Hi ALL, I need to calculate the Residense time for my flow model. In my model a flow sample will come in contact with the sensor through a external loop from the main pipe stream.

when I used user routine(Junction Box Example) as per CFX help, I got the below error message.

Unable to find library winnt/user output.dll on path "C:\Program Files\ANSYS Inc\v110\CFX\examples\UserFortran"

Is it due to unavailability of Fortran compiler? Is there any other way to calculate residence time?

Please help. -Selva

Hi

This article may be interesting: "The use of CFD in the evaluation of UV treatment systems": http://www.iwaponline.com/jh/003/jh0030059.htm

From the article: "In order to obtain residence times from CFD models a user scalar is used to represent residence time. This variable has a source term of 1.0 s sâˆ'1 throughout the flow domain so that fluid that remains in the system for 1 second has a 1 second increase in residence time. A steady state solution is then obtained based on a previously calculated velocity and pressure field and the calculated 'concentration' of this scalar at each point is equal to the residence time of fluid passing through that point."

The simulations were done with CFX-5.3

Hi,

Rui has suggested an interesting way of getting residence time. It can also be calculated in CFX-Post without adding an additional variable by generating a streamline and displaying the time along the streamline.

Glenn Horrocks

There is one question in the solution as Glenn Horrocks advised, models should be calculated first. Or streamlines can not be created. Maybe u can calculate the model with a timestep(not precise), Advection Time will be shown in the .out file. U can take it as a reference.

There is one question in the solution as Glenn Horrocks advised, models should be calculated first. Or streamlines can not be created. Maybe u can calculate the model with a timestep(not precise), Advection Time will be shown in the .out file. U can take it as a reference.

As you said, I calculated the residence time by ploting "time on streamline" variable for the streamline. Thanks for the help.

Add "age" to your solver run. http://www.cfd-online.com/Forum/cfx_...cgi/read/11571 -Dr. Flow Squad