CFD Online URL
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[GAMBIT] Question about Boundary Conditions with mobile cylinder involved

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

Like Tree1Likes
  • 1 Post By -mAx-

Reply
 
LinkBack Thread Tools Display Modes
Old   May 29, 2012, 17:43
Default Question about Boundary Conditions with mobile cylinder involved
  #1
New Member
 
Sam
Join Date: May 2012
Posts: 8
Rep Power: 4
samolcue is on a distinguished road
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:



If anyone can explain me I will be so grateful.
samolcue is offline   Reply With Quote

Old   May 29, 2012, 23:39
Default
  #2
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,902
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
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.
Far is offline   Reply With Quote

Old   May 30, 2012, 01:31
Default
  #3
New Member
 
Sam
Join Date: May 2012
Posts: 8
Rep Power: 4
samolcue is on a distinguished road
Quote:
Originally Posted by Far View Post
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?
samolcue is offline   Reply With Quote

Old   May 30, 2012, 01:43
Default
  #4
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,861
Rep Power: 29
-mAx- will become famous soon enough
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
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   May 30, 2012, 02:34
Default
  #5
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,902
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
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?
Far is offline   Reply With Quote

Old   May 30, 2012, 02:48
Default
  #6
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,861
Rep Power: 29
-mAx- will become famous soon enough
Quote:
Originally Posted by Far View Post
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.
Far likes this.
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   May 30, 2012, 15:39
Default
  #7
New Member
 
Sam
Join Date: May 2012
Posts: 8
Rep Power: 4
samolcue is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
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 View Post
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- View Post
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
samolcue is offline   Reply With Quote

Old   May 31, 2012, 01:49
Default
  #8
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,861
Rep Power: 29
-mAx- will become famous soon enough
Quote:
Originally Posted by samolcue View Post
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 View Post
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
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   June 25, 2012, 13:47
Default
  #9
New Member
 
Sam
Join Date: May 2012
Posts: 8
Rep Power: 4
samolcue is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
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
samolcue is offline   Reply With Quote

Old   June 26, 2012, 04:11
Default
  #10
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,861
Rep Power: 29
-mAx- will become famous soon enough
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)
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- 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
Boundary Conditions Thomas P. Abraham Main CFD Forum 20 July 7, 2013 06:05
question about boundary conditions Nick R CFX 2 February 21, 2011 19:58
Question about boundary conditions Damiano FLUENT 2 January 30, 2007 04:59
Basic Boundary Conditions Question vcoralic OpenFOAM Pre-Processing 0 June 26, 2006 08:56
Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 05:15


All times are GMT -4. The time now is 23:11.