CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Dynamic mesh, hinged flap

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   April 28, 2010, 12:52
Default Dynamic mesh, hinged flap
  #1
New Member
 
Join Date: Mar 2010
Posts: 19
Rep Power: 7
Randre is on a distinguished road
Hi

I'm simulating the reaction of a hinged flap to the ocean waves in 2D and 3D. 2D mesh is triangular and 3d is tetrahedral. My domain repesents only the fluid zone, with the following BC:
top - pressure outlet
left wall - velocity inlet
right wall - wall
bottom - wall
flap - wall

When I run the simulation without moving mesh, only to check the propagation of the waves with the flap stationary all is well and the solution converges.

However, when I activate dynamic mesh method for rigid body motion, naming smoothing, remeshing and 6DOF, the solution diverges even with a very (very!) refined mesh.

The 6DOF UDF with DEFINE_SDOF_PROPERTIES macro only permits rotation in z-axxis and the dynamic mesh zones are: Flap (6DOF solver options - ON) and interior fluid ((6DOF solver options - ON and PASSIVE) and body CG is also considered.

Multiphase model: VOF, open channel flow, implicit body force
Turbulence model: k-e realizable

Solution methods
scheme: PISO
pressure: PRESTO!
momentum: 3rd order MUSCL
rest: default

Time step is 0.01s with 20 iterations TS.

What I am missing???

Best regards
Attached Images
File Type: jpg vf_contours.JPG (14.6 KB, 264 views)
File Type: jpg ref_mesh_detail.jpg (92.3 KB, 247 views)

Last edited by Randre; April 29, 2010 at 04:54.
Randre is offline   Reply With Quote

Old   April 29, 2010, 01:09
Default
  #2
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,964
Rep Power: 30
-mAx- will become famous soon enough
did you checked your mesh motion?
No skewed cells or whatever?
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   April 29, 2010, 04:52
Default
  #3
New Member
 
Join Date: Mar 2010
Posts: 19
Rep Power: 7
Randre is on a distinguished road
i've checked mesh motion for a determined number of TS. The statistics (and warnings) with a 2D very refined mesh are the following:

Updating...
Warning: dynamic mesh zone 1 (flap wall) with different CG uses 6DOF...
6DOF flap::libudf:: reference CG (1.00100002e+1, -2.00000000e+0.000)
6DOF flap::libudf:: different CG (1.00100002e+1, -2.00000000e+0.000)
and exactly same warning for fluid interior. What about this warning, CG is the same! What does it mean?

Dynamic mesh statistics
Minimum volume = 5.00011e-004
maximum volume = 1.25002e-003
Maximum Cell Skew = 4.71557e-001

Wich are the same for each TS. Please, check first post for refined mesh / flap detail.

Thank you
Randre is offline   Reply With Quote

Old   April 29, 2010, 05:00
Default
  #4
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,964
Rep Power: 30
-mAx- will become famous soon enough
Does it mean that you defined the fluid interior as rigid body?
Is your motion in accordance with your wish?
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   April 29, 2010, 06:07
Default
  #5
New Member
 
Join Date: Mar 2010
Posts: 19
Rep Power: 7
Randre is on a distinguished road
I didn't saw any motion... while it was doing calculations my mesh disappear (I've got display mesh option checked).

edit: Now i've made some changes and previewed mesh motion and all of the domain rotate (fluid + flap) and then stopped : Negative cell volume detected and the right wall of the domain was all messed up.

2nd edit: Well, i've made a research within fluentusers files and noticed something in example of 2D store separation:

"DM philosophy:

- Move the zone fluid-bl and wall-store using rigid body motion.
- The fluid-bl zone is moved with the store in order to maintain a high quality boundary mesh around store. "


which means that one possible error is my definition in dynamic mesh zones, I'm applying rigid body motion to ALL fluid domain....

I'm going to create a boundary zone around flap to check if it works.

