How create and use Profile txt file as a boundary condition in FLUENT?

José MantovaniJosé Mantovani São Paulo, BrazilMember

Hello guys!

I need to create a txt file (velocity profile) to use as boundary condition in 2D simulation using FLUENT. Look, this is not a UDF, this is a txt file... Someone can help me? With some file model or video tutorial? I need know how to create ths file with velocity profile and turbulence information. 

The archieve: 

Re_delta* = 1000, Re_theta = 670, Re_delta+ = 325.

 

Mean and mean-square fluctuations:

  J    y/delta      y+           U+         uu+          vv+         ww+        uv+

  1  7.9361E-04  2.5864E-01  2.5869E-01  1.0687E-02  7.7580E-07  4.8148E-03 -2.0170E-05

  2  1.9512E-03  6.3591E-01  6.3602E-01  6.4130E-02  2.4659E-05  2.6552E-02 -3.0967E-04

  3  3.6251E-03  1.1814E+00  1.1811E+00  2.1866E-01  2.4991E-04  8.0063E-02 -2.0531E-03

  4  5.8172E-03  1.8958E+00  1.8922E+00  5.5397E-01  1.3473E-03  1.7426E-01 -8.6438E-03

  5  8.5301E-03  2.7800E+00  2.7618E+00  1.1537E+00  4.8586E-03  3.0742E-01 -2.6780E-02

  6  1.1767E-02  3.8349E+00  3.7697E+00  2.0565E+00  1.3253E-02  4.6777E-01 -6.5352E-02

  7  1.5532E-02  5.0619E+00  4.8781E+00  3.1983E+00  2.9468E-02  6.4116E-01 -1.3083E-01

  8  1.9829E-02  6.4624E+00  6.0319E+00  4.4055E+00  5.6196E-02  8.1625E-01 -2.2210E-01

  9  2.4664E-02  8.0381E+00  7.1703E+00  5.4726E+00  9.5323E-02  9.8598E-01 -3.2983E-01

 10  3.0043E-02  9.7910E+00  8.2412E+00  6.2592E+00  1.4761E-01  1.1473E+00 -4.4081E-01

 11  3.5972E-02  1.1723E+01  9.2108E+00  6.7224E+00  2.1258E-01  1.2962E+00 -5.4343E-01

 12  4.2459E-02  1.3837E+01  1.0065E+01  6.8949E+00  2.8851E-01  1.4285E+00 -6.3084E-01

 13  4.9512E-02  1.6136E+01  1.0806E+01  6.8461E+00  3.7247E-01  1.5420E+00 -7.0102E-01

 14  5.7140E-02  1.8622E+01  1.1444E+01  6.6460E+00  4.6087E-01  1.6344E+00 -7.5503E-01

 15  6.5353E-02  2.1299E+01  1.1993E+01  6.3545E+00  5.4993E-01  1.7056E+00 -7.9554E-01

 16  7.4163E-02  2.4170E+01  1.2468E+01  6.0193E+00  6.3615E-01  1.7579E+00 -8.2536E-01

 17  8.3581E-02  2.7239E+01  1.2881E+01  5.6693E+00  7.1679E-01  1.7923E+00 -8.4677E-01

 18  9.3621E-02  3.0511E+01  1.3244E+01  5.3236E+00  7.8985E-01  1.8123E+00 -8.6175E-01

 19  1.0430E-01  3.3990E+01  1.3568E+01  4.9960E+00  8.5407E-01  1.8233E+00 -8.7156E-01

 20  1.1562E-01  3.7682E+01  1.3860E+01  4.6921E+00  9.0905E-01  1.8261E+00 -8.7708E-01

 21  1.2762E-01  4.1591E+01  1.4128E+01  4.4171E+00  9.5483E-01  1.8214E+00 -8.7964E-01

 22  1.4030E-01  4.5724E+01  1.4378E+01  4.1732E+00  9.9176E-01  1.8116E+00 -8.8001E-01

 23  1.5369E-01  5.0088E+01  1.4614E+01  3.9555E+00  1.0206E+00  1.7961E+00 -8.7819E-01

 24  1.6781E-01  5.4689E+01  1.4840E+01  3.7628E+00  1.0416E+00  1.7765E+00 -8.7484E-01

 25  1.8268E-01  5.9536E+01  1.5058E+01  3.5919E+00  1.0552E+00  1.7538E+00 -8.7022E-01

 26  1.9833E-01  6.4636E+01  1.5272E+01  3.4352E+00  1.0625E+00  1.7273E+00 -8.6393E-01

 27  2.1479E-01  7.0000E+01  1.5485E+01  3.2932E+00  1.0640E+00  1.6968E+00 -8.5582E-01

 28  2.3208E-01  7.5636E+01  1.5697E+01  3.1666E+00  1.0601E+00  1.6632E+00 -8.4605E-01

 29  2.5025E-01  8.1556E+01  1.5910E+01  3.0517E+00  1.0511E+00  1.6253E+00 -8.3476E-01

 30  2.6932E-01  8.7772E+01  1.6122E+01  2.9443E+00  1.0375E+00  1.5822E+00 -8.2158E-01

 31  2.8935E-01  9.4298E+01  1.6337E+01  2.8398E+00  1.0193E+00  1.5347E+00 -8.0567E-01

 32  3.1036E-01  1.0115E+02  1.6554E+01  2.7352E+00  9.9673E-01  1.4822E+00 -7.8731E-01

 33  3.3242E-01  1.0833E+02  1.6772E+01  2.6334E+00  9.7044E-01  1.4264E+00 -7.6688E-01

