2d Dynamic Mesh with udf
 

HI
i m try to moving mesh problem
my geometry like simple square box inside small rectangle blade with tet mesh
successful . But when i m using pave mesh it is not successful error came while mesh motion negative volume created .
please help me . Is there problem with udf? or dynamic parameter setting ?
:confused:

#include "udf.h"

#define omega 5.0 /* rotational speed, rad/sec */


DEFINE_CG_MOTION(butterfly_flex_UDF, dt, cg_vel, cg_omega, time, dtime)
{
cg_vel[0] = 0.0;
cg_vel[1] = 0.0;
cg_vel[2] = 0.0;

cg_omega[0] = 0.0;
cg_omega[1] = 0.0;
cg_omega[2] = omega;
}

DEFINE_GRID_MOTION(moving_arc, domain, dt, time, dtime)
{
Thread *tf = DT_THREAD (dt);
face_t f;
Node *node_p;
SET_DEFORMING_THREAD_FLAG (THREAD_T0 (tf));

}


this is my udf thank you........

Hi there,

what mesh do you mean with pave mesh?

I mean you can do paved meshes of quad cells or tri cells in gambit?

If you're using quad cells you have to enable spring based smoothing for them, by default its only enabled for tri-cells (and see 11.3.2. of the user guide (6.3.26) for dynamic-mesh issues:

define / models / dynamic-mesh-controls / smoothing-parameter / spring-on-all-shapes? yes

[QUOTE=O.D.Y.;235705]Hi there,

what mesh do you mean with pave mesh?

I mean you can do paved meshes of quad cells or tri cells in gambit?

If you're using



thanks for your suggestion I am using quad pave mesh
but when i try for mesh motion only boundary node moves internal node dosent move I also use cell height option .

well if you mean the cell height option in the dynamic mesh zones menu, this one just plays a role for remeshing.

if only the boundary nodes move, make sure that the interior-domain is given a deforming flag in the dynamic-mesh-zones menu.
if this is the case, try to reduce the spring constant factor and to increase the number of mesh motion iteration, this distributes the displacement more over the entire domain.

If your displacements are bigger than the cell sizes, you should use remeshing-option to avoid negativ volumes.

hope this helps, let me know if it works!

[QUOTE=O.D.Y.;235716]well if you mean the cell height option in the dynamic mesh zones menu, this one just plays a role for remeshing.

if only the boundary nodes move, make sure that the interior-domain is given a deforming flag in the dynamic-mesh-zones menu.
if this is the case, try to reduce the spring constant factor and to increase the number of mesh motion iteration, this distributes the displacement more over the entire domain.


Thank you for kind suggestion I also work on that but same problem occur internal node not moving so negative volume created .
If you want try on this i am giving you link for mesh file and udf file.

http://www.megaupload.com/?d=YWUI5DAG
mesh file

http://www.megaupload.com/?d=NSBYW5BN
udf file

Thank you.

I have one more problem in 3d tetrahydral mesh this udf not works can you tell
me how to change in udf so that negative volume will not create because only
boundary node moves internal element doesnt move .

Thanks a lot

Hi there,

I took a short look in the user guide and i found:

You can use the local remeshing method only in cell zones that contain tetrahedral or triangular cells.

So you can use dynamic mesh only on triangular cells.

But you might think about doing the caculation as moving reference frame with assigning the outer wall zero absolute veloctiy.
This surely depends on how the configuration looks like in reality....

cheers

[QUOTE=O.D.Y.;235804]Hi there,

I took a short look in the user guide and i found:

You can use the local remeshing method only in cell zones that contain tetrahedral or triangular cells.

So you can use dynamic mesh only on triangular cells.

But

No i actually want do simulation in 3d tetrahydral dynamic meshing
I already done moving referance frame simulation but now i want give actual motion to the rigid body
thanks for reply

Are you sure about that? I'm asking, because that is what I'm doing right now... and I also use Fluent 6.3

Hi,

and is it working?

I mean this is what the user guide is telling me:

FLUENT includes several remeshing methods that include local remeshing, local face remeshing (for 3D flows only), face region remeshing, and 2.5D surface remeshing (for 3D flows only). The available remeshing methods in FLUENT work for triangular-tetrahedral zones and mixed zones where the non-triangular/tetrahedral elements are skipped

I made an simple example and there was no remeshing....
What's your experience?

Oh, just noticed that I mixed up remeshing and smoothing. I'm sorry!!!
Acutally, I do have the same problem with the remeshing. It's a shame that fluent isn't able to remesh quad grids...

So that's my problem too...

I switched to hybrid meshes with quad/hex-boundary layer mesh and tri/tet-meshes in the domain, that works pretty well.

Okay, very good to know!

Thank you for the advice, this will probably work for my problem either.

