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

Problem in initializing transient simulation with a finer mesh

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 22, 2013, 11:48
Default Problem in initializing transient simulation with a finer mesh
  #1
New Member
 
Mustafa
Join Date: Jan 2012
Posts: 7
Rep Power: 5
sidd is on a distinguished road
Hello,

I am trying to initialize a transient simulation in CFX 14.5. The domain represents a nuclear fuel pin with wire spacers.

I run a steady state simulation (inlet outlet BCs) with around 4 hundred thousand nodes. I get the steady simulation results file and initialize the same mesh transient simulation (periodic BCs). It runs fine. (See Attachments)

Next I refine that mesh to a 3 million node mesh and then follow the same procedure: Get a steady state results file to initialize a transient simulation. For some reason, this does not work! My velocity goes to near zero in the mean flow at the very first time step of the transient simulation. (See Attachments)

I have the same setup and everything. The only thing I change is that I scale my mesh in ICEM to a higher node code.

I don't know what I am doing wrong, but this does not make sense to me.

P.S.: Even if I initialize with a csv file, it doesn't work.

Thanks,
Mustafa
Attached Images
File Type: jpg Figure_1.jpg (87.9 KB, 53 views)
File Type: jpg Figure_2.jpg (86.1 KB, 49 views)
sidd is offline   Reply With Quote

Old   April 22, 2013, 18:31
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,665
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Looks like a problem with interpolation of the initial conditions onto the fine mesh.

The output file contains some information about the interpolation process at the start. Can you post this?

You might have to manually interpolate the initial condition using the command line cfx5interp. This will give you more control about what is goign on and hopefully a path to fix it.
ghorrocks is offline   Reply With Quote

Old   April 23, 2013, 11:29
Default
  #3
New Member
 
Mustafa
Join Date: Jan 2012
Posts: 7
Rep Power: 5
sidd is on a distinguished road
Hello Ghorrocks,

I tried to look at the interpolation information and other information in the two files, but they look very "similar" to me.

I am attaching two output files with this message. You might notice that the one that works has a mesh of 2.4 million nodes, while the other that does not work has 2.8 million nodes.

I am guessing it is not a mesh problem. If it was a mesh problem, I would see regions of unrealistic behavior, but here the whole domain seems to have almost zero velocity. Am I right in thinking this way?

Thanks
Attached Files
File Type: docx Works.docx (40.2 KB, 20 views)
File Type: docx Does_not_work.docx (49.3 KB, 5 views)

Last edited by sidd; April 23, 2013 at 15:38.
sidd is offline   Reply With Quote

Old   April 23, 2013, 17:04
Default
  #4
Senior Member
 
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 471
Rep Power: 10
singer1812 is on a distinguished road
Umm. Your GGI isnt set right on your 2.8M element case.

2.8M case (no connection):

Domain Interface Name : Domain Interface 1

Discretization type = GGI
Intersection type = Direct
Non-overlap area fraction on side 1 = 1.00E+00
Non-overlap area fraction on side 2 = 1.00E+00

2.4M case (connection):

Domain Interface Name : Domain Interface 1

Discretization type = GGI
Intersection type = Partitioner
Non-overlap area fraction on side 1 = 0.00E+00
Non-overlap area fraction on side 2 = 0.00E+00


Might want to fix that.
singer1812 is online now   Reply With Quote

Old   April 24, 2013, 20:41
Default
  #5
New Member
 
Mustafa
Join Date: Jan 2012
Posts: 7
Rep Power: 5
sidd is on a distinguished road
Hi Singer and Ghorrocks,

I think I have got something. I think it is a mesh problem.

You can see me domain in the attachments with the first post. If you look carefully in the fine mesh case in Figure 2, you will see a black line that follows the pin axially and this line is not present in the coarse mesh case.

So what was happening was that the fine mesh had automatically created a region called Primitive 2D for some reason. And due to that it was not initializing properly.

I will run some more tests to confirm this and explain what I am talking about.

It's quite late here now.

Thanks,
Mustafa
sidd is offline   Reply With Quote

Old   May 2, 2013, 12:29
Default
  #6
New Member
 
Mustafa
Join Date: Jan 2012
Posts: 7
Rep Power: 5
sidd is on a distinguished road
Hello,

Sorry for the late response. So I figured out the problem and fixed it. Take a look at the two attachments and it explains that there was some mesh error that was causing the problem. You can see that the mesh looks fine in ICEM, but when it is imported into CFX, you find an extra region in the mesh.

As a reminder: I was trying to initialize a transient simulation with some data, but it worked for a coarse mesh but not for a fine mesh.

How did I fix it? I just reduced some nodes in the region where that "Primitive 2D region" was appearing.

Why was the software doing it? I am not quite sure about it. Maybe I could ask this question in the ICEM forum that the mesh looks fine in ICEM but adds an extra part in CFX.

Thanks,
Mustafa
Attached Images
File Type: jpg Found_the_cause.jpg (85.6 KB, 35 views)
File Type: jpg ICEM_Mesh_closeup.jpg (52.0 KB, 43 views)
sidd is offline   Reply With Quote

Old   April 1, 2015, 16:41
Default
  #7
New Member
 
Join Date: Nov 2014
Posts: 9
Rep Power: 2
venkatesh92 is on a distinguished road
Hi,

I am not sure if you sorted this problem out! But my best guess is that an edge was not suppressed in the geometry and it shows up in fluent as a weird solid body. It is best to suppress all the edges/faces in the geometry and leave the solid body alone for the mesher to handle!
venkatesh92 is offline   Reply With Quote

Reply

Tags
ansys cfx, initialization, transient analysis

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
SnappyHexMesh for internal Flow vishwa OpenFOAM Native Meshers: snappyHexMesh and Others 23 August 6, 2014 03:50
2D Mesh Generation Tutorial for GMSH aeroslacker Open Source Meshers: Gmsh, Netgen, CGNS, ... 12 January 19, 2012 04:52
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10
Problem about 3D blunt body high Re simulation David FLUENT 0 September 27, 2002 10:59
unstructured vs. structured grids Frank Muldoon Main CFD Forum 1 January 5, 1999 11:09


All times are GMT -4. The time now is 13:11.