How to export velocity profile and load it as inlet condition
 

I am using ANSYS Fluent 13.0 to model a 3D microchannel fluid and heat transfer. Anyone can tell me how to input hydrodynamic fully developed flow as inlet flow condition? I want to extract the 3D velocity profile from another FLUENT calculation and load the velocity file as the input, but I don't know how to get the velocity file. I read some tutorial saying the velocity file can be obtained as a file format of "XY".

In Fluent, Solution XY plot and write to file, the variable you are interested in...

While reading the boundary condition, you can read as a profile instead of constant.

write the file by xy plot, u hav to select a face wher you want to get an profile.
be careful, the upper values in the exported profile file represents 'x , y, and z' coordinates respectively. The last column values are the magnitudes (or etc) that u hav just taken on the surface...

Now u can give these profiles to ur face by importing profiles first, then u can select this in the boundary condition window-->velocity (or other)
instead of giving constant velocity profile.

enjoy.

You also have the ability to export a profile from File>Export>Profile... This will take you through a dialog where you select quantities and surfaces to export. You can then import this into the next case.

Hi swetkyz

I have a question: if I want to export a velocity outlet profile from fluent and then import also in fluent, when u mentioned that this dialog comes up, in which format do I have to export it? I see Abaquis, ASCII but no fluent....

thanks!

Hi Alro,

It is simply File>Export>Profile. This allows you to export data for any quantity on any surface in a ".prof" format. From there, you start your next simulation, and in the Boundary Conditions tab, select the surface you want to apply the profile to. Once selected, you just hit the "Profiles..." button on the same tab, and it is self-explanatory from there.

Hope that helps.

Is it possible to collect a mean of a outlet profile from a transient analysis and use this for a inlet profile in a steady state analysis?

I have a similar question: Is it also possible to export a velocity profile at a certain cross-section (resp. a simple line in a 2D model) in CFD-Post?
Thanks for your help!

Hi Marabelle,

It is possible to export the velocity/other parameters from a certain cross section. I run an analysis for the seabed and extracted the velocity from the layers above.
You can use Insert-> Location-> User surface and in the method field you can use transformed or Offset ... this will offset your surface and then you can create a contour etc for this new surface and then File-> Export.
Not sure about 2D line as you mentioned - you can use the data from 3D and process it (find the values you are interested in). there might be a way to export only those you want ....

hope this helps! :)

hi
I have a similar problem. I want to use the velocity outlet of a flow in a pipe for inlet boundary condition of another pipe. my geometry is a 2D one. but when I want to export I can't find the term "profile" or sth by a ".prof" format as is shown in the picture. can anyone help me and explain what exactly I should do?

You should use File>Export>Profile
from the image it seems you are using export solution data.

Hello,
I have a similar problem. I want to import a surface velocity profile from a file and to export it on another surface of another file.
I did:
file->write->profile and I select the surface (outlet) and Velocity Magnitude, X velocity, Y velocity and Z velocity.

Then I open the other file and I select my Input surface on the Boundary Conditions. I open "Profile" and I read the file ".prof"

But after I run the calculation and I look the Contours, my Inlet surface profile is constant and the constant value of my velocity profile is the maximum value of the velocity input surface. So it takes only the maximum value and not the whole velocity profile.

How can I load the whole profile? maybe the problem is that the mesh surface are different?

Thank you for your help!

Once you import the profile each scalar is loaded as an individual variable. You still have to assign it to the the bc you want them to represent.

You have to individually select the x,y,z at the new surface and assign the corresponding velocity magnitude which is displayed in the drop down tab at the right.

Thank you Marauder, I already did it but it didn't work.

Howewer,I solved the problem doing this things:

- when I read the profile, I changed the Interpolation methods to Inverse Distance.

- in the b.c. I changed the Velocity Specification Method to "Components" and I insert only X,Y,Z velocity inlet.

- after my first iteration, to check if the inlet profile was right, I stopped iterations and in Contours I click to Auto Range.

Now I have the right profile, even if I don't know which of these 3 changes solved my problem.

Thanks for your help!

This is what solved your problem. That's what I was trying to tell in the last post. Inverse Distance helps in accurate interpolation only as far as I know.
Glad that you resolved it by yourself.

fully developed turbulent velocity profile at inlet
 

Dear friends,
I'm doing 2D-axisymmetric vertical flow boiling simulation through a simple circular pipe. For this I have to apply fully developed turbulent velocity profile at the inlet. First I run the simulation for single phase and obtained the fully developed velocity profile at outlet. My question is how this fully developed velocity profile can be correctly applied at inlet in next simulation?

Hi rampal,
I've never done a 2-D simulation, but I can explain you how I did it for a 3-D case. I think it should not be so different.
You have first to write the profile you need: File--> write--> profile, and you can select the surface where you have this profile and the quantities you need (e.g. the components of velocity).

Then, in the next simulation, when you are in the Inlet boundary condition, selecting Profile , you can Read the file that you wrote in the previous step. Then you have to Apply this profile.
At the end, you have to Edit the b.c. of the Inlet, select "Components" in the Velocity specification method and select the Inlet components (inlet x-velocity, inlet y-velocity and inlet z-velocity for a 3-D case).
If you'd like to check if your profile is a fully developed profile, you can start the simulation with only one iteration and then you can check the contours of your Inlet for example.

