CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

How to export velocity profile and load it as inlet condition

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree6Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   November 16, 2011, 18:40
Default How to export velocity profile and load it as inlet condition
  #1
New Member
 
Yingying Wang
Join Date: Nov 2011
Posts: 2
Rep Power: 0
wangy16 is on a distinguished road
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".
wangy16 is offline   Reply With Quote

Old   November 16, 2011, 19:47
Default
  #2
New Member
 
raj
Join Date: Nov 2011
Posts: 22
Rep Power: 6
raj.cfd is on a distinguished road
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.
raj.cfd is offline   Reply With Quote

Old   November 17, 2011, 08:13
Default
  #3
Senior Member
 
Emre G
Join Date: May 2011
Location: Turkey
Posts: 120
Rep Power: 7
emreg is on a distinguished road
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.
emreg is offline   Reply With Quote

Old   November 17, 2011, 18:29
Default
  #4
Member
 
Zachariah Swetky
Join Date: Aug 2011
Posts: 36
Rep Power: 6
swetkyz is on a distinguished road
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.
swetkyz is offline   Reply With Quote

Old   February 7, 2013, 07:19
Default
  #5
New Member
 
Oscar Albo
Join Date: Nov 2012
Posts: 1
Rep Power: 0
Alro is on a distinguished road
Quote:
Originally Posted by swetkyz View Post
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!
Alro is offline   Reply With Quote

Old   February 7, 2013, 10:23
Default
  #6
Member
 
Zachariah Swetky
Join Date: Aug 2011
Posts: 36
Rep Power: 6
swetkyz is on a distinguished road
Quote:
Originally Posted by Alro View Post
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.
Alro and haitham osman like this.
swetkyz is offline   Reply With Quote

Old   May 8, 2013, 15:26
Default
  #7
New Member
 
Heini Rasmussen
Join Date: Dec 2010
Posts: 9
Rep Power: 7
Heini is on a distinguished road
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?
Heini is offline   Reply With Quote

Old   November 8, 2013, 10:55
Default
  #8
New Member
 
Tamara Annabelle
Join Date: Jul 2013
Posts: 26
Rep Power: 5
Marabelle is on a distinguished road
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!
Marabelle is offline   Reply With Quote

Old   August 18, 2014, 07:52
Default
  #9
New Member
 
Pavel
Join Date: Aug 2014
Posts: 15
Rep Power: 3
powpawell is on a distinguished road
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!
powpawell is offline   Reply With Quote

Old   April 11, 2015, 09:55
Default
  #10
Member
 
Lida
Join Date: Apr 2015
Posts: 38
Rep Power: 3
chem engineer is on a distinguished road
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?
Attached Images
File Type: jpg Capture.JPG (83.2 KB, 161 views)
chem engineer is offline   Reply With Quote

Old   April 16, 2015, 00:19
Default
  #11
Member
 
Anonymous
Join Date: Mar 2014
Posts: 73
Rep Power: 4
marauder is on a distinguished road
Quote:
Originally Posted by chem engineer View Post
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.
marauder is offline   Reply With Quote

Old   December 15, 2015, 12:01
Default
  #12
New Member
 
Join Date: Nov 2015
Posts: 5
Rep Power: 2
peppe7 is on a distinguished road
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!
peppe7 is offline   Reply With Quote

Old   December 15, 2015, 22:53
Default
  #13
Member
 
Anonymous
Join Date: Mar 2014
Posts: 73
Rep Power: 4
marauder is on a distinguished road
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 likes this.
marauder is offline   Reply With Quote

Old   December 16, 2015, 11:54
Default
  #14
New Member
 
Join Date: Nov 2015
Posts: 5
Rep Power: 2
peppe7 is on a distinguished road
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!
peppe7 is offline   Reply With Quote

Old   December 16, 2015, 22:58
Default
  #15
Member
 
Anonymous
Join Date: Mar 2014
Posts: 73
Rep Power: 4
marauder is on a distinguished road
Quote:
Originally Posted by peppe7 View Post
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.
haitham osman likes this.
marauder is offline   Reply With Quote

Old   February 22, 2016, 09:37
Default fully developed turbulent velocity profile at inlet
  #16
New Member
 
Ram Kumar Pal
Join Date: Apr 2015
Posts: 21
Rep Power: 3
rampal is on a distinguished road
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?
rampal is offline   Reply With Quote

Old   February 22, 2016, 10:39
Default
  #17
New Member
 
Join Date: Nov 2015
Posts: 5
Rep Power: 2
peppe7 is on a distinguished road
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.
rampal likes this.
peppe7 is offline   Reply With Quote

Old   March 1, 2016, 06:11
Question
  #18
New Member
 
Piyush
Join Date: Apr 2015
Location: Kolkata
Posts: 10
Rep Power: 3
piyupant is on a distinguished road
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 is offline   Reply With Quote

Old   March 1, 2016, 06:14
Default
  #19
New Member
 
Piyush
Join Date: Apr 2015
Location: Kolkata
Posts: 10
Rep Power: 3
piyupant is on a distinguished road
where to read the dpm concentrations from previous case.
piyupant is offline   Reply With Quote

Old   March 1, 2016, 06:34
Default
  #20
Member
 
Anonymous
Join Date: Mar 2014
Posts: 73
Rep Power: 4
marauder is on a distinguished road
Quote:
Originally Posted by piyupant View Post
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...
marauder is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
how to export every data w.r.t time to txt file jaho CFX 94 August 25, 2015 09:45
How to apply velocity profile at inlet Sam CFX 12 April 1, 2012 06:52
WSS ASCII export problem Birkov FLUENT 1 July 27, 2009 14:09
Fluent UDF load and apply inlet velocity b.c. Knut Lehmann Main CFD Forum 2 June 29, 2007 04:53
applying profile data as a boundary condition vadivel CFX 1 June 9, 2007 07:11


All times are GMT -4. The time now is 04:48.