[wangy16]

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".

[raj.cfd]

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.

[emreg]

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.

[swetkyz]

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.

[Alro]

Originally Posted by swetkyz

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!

[swetkyz]

Originally Posted by Alro

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.

[Heini]

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?

[Marabelle]

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!

[powpawell]

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!

[chem engineer]

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?

[marauder]

Originally Posted by chem engineer

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.

[peppe7]

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!

[marauder]

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.

[peppe7]

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!

[marauder]

Originally Posted by peppe7

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

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

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.

[rampal]

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?

[peppe7]

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.

[piyupant]

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

[piyupant]

where to read the dpm concentrations from previous case.

[marauder]

Originally Posted by piyupant

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

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...