Hi all, I have to model a solid wall pyrolysis.As a starting point I would like to do it in single phase.

So I have to have a wall (or some inlet) from which a fixed mass flux should come in.

The essence of this modeling is that the flow has to be normal to the surface. Is there any boundary condition other than the "velocity inlet" or any other way where I can set the tangential velocity zero and keep only the normal component?

FYI:I use compressible flow.I cannot use incompressible flow and so I cannot use velocity inlet boundary condition also.

Thanks. Pal.

Hi Pal,

You can specify all inlet boundary conditions to allow the flow to enter the domain normal to the boundary. I would suggest you use the mass flow inlet BC although this means that you can not calculate heat flux at the fuel surface. Another possible solution is that you define a thin fluid zone adjacent to the fuel surface to which a species source term can be defined relative to the specified mass flux. By doing this you allow pyrolysis species to enter the domain whilst being able to calculate heat transfer at the fuel surface by setting it as a wall BC. Hope this helps

Neil

Thanks Neil for your reply..I will try the source term definition..

I have already tried the mass flow inlet one..My problem is little more complex..I actually am modeling the hybrid rocket motor combustion chamber..So there is an oxidiser flow perpendicular to the fuel flow..What happens at the fuel mass inlet is that when I have this oxidiser coming in, even though I specify normal flow, when the non-reacting flow converges, there are some tangential as well as normal non-zero components seen..That means that the flow is no longer normal even if I specify it to be..It is a violation of the bc that I apply at the boundary.

It becomes still worse when I switch on the reactions..I am getting reverse flow in the fuel mass inlet boundary..Reverse flow also means it is not at all applying the condition what I want it to apply in the boundary..

What could be the problem..??

Thanks

Pal.

1)You can't expect the velocity component of the fuel flow to be normal to the boundary because of the influence of the axial oxidiser flow. The velocity of the oxidiser flow is alot higher than the fuel inlet velocity so the normal (-VE radial) velocity component at the fuel surface will be smaller than the axial component.

2)You say you get a tangential velocity component at the fuel surface. Ive seen your mesh from the link in a previous post and considering you are injecting oxidiser flow axially this is unlikely. Check to see whether your co-ord system is correct.

3)Reversed flow does not mean the BCs are being applied incorrectly and occurs throughout many simulations. It occurs because the initial inlet pressures/velocities are too high, try increasing them steadily throughout the simulation. Otherwise extend the domain which in your case is easily done by placing a tube at the nozzle throat about 2-3 times the length of the chamber. Reversed flow is still likely to occur during initial iterations but will subside as the solution progresses.

Neil

Dear Neil

1. At the boundary I am specifying normal mass-flux..So atleast at the boundary node I can expect the velocity to be normal, can't I?? It will surely be different at the first node..I accept it..But I guess I decide what has to be at the boundary and the code has to calculate the interior with the conditions that I give..Am i wrong??

2. I used the wrong terminology to indicate the velocity component in my previous post..It is the axial component that I detect at the boundary nodes even..There is no tangential component, as u said..sorry for that silly mistake..

3. When combustion is happening, any sort of reversed flows disturb the fuel flux which makes the whole flame unstable..So I do not think giving mass flux bc for fuel is going to help..The "wall+mass source added zone" that u proposed seems to be promising. i have only one thing that is confusing here..

I have a very thin zone, 0.1mm thick inside the cylindrical wall, where I have added a mass source, an axial momentum source, turbulence sources and an energy source..I have the values so, that the fuel enters approximately normally with desired velocity (~2 m/s) and around 750K..

But when I switch on the reaction, after some iterations the temperature of the fuel coming in drops..(I have added a couple of pictures of the temperature contour at the same folder.. http://picasaweb.google.com/guru.palani/Project )I checked with the energy source term and could not find any deviation there..What could be the problem..???(the first picture shows the temperature contour, which shows a yellow region which is expected to converge as flame..the second one is the closeup near the boundary..the first 2 grids form the source added zone..wall is kept at 800K, so it is hotter in the first cell..)

Pal.

1)I assume your using a cell based gradient option which means a purely normal velocity will not be calculated as there will be axial velocity components contained within the cell adjacent to the boundary. If you think about the velocity profile in the boundary layer it is predominantly axial with zero axial velocity occuring at the surface. Which means that a completely normal velocity component will occur in a very very small region of the viscous sublayer of the boundary layer. Meaning you need to use the EHT wall function to resolve this despite the NE wall function being most suitable for this case. Basically the solution is correct as youve defined your BCs correctly, even in the boundary layer the fuel velocity has axial and negative radial components. So don't worry about it.

2)By the sound of it your solving combustion from the initial solution as your still getting reversed flow which in your case dissapears relatively early on during the calculations. First solve the flow for the non-combusting case with species transport then when the solution is converged and reversed flow has ceased, then activate the combustion model.

3)You only need to add a mass source term as axial momentum, turbulence and energy are provided by the flow. Just patch the 750K temperature into the zone to spark combustion.

Dear Neil

The concept behind myself using high temperature fuel entering the zone is that, practically the fuel is in solid state inside the motor and it pyrolyzes and enters the combustion zone. The pyrolysing temperature is usually higher, of the order of 800 - 1000K. That is why I want to specify an energy source. I tried without specifying energy source, and that lets the fluid enter with zero kelvin which is practically not feasible.

I donot have any problem with this model as long as I have the flow alone. When I switch on the reaction, there comes the problem. As I said in my previous post, I donot understand the reason why the temperature reduces after it leaves the source zone. Is it that the energy source that I added has not been considered???

<Quote: the second point of ur previous post>

I have converged the flow and then only I have tried switching on the reactions..Even after that reversed flow comes that alters the mass flux of fuel which destabilizes the flame..

This solid-wall + source modeling seems to be promising, but for the low temperature detected after switching on combustion..Any suggestions???

Thanks

Pal.

I dont see why your adding an energy source when you could just patch the fuel source zone with a high temperature. Or why the mass flux of the fuel is altered as you have defined it as a constant value under the source terms. Did you extend the domain to reduce reversed flow? With respect to destabilising the flame this should not happen because you are not modelling the flame front. Try using the non-premixed combustion model instead of defining chemical reactions. It has shown to give more accurate chamber temperatures compared to finite rate/eddy dissipation. It should also alleviate the problem with low temperatures as they are already calculated based on the O/F.

Neil