27.