One more question: it is possible to be something wrong with the flap definition? I've suppressed it from fluid zone an bottom wall now has a little gap

Last edited by Randre; April 29, 2010 at 07:02.
Randre is offline   Reply With Quote

Old   April 29, 2010, 07:47
Default
  #6
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,964
Rep Power: 30
-mAx- will become famous soon enough
Quote:
Originally Posted by Randre View Post
which means that one possible error is my definition in dynamic mesh zones, I'm applying rigid body motion to ALL fluid domain....
yes you need to define the region surrounding your flap with sypecify continuum tool (eg: to treat it separately as the remaining fluid domain.

Quote:
Originally Posted by Randre View Post
One more question: it is possible to be something wrong with the flap definition? I've suppressed it from fluid zone an bottom wall now has a little gap
post a picture prior to iterations, and another one with this issue
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   April 29, 2010, 10:13
Default
  #7
New Member
 
Join Date: Mar 2010
Posts: 19
Rep Power: 7
Randre is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
region surrounding your flap with sypecify continuum tool (eg: to treat it separately as the remaining fluid
Is that available were? My pre-processing software is DM / Meshing from WB 12 . I defined a separate box in DM, then remeshed all domain, but when I tested mesh motion all of the box has moved...

don't know what to...

Thanks for your support!
Attached Images
File Type: jpg mesh_2.JPG (93.0 KB, 215 views)
Randre is offline   Reply With Quote

Old   April 30, 2010, 01:19
Default
  #8
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,964
Rep Power: 30
-mAx- will become famous soon enough
Continuum Tool is for gambit.
For DM, I don't know, but for sure there should be something like the one in gambit. (Look in boundary conditions, or something like that)
...
Just for information, in your picture the box which has moved, doesn't seem to be connected to the other domain. Else you should receive error regarding skewed cells, etc...
Or pehaps you are dealing with interfaces
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   April 30, 2010, 11:35
Default
  #9
New Member
 
Join Date: Mar 2010
Posts: 19
Rep Power: 7
Randre is on a distinguished road
Hi again

Got a new development. Check attach. How do I avoid that? I will try to increase mesh refinement around fluid block.

My fluid block is connected to two BC:
Bottom, in white - Wall;
at back, in yellow - Symmetry.

Could that be the reason to this error? My fluid block cannot be connected to other BC that aren't in my dynamic mesh zones?

And seems that the flap is rotating by its CG. How do I restrict rotation for its foundations?

My UDF is very simple, and I guess that it would do what I want, any help?

DEFINE_SDOF_PROPERTIES(flap, prop, dt, time, dtime)


{
/* Define the mass matrix */

prop[SDOF_MASS] = 480.0;
prop[SDOF_IXX] = 0.066667;
prop[SDOF_IYY] = 0.000167;
prop[SDOF_IZZ] = 0.288;

/* Define the Degrees of Freedom allowed - Only z rotation is allowed */

prop[SDOF_LOAD_LOCAL] = TRUE; /* Determine wheter the forces and moments are expressed in terms of global coordinates(false) or body coordinates
(true) */

prop[SDOF_ZERO_TRANS_X] = TRUE;
prop[SDOF_ZERO_TRANS_Y] = TRUE;
prop[SDOF_ZERO_TRANS_Z] = TRUE;
prop[SDOF_ZERO_ROT_X] = TRUE;
prop[SDOF_ZERO_ROT_Y] = TRUE;
Attached Images
File Type: jpg cel_vol_error.jpg (86.4 KB, 236 views)

Last edited by Randre; April 30, 2010 at 14:33.
Randre is offline   Reply With Quote

Old   May 3, 2010, 01:01
Default
  #10
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,964
Rep Power: 30
-mAx- will become famous soon enough
the fluid domain around your flap doesn't seem to move
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   May 3, 2010, 05:00
Default
  #11
New Member
 
Join Date: Mar 2010
Posts: 19
Rep Power: 7
Randre is on a distinguished road
I've changed Dynamic Mesh conditions and now seems that the fluid domain around the flap ajusts to the movement. But something is wrong, when I initialize the solution the flap starts to move immediately in the opposite direction of flow! I need the flap to move when pressure conditions around it changes. Is something wrong with my UDF? I don't apply any force or momentum to it!
Randre is offline   Reply With Quote

