[ehecboy]

Hey guys,
im currently working on my master thesis. Im simulating a combustion which needs a lot of time. Therefore I want to export a Profil in fluent, which includes the x-, y-, z-coordinates, velocities and temperature at a certain plane at every timestep. This Profil should be used in another case as boundary condition.
Is it possible to get these informations in just one file?

Thanks for helping
Simon

[vinerm]

Doable but not using standard approach. However, how do you plan on using merged profiles?

[ehecboy]

My idea is that I first simulate the entire combustion chamber and then cut out a cuboid and then only calculate this new small region. For this I need the time-dependent boundary conditions of the cuboid's walls.

I tried a execute command, that writes every second a Profil. But the problem is, that this file has a constant name and after every second fluent wants to overwrite or cancel the new data.

my execute command:

file/write-profile/ profil-name interior-fluid_domain() temperature

What is your suggestion?

[vinerm]

You cannot apply time-dependent profile using profile files. Profiles are either time-dependent or space-dependent, not both. So, you need to export profiles separately for each time-step. Modify your command to include time-step in the file name. So, instead of using profile-name, use profile-name_%t. %t is automatically replaced by time-step and you will end up having a lot of different profile files.

[ehecboy]

Perfect, it worked thanks a lot

And what would be the smartest way to read these files?

also a execute command which reads and sets the boundary condition after every second?

[vinerm]

Yes, you can read it same way. You only need to set bc once. After that, just keep on reading profiles every time-step. No need to set the bc again.

[ehecboy]

Thanks a lot for helping.

To read the files the same way didnt work. When I want to read the file: name_%t, fluent says that the file does not exist

[vinerm]

%t and %i can be used for writing but not for reading a file. You have to use scheme command to read those files.

(ti-menu-load-string (format #f "file read-profile name_~04d.prof" (rpgetvar 'time-step)))

where you need to replace name_ with actual basename. 04 specifies number of 0s before value at the end. So, if the file name is name_0003.prof, then the command above will read it. If it is 00003, then use 05 in place of 04.

[ehecboy]

Thank you, it worked

I see there is so much more to learn in fluent

[hassanayaz]

Hello
i am working on gas-solid fluidization and want to save volume fraction of solid for each second. How it can be done in fluent kindly help me.

[vinerm]

For that, you don't need anything special. Just setup a volume monitor under Report Definitions. However, in a fluidized bed, you don't expect solid volume fraction to change.

[hassanayaz]

Hello!
I want to know how to calculate RMS of bed pressure fluctuations in fluidization bed during simulation using Ansys Fluent?????????

[vinerm]

RMS values over space or over time. If it is over time, then you need to run transient simulation with statistical sampling enabled. Then, Fluent will directly report RMS and mean values. If you have already run a transient simulation and did not enable sampling, but you have saved intermediate files, then you can determine RMS manually or using CFDPost.

[hassanayaz]

Thank you Vinerm
actually i am beginner on Ansys fluent and i have assigned a task to plot a standard deviation (pascal) vs superficial gas velocity(independent variable) in fluidization column. someone said it is rms bed fluctuation, so kindly guide me can it be rms value or something else..... also tell how standard deviation can find using fluent.

[vinerm]

Yes, rms and standard deviation are same. However, you need data to determine that. And data collection requires transient simulation. Once you setup a transient simulation, Fluent has an option under Run Calculation to enable sampling. Once sampling is enabled, RMS values are available for post-processing once the simulation is complete.

[hassanayaz]

How can i calculate slip velocity in fluidization colunm using fluent cfd??? guide in detail with steps.

[vinerm]

Just take a difference of velocities of primary and secondary phase.

[hassanayaz]

How i can judge that in fluidization steady state is reached or not doing simulation on Ansys Fluent

[vinerm]

If it is steady, it is not fluidized. Fluidization is an inherently unsteady phenomenon. However, you can certainly look at statistical steadiness. For that, you can look at various fields, such as, average velocity of solids or the average height of fluidized zone. If these fields are varying with a certain frequency, then you can consider the fluidization to be statistically steady.

[hassanayaz]

Hello
i want to create a custom field function for the slip velocity in ansys fluent can any body guide me in detail??? what values will use etc