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

Unsteady Boundary Profile with data file

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

Like Tree6Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   August 7, 2012, 10:00
Default
  #21
New Member
 
MINNESOTA
Join Date: Aug 2012
Posts: 2
Rep Power: 0
parvin is on a distinguished road
Sponsored Links
Hi MAX

Thank you for your help.
Could you please tell me where I should write a profile, actually I'm getting confused, Should I create through define profile option in Fluent or I can creat by myself in a text format and then saved it and uploading it in fluent? Thank you so much..

Quote:
Originally Posted by -mAx- View Post
parvin is offline   Reply With Quote
Sponsored Links

Old   August 8, 2012, 00:33
Default
  #22
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 3,232
Rep Power: 34
-mAx- will become famous soon enough
in 6.3 you could create your profile as text file, or also in Fluent
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 2, 2013, 23:04
Default Udf
  #23
New Member
 
Join Date: Mar 2013
Posts: 4
Rep Power: 6
amaly is on a distinguished road
I need the UDF
amaly is offline   Reply With Quote

Old   July 3, 2013, 08:49
Default
  #24
New Member
 
Victor
Join Date: Apr 2013
Posts: 8
Rep Power: 6
VictorLP is on a distinguished road
Hello.
I have simulation divided into two steps.
To set a boundary condition as transient profile in second step i need to write this transient profile during calculation of first step. Or may be i can compose this profile, using resulting .dat files? But i can't find how to do it automatically.
I know how to write simple profile (x y z parameter1 parameter2) but it is not transient. It is very hard to open all dat files and save profiles and then compose full transient profile.

Thank in advance for all help.
VictorLP is offline   Reply With Quote

Old   March 24, 2014, 05:15
Default profile file doubt
  #25
New Member
 
amit
Join Date: Mar 2014
Posts: 13
Rep Power: 5
akjha is on a distinguished road
there is a good help on this thread, but i have a doubt
if my simulation has run for 1000s and now i want to change my pressure outlet BC by giving a profile should my first point be pressure at 1000s or i should start from 0.
akjha is offline   Reply With Quote

Old   March 24, 2014, 06:52
Default
  #26
New Member
 
Victor
Join Date: Apr 2013
Posts: 8
Rep Power: 6
VictorLP is on a distinguished road
Quote:
Originally Posted by akjha View Post
there is a good help on this thread, but i have a doubt
if my simulation has run for 1000s and now i want to change my pressure outlet BC by giving a profile should my first point be pressure at 1000s or i should start from 0.
I not fully understand what you mean. But if you have already calculated 1000s and you want to continue with new BC profile, you just can read profile with data like this for example

time
1000
2000
3000
pressure
500
700
1300

or like this if your BC was steady

time
0
999
1000
2000
3000
pressure
30
30
500
700
1300

and you can continue your calculation.
But problem is in difference between your outlet bc until moment 1000s and after. If difference is significany it may be a problem.
VictorLP is offline   Reply With Quote

Old   March 24, 2014, 06:55
Default
  #27
New Member
 
amit
Join Date: Mar 2014
Posts: 13
Rep Power: 5
akjha is on a distinguished road
i got the answer, thank you very much.
akjha is offline   Reply With Quote

Old   August 9, 2015, 14:56
Default Coordinates
  #28
New Member
 
Christian Mahr
Join Date: Aug 2015
Posts: 11
Rep Power: 4
chri is on a distinguished road
Hi everybody,
I am facing a problem including pofiles as well. I managed to create a .prof file in the correct format where I put velocity magnitudes for the use as a velocity-inlet profile. As it is a point profile, I have to give it the point-coordinates.
To which coordinate system does it refer?!
my geometry is kind of complex so the points are situated somewhere I dont really know about coordinatewise, reffering to the global coordinate system.
can I read specific coordinates out of the geometry?!

all the best,christian
chri is offline   Reply With Quote

Old   October 29, 2016, 15:24
Default help wanted
  #29
New Member
 
mike
Join Date: Oct 2016
Posts: 2
Rep Power: 0
shalamike is on a distinguished road
Hi there,

I am fairly new to ansys fluent and I need to create a tabular transient profile for a two phase flow system with fuel vapor going into a cylinder from a very small inlet. The velocity profile of the fuel is not constant as it needs to create vortex rings so adjusting for time will be the easiest way to do it.
however i don't understand all the aspects to the table form and my first try at making this table does not seem to show on user defined profiles for inlet after i read the profile.
my transient table looks like this so far

inlet 2 6 0
time velocity
0.1 0.0000008
0.2 0.0000800
0.3 0.0080000
0.4 0.8000000
0.5 0.0008000
0.6 0.0000008
(could someone also please explain what these 3 numbers next to the profile inlet is meant to represent, i know this may seem like a stupid question but have my own interpretations and i could easily be wrong)