Old   May 3, 2010, 05:34
Default
  #12
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,964
Rep Power: 30
-mAx- will become famous soon enough
before turning on your udf, check your motion with a simple velocity profile.
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   May 3, 2010, 06:08
Default
  #13
New Member
 
Join Date: Mar 2010
Posts: 19
Rep Power: 7
Randre is on a distinguished road
New update, Mesh motion is correct now, but when I initialize the solution, everything goes wrong.
Attached Images
File Type: jpg 03-05-2010_case_movement_2.jpg (96.6 KB, 151 views)
Randre is offline   Reply With Quote

Old   May 3, 2010, 06:42
Default
  #14
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,964
Rep Power: 30
-mAx- will become famous soon enough
initialized with your udf or profile?
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   May 3, 2010, 08:08
Default
  #15
New Member
 
Join Date: Mar 2010
Posts: 19
Rep Power: 7
Randre is on a distinguished road
I've got two UDF's. One is related to ocean waves, where linear ocean wave theory is applied. The other one is presented in this thread. I've initialized with a constant velocity of 2 m/s at the inlet zone, and the result is also wrong.

Don't know why but the flap moves right in the first TS of my simulation, and that's inconsistent with the distance of it from velocity inlet boundary - 10 meters. The flap doesn't move due to pressure difference. Are BC wrong?

Thank you

Last edited by Randre; May 3, 2010 at 10:41.
Randre is offline   Reply With Quote

Old   August 29, 2010, 21:47
Default
  #16
New Member
 
Join Date: Aug 2010
Posts: 1
Rep Power: 0
Coffstah is on a distinguished road
I'm trying to do something very similar to this. I am simulating a heart valve and I want the leaflets to rotate in only one direction, and was hoping to use the built in 6-dof. I am very confused by this discussion though. Particularly the sample UDF you posted Randre. I don't see any evidence of the properties you used to constrain only z rotation (i.e. SDOF_ZERO_ROT_X) in the documentation. Do these properties actually exist? Is there any documentation of them I can see? Is it actually possible to do this with the built in 6-dof, or do I have to calculate the motion on my own.
Coffstah is offline   Reply With Quote

Old   September 1, 2010, 15:49
Default
  #17
New Member
 
Join Date: Mar 2010
Posts: 19
Rep Power: 7
Randre is on a distinguished road
Do you know the work of K.Dumont from Gent University about numerical modeling of heart valve dynamics? Try a quick search in google and you'll find out information related to it.
To restrict a certain object to only one degree of freedom, you will need to use the built in 6DOF solver in dynamic mesh options and the following UDF:

#include "udf.h"
{
DEFINE_SDOF_PROPERTIES(flap, prop, dt, time, dtime)

prop[SDOF_MASS] = x;
prop[SDOF_IXX] = x;
prop[SDOF_IYY] = xx;
prop[SDOF_IZZ] = xxx;

prop[SDOF_ZERO_TRANS_X] = TRUE;
prop[SDOF_ZERO_TRANS_Y] = TRUE;
prop[SDOF_ZERO_TRANS_Z] = TRUE;
prop[SDOF_ZERO_ROT_X] = TRUE;
prop[SDOF_ZERO_ROT_Y] = TRUE;
}
And this will restrict the translation movement in x,y,z and rotation in x and y.
Randre is offline   Reply With Quote

Old   March 23, 2011, 19:39
Smile Help please
  #18
New Member
 
giovanni ingrassia
Join Date: May 2010
Posts: 16
Rep Power: 7
giov_ingr is on a distinguished road
Hello
I have a question about the
SDOF_ZERO_TRANS e SDOF_ZERO_ROT properties.
When I try to compile the UDF with these strings FLUENT shows me that it cannot recognize these strings .

