CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Unsteady Boundary Profile with data file (http://www.cfd-online.com/Forums/fluent/50373-unsteady-boundary-profile-data-file.html)

Arianna January 23, 2009 10:32

Unsteady Boundary Profile with data file
 
Hi there,

I'm working with an unsteady case and I need to set some boundary conditions by using a file data, every line of this file should contain the flow time value and the linked boundary value.

Is it available a function to load this file with somethingh like DEFINE_PROFILE, or I have to write some code on my own..

Any help will be really appreciated!!!

Thanks in advance,

Arianna


person January 28, 2009 13:12

Re: Unsteady Boundary Profile with data file
 
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.


jackmarlowe November 4, 2009 02:32

Unsteady Boundary Profile with data file
 
Hi,
I have a similar problem. I am trying to solve a pipe flow problem in fluent 6.3.26.
I have a transient pressure data which I read through
file>>read-transient-table
command.

My question is,
Does fluent read the time data according to the order of data given or does it read it according to the timestep I give?

Ex:
-------------
pre 2 5 0
time pressure
2 20
4 25
6 30
8 35
10 40
-------------
It is normal to give time step size (s) = 2 for this configuration, yet I start my iterations giving time step size (s) = 1, and it solves something. How does it solve it, does it interpolate?
And finally, if I give time step size (s) = 4 will it take 25 Pa for the first time step?

Thanks.

-mAx- November 4, 2009 06:53

If the transient table works like the profile, then fluent just makes linear interpolation.
Since you don't give any value at time 0, I assume fluent will start at time 0 with a pressure of 0.
Then between time 2 and 4, fluent rises the pressure from 20 to 25 (linear)
So as you understand, it is not time step.
There are just reference points.

jackmarlowe November 5, 2009 03:52

Unsteady Boundary Profile with data file
 
Hi Max,
Thanks a lot for your answer. It sounds very reasonable. It is probably the right answer to it yet, I wonder if there are any user manual/tutorial references to it.
Btw, I crop my data according to the timestep I use, adding the zeroth timestep value of pressure to the beginning and solve my problems. But it is a long and clumsy way.

-mAx- November 6, 2009 00:56

Check Help Chapter 7.26.2 "Boundary Profile File Format".
If the pressure doen't change non-linearly with the time step, you don't have to describe the profile with your time-step increment.
If it is a long way, as you mentionned, you may try a udf for desribing your inlet BC (Chapter 8.2.1 Boundary Conditions from UDF Help)

davesmith_01 October 11, 2010 12:10

setup local axis rotation for blades?
 
Hi

I am trying to write a transient data file for rotation of helicopter blades (4 blades) inclined at a plane. The rotation needs to take place around an inclined planed so I have created a local axis in gambit at 25deg (with rotation about the z axis, so the y and x axis have moved out of poisition compared to global axis).

So it has all been setup in gambit and the active axis is the local axis. But when I put this in fluent and install a udf for rotation about x axis it starts to rotate the blades around the global x axis rather than the local x axis which is what it should be using. I dont understand how to set in fluent that rotation needs to be around the local x axis?

If I write a transient data file then I want to write something like this
sampledata 10 1
time thetax thetay thetaz
0 0 0 0
1 4 25 0
2 8 25 0
and so on

I have only selected 25 for theta y as the inclined plane is 25deg to the vertical axis, is this the correct way for writing this file?

Please advise

Any advice regarding this would be helpful

Dave

-mAx- October 12, 2010 02:01

if you only need the local axis, then translate and rotate your domain untill local axis reach global one.
For instace if your local axis has a translation vector (1 0 0) and a 45-rotation about (0 0 1), then move all your domain with translation vector (-1 0 0) and a 45-rotation about (0 0 -1).
Just check that origine (0 0 0) match origin from your "previous" local axis

davesmith_01 October 12, 2010 04:45

Thanks for helping Max. The local axis in gambit is set at 25deg, but when I save the mesh file, the local axis is not saved (when I opened that msh file in gambit again, I couldnt see the local axis, I think thats why fluent does not see it). In your idea are you saying that I should rotate the grid by 25deg and the carry out the blade rotation around the x axis?

But can I still take Lift (vertical direction) and Drag results (horizontal direction)? As the grid has now been turned can these readings be taken as usual, or do I need to work out the angle and then calculate lift force?

Also what I want to know is if I rotate the entire grid by 25deg so the blade rotation is about this angle (so essentially, rotation is about the x axis, but the plane is inclined at an angle of 25deg, thus rotation is about the x axis and a constant rotation about y axis can be said to take place as the blade will be moving in a forwards direction whilst moving downwards), and when lift a dn drag measurements are taken are they also taken at this plane (25deg angle, as the entire grid has been rotated) or do they just stay as they were and take readings along the vertical (lift) and horizontal (drag) directions?

Sorry about the long reply. Again thank you for helping all suggestions are welcome I really need help on this and understanding if the force measurements are affected at these planes

Dave

-mAx- October 12, 2010 05:01

post a sketch because it's hard to imagine...
Fluent recognizes (as far as I know) only the global axis in gambit.
So if you only needs the local axis, move your domain untill the top-level axis (global) matches your local one.
In other words, if you need 2 differents local axis, then I don't know.
But maybe there are workarounds, like moving your domain during post-processing. (compute force with global axis, then translate/rotate your grid and re-compute force on your other body)

davesmith_01 October 20, 2010 10:04

rotation about local axis
 
Hi Max

Sorry I have replied late. I have tried rotating the grid in fluent but unfortunately by rotating the grid the global axis remains constant and any rotation you chosse about the x axis will be performed around the global x axis.

