Hello everyone,

I am trying to model tracer performace in a reactor with cfx 5.6. If you did it before, could you please provide some ideas of how to conduct such a simulation? Or could you please tell me which example in CFX help file I should read to find solution?

Thanks!

Jim

Hi Jim,

If you are looking for an example of how to do particle tracking in the flow, look at tutorial 9, flow through a butterfly valve.

Regards, Glenn

Hi, Glenn,

Thanks a lot for your reply. I am trying do tracer dye simulation, not particle tracking. So which example has solutions for such a modelling? Thanks!

Best regards!

Jim

In CFX 5.6 release note(http://www.zserv.tuwien.ac.at/sc/dow...otescfx5.6.pdf), it was said: "It is not possible to run a simulation that includes mass sources without solving for the mass and momentum equations. For example, it is not possible to run a simulation solving only for a scalar transport equation if mass sources are included, even if you are restarting from a previous simulation where the flow field was established."

Does this mean that I can't model tracer by---- conducting a steady state solution firstly, then freeze hydraulic model, add tracer scalar, then run simulation restarted from steady state (hydro off) as a steady state? (said in a previous post).

Anyone can tell me the details of how to attain tracer dye performance with CFX5.6?

Thanks!!

Jim

Jim, Does your tracer need tohave mass ? If the mass is noty important then all you need to do is introduce a dimensionless scalar. I guess it depends upon how you intend to use the tracer. In ventilation problems, we use a mass less scalar to model the age of air within a building, or to assess the ventilation within a building. Effectively we use the scalar as a marker to track the path of air through a room. Bob

Hi, Bob, Thanks a lot for sharing your experience! The tracer experiment I did is to pulse inject some tracer (NaCl solution) to the inlet of a water tank, and monitor the concentration at outlet to obtain the residence time ditrubution curve. Now, what I am trying to do is to model this process with CFD. Do you think this is similar to your case? And could you provide more detailed procedures for solving such a problem? I am a new CFX 5.6 user.

Thanks again! And have a nice weekend!

Jim,

I've done this very thing before. If your concentration is low enough (i.e. less that 1%) then you can probably ignore the mass. Simply add in an additional variable that is massless and pulse it at some interval as a boundary condition on the inlet. You can then solve the problem transiently and track the concentration at the outlet. You may need a user routine to integrate the outlet concentration at each time step and print it to a file (otherwise you've got to load each simulation time step into Post by hand and calculate the concentration). See the last chapter of solver models on doing this.

Jeff

Jeff

Thanks a lot for your help. I found an example(4) in CFX5.6 help file, which is very similar to what you said. Now I am more clear of how to add scalars, and how to get tracer output. I will try to solve my problem this week. Thanks again!

With best regards!

Jim

As an added note, you will get much better results using both the High Order Differencing Scheme as well as the Second Order Forward Time Differencing Scheme. I've done numerical diffusion studies which show very bad smearing of the scalar values (this is inherent with any finite volume/difference code) when using either first order in time or space. Second order in one or the other doesn't cut it either, you have to do both.

Jeff