Could you help me please?
Here there is my UDF

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

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

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

DEFINE_SDOF_PROPERTIES(eolico, prop, dt, time, dtime)
{

prop[SDOF_MASS] = 0.022;
prop[SDOF_IXX] = 3e-3;
prop[SDOF_IYY] = 2e-5;
prop[SDOF_IZZ] = 3.02e-3;

prop[SDOF_LOAD_LOCAL] = TRUE;
prop[SDOF_ZERO_TRANS_X] = TRUE;
prop[SDOF_ZERO_TRANS_Y] = TRUE;
prop[SDOF_ZERO_TRANS_Z] = TRUE;
prop[SDOF_ZERO_ROT_X] = TRUE;
prop[SDOF_ZERO_ROT_Y] = TRUE;


printf ("\n2d_eolico Updated 6DOF properties");
}

Thank you for your attention
giov_ingr is offline   Reply With Quote

Old   April 9, 2011, 12:40
Default
  #19
New Member
 
mamadreza
Join Date: Mar 2011
Posts: 22
Rep Power: 6
mamyjooooon is on a distinguished road
Hello giovanni and Randre and...
I have the some problem about the
SDOF_ZERO_TRANS e SDOF_ZERO_ROT properties.

i want to solve flow in a radial turbine wheel(with high RPM).
Because the flow work is done on the blades to make the blades rotating,I decided to use dynamics mesh with 6dof.
When I try to compile the UDF,FLUENT shows me:

..\..\src\stage.c(6) : error C2065: 'SDOF_ZERO_TRANS_X' : undeclared identifier
..\..\src\stage.c(7) : error C2065: 'SDOF_ZERO_TRANS_Y' : undeclared identifier
..\..\src\stage.c(8) : error C2065: 'SDOF_ZERO_TRANS_Z' : undeclared identifier
..\..\src\stage.c(9) : error C2065: 'SDOF_ZERO_ROT_X' : undeclared identifier
..\..\src\stage.c(10) : error C2065: 'SDOF_ZERO_ROT_Y' : undeclared identifier

Here there is my UDF
Quote:

#include"udf.h"

DEFINE_SDOF_PROPERTIES(stage, prop, dt, time, dtime)
{

/* Define the mass matrix */

prop[SDOF_MASS] = 0.02;
prop[SDOF_IXX] = 0.000067;
prop[SDOF_IYY] = 0.000067;
prop[SDOF_IZZ] = 0.000288;

/* Define the Degrees of Freedom allowed - Only z rotation is allowed */

prop[SDOF_ZERO_TRANS_X] = TRUE;
prop[SDOF_ZERO_TRANS_Y] = TRUE;
prop[SDOF_ZERO_TRANS_Z] = TRUE;
prop[SDOF_ZERO_ROT_X] = TRUE;
prop[SDOF_ZERO_ROT_Y] = TRUE;
printf (
"\nstage: updated 6DOF properties");
}

Could you help me please?
Thank you. Kind regards, mamadreza

Last edited by mamyjooooon; April 11, 2011 at 04:22.
mamyjooooon is offline   Reply With Quote

Old   April 9, 2011, 12:53
Default Answer
  #20
New Member
 
giovanni ingrassia
Join Date: May 2010
Posts: 16
Rep Power: 7
giov_ingr is on a distinguished road
hello mamyjoooon,
I have the answer...
The SDOF properties about the zero trans and zero rot are valid only for ansys fluent!! I think from the 10.0 version until 13.0 one.
I used my UDF on ANSYS FLUENT 13.0 and finally it works!!
If anybody knows how to set these properties on fluent 6.2 version please tell me.

Have a good work!
giov_ingr is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[ICEM] Generating Mesh for STL Car in Windtunnel Simulation tommymoose ANSYS Meshing & Geometry 48 April 15, 2013 04:24
Dynamic Mesh on Pintle type injector. herntan FLUENT 15 January 4, 2012 04:31
Dynamic mesh + grid adapt = Crash! (Files included BillH FLUENT 4 July 24, 2007 15:31
Dynamic Mesh Pj FLUENT 1 March 12, 2007 16:16
Gambit problems Althea FLUENT 21 February 6, 2001 08:05


All times are GMT -4. The time now is 01:26.