What I want is that a local axis is created at an inclined plane(rotate global z axis by 30deg) and a local axis is now created. This does not happen by rotating the grid using fluent options.

I have attached a picture, what I want is to rotate the helicopter blade around the X1 axis (red axis, as this is the inclined plane). The first image(left side) shows all the blades on the x axis, the second image is more clear as it just shows one blade, now this blade needs to be rotated around the local X1 axis only, and it will then be rotating like a helicopter blade but at an inclined plane.

My question is how can I create this in fluent as everytime I incline the plane to create a local axis this does not work, thus I can try and use the global axis which fluent works in and have a transient boundary profile like that shown below. But I need to have components of theta_x , theta_y and theta_z.

For global axis
sampletransient 2 4 1
time theata_x theta_y theta_z
0 0
0.01 0.5 30 0
0.02 1 30 0
0.03 1.5 30 0
etc

(theta_y has 30deg so that the plane can be continuosuly inclined at 30deg)

Can a transient boundary profile be setup like this?

Or if the local axis can be setup I can have something like this, shown below (but the transient boundary profile may not be written in the correct format as I do not know how to introduce variable theta _x, theta_y and theta_z.

For local axis
sampletransient 2 4 1
time theata_x theta_y theta_z
0 0
0.01 0.5 0 0
0.02 1 0 0
0.03 1.5 0 0
etc


Can something like this be written, how can I put the theta values in a transient profile, an example is given for crank angle but how can you display the theta values in the transient boundary profile?

Can anyone offer any help aswell?

davesmith_01 October 20, 2010 10:07

1 Attachment(s)
P.S I am sorry about the very long message above I wanted to be as clear as possible pictures are attached to this post

-mAx- October 22, 2010 02:15

I never did that, and maybe there is a trick (which I ignore)
But I would split your calculations in 2 phasis. First you compute with blades rotating around x-axis (end of first calculation)
Read case and data at latetest Timestep, and rotate the grid as I mentionned earlier (don't know where is the problem). So you go in Grid/rotate, and set the rotation around z-axis (according to your sketch). Now your axis is (O x1 y1 z)
Second you compute with blades rotation around the new x-axis (x1 in your sketch).

davesmith_01 November 10, 2010 13:41

Hi Max

I have left the other problem for now as it is taking a long time to solve. I have another question. I am using dynamic meshing for my rotor blade, can I use dynamic meshing in Fluent for a structured grid?

If yes, what type of structured grid would work?

Also is layering and remeshing required if I use a structured grid?

The mesh will have to remesh is this even possible in fluent to remesh a structured grid?

In addition does it matter which software I use to grid my model, I usually use Gambit or Turbo grid?

And as a questions for CFD physics, what are the actual advantages of using a structured grid compared to an unstructured grid?

Thanks

Dave

-mAx- November 11, 2010 01:43

smoothing and remeshing can only be used with tetra.
You can use Layering with hexa (or wedge)
...
advantage of hexa: more accurate, and generally hexa-grid will ask less cells in comparison with tetra
disadvantage: will ask more time to generate the grid

davesmith_01 November 11, 2010 09:53

Hi Max

I have another question. I can write a UDF for the 4 blade rotor motion which is fine and the forces produced are good, but there is also methods for transient table or profile that can be used. When I put a column for time and another for theta_x (as rotation is about the x axis), the forces produced for this simulation are not good at all. Thus the forces produced for the UDF simulation are good and using the same parameters and settings, the forces produced whilst using transient table or profile are not good at all, they actually look completely wrong. Have you ever encountered this? Please advise what I can try, and what I may be doing wrong.

Thanks

Dave

-mAx- November 12, 2010 01:14

no idea since I don't have your data. You need to investigate.
are your pressure distributions on blades ok?
compare your wrong values, with the right ones (but computed in the global axis)
etc...
this is debugging and it's a part a CFD
;)

sheikh nasir February 27, 2012 22:06

Please help me
 
hello,
i am working on fluent 6.3.26 , i am trying to solve the unsteady problem of train moving in tunnel. i am not able to solve that . can any body help me . my email is sheikhnasir39@gmail.com
thanks:confused:

parvin August 6, 2012 21:09

Requesting help in Fluent
 
Hi Max

I have a data set in excel and I would like to have this data as a boundary condition of one of walls as a input flux. I'm a beginner in Fluent and I don't know ho to rite a UDF or create profile, Could you help me with this problem,Thank you so much.



Quote:

Originally Posted by -mAx- (Post 278771)
post a sketch because it's hard to imagine...
Fluent recognizes (as far as I know) only the global axis in gambit.
So if you only needs the local axis, move your domain untill the top-level axis (global) matches your local one.
In other words, if you need 2 differents local axis, then I don't know.
But maybe there are workarounds, like moving your domain during post-processing. (compute force with global axis, then translate/rotate your grid and re-compute force on your other body)


-mAx- August 7, 2012 01:25

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


All times are GMT -4. The time now is 14:02.