CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Axisymmetric simulation with circumferencial outlets

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 31, 2018, 07:49
Default Axisymmetric simulation with circumferencial outlets
  #1
New Member
 
Gioacchino La Rochelle
Join Date: Jul 2016
Posts: 19
Rep Power: 9
Gioacchino La Rochelle is on a distinguished road
Hello all,
To reduce computational costs, I decided to pass to a 2D simulation of my geometry.
It is a receiver with a single inlet (bottom) and many outlets set radially and an open side to environmental air.

My question is whether my workflow is ok (after collecting infos on the web):
1. geometry obtained by revolution of a plane (about 3)
2. mesh of 1 element depth (and for not sweepable bodies?)
3. setting interface 'rotational periodicity' on the symmetry planes?

Thanks
Gioacchino La Rochelle is offline   Reply With Quote

Old   July 31, 2018, 18:41
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,692
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
1. Yes, a 3 arc is in the normal range.
2. Yes, the mesh should be 1 element thick. I do not understand the comment about sweepable bodies.
3. Normally you would put symmetry planes on both faces. You can put rotational periodicity - this will allow a velocity normal to the faces and will allow you to model swirling flows.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   August 1, 2018, 07:19
Default
  #3
New Member
 
Gioacchino La Rochelle
Join Date: Jul 2016
Posts: 19
Rep Power: 9
Gioacchino La Rochelle is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
1. Yes, a 3 arc is in the normal range.
2. Yes, the mesh should be 1 element thick. I do not understand the comment about sweepable bodies.
3. Normally you would put symmetry planes on both faces. You can put rotational periodicity - this will allow a velocity normal to the faces and will allow you to model swirling flows.
Thank you for the answer!
The problem I have on mesh (I haven't fixed it yet) is that even though I apply sweep method on my mesh and set 1 division, it happens that more than 1 division realises actually.

The deficit of swepable bodies is in CFX-pre, because of the setting of boundary conditions and the large number of interfaces/connectivity to set.
Is there any way to glue the mesh still in the ANSYS mesher so that I can read only outer face on CFX-pre?
I'm a bit warried about too much setting on interfaces on CFX-pre ...
Gioacchino La Rochelle is offline   Reply With Quote

Old   August 1, 2018, 08:03
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,692
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Quote:
The problem I have on mesh (I haven't fixed it yet) is that even though I apply sweep method on my mesh and set 1 division, it happens that more than 1 division realises actually.
Things like this is exactly why I don't like ANSYS Meshing. You will find you have much better control over the mesh with ICEM, but it will require some effort to learn. If you want to stick with ANSYS Mesh there are ways to get it to give you the mesh you want but it is always frustrating finding it.

In DesignModeller, if you define the large number of bodies as a multi-body part then they will be meshed with a contiguous mesh and there is no need for interfaces.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   August 1, 2018, 08:52
Default
  #5
New Member
 
Gioacchino La Rochelle
Join Date: Jul 2016
Posts: 19
Rep Power: 9
Gioacchino La Rochelle is on a distinguished road
I succeded!
I write a little guide below.

Guide 'How to mesh any 2D domain single-body with topological issue (e.g. no sweepable bodies) using the Sweep method and local refinement without compromise mesh quality and aspect ratio'
1. Spaceclaim: build your mesh starting from a 2D sketch and pull along a rotation axis (this will reduce the error of face size) of an angle below 3
2. ANSYS mesher: set 'Uniform' size function in global mesh setting. Set the element size and max element size as you wish according to your geometry pattern.
3. Right click on 'mesh' and add method>sweep>manual selection of source and target face. Now select the two faces of axisymmetric domain. Remember to set the number of division equal to 1.
4. Right click on 'mesh' and add 'Match control'. Select the same faces as High/Low and express the rotation axis.
5. Mesh refinement: use sphere of influence (preferred for cavity or closed volumes) or edge sizing (warning to the characteristic length of the side your considering).

Using the manual sweep setting together with the sphere of influence one can build a mesh for profile don't recognised sweepable and with aspect ratio below 20 for a domain of 24x24 m^2.

Last edited by Gioacchino La Rochelle; August 6, 2018 at 08:50.
Gioacchino La Rochelle is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Simulation of Axisymmetric Free Jet using LRR Reynolds Stress Model skyinventorbt OpenFOAM 1 January 2, 2022 17:42
Use homogeneous results as the initial guess for an inhomogeneous simulation JuPa CFX 5 December 26, 2014 13:44
High Frequency Residual Oscillation in Axisymmetric with Swirl Simulation newbie384 FLUENT 0 July 8, 2013 08:25
Axisymmetric simulation alexandre FLUENT 6 March 7, 2003 04:31
3-D Contaminant Dispersal Simulation Apple L S Chan Main CFD Forum 1 December 23, 1998 10:06


All times are GMT -4. The time now is 13:47.