Would this table be sufficient for two phase flow (correct format excluding the brackets)or would i have to add something extra to specify which phase this will apply to. Also could someone please instruct me on how to read this on ansys from notepad, i tried using the text command to read transient table and ansys says its reading file but nothing happens, any advice?
Any help will be appreciated.
shalamike is offline   Reply With Quote

Old   December 6, 2016, 08:02
Default
  #30
Senior Member
 
Onur Özcan
Join Date: Feb 2016
Location: Istanbul/Turkey
Posts: 424
Rep Power: 5
oozcan is on a distinguished road
how can we create unsteady tabular boundary conditions?

I could not see anywhere to write it?

time velocity
0 5
3 0
6 5
9 0
12 5
... going on so,
oozcan is offline   Reply With Quote

Old   April 30, 2017, 09:20
Default
  #31
New Member
 
Sadia
Join Date: Oct 2016
Posts: 11
Rep Power: 2
khattaksadia is on a distinguished road
Quote:
Originally Posted by person
;156255
Here is the answer to your question

Standard Transient Profiles

--------------------------------------------------------------------------------

The format of the standard transient profile file (based on the profiles described in Section 7.26) is

((profile-name transient n periodic?) (field_name-1 a1 a2 a3 .... an) (field_name-2 b1 b2 b3 .... bn) . . . . (field_name-r r1 r2 r3 .... rn))

One of the field_names should be used for the time field, and the time field section must be in ascending order. The periodic? entry indicates whether or not the profile is time-periodic. Set it to 1 for a time-periodic profile, or 0 if the profile is not time-periodic.

An example is shown below:

((sampleprofile transient 3 0) (time 1 2 3 ) (u 10 20 30 ) )

This example demonstrates the use of crank angle in a transient profile

((example transient 3 1) (angle 0.000000e+00 1.800000e+02 3.600000e+02) (temperature 3.000000e+02 5.000000e+02 3.000000e+02) )

All quantities, including coordinate values, must be specified in SI units because FLUENT does not perform unit conversion when reading profile files. Also, boundary profile names must have all lowercase letters (e.g., name). Uppercase letters in boundary profile names are not acceptable.

You can read this file into FLUENT using the Boundary Profiles panel or the File/Read/Profile... menu item.

Define Profiles...

File Read Profile...

See Section 7.26.3 for details.

Tabular Transient Profiles

--------------------------------------------------------------------------------

The format of the tabular transient profile file is

profile-name n_field n_data periodic? field-name-1 field-name-2 field-name-3 .... field-name-n_field v-1-1 v-2-1 ... ... ... ... v-n_field-1 v-1-2 v-2-2 ... ... ... ... v-n_field-2 . . . . . v-1-n_data v-2-n_data ... ... ... ... v-n_field-n_data

The first field name (e.g. field-name-1) should be used for the time field, and the time field section, which represents the flow time, must be in ascending order. The periodic? entry indicates whether or not the profile is time-periodic. Set it to 1 for a time-periodic profile, or 0 if the profile is not time-periodic.

An example is shown below:

sampletabprofile 2 3 0 time u 1 10 2 20 3 30

This file defines the same transient profile as the standard profile example above.

If the periodicity is set to 1, then n_data must be the number that closes one period.

An example is shown below:

periodtabprofile 2 4 1 time u 0 10 1 20 2 30 3 10

The following example uses crank angle instead of time:

example 2 3 1 angle temperature 0 300 180 500 360 300

All quantities, including coordinate values, must be specified in SI units because FLUENT does not perform unit conversion when reading profile files. Also, boundary profile names must have all lowercase letters (e.g., name). Uppercase letters in boundary profile names are not acceptable. When choosing the field names, spaces or parentheses should not be included.

You can read this file into FLUENT using the read-transient-table text command.

file read-transient-table

After reading the table into FLUENT, the profile will be listed in the Boundary Profiles panel and can be used in the same way as a boundary profile. See Section 7.26.3 for details.
Thank You for your insight about tabular transient udf. I'm also trying to implement it in my udf. I need to apply gaussian heat flux using temporal udf. I've calculated the heat flux for each time. I could understand by your example how to frame a particular command (tabular transient udf) but I'm unable to get how to use it.