Dear Users,
I want to export the particle data from one case to another case.Things i am confused:confused: about is:

How should i export the data from case 1, let say i write the profile in case 1 at a desired plane having particle velocity and dpm concentration. then do i have to use DPM model in second case to further study the flow or if i use dpm model in second case how to give injection from the profile created from previous case.

Thanking You

Piyush

where to read the dpm concentrations from previous case.

This is what I'm trying to do and apparently there is no easy way to do it. You have to write an UDF using the DEFINE_DPM_OUTPUT to display or write the particle properties at your desired plane...

thank you for prompt reply.
did you figured out the problem?
however if i write udf using DEFINE_DPM_OUTPUT than how to use it further as a injection file as injection file has format like [ ((injection-0 ((type . inert) (injection-type . surface) (numpts . 1) (dpm-fname . " ") (surfaces 31 33) ].

Thanking You

Piyush

Today only posted the query at the following link and I'm stuck at compiling as interpretting is not working, have to install Visual Studio, will post the progress if I get to there...

http://www.cfd-online.com/Forums/flu...es-outlet.html

fully developed flow in the inlet
 

hi,
im trying to simulate graetz problem in fluent. for this i need to form a fully developed flow in the inlet. i tried in by importing the profile of the outlet of same dimension,same mesh specifications geometry and import in to the inlet.but this really did not work. i tried appling the specific x velocity component and the x velocity after the fully developed flow as well. but still i cannot simulate the fully developed profile in the inlet.i tries inverse distance method in interpolation as mentioned in previous thread but still the results are the same. i do really appreciate your kind help on this matter thank you.

fully developed flow in the inlet
 

Have you checked that at outlet velocity profile is fully developed ? First check this. I mean channel length should be sufficient. If you are sure that at outlet velocity profile is fully developed then write the profile for x-velocity, y-velocity at outlet. In next simulation read this profile at inlet. Change the inlet boundary condition for velocity specification method as "components" and apply outlet x-velocity for x component and outlet y-velocity for y component.

hi every body
 

How can i write the profile of two different velocity ? and then import it to my geometry with two inlets?

please help me

How can i write the profile of two different velocity ? and then import it to my geometry with two inlets?

please help me

write the profile
 

You have only one outlet or more than one outlet in your geometry.

2 inlet and one outlet

write profile
 

There is no need to write two profile. First write the profile of properties at outlet like velocity, turbulence and others, what you want to apply at inlet. Then in next simulation read this profile at inlet and apply the properties at inlet according to your problem.
You can do this by writing two different profile at outlet for inlet (i.e. for two inlet) and then apply at each inlet separately.

hope u will do this

i mean that when i want to read both profiles.the soft ware (fluent) just read the last profile that u read .

Is there a way to write UDF to automate exporting a profile at the outlet and use it as an inlet condition in the same case?

internal surface extract?
 

Is it possible to extract profile from surface which is not outlet or inlet- internal?

Yes as long as it shows up in selection menu. I have done it at interfaces etc.

Tanks for the fast reply :)

manual CFD
 

Hi guys
please i am new user for Ansys fluent
anybody could to send me manual about how to use Ansys fluent? and pls let me know how to add inlet velocity in fluent ansys?
this is my email
alburkatyhasan@gmail.com
many thanks
hasan

How to create a profile for poison in Ansys fluent
 

Hi guys!
I'm doing cfd simulate of engine.
And i want to give the velocity to the poison but idon't know how to create the external profile for giving this so ineed your help.
Please mail me the suggestion asap.
vipulparmar174@gmail.com

problems using profile as inlet boundary condition
 

Dear all,

I am trying to use an outlet profile as inlet BC for a RANS simulation (turbulence modell: Reynolds-Stress, stress-omega) in a backward-facing step using Fluent.
I have the coordinates, all velocity components, pressure, turbulent kinetic energy, turb dissipation rate, specific dissipation rate and Reynolds stresses exported from a simulation in CFX.
After reading the profile, using it in the inlet boundary condition and initializing the simualtion I checked the contours at the inlet and received the following errors:
1. x,y,z-velocities are lower than in my exported profile (e.g. max velocity in the profile file was 0.46m/s in Fluent it is now 0.4 m/s)
2. tke, sdr, tdr and Reynolds stresses are not shown as a profile but as a constant value over the inlet (this value is again lower than in the profile data)
3. Reynolds-stresses uv, vw, uw are set to 0

I have checked the coordinate system, the units and the velocity vectors, all seems fine.

Have you had this error before? Do you know what could be wrong?

This is how I do it:
1. Adapt the CFX profile to Fluent syntax
2. Fluent: Boundary conditions > Profiles > Read Profile > choose .prof file
3. set velocity inlet: velocity specification method: Components (choose x,y,z velocities from profile); turbulence specification mehtod: k and epsilon (choose k and epsilon from profile); Reynolds-stress specification method: Reynolds-stress-components (choose stresses from profile)
4. Initiliaze

Thanks a lot for your help!

Exporting an outlet profile to an inlet is not so straightforward. It sounds like you did everything right except maybe...


When you export it at the outlet, it takes the coordinates (x,y,z)'s at the outlet location. You inlet is (probably?) at a different location. Then when it interpolates from the old coordinates to the new, it causes these errors because your new locations.


If this is the case, you need to translate the coordinates at the outlet to the inlet. Either you edit the text file generated using a text editor, or you translate the mesh in CFX before you export it so that it can be read properly.

I'd like to do the same thing, creating a UDF to automate the export of the outlet profile and then using it to define the inlet at every time step. Does anyone know how to go about this?