Hi everyone,

I am having this negative volume problem as well. My problem is a simulation of an aerofoil pitching upwards around the quarter chord. Let me just show you all how I have set up my mesh.

http://i932.photobucket.com/albums/a...e/NACA0012.jpg

http://i932.photobucket.com/albums/a...NACA0012-2.jpg

Basically it is a hybrid mesh with hex near the boundary and triangles everywhere else.

Ive tried to reduce the time step, but the mesh previews gives me a negative volume message at the very 1st iteration. I have also turned on the dynamic mesh parameter for quad mesh which was turned off by default but did not fix the problem.

Just for your information, I have tried the dynamic mesh with a purely triangular mesh and that worked. It is only when I added the hex mesh near the boundary that it stopped working. So i am assuming it has something to do with the hexa mesh?

ODY you mentioned that you got your simulation working with a hybrid mesh?? could you shed some light on this for me??

Thanks in advance

Darren

Hi Darren.

Well I did calculation with "dynamic mesh" with meshes similar to yours.

1st thing is to make sure, that you enable spring-based-smoothing for all types of elements (spring on all shapes). But you wrote that you already did this, right?

Next thing is to use smoothing and remeshing.
you may want to try my dynamic mesh parameters:

spring factor: 0.01
boundary relaxation: 1
convergance tolerance: 0.0001
number of iterations: 150

and for remeshing you need to set the parameters according to your mesh.

set the remesh interval on 1.

That's how I'm doing it. Give it a try and let me know, I'm curious about it.

BTW: is this an inviscid calculation?

cheers

Hey ODY,

Ive tried your settings and they work for me perfectly. Thanks a bunch!!!. I think the trick is to get it to move real slow so that it dosent deform to the point of negative volume. Ill have to fine tune it a little bit more and see how it all goes.

FYI i am actually running a compressible viscous calculation as I am simulating this at quite high mach numbers.

By the way, do u happen to use ICEM to build your 2d hybrid mesh? Apparently there are alot of methods to do this, and the way I do it (just specifying layer params in curve mesh setup' is not very good. Did you use '2dBlayer' in advanced prism meshing?

Thanks again!

Regards,
Darren

hello people
 

I am trying to rotate a butterfly valve, but I can´t make the valve move at all,
can you help me out, please?
I have been trying to compile this code that you attached here without success

I send you a .jpg
I hope you can lead my way,
thanks

Hey euzinho,

how large should the displacement of your body you showed in the picture get? If its only a small one, the smoothing should be sufficient.
But then you need to specify smoothing for all cell types via TUI as decribed above...

Did you properly assign the rigid body movements to your body in the dynamic mesh option? Can you post your udf?

cheers

thanks for your response,
Actually i am trying to rotate this body 45º because it simulates a butterfly valve that opens

the idea is to create a transient simulation that studies the behaviour before and after the valve opens. So I need to rotate it just 45º. No displacement whatsoever, just rotation

the UDF ? well, I don´t have one concrete code developed at the moment but a lot instead,
because I am evaluating different options since I don´t have a clear idea about how it works.

for example:
#include "udf.h"
DEFINE_CG_MOTION(pod,dt,vel,omega,time,dtime)
{
NV_S(vel,=,0);
NV_S(omega,=,0);
omega[0]=1;
}

this one moves rotating through the x egde
the same one with omega[1] rotates through the y egde
and omega[2] should rotate through the z egde (what I need) but.. it doesn´t work..

And also it rotates according to a center o gravity far away from the one what I need... so not only I have to rotate this valve but also to specify its center of gravity...

I hope you can help me out because I am also dreaming about it during the night

thanks

by the way,
I´ve read something about sliding mesh to resolve problems related with rotation... do you think it could be another way to face my problem instead of using UDF ?

thanks

hi friend
 

this is exactly what I want to resolve
a udf or any other way to get this movement in a transient study

Well sliding mesh could be an option...
The idea would be to split the flow domain into two parts.

Lets say one circle domain containing the valve and one for the rest of the domain, and the boundary between them could be defined as sliding mesh.

But as far as I know you can only specify constant movement, or you have to use an udf...

But the thing you want to do is quite easy to do with UDF...

Here is a simple version of what I am using:

#include <stdio.h>
#include <math.h>
#include "udf.h"

DEFINE_CG_MOTION(move_body, dt, vel, omega, time, dtime)
{
real ampl,disp,omg,count;

/* reset velocities */
NV_S (vel, =, 0.0);
NV_S (omega, =, 0.0);

/* motion */
ampl = 0.008726646 ; /* amplitude of rotation in radians (0.5deg) */
omg = 116.0219; /* angular frequency (18.465Hz) */
disp = ampl * sin(omg * time); /* resultant displacement */

omega[2] = ampl * omg * cos(omg * time);
}

So this is for a sinusoidal vibration with 0.5deg amplitude around the z-axis.
for your case you could take another functional dependency on time or let it only work in a certain time period using an if condition.