 34  3.5557E-01  1.1588E+02  1.6993E+01  2.5305E+00  9.4086E-01  1.3701E+00 -7.4344E-01

 35  3.7987E-01  1.2380E+02  1.7219E+01  2.4191E+00  9.0780E-01  1.3111E+00 -7.1651E-01

 ....

It's just to everyone see how is the archieve which I have. 

Thank's.

Mantovani. 

«1

Comments

  • KremellaKremella Admin
    edited August 2018

    Hello Jose,

    Just to give you a quick resource for you to move forward, please have a look at Section 6.6.2 'Profile File Formats' (Fluent Users Guide, R18.2). This should help you get started. I am copying an example from this section here.

    In short, you have to specify x, y, and z coordinates, along with the physical quantities you want to input as profiles.

    I hope this helps.

    Best Regards,

    Karthik

  • José MantovaniJosé Mantovani São Paulo, BrazilMember
    edited August 2018

    So, I found the same image in FLUENT user's guide. But, In just one file I can input all? Or I need create one file for velocity, one for turbulence parameters...?

    And, the file I have is up. It is not complete ... Should I do like? Do I use the y value and relate it to velocity? I do not know how to start ...

    Is there any video tutorial on this? If it does not exist as soon as I can do it, I'll create one because I think it's very useful. This method for this kind of case seems to me much faster and easier than UDF.

    If I want input this in a inlet boundary of my 2D computational domain in beginning of file I need read:

    (vel-prof line) ? Like this?

    Thank's.

    Mantovani. 

  • KremellaKremella Admin
    edited August 2018

    Hello Jose,

    I have a quick dirty way. Please write out a profile file of the parameters you want to create from an existing simulation. Open this written file in excel. Change the values of the physical parameters (do not change the x, y , z coordinates) and modify it according to your use. Then save it as a profile file and use it for your simulation.

    To illustrate this: say I want to create a profile for velocity and I already have my mesh file. I will write out a profile file (by setting up a constant velocity BC in Fluent). I will read this file in Excel and will not touch the coordinates. I will just modify the velocity values (say using an analytical expression) to reflect the new values I want to use for my simulation. I will then save this excel sheet as a new profile file 'new_vel.prof' and read this new file into Fluent for my latest calculation. 

    I am not sure if there is a video tutorial, but this would make an excellent resource. Please let me know if you have any additional questions about this.

    Thank you.

    Best Regards,
    Karthik

  • José MantovaniJosé Mantovani São Paulo, BrazilMember
    edited August 2018

    Thank you Kremella, I should thank ... Wait some minutes, I will try in this way.

    Yes, I already have the mesh ready, and I have the data for the velocity profile and turbulence parameters in a txt file. I want to just format in the FLUENT pattern so that I load this as inlet condition of my 2D domain. I'll try as you say.

    I already told you, it worked.

    Thank's.

    Mantovani. 

  • José MantovaniJosé Mantovani São Paulo, BrazilMember
    edited August 2018

    Kremella, How Can I write out a profile file of the parameters which I want to create from an existing simulation? To use this file for change for the values which I want... I need get this at FLUENT in BC sets? 

