hi giovanni
Thanks for your reply!
I have problem in the compiled UDF with ANSYS FLUENT 12!
I used visual studio 2008 to compile udf in fluent 6.3.26,but it can't find this version of fluent(12)
how can I compile udf in ANSYS FLUENT 12?
Thank you

Compiling UDF in ANSYS
 

Hi mamyjooon,
I can explain you how to start ANSYS FLUENT able to compile UDFs. I have never tried to start ANSYS WORKBENCH able to compile UDFs.

The answer to your question is:

>Start the Visual Studio 2008 Prompt Command windows.

>After that, you must go into the following directory (or something like that):

C:\Program Files\ANSYS Inc\V120\fluent\fluent12.0.0\launcher\ntx86

>Now, writing the command: launcher1 you will open the fluent startup windows. Set your configuration and launch the program.

Try to compile your UDFs.

Let me now if this post solve your problem. If not, contact me because it means that you need to set your environment variables. :D

Regards and apologize for my english.:(

hi giovanni
thank you very much for reply
my problem is solved with your help.I used the environment variables.
but i have new problem,when i solved my case,after some time steps,my solution encountered with various errors like "skewness exceed 0.98 " and "negative volume detected" and "Divergence detected".
meantime I am using both smoothing and remeshing methods.
are errors because the mesh is too coarse,also can I use the Remeshing and Smoothing for structure mesh on Ansys Fluent 12?
can you help me to solve my problem and to remove my errors?
thanks for your attention

Reply
 

Hello mam,
after i sent the latest reply to your question, my ansys misteriously stopped to compile the UDFs and after 4 crazy days of work to fix it the result is that my windows crashed definitively :(
This is just to say that u must be happy that your machine works :D.

About your problem i need to know more about your geometry... you could post a mesh grid contour (only if it happens on a small region) after the skewness jumps to 0.98.

Anyways my idea is that there are 2 possible reasons:
1. The time step is too large
2. The sizing and remeshing start after a too large number of iterations.

In the Dynamic Mesh control panel between the options avaible on sizing, you could reduce the number of iterations and set a fixed values of maximum skewness value, forcing the mesh to be better.

Let me know about your progress.
Did you do Mesh Motion Preview? Have you looked properties of the blades to monitor the CG coordinates and velocities? Are they right?

regards...

PS. I have questions about your stuff? How many processors do you have and
how many volume cells there are in your case? What about your RAM?

Hi dear giovanni
I use unstructured mesh in my geometry. the number of cells is about 300000 and
initial max skewness is 0.78. I think time step is small enough (1e-6 second), but
as you said the remeshing start after 50 iterations. In Dynamic Mesh control panel
i set number of iteration to default value (i.e. 10) and reduce the maximum skewness
value to 0.7; Since i constrained 5 DOF, there is no CG trans and it has rotation
only around z axis. These values remain logical and i checked them.
I use 4 processors and 4 GB memory of RAM.
I have previous problem yet, what's wrong?
I did'nt preview my mesh in mesh motion, is it necessary? can it help me?

Thanks
mamadreza

Reply
 

Hi dear mamadreza

I have no confidence with unstructured mesh, but 6dof works only with TETRAHEDRAL mesh.
The time step is small enough and for first instance i would set remeshing interval at 5 iterations.

About the mesh motion, it calculates the motion of the body without solve the NS equation for all the volume. It is a faster quality checker, and shows you the grid evolution until negative volume is checked.
I would set the max skewness value about 0.85 for 3d simulations, 0.75 is too restrictive and is lower than the value in input. (I don't know how this condition affects the remeshing).

About the dynamic mesh settings: What about ZONES PROPERTIES? I am sure you defined a stator zone, a deforming zone and a rigid wall. Have you thought about the possibility to set the deforming zones as rigid body and set it as passive? Does it affects the physics of your configuration?

Now I have a question for you. I am working with a very complex geometry and the best i have done until now is 6M elements with Gambit. Have you used ansys mesher or other programs or some particular method to obtain 0.3M elements?