Then you need to hook this udf as rigid body motion and as center of gravity you just set the coordinates of the geometrical center point of your valve.

let me know if it works.

cheers

wow! friend, thanks so much for taking your time and help me out.
finally it works! this is the certain code for sure,
and actually this is what I did earlier but omega[2] coordenate didn´t work that time... I wonder why...

it leads me to another problem, however... so two more question, please
How can I define my CG "set the coordinates of the geometrical center point of your valve."
and how can I resolve negative cell volume problems..? is that because a wrong definition of my mesh?

thans again,

Hi,

well you just set the center of gravity in the dynamic mesh module to the coordinates of the geometric center of the body thats supposed to rotate.

the negative volumes may have different reasons.

As you are using quad-elements you have to set

/define/models/dynamic-mesh-controls/smoothing-parameter/spring-on-all-shapes? yes

via TUI otherwise the smoothing only works for tri- and tet-elements.

If you still have negative volumes you should think about making smaller displacement per time step (e.g. taking a smaller time step size).
You can also vary the parameters for smoothing and use the remeshing technique additionally.

good luck

thanks so much for your response,
actually I am setting my CG when I design the project in Solidworks, and it works

other question, where can I reset the "current mesh time" in order to start from the beginning?
I mean, after the body moves, How can I put it back at its initial position? what I do is to shut fluent down and start it over.. and it´s suck!


thanks

good question, you could reset the current mesh time in the mesh motion module in former versions, but I guess in 6.3.26 and newer versions this isn't possible anymore... This time is saved in the *.dat file.

You could just substract this time from the time variable in the udf and compile again... I don't know about another way..

I did it!
it is a simple armonic movement
what I cannot get is to set certain movement in a given period of time.
I mean, I have to open the valve in 2 seconds. that´s all

after that, the aim is to maintain the valve opened
but If I cannot have a control of "time" I cannot control that..

I was thinking about something like:

if (time=2) (guessing that Time in seconds) then omega[2] = 0 (because the valve will stop once reached that time)

any suggestion?

thanks

Why not, that should work....

well, it doesn´t work because "time" is greater than 2 and there is no way to resert its value...

Hi guys,

I'v read all your posts, I tried everything you've said, but (yes there is always a 'but') I always have the best answer in the world

'Update dynamic mesh failed. Negative cell volume detected'

My project is blood simulation in artery, and what I want to do now is a simulation of the movement of the artery.

First of all I'll try to do that with an easy one, that's mean with a pipe.
Here is my UDF :

# include "udf.h"
# include "dynamesh_tools.h"
# define D 0.2e-2 /* diameter of the pipe */
# define H 0.03e-2 /* amplitude of the wave */
# define L 1e-2 /* length of the wave */
# define l 2e-2 /* lenght of the pipe */
# define speed_wave 1 /* speed of the wave */
static real F(real x)
{
if (x>=0 && x<L)
{ return H*sin(2*M_PI/L*(x-0.25*L))+0.5*D+H; }
else if(x>=L && x<=(L+l))
{ return 0.5*D; }
else
{ Message0("x = %12.4e Wrong range of x-aborting", x);
exit(1); }
}

static real f_top(real x)
{
real x1;
double tmp;
x1 = modf(x/(L+l), &tmp);
if (x1>=0)
{
return F(x1*(L+l)); }
else
{
return F((1+x1)*(L+l)); }
}
static real f_bottom(real x)
{
return -f_top(x);
}

DEFINE_GRID_MOTION(grid_top, domain, dt, time, dtime)
{
face_t f;
Thread *tf = DT_THREAD ((Dynamic_Thread *)dt);
int n;
Node *v;
/* Activate the deforming flag on adjacent cell zone, which means that
the cell adjacent to the deforming wall will also be deformed in
order to avoid skewness. */
SET_DEFORMING_THREAD_FLAG (THREAD_T0(tf));

/* Loop over the deforming boundary zone's faces; inner loop loops over
all nodes of a given face; */
begin_f_loop(f, tf)
f_node_loop(f, tf, n)
{
v = F_NODE(f, tf, n);
{
/* Update the current node only if it has not been previously visited to
avoid to visit the same nodes multiple times */

if (NODE_POS_NEED_UPDATE(v))

{
/* Set flag to indicate that the current node's position has been
updated, so that it will not be updated during a future
pass through the loop */
NODE_POS_UPDATED(v);
real x;
x = NODE_X(v);
/* f_top(x-ct) defines the wave equation */
NODE_Y(v) = f_top(x-speed_wave*time);
}
}
Update_Face_Metrics (f, tf);
}
end_f_loop (f, tf);
}

