[Vinoo_P]

Hi everyone i want to run a shock tube simulation case to verify if the data can match experimental data from our lab. What boundary condition do i assign to the diaphragm of the shock tube in Fluent? Ive tried interior, symmetry and internal but they dont work. Please help. Thx.

[agd]

Don't use a BC - set the initial distributions of density, temperature, and pressure as if the diaphragm is there (i.e. step in pressure and density with constant temp across the diaphragm is the normal setup). Then let the simulation run. You are simulating the situation where the diaphragm is instantly removed from the system, so no BC for the diaphragm.

[Vinoo_P]

Ok I will try that right away

[alikami]

can u mail me ur case file....a1k1s1@yahoo.com
thanks
regards

[vchhabra18]

Hi everyone here,

I just this post after searching for the same question for such a long. Even I am doing an MSc project on a shock tube and not too sure how to go about the diaphragm.

'agd' Your suggestion sounds very promising but to be honest, I am not too clever in fluent so would you mind just expalining the same thing a little more. It'll be of great help if you can please.

And Vinoo if you understood what agd was explaining and you tried that method too, than again it'll be very helpful if you could send me your case file to have a better idea.

Many thanks in advance

I will be waiting for the replies
Best Regards

[agd]

Let your tube be length L. From 0 to L/2 initialize your field as (p1,T1,rho1,u1=0). From L/2 to L, initialize the field as (p2,T2,rho2,u2=0). Run simulation for some time length, post-process results.

[vchhabra18]

Thanks a lot AGD for your prompt reply. I guess I know what you mean now. I will try this out tmrw or day after and will get back if any more issues will come up.

I hope you would not mind helping me out than as well.

Many thanks once again
Best Regards
Vivek Chhabra

[praveen2008]

Hi,

can anyone tell me if i could model a shock tube simulation using ansys design modeller, ansys meshing and ansys fluent??? and if someone could send me a case file to praveen2008@gmail.com just to get a glimpse of the problem as I am new to ansys. It would be a great help if someone could help with how to define the diaphram and how to give the boundary conditions.

Please Help

Thankyou

[esikhatar]

Dear agd,
How we can do this initialize in the Fluent?
I cann't do that! :-(
Can you please send me a case file?
Thanks
zztnshn_2@yahoo.com

Originally Posted by agd

Let your tube be length L. From 0 to L/2 initialize your field as (p1,T1,rho1,u1=0). From L/2 to L, initialize the field as (p2,T2,rho2,u2=0). Run simulation for some time length, post-process results.

[agd]

I'm sorry, but I do not use Fluent. Perhaps someone else can supply the case file you are looking for.

[moein_joon27]

Hi Everyone

Here's my solution to your problem in initializing fluent with separate values and simulating a shock tube. I have tested it, I have got the results and I am sure it works properly.
you need a very simple grid which should be like a 2D rectangle. you don't need to separate it or create 2 zones. A simple 1-zone grid will work just fine. we will try to initialize that zone with different values.

suppose the problem says the parameters ( as an example ) are as the case in Hirsch's book:

length of tube=10 m.
width of tube is not important ( because the problem is actually one dimensional when considered inviscid ) i.e. give the width as you wish!


Left:
Pressure=100,000
density=1.
velocity = 0

Right:
Pressure=10,000
density=0.125
velocity = 0

you should introduce the UDF mentioned below to fluent. Save it to a text file:


#include "udf.h"

DEFINE_INIT(moein_shock_tube_init,d)
{
cell_t c;
Thread *t;
real xc[ND_ND];

/* loop over all cell threads in the domain */
thread_loop_c(t,d)
{

/* loop over all cells */
begin_c_loop_all(c,t)
{

C_CENTROID(xc,c,t);

if (xc[0] < 5. )

{

C_U(c,t) = 0.;
C_V(c,t) = 0.;
C_P(c,t) = 100000.;
C_T(c,t) = 348.362;
C_R(c,t) = 1.;
}

else

{

C_U(c,t) = 0.;
C_V(c,t) = 0.;
C_P(c,t) = 10000.;
C_T(c,t) = 278.689;
C_R(c,t) = 0.125;



}

}
end_c_loop_all(c,t)
}
}


then go to Define> User Defined > Functions > interpreted and browse to the text file ( you must save it as *.c first) then again go to Define> User Defined > Function Hooks > initialization > Edit > select the name "moein_shock_tube_init" and then click on Add and then Ok.

then go to Solve > Initialiaze > press Init.
Dont' worry. the numbers like 300 kelvin in initialization dialog box will not influence your simulation and the udf will override them.
now you can plot contours or XY Diagrams and see the result.

Some more tips:
Is giving the temperature values like 348.362 necessary?
I don't think so, because you define your material as an ideal gas, since there is an ideal gas relation P = density * R * T. but I haven't tried eliminating that. you can try!
Also make sure to go to Operating Conditions and set the pressure to 0, since you must work with Absolute Pressures.
if you don't understand the commands in the UDF, search them in internet.

Define_init was the the key to this solution, but I'm happy I turned that key to open a door to salvation. I am now tired of typing, but I have a good sensation...

