How to specify surface flux of a species?

 Register Blogs Members List Search Today's Posts Mark Forums Read

 February 1, 2006, 15:56 How to specify surface flux of a species? #1 ked Guest   Posts: n/a Hi I am modeling species transport with volumetric reaction in a rectangular channel. I have 4 species in the mixture. Two species enter domain through inlet of the channel. I want to define surface flux of thrid species from the bottom face of the channel and reacting with one of the species entering through inlet. fourth species being reaction product. My questioin is how to define surface flux of the species? I want no velocity of this species just surface flux. Which boundary condition shall I use? Thanks.

 February 1, 2006, 16:18 Re: How to specify surface flux of a species? #2 Ynot Guest   Posts: n/a use a wall BC Open the setting of your wall BC. There will be a tab named "Species" where you can specify a mass fraction flux of your desired species. Hope this helps. Ynot - Tsaad

 February 1, 2006, 19:20 Re: How to specify surface flux of a species? #3 Ked Guest   Posts: n/a Thanks a lot for your reply. The setting that you have mentioned specifies either mass fraction of the species or zero diffusive flux. But that does not specify surface flux of that species. How can I specify surface flux of that species in kg/m2-s. Thanks again.

 February 1, 2006, 19:26 Re: How to specify surface flux of a species? #4 Ynot Guest   Posts: n/a Oh... i see, you want a mass flux. well, am not sure if you can specify that in fluent. what you can do, is use a mass flow boundary condition. compute your net mass flowrate across the surface and use that value.

 February 1, 2006, 21:50 Re: How to specify surface flux of a species? #5 Ked Guest   Posts: n/a Thanks again. Yeah I thought about giving mass flow inlet boundary condition. But that would give velocity in that direction and the requirement of my problem is that there should not be any velocity. I can only specify surface flux as if that species is generating from the bottom surface and reacting in the fluid zone.

 February 1, 2006, 22:20 Re: How to specify surface flux of a species? #6 Ynot Guest   Posts: n/a Hi Ked, you cannot have a mass flux without having a velocity. Fluent will compute the mass flowrate at the boundary faces, whether you input a velocity or a flowrate. Furthermore, when you input the total flowrate (Kg/s) across the whole boundary surface, Fluent will automatically divide that flowrate along the boundary faces, so it is exactely the same as inputing a mass flux (Kg/m2.s). Now, it seems to me like you are trying to simulate something like a Hybrid rocket motor. Your problem is very similar to that i beleive. From what i understood, you have a solid layer of fuel across the bottom surface, and your oxidizer is injected from the left, for example... and the reaction proceeds. The usual way we do this in analytical methods, is as follows: as the solid fuel burns the rate of depletion of the solid fuel is identically equal to the mass flux that you are talking about. Again, you can never have a mass flux without a velocity, it is unphysical! So we model this as a velocity or mass flow bundary condition. If you can give me a complete description of your problem, maybe we can brainstorm on how to model your case. Note that when you have diffusion flames, they are usually very thin, and you can safely consider a species flowrate across that boundary. That's how we do it in hybrid rocket motors. Ynot - Tsaad

 February 1, 2006, 23:36 Re: How to specify surface flux of a species? #7 Ked Guest   Posts: n/a I really really appreciate your help. Here is the description of my problem. In human body nitric oxide is generated at the surface of an artery at a particular surface flux. In body it goes in the blood and gets dissociated into nitrogen and oxygen. I am trying to model same situation. I have modeled a rectangular channel. At the inlet of the channel mass flow rate of blood is specified. Now comes the difficult part. I want to specify surface flux of nitric oxide at the bottom face of the channel or say Nitric oxide generates and goes in the channel at a specified mass flux and is dissociated into nitrogen and oxygen. For the dissociation I have defined the volumetric reaction. I want to see the concentration profile of niric oxide in the channel. Now how to define mass flux of nitric oxide at the bottom face of the channel? I hope I am clear enough in defining my problem. Thanks aganin.

 February 1, 2006, 23:48 Re: How to specify surface flux of a species? #8 Ked Guest   Posts: n/a One more thing I wish to add. There is a analytical model available in literature for this mechanism. In that model, diffusion of nitric oxide was modeled by Fick's law of diffusion.