/* Similar udf for the bottom wall */
DEFINE_GRID_MOTION(grid_bot, domain, dt,
time, dtime)
{
face_t f;
Thread *tf = DT_THREAD ((Dynamic_Thread
*)dt);
int n;
Node *v;
SET_DEFORMING_THREAD_FLAG
(THREAD_T0(tf));
begin_f_loop(f, tf)
{
f_node_loop(f, tf, n)
{

v = F_NODE(f, tf, n);
if (NODE_POS_NEED_UPDATE(v))
{
NODE_POS_UPDATED(v);
real x;
x = NODE_X(v);
NODE_Y(v) = f_bottom(x-speed_wave*time);
}
}
Update_Face_Metrics (f, tf);
}
end_f_loop (f, tf);

}

I'm waiting for your possibilities and advices.

Thanks a lot in advance.

Christophe

rotation about z axis
 

update-dynamic-mesh failed. negative cell volume detected.
 

hi dear all...
I was running fluent and waiting to get results but faced an error:

update-dynamic-mesh failed. negative cell volume detected.

i changed time step from 0.0001 to 0.00001 but again this error showed up,could you help me out plz?
thank u in advanced for any help provided:)

How to activate"spring-all-shapes"?
 

hi dear all...
i faced an error message,negative cell volume detected,i think if i activate spring-on-all shapes this error does show again,but i do not know hoe to activate it in ansys 12.0,
any help will be appreciated...

butterfly valve
 

I O.D.Y how it is going?
I am in trouble one more time with butterfly valve move... I hope you can manage to help me out.
Time ago you gave me the following code to resolve butterfly move and I have been changing some parameter to adapt your code to my requirements without success
what I have to do is to stop this valve after 45º displacement. that´s all.

If you have any idea to do it, I would appreciate if you share this thoughs.
regards


DEFINE_CG_MOTION(rotating_body, dt, vel, omega, time, dtime)
{
real ampl,disp,omg,count;

NV_S (vel, =, 0.0);
NV_S (omega, =, 0.0);

/* motion */
ampl = 0.785423 ;
omg = 516.0219;
disp = ampl * sin(omg * time);

omega[2] = 0.785423*sin(time);

Hi O.D.Y.,

you mentioned that negative volume problems can be solved tuning the smoothing or re-meshing parameters.

But I have this problem even if I work with sliding mesh (circle inner quad-mesh oscillating, and outer tri-mesh steady), so without smoothing or re-meshing.

Any idea about why I get negative volumes (when I run a preview mesh motion on Fluent) and how to solve it, please?

Many thanks.
Kind regards,

Alberto

I am using dynamic mesh to simulate a 2d square cylinder.My problem is only the cells adjacent to boundary deforms.Can any1 tell me what I should do to deform more portion of the mesh?

Hi All..

Sir,
I am trying to rotate a 2D box or a 2D cup structure in Fluent using smoothing and remeshing. I am using tri mesh and as mentioned in Fluent Manual I am using smoothing and remeshing and also set the remeshing parameters from mesh info tab given in the remeshing menu. But the problem is that when i start simulation and it goes to first time step Fluent display "Updating mesh at time level N..." and here it stops and it happened alot of time and even waiting after a whole day it didnt worked. I also tried time step size from 0.01 to 0.000001 but it still show this problem.

Can you plz help in this case?

Thank u in advance

2D airfoil O Grid- negative volume
 

Hi,

I'm carrying out a 2D pitching airfoil simulation using dynamic meshing with a "O" Grid. The dynamic conditions i have given were
1) airfoil - rigid body with UDF with pitching over X=0.25
2)interior - deforming with the min and max length scale from zone scale info
3) fluid -deforming with the min and max length scale from zone scale info.

The spring constant i gave was 0.001 and
convergence tolerance 0.0001
No of iterations 150.

The time step tat i used is 0.001.

After running the iterations and after about 500 time steps i'm getting the following error

negative volume detected
dynamic mesh update failed.
i have worked around with the spring constant and also with the time step nothing worked.
could someone help me out rectify this issue..
thanks in advance,
sam

Sam cfd
can you tell me what options of fluent you choose for doing airfoil pitching analysis, I am doing bird wing flapping analysis. My email id is pradip.c1000@gmail.com
Thanks in advance.

Hi everyone,

I am simulating flapping wing of aerofoil. I have created three zones, zone 1, 2 and 3. Zone 1 has aerofoil with structured mesh around the aerofoil. Zone 2 and 3 has unstructured gird. My problem is I have properly followed all the steps. But I am not able to achieve what I want. Because the shadow of the interface is taking as wall and is not moving along with the domain. Kindly someone help in sorting out this issue. I have attached my UDF alos. Please have a look. Thank you so much

https://drive.google.com/file/d/0B7L...ew?usp=sharing
https://drive.google.com/file/d/0B7L...ew?usp=sharing