Ozen Engineering Newsletter – October 2016

In an advanced software like ANSYS Fluent you often need to specify things in more detail than a constant value. Perhaps you have a radial velocity profile of fully developed flow at an inlet, a time history of mesh motion or an axially varying heat generation. You don’t need to dust off your C++ compiler, though, there is an easier way: profiles.

Say we want to apply the following x displacement over time to a mesh motion:

We can accomplish this with the following text file:

((foil 3 point)
 (time 0 1 5)
 (v_z 0 10 10))

Load it into Fluent with the File -> Read -> Profiles menu item and it can be selected like a UDF in the dropdown menu:

It’s that easy.

There are several ways to specify profiles in Fluent but some of the most common are:

A Radial Profile

((<profile_name> radial <n>)
 (r <r1> <r2> <r3> ... <r_n>)
 (<field name 1> <f1_1> <f1_2> <f1_3> <f1_n>)
 (<field name 2> <f2_1> <f2_2> <f2_3> <f2_n>)
 ...
 (<field name m> <fm_1> <fm_2> <fm_3> <fm_n>))

An Axial Profile

((<profile_name> axial <n>)
 (z <z1> <z2> <z3> ... <z_n>)
 (<field name 1> <f1_1> <f1_2> <f1_3> <f1_n>)
 (<field name 2> <f2_1> <f2_2> <f2_3> <f2_n>)
 ...
 (<field name m> <fm_1> <fm_2> <fm_3> <fm_n>))

A Transient Profile

((<profile_name> transient <n> <periodic? (1/0)>)
 (time <time1> <time2> <time3> ... <time_n>)
 (<field name 1> <f1_1> <f1_2> <f1_3> <f1_n>)
 (<field name 2> <f2_1> <f2_2> <f2_3> <f2_n>)
 ...
 (<field name m> <fm_1> <fm_2> <fm_3> <fm_n>))

The above are extremely convenient ways to specify spatially or time varying boundary conditions from analytical or empirical equations. You can easily generate these models with either a text editor or an Excel spreadsheet similar to the the pictured below (save as a tab separated text file)

If you open the Profiles Manager in Fluent, you can write more complex profiles from your solution data, orient profiles to a certain coordinate system and other such operations.

For more information on profiles in Fluent, check out the documentation section at Fluent -> User’s Guide -> Cell Zone and Boundary Conditions -> Profiles. Good luck on making your simulations more accurate!