Can you please post a complete example of udf starting from the first step (#include "udf.h") till last step i.e.
(end_f_loop(f,t)
})
using tabular transient udf.

Thanks in advance!
khattaksadia is offline   Reply With Quote

Old   May 6, 2017, 04:28
Default
  #32
New Member
 
Sadia
Join Date: Oct 2016
Posts: 11
Rep Power: 2
khattaksadia is on a distinguished road
Quote:
Originally Posted by person
;156255
Here is the answer to your question

Standard Transient Profiles

--------------------------------------------------------------------------------

The format of the standard transient profile file (based on the profiles described in Section 7.26) is

((profile-name transient n periodic?) (field_name-1 a1 a2 a3 .... an) (field_name-2 b1 b2 b3 .... bn) . . . . (field_name-r r1 r2 r3 .... rn))

One of the field_names should be used for the time field, and the time field section must be in ascending order. The periodic? entry indicates whether or not the profile is time-periodic. Set it to 1 for a time-periodic profile, or 0 if the profile is not time-periodic.

An example is shown below:

((sampleprofile transient 3 0) (time 1 2 3 ) (u 10 20 30 ) )

This example demonstrates the use of crank angle in a transient profile

((example transient 3 1) (angle 0.000000e+00 1.800000e+02 3.600000e+02) (temperature 3.000000e+02 5.000000e+02 3.000000e+02) )

All quantities, including coordinate values, must be specified in SI units because FLUENT does not perform unit conversion when reading profile files. Also, boundary profile names must have all lowercase letters (e.g., name). Uppercase letters in boundary profile names are not acceptable.

You can read this file into FLUENT using the Boundary Profiles panel or the File/Read/Profile... menu item.

Define Profiles...

File Read Profile...

See Section 7.26.3 for details.

Tabular Transient Profiles

--------------------------------------------------------------------------------

The format of the tabular transient profile file is

profile-name n_field n_data periodic? field-name-1 field-name-2 field-name-3 .... field-name-n_field v-1-1 v-2-1 ... ... ... ... v-n_field-1 v-1-2 v-2-2 ... ... ... ... v-n_field-2 . . . . . v-1-n_data v-2-n_data ... ... ... ... v-n_field-n_data

The first field name (e.g. field-name-1) should be used for the time field, and the time field section, which represents the flow time, must be in ascending order. The periodic? entry indicates whether or not the profile is time-periodic. Set it to 1 for a time-periodic profile, or 0 if the profile is not time-periodic.

An example is shown below:

sampletabprofile 2 3 0 time u 1 10 2 20 3 30

This file defines the same transient profile as the standard profile example above.

If the periodicity is set to 1, then n_data must be the number that closes one period.

An example is shown below:

periodtabprofile 2 4 1 time u 0 10 1 20 2 30 3 10

The following example uses crank angle instead of time:

example 2 3 1 angle temperature 0 300 180 500 360 300

All quantities, including coordinate values, must be specified in SI units because FLUENT does not perform unit conversion when reading profile files. Also, boundary profile names must have all lowercase letters (e.g., name). Uppercase letters in boundary profile names are not acceptable. When choosing the field names, spaces or parentheses should not be included.

You can read this file into FLUENT using the read-transient-table text command.

file read-transient-table

After reading the table into FLUENT, the profile will be listed in the Boundary Profiles panel and can be used in the same way as a boundary profile. See Section 7.26.3 for details.
Can we use the same for temporal yet steady state profile too?
khattaksadia is offline   Reply With Quote

Old   May 7, 2017, 04:18
Default Transient 3D for finite volume methods
  #33
New Member
 
SGrozny's Avatar
 
Sahidah Grozny
Join Date: May 2017
Location: Central Jakarta 10550, Indonesia
Posts: 2
Rep Power: 0
SGrozny is on a distinguished road
Assalamualaikum wr. wb
good morning,
i've problem in formula numerical analysis for my script?
if my (simulation) condition is 3D Transient at cylindrical pipe 3/4 inch.

thanks before, Have a good activity guys.
SG
SGrozny 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
Getting Time Series data from saved unsteady data Atul FLUENT 4 November 26, 2008 06:12
applying profile data as a boundary condition vadivel CFX 1 June 9, 2007 07:11
file/write-profile ... journal file MM FLUENT 5 November 30, 2006 04:07
2D setup and 2D profile data file in CFX10 Se-Hee CFX 3 October 30, 2006 10:49
Profile Data Velocity Boundary Condition Changes?? Maria Angelica CFX 9 June 14, 2006 02:44

Sponsored Links


All times are GMT -4. The time now is 03:18.