CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [GAMBIT] Question about Boundary Conditions with mobile cylinder involved (http://www.cfd-online.com/Forums/ansys-meshing/102604-question-about-boundary-conditions-mobile-cylinder-involved.html)

samolcue May 29, 2012 16:43

Question about Boundary Conditions with mobile cylinder involved
 
I want to solve the following problem, how affects an airfoil the attachment of one cylinder with blades that redirects the airflow toward the airfoil.

First, I'm trying to solve it as a 2D problem but I'm having some problems when I have to put the "Boundary Conditions".

How can I impose that the cylinder with blades can move because of the airflow and this affect the airfoil?

This is an image of what I'm trying to explain:

http://i46.tinypic.com/1pjc4y.jpg

If anyone can explain me I will be so grateful.

Far May 29, 2012 22:39

Quote:

How can I impose that the cylinder with blae.des can move because of the airflow and this affect the airfoil?
This cannot be done. However you can adopt the approach of turbomachinery, where you simulate the case for different condition i.e. specifying the inlet velocity, rpm of blade disk and check the results. Got it? I can tell you how to set interfaces for the both domains.

samolcue May 30, 2012 00:31

Quote:

Originally Posted by Far (Post 363700)
This cannot be done. However you can adopt the approach of turbomachinery, where you simulate the case for different condition i.e. specifying the inlet velocity, rpm of blade disk and check the results. Got it? I can tell you how to set interfaces for the both domains.

First of all, thanks for you reply.

When you say that it cannot be done, do you mean in GAMBIT-FLUENT or in all kind of CFD software?

In that case if you can explain me how to implement the two different conditions and I will make some calculations...

Is necesary to make a dynamic mesh in order to implement that?

-mAx- May 30, 2012 00:43

what about sliding mesh with rotor-stator?
you can draw a circle around your impeller, split your domain with this circle.
Then you disconnect the disk (with impeller) from domain, assign interfaces on both fluid domains.
Then in Fluent set up moving mesh with rigid body motion (rotation) and for sure you can describe rotation from torque with a udf

Far May 30, 2012 01:34

Quote:

How can I impose that the cylinder with blades can move because of the airflow and this affect the airfoil?
Quote:

When you say that it cannot be done, do you mean in GAMBIT-FLUENT or in all kind of CFD software?
It cannot be done in all softwares that you just give inlet velocity and it rotates the disk or blades. You have to separately specify the inlet velocity and RPM and that should be based on some preliminary calculations for rough idea.

Another important point is that bladed disk center should be placed at origin or otherwise you will have to specify the offset in the solver. So better idea is to put the disk center at origin.

Quote:

what about sliding mesh with rotor-stator?
you can draw a circle around your impeller, split your domain with this circle.
Then you disconnect the disk (with impeller) from domain, assign interfaces on both fluid domains.
Thats the method and -mAx- described it very nicely.

Quote:

Then in Fluent set up moving mesh with rigid body motion (rotation) and for sure you can describe rotation from torque with a udf
But how we will define the torque? Or in other words without specifying the RPM how can we determine the torque?

-mAx- May 30, 2012 01:48

Quote:

Originally Posted by Far (Post 363714)
But how we will define the torque? Or in other words without specifying the RPM how can we determine the torque?

There is a 6DOF udf : pressure force/torque is computed on body and with twice integration you get the displacement/angle for your motion.

samolcue May 30, 2012 14:39

Quote:

Originally Posted by -mAx- (Post 363712)
what about sliding mesh with rotor-stator?
you can draw a circle around your impeller, split your domain with this circle.
Then you disconnect the disk (with impeller) from domain, assign interfaces on both fluid domains.
Then in Fluent set up moving mesh with rigid body motion (rotation) and for sure you can describe rotation from torque with a udf

Ok, I'm gonna try doing this the problem is that I don't have much knowdledge of GAMBIT and I don't know if I'm doing any error. So is possible that when I have it done I attached it and you check things are done as you said?


Quote:

Originally Posted by Far (Post 363714)
Another important point is that bladed disk center should be placed at origin or otherwise you will have to specify the offset in the solver. So better idea is to put the disk center at origin.

This is not a problem, I have it placed at the origin.

Quote:

Originally Posted by -mAx- (Post 363716)
There is a 6DOF udf : pressure force/torque is computed on body and with twice integration you get the displacement/angle for your motion.

So I understand that I can solve this problem (as I say at the beginning) without impossing a RPM speed to the disc. Is that correct?

Thanks all 2 of you

-mAx- May 31, 2012 00:49

Quote:

Originally Posted by samolcue (Post 363900)
Ok, I'm gonna try doing this the problem is that I don't have much knowdledge of GAMBIT and I don't know if I'm doing any error. So is possible that when I have it done I attached it and you check things are done as you said?

Quote:

Originally Posted by samolcue (Post 363900)
So I understand that I can solve this problem (as I say at the beginning) without impossing a RPM speed to the disc. Is that correct?

I don't have Fluent anymore
I would advice you to test the mdm first with a simple rotor-stator, and with a fixed rpm.
Then try the 6dof, and finally introduce your airfoil

samolcue June 25, 2012 12:47

Quote:

Originally Posted by -mAx- (Post 363712)
what about sliding mesh with rotor-stator?
you can draw a circle around your impeller, split your domain with this circle.
Then you disconnect the disk (with impeller) from domain, assign interfaces on both fluid domains.
Then in Fluent set up moving mesh with rigid body motion (rotation) and for sure you can describe rotation from torque with a udf

Max, I thing that I have done all that you said to me correctly, but I don't know if here I could made some error because when I go to Fluent I don't have the Mesh Interfaces options.

Please correct me if I have done something wrong

1.Import impeler geometry (face)
2.Domain Geometry(face)
3.Circle around impeler.(face)
4.Split Domain face with circle
5.Substract Circle face with impeller.
6.Mesh
7.BC
8.Define 2 cell zones as fluids

I think that I'm doing it correctly but I just wanna be sure, because I don't know if when you said "Then you disconnect the disk (with impeller) from domain" it is well done with my procedure.

Thanks

-mAx- June 26, 2012 03:11

important is that your rotor and stator domain aren't connected.
For that try to move (not copy!) the rotor domain with any vector.
If you are able to do it, then both domains are disconnected
If not, then copy the rotor domain with any vector, delete the original rotor domain, and move back(not copy) the rotor domain.
Take the advantage from this "move" procedure to pick and define the interfaces (else it is more obscur, since they are superposed)


All times are GMT -4. The time now is 11:07.