[parvin]

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..

Originally Posted by -mAx-

check online help
http://aerojet.engr.ucdavis.edu/flue...ug/node303.htm

[-mAx-]

in 6.3 you could create your profile as text file, or also in Fluent

[amaly]

I need the UDF

[VictorLP]

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.

[akjha]

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.

[VictorLP]

Originally Posted by akjha

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.

[akjha]

i got the answer, thank you very much.

[chri]

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

[shalamike]

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.

[oozcan]

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,

[khattaksadia]

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]

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?

[SGrozny]

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

[ujwal rajan]

Hey guys,

I am using fluent and matlab to run a fluid structure interaction over an airfoil. I am making use of matlab to feed all the commands into fluent and perform the necessary actions.

I have to input the profile for a gust of wind at the inlet (which is a pressure-farfield) in my case.

i have used the following command in matlab to input the gust:
fprintf(fid,'(ti-menu-load-string "file interpolate read-transient-table " "
\\n")\n');

However, i do not know what to fill in after using the command read-transient table. Also, how do i specify on what zone the profile has to be used in??

Any help is massively appreciated!
Thank you!

[madmechanic]

Hi, I am also trying to use a transient tables to apply my boundary condition. However when I type in the following commands into the ansys console
file

/file>read-transient-table
transient-table file name [] (insert name)

ANSYS displays the error shown below. I made file on wordpad using the correct format and saved with txt extension. I saved the file to my desktop. Can you help me with this?

Error: File "insert name" not found!
Error Object: #f