Regards
giovanni

hello dear giovanni

i have only a rigid zone(my rotor contains the twenty blades;which i defined all blades a rigid zone and fluid,inlet,outlet
are the stationry zone because of i defined nothing for their in the zone box,
although i'm not sure about this zones definition.

my friend,what's 0.3M elements or 6M elements?

meantime i am meshing with gambit 2.3.16
thanks

Dear friend,

M=10e6 :)
Anyways, about the zones, look up the dynamic mesh tutorials, like as the missile launch (not the silo launch) to understand the best settings for you case.
Definitively u need a zone between rotor blades and stationary because the remeshing and the sizing will not be applied to rigid or stationary zones, then the mesh fall into negative volume, cause to the movement of nodes on the blades faces.

When my laptot will be fixed i would like to start a comparative session of simulations to investigate dynamic mesh analisys, if you want.

Regards
Giovanni

hello guys, please help me out in my project. i wana know how to enter the inlet pressure in fluent as i am dealing with just 2d now, in practical suppose if i had 4 bar pressure at inlet then how much i mist give in fluent?

Hi dear giovanni

I'm sorry for delay in reply.
I have the missile silo launch tutorial only and according to it i defiend
blade walls and fluid zone rigid body, and simulation has problem in remeshing yet.
My geometry has minimum cell volume equal to 10e-12 and maximum cell volume equal to 10e-10.
Dear friend, thanks for your suggestion. I become pleased to investigate
dynamic mesh analysis.
Thanks
mamadreza

Reply
 

Dear friend,

I'm sorry for the delay.

You should define the faces between rotor and stator as interfaces, they should be different and meshed with non-conformal mesh to avoid the sliding for the volumes during the simulation.

With gambit you can do this using the "split volume" command paying attention to the bidirectional and connect options... you must retain the subtracted volume wich must not be connected!!!

In boundary conditions now, you will find identical surfaces, but with different name, set them for stator and rotor and have a good work finally :)

Read on fluent manual how to set interfaces, is not difficult.

Regards
Giovanni

Reply Qasim
 

Dear Qasim

When you want to set a pressure conditions you must set the inlet edge as PRESSURE INLET and insert the value of pressure expressed in Pascal, or in bar if u change general settings, in the gauge total pressure value (i.e. 400000).

This implies that u will have a costant overpressure of 4 bar starting from the inlet and propagating over a domain with 1 atm pressure. (This affects the gas velocity as u can see in initializing solution panel)

If u want to set a general domain pressure of 4 bar (i.e. u want to analize an airfoil working at a different altitude (obviously in that case the pressure should decrease)) u must set the operating condition to 4 bar and set the over-under pressure in the inlet BC.

I hope to have been clear, if not send me a message.

Regards
Giovanni

Dear Giovanni
Hi
I'm sorry for delay in reply.
I am simulating only a turbine rotor, so I haven't any interface
between rotor and stator.
I can't simulate my mesh yet. I'm challenging with negative volume
now. I tested several options in cell number and size, also different
dynamic mesh parameters. Also I reduced time step to 1e-6 seconds,
but I can't solve the problem.
I'm now trying about layering scheme.
please help me to solve my problem
Thanks for your help
Mamad reza

Dear Mamed,

To help you definitively i must see the geometry and the control volume, if you cannot show me the original ones, send me a draw or a scheme to completely understand the problem.
My personal email is giovanni.ingrassia@gmail.com.
I hope to have your news soon.

I am proud to announce you that my simulation started and the results looks like correct!

Regards,
Giovanni

I'm sorry... Mamad
Too many hours working... :)

hi dear giovanni
i sent my simulation to your email
i am waiting for your reply
send for me as soon as possible,please
Thanks
mamadreza

Using 6dof for 3D turbine blade rotation
 

Hi, I am working on a problem where I have a turbine driven by the flow. My intention is to use 6dof and rotate the turbine along with the enclosed zone (similar to what we do in sliding mesh where layering, smoothing and remeshing will not take place).
The approach I am doing is
1. hooking 6dof to Turbine (which is defined as wall in BC) with 6dof-on, passive-off

2. Hooking 6dof to fluid Zone enclosing the turbine (which has all exterior surfaces defined as interface). The only wall inside the zone is turbine. here 6dof-on, passive-on

Will this kind of a strategy calculate fluid forces and moments on the turbine and rotate the turbine along with the zone enclosing it?

My axis of rotation is Y and I am restricting the all translation and x,z rotation using

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_Z] = TRUE;

Please discuss if you have some thoughts..
Mithun MG

Hi everyone

I have been working on moving projectile in barrel. I need udf for dynamic mesh(Six degree of freedom solver). can anyone help me?