    Can someone do this for me? Should I make the file available here?

  • KremellaKremella Admin
    edited August 2018

    Hello Jose,

    Here is how you might want to write your profile files.

    You can then select the boundary and the physical parameters you want to write. Is this what you are asking?

    Thank you.

    Best Regards,

    Karthik

  • José MantovaniJosé Mantovani São Paulo, BrazilMember
    edited August 2018

    Yes, thank's Kremella, I will try. 

  • José MantovaniJosé Mantovani São Paulo, BrazilMember
    edited August 2018

    Kremella for me, doesn't appear this 'profile' option... See in the image below.

    I don't know, Why... 

  • KremellaKremella Admin
    edited August 2018

    Jose,

    Did you load the mesh, set-up your model, initialize, and run a few iterations of the model (perhaps?)? If you are interested in a velocity profile, I'd set-up a velocity inlet condition with constant velocity and run a small steady-state simulation for a few iterations. Please try this and let us know what you find.

    Thank you.

    Best Regards,

    Karthik

  • José MantovaniJosé Mantovani São Paulo, BrazilMember
    edited August 2018

    Ok, just wait some minutes I will try. I tried in a file which simulation was already done... I will try in a new file. 

  • José MantovaniJosé Mantovani São Paulo, BrazilMember
    edited August 2018

    Kremella, I got it. But I make this in other way. Instead of going through the Write path ... I was in Export ... -> Profile ... -> so opening the window seen in the image below.

    But for me to have the input file with the turbulence parameters beyond the velocity magnitude, should I select which other values? I would like in just one file to compute everything (velocity profile and turbulence parameters) so I change to the values of non-uniform velocity profile and use as boundary condition in another simulation.

    When clicking Write ... I got a .csv file with just the spatial values for x, y relating the velocity magnitude. As I've been, I should now change only the velocity values, but I need to enter the turbulence parameters ... How to have a file with profile and turbulence parameters, so I can change this values.

    Really thank's for helping, attention and mainly PATIENCE... 

    Mantovani. 

  • José MantovaniJosé Mantovani São Paulo, BrazilMember
    edited August 2018

    The file with inlet parameters which I have, The file have this parameters see in image below:

     So I need generate a file with this values. Or with just velocity profile and dissipation and production maybe... What do you think about it? Perhaps turb diff, visc diff, advection and sum need not be imputed.... 

  • brbellbrbell Member
    edited August 2018

    Hi Mantovani,

    I saw your post in the other thread but then I saw this thread and it seemed a better place to reply.

    In the picture from two posts ago, select Velocity Magnitude, Turbulent Kinetic Energy (after scrolling down a bit) and Turbulent Dissipation Rate (epsilon).  It is probably easiest to use .csv format after you click Write and it asks you for the file name.  It is easy to open in Excel, replace the numbers written by Fluent in the .csv file with numbers from the data and re-save in .csfv format.

    Be careful with the data you are showing, because they are scaled (y+,u+) and will need to be converted back to physical dimensions (y,u) based on u_tau and nu from the experiment.  The uu+,vv+,ww+ values are also scaled and need to be converted to uu,vv,ww to get physical turbulent kinetic energy.  

    I would probably use the definition of turbulent viscosity to extract a value for epsilon from the data, as in the attached image.  The mean velocity gradient can be computed from the values of u and y.  

     

  • KremellaKremella Admin
    edited August 2018

    Hello Jose,

    If you are going to be using Velocity inlet boundary condition (along with, say, k-eps turbulence model), there are only a certain number of parameters you input into your simulation. If you open the velocity inlet BC panel, you would see all your options:

    • Velocity magnitude (or you can specify as x, y, and z components of velocity)
    • Turbulent kinetic energy (k) and Turbulent Dissipation rate (eps)

    You can write them all into a single file, open this file, make modifications, and reload the file into another set of simulation. 

    Other options such as turbulent intensity and hydraulic diameter are generally a single number input. You will have to convert your data to these input quantities and use the profile files to input them into Fluent as a velocity inlet condition.

    Again, your inputs depend on what kind of boundary condition you are planning on using and what Fluent allows. It also depends on what your analysis is meant for. Hope this answers your question.

    Thank you.

    Best Regards,

    Karthik

  • brbellbrbell Member
    edited August 2018

    Hi Karthik,

    I didn't know you were posting at the same time as me.  Sorry for any confusion I might be causing.  I will go silent from here.