[troymcfont]

Hi! Thanks for the UDF Moein.
Just a couple of question. Which BCs do you use at the left and the right of the tube? And also in my case the density is not patched correctly. After initializing I can only see the same value (1.62 kg/m3) everywhere even though I specified 2 different values for the left and the right states of the shock tube. I am using the density based solver with the ideal gas option for the density of the material.
Thank you so much.

[POI]

Hi,

please am new to CFD can someone send me a case file on shock tube simulation to guide me on various boundary conditions at the inlet, outlet, diaphragm and how to determine mach number, to peacefisimiintl@yahoo.com
Please Help

Thank you

[ADI]

Any one getting a parse error when interpreting this UDF?

I get parse error for the 'if loop' start line, 'else' line and the final '}s'...

Can any one help?

[hello-fluenttt]

Originally Posted by moein_joon27

Hi Everyone

Here's my solution to your problem in initializing fluent with separate values and simulating a shock tube. I have tested it, I have got the results and I am sure it works properly.
you need a very simple grid which should be like a 2D rectangle. you don't need to separate it or create 2 zones. A simple 1-zone grid will work just fine. we will try to initialize that zone with different values.

suppose the problem says the parameters ( as an example ) are as the case in Hirsch's book:

length of tube=10 m.
width of tube is not important ( because the problem is actually one dimensional when considered inviscid ) i.e. give the width as you wish!


Left:
Pressure=100,000
density=1.
velocity = 0

Right:
Pressure=10,000
density=0.125
velocity = 0

you should introduce the UDF mentioned below to fluent. Save it to a text file:


#include "udf.h"

DEFINE_INIT(moein_shock_tube_init,d)
{
cell_t c;
Thread *t;
real xc[ND_ND];

/* loop over all cell threads in the domain */
thread_loop_c(t,d)
{

/* loop over all cells */
begin_c_loop_all(c,t)
{

C_CENTROID(xc,c,t);

if (xc[0] < 5. )

{

C_U(c,t) = 0.;
C_V(c,t) = 0.;
C_P(c,t) = 100000.;
C_T(c,t) = 348.362;
C_R(c,t) = 1.;
}

else

{

C_U(c,t) = 0.;
C_V(c,t) = 0.;
C_P(c,t) = 10000.;
C_T(c,t) = 278.689;
C_R(c,t) = 0.125;



}

}
end_c_loop_all(c,t)
}
}


then go to Define> User Defined > Functions > interpreted and browse to the text file ( you must save it as *.c first) then again go to Define> User Defined > Function Hooks > initialization > Edit > select the name "moein_shock_tube_init" and then click on Add and then Ok.

then go to Solve > Initialiaze > press Init.
Dont' worry. the numbers like 300 kelvin in initialization dialog box will not influence your simulation and the udf will override them.
now you can plot contours or XY Diagrams and see the result.

Some more tips:
Is giving the temperature values like 348.362 necessary?
I don't think so, because you define your material as an ideal gas, since there is an ideal gas relation P = density * R * T. but I haven't tried eliminating that. you can try!
Also make sure to go to Operating Conditions and set the pressure to 0, since you must work with Absolute Pressures.
if you don't understand the commands in the UDF, search them in internet.

Define_init was the the key to this solution, but I'm happy I turned that key to open a door to salvation. I am now tired of typing, but I have a good sensation...

Hey..!!! Thanks for your post...the density contour is coming wrong and could you explain how can we make the shock wave to move inside it under transient flow...

[KLG]

can anyone send me .cas case file of shock tube simulation in my email. I have been having problem regarding patching and assigning BCs on the tube?
kanchugurung94@gmail.com

[hello-fluenttt]

you can simply copy the code and write it in a .c file and compile and use it in fluent solver. no BC or patching required. The udf will simply initialise the problem and that will be sufficient. see Moin's post .....

[KLG]

can anyone mail me the journal or article regarding results obtained by simulating open type shock tube in fluent?
I have no idea what type of contours comes as a result of the simulation of open type shock tube?
mail: kanchugurung94@gmail.com

[jzapatau]

Hi, sorry to bother, but I am dealing with a similar problem. I am trying to simulate the high pressure discharge of a nitrogen tank (tube shape )with an initial pressue of ~80 bar. So far I have a good capture of the underexpanded jet on the outlet, though I am suspicious of the expansion wave that develops within the tube. This phenomena is something characteristic of shock tubes.
What happens is that the front expansion wave dissipates while it moves across the tube, and I my understanding is that it shouldnt dissipate, so my suspicious goes that I might be having some numerical diffusion.

The order of the method Im using is second order upwind for the convective term, and the solver is density based. Do you have any recommendation on which method I should use to avoid this dissipation?

I would appreciate any comment on this issue and I thank you for taking the time for readind this.

Regards,

jzapatau

[vek123]

hi, i tried your udf and i get wrong pressure distribution i get separate regions but not as written in the text file i get very small pressures like between 10e-8 and 10e-5. i am messing something because i went through a pdf of how to make the udfs and the one you provided is correct, but somehow the fluent overwrite it or something