 February 2, 2006, 03:57 Re: How to specify surface flux of a species? #9 Ynot Guest   Posts: n/a Hi Ked, I've done some reading and here's what i suggest. You can, as a first iteration, try these methods (by order of complexity). The first one, is simply to use a mass flow inlet and see what's happening. It won't hurt to try it. Now, the second one, you can use a species mass fraction of 1 at the wall, and then set the "correct" diffusion coefficient for nitric oxide in the materials panel. Although Fluent will use the wall BC as a Dirichlet or fixed BC, and will identify the mechanisms of nitric oxide getting into the blood. It is defintely diffusion dominated, and the convection will be very low, if there will be any! Finally, the third method is to define your own scalar that will designate the mass fraction of NO2. I am not sure how well this will work, but it would be great if you give it a try. It is very easy to do it. Simply go to Define/user defined/scalars and a new scalar will be defined for you. When you go the BC setting of the surface, you will see a specified flux input... I'll be doing some more reading on surface reactions. You can also take a look on that section in the fluent manual. But form the physical point of view, the second method should work fine, just input the correct diffusion coefficient.(at the wall, the velocity is zero and your process will be dominated by diffusion). You can then validate your results by computing the surface flux. good luck! Ynot - Tsaad

 February 2, 2006, 04:39 Re: How to specify surface flux of a species? #10 Markus Guest   Posts: n/a hello ked, There is another possibility: if you know the diffusive mass flux in kg/s-m2 and the surface area across this flux enters you easily can calculate the mass flow in kg/s. Actually this can be regarded as some kind of species "mass source" for the cells next to your bottom boundary. This leads to the idea, to implement this diffusive flux as volumetric mass source of your species. In other words, use a DEFINE_SOURCE UDF which returns the desired mass "flow" divided by the cell volume to give kg/s-m3. Activate this UDF only for cells adjacent to bottom. I hope this is clear enough and helps Markus

 February 2, 2006, 18:11 Re: How to specify surface flux of a species? #11 ked Guest   Posts: n/a Thanks. I am working on all these three cases that you mentioned. I am having a hard time in getting the convergence. I am particularly troubled by reversed flow warning and divergence. I have specified mass flow inlet for the inlet face, mass flow inlet for bottom face. outflow for outlet and wall for the top wall. One more thing is for the first case that you mentioned. If I specify the mass fraction of nitric oxide as 1 in the boundary condition, I get exagerated concnetration after postprocessing which is not right. If I specify the mass fraction I desire (1.5e-10) at the start of calculations, then that means blood will also come in from the bottom face along with nitrif oxide and that is not desirable. I am trying to work it out. I will let you know which of these three cases work. Thanks again.

 February 2, 2006, 18:13 Re: How to specify surface flux of a species? #12 ked Guest   Posts: n/a Hi Markus Thanks for joining in. Do I need to right DEFINE_SOURCE UDF? or is it available in fluent? One more thing can I define source term in the FLuid zone boundary condition? Can you throw some light on these issues.

 February 3, 2006, 04:32 Re: How to specify surface flux of a species? #13 Markus Guest   Posts: n/a hello ked, Yes, you have to write the UDF by your own. Check the UDF manual for DEFINE_SOURCE where you can find some examples which should do the job for your problem. Once you have written and compiled the subroutine it can be hooked to your model as mass source for the species in each seperate fluid zone (BC panel). For you it is advantageous to define a fluid zone which comprises a single cell layer just next to bottom and activate the UDF only here. br Markus

 February 4, 2006, 04:33 Re: How to specify surface flux of a species? #14 Ked Guest   Posts: n/a Hi Markus, Why do I need to write a UDF? I have a constant source not a functional source. So cant I just define a fixed source in the fluid panel for that species. Only problem is how to assign that mass source to specific cells (near boundary)? Can you suggest me something? Thanks a lot.

 February 6, 2006, 14:22 Re: How to specify surface flux of a species? #15 Markus Guest   Posts: n/a hello, yes, if the source is constant then there is no need for a UDF. The cells containing the source must be gathered in a separate fluidzone, which can be defined either in Gambit, or for your problem i would suggest to mark cells near the bottom boundary using adapt/boundary distance and to split the existing fluid zone with them. Markus

 February 7, 2006, 18:27 Re: How to specify surface flux of a species? #16 Ked Guest   Posts: n/a Thanks Markus

 February 9, 2006, 21:14 Re: How to specify surface flux of a species? #17 Ked Guest   Posts: n/a Hi Ynot I have tried all the three methods that you mentioned. But they are not giving me correct results. I read about surface reactions but could not figure out anything helpful. Do you have anything else in your mind? In the meanwhile I am trying what Markus has suggested. Thanks.

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post tommymoose ANSYS Meshing & Geometry 0 August 5, 2011 16:02 joe Phoenics 1 November 30, 2005 06:34 Karthick FLUENT 0 May 26, 2004 05:24 massimo CD-adapco 5 December 11, 2002 06:55 Chie Min CFX 5 July 12, 2001 23:19

All times are GMT -4. The time now is 09:46.