    Regards,

    Brian

  • José MantovaniJosé Mantovani São Paulo, BrazilMember
    edited August 2018

    Any help are welcome! Thanks Kremella and Br Bell, one answer completed the other. Without the mathematical part that indicated by Br Bell and Kremella's comment regarding the process I would not be able to, since I thought the data in my file were already ready to be used. And from what Br Bell said, no, I need convert to physical dimensions. 

    Many thanks guys, without you would be very difficult. I will try to make the file and run, working I have the results here tomorrow, or another doubt hahahaha.

    Thank you so much, Kremella and Br Bell, from the bottom of my heart!

    Mantovani. 

  • José MantovaniJosé Mantovani São Paulo, BrazilMember
    edited September 2018

    Hello Br Bell!

    Just today I had time to see this, I make other projects. 

    So Can you give me some help? 

    I caugth the profile txt file from a ANSYS FLUENT solution to change the parameters as we discussed through this thread. So here I have a file with y, U, V, k and eps from FLUENT. From what we discussed I think I need replace the values of U and V correlating with the y values. In image below have the last data that I said to you and you checked Br Bell. I need multiply the y/h column per h value to return to y dimension and the values u', v', w' multiply by Uo do return to true values, as you said. But, my doubt is: in txt profile that I got in FLUENT have the values of k and eps and not to u', v', w'. Below have image of values that I said.

    According to the literature the formula to k is k= 1/2 (u'^2+v'^2+w'^2) so I need correlate for first y value the values of first line of "column 1" (already multiplied by Uo) and add them (sum) and multiply by 1/2, its correct? And another doubt is about epsilon, How is the formula of epsilon? If I use the formula that you posted I need the values of Cmhu and vt and I think this way is more complicated, have other way to get the epsilon values? Or, how to get a file from FLUENT with the values separated? There's a possibility? Maybe a txt file from a LES solution?

    Thanks for helping. I'm waiting here.

    Mantovani. 

     

  • brbellbrbell Member
    edited September 2018

    Hi Mantovani,

    What you suggested for K sounds like it is correct.  I would copy the u', v', and w' columns in Excel, create new columns with (u'*Uo)^2, (v'*Uo)^2 and (w'*Uo)^2 and then one more column with 1/2 * sum of the three new columns.

    Concerning epsilon, it is always complicated.  That is one reason I prefer just to do an auxiliary calculation of the boundary layer and get the profiles from the CFD simulation.  I think there might have been dissipation values reported in one of the references that have been noted in this thread or the other thread, but even so they would probably use a different normalization than the ERCOFTAC website data in your above post.

    The standard value for c_mu is 0.09 and that is more than sufficient to use for estimation of epsilon.  The value for nu_t can be computed from u'v' and dU/dy using the formula from a few posts above this.  The u'v' is in column 7 from the data  (would have to be multiplied by Uo^2 to have correct units) and dU/dy can be calculated from U and y.

    I will be on vacation for a couple of weeks.  I will check in when I get back.

  • José MantovaniJosé Mantovani São Paulo, BrazilMember
    edited September 2018

    Hello.

    So, as we can see, tried to make this and  is a very difficult. By this, I make some study of profile velocity behavior in FLUENT by a uniform velocity profile at inlet and I get this in image below. I created, as have the image in thread of BFS, a inlet channel of 10h with h= 0.0098 m and the inlet have a length of 5h. So, 10h is insuficient to developing (Think that 10h is 2 times length of inlet length), and for a same 20-30 times the inlet length the profile is not developed. 

    So I create just the inlet channel with 5h of inlet length (named as D) and with 50D of length and I get the profiles for different stations as we can see in image below. Now I can test some profiles as inlet of my domain of the BFS thread.

    The profile at x/D =50 used as inlet in the domain BFS, which inlet duct have 10h, we have more length to this profile develop until the step. I will try to make this and soon I share results here. 

    I wanted share this here, because can be useful for someone.

    Mantovani. 

  • KremellaKremella Admin
    edited September 2018

    Hello,

    Thanks for sharing this. You should totally write a short report on your findings and experience on solving the BFS problem and share it here. It would be a useful resource for someone who might be looking to understand the various models.

    Best Regards,

    Karthik

Sign In or Register to comment.