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

A wall has been placed

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 18, 2010, 03:37
Default A wall has been placed
  #1
Senior Member
 
Join Date: Mar 2009
Posts: 138
Rep Power: 8
camoesas is on a distinguished road
Hello Everybody,

I have a problem with a simulation in CFX. The Problem is:

The geometry is as simple as that: a board with an ellipse at the beginning. In the middle of the board i have a hot aluminium plate. Three Free Slip walls, one Symmetry plane, Inlet, Outlet, 10e6 nodes, structured mesh

I have already done a simulation with the following boundarys:

- SST
- Inlet: 10 (m/s), Tu = 0.1 ; l=10mm, 300K
- Outlet: 0 Pa
- Ansys V11

and it worked fine.

Now I have the same case just with a little change, there is a wire behind the ellipse to increase turbulence.

But now it isnt working at all, I get the message:
- " A wall has been placed at portion(s) of an OUTLET..."
- The maximum Mach number is about 10
- The Residuals drop to 1e-100
- The Result File is completely empty

I have already changed a lot of parameters but nothing helped.

Any Ideas, Solutions, deja vus? Any more informations?

Thanks a lot

Camoesas
camoesas is offline   Reply With Quote

Old   May 18, 2010, 07:57
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
What is your reference pressure? If your outlet is 0 Pa then you will need a finite reference pressure or you will have problems.

The error message suggests the wire is causing convergence problems. A wire in high Ma flows is going to have shocks and rarefactions and all sorts of complex stuff happening so will be a lot harder to converge than high Ma flow over a flat plate.

You will probably need to start with small time steps and increase them as the simulation proceeds. Also make sure your mesh quality is good.
ghorrocks is offline   Reply With Quote

Old   May 18, 2010, 08:50
Default
  #3
smn
Member
 
Join Date: Jun 2009
Posts: 56
Rep Power: 8
smn is on a distinguished road
have you used "outlet" or "opening" boundary conditions?
smn is offline   Reply With Quote

Old   May 19, 2010, 03:32
Default
  #4
Senior Member
 
Join Date: Mar 2009
Posts: 138
Rep Power: 8
camoesas is on a distinguished road
HI,

My reference Pressure is 101325 Pa. The Flow velocity should be 10 m/s, thus far far away from supersonic.
For the Outlet I use outlet and not Opening

Regards
camoesas is offline   Reply With Quote

Old   May 19, 2010, 18:28
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Then why are you running a compressible flow solver? You have to be using a compressible solver as it was talking about Mach numbers. Go back to an incompressible solver and I bet it converges just fine.
ghorrocks is offline   Reply With Quote

Old   May 21, 2010, 04:05
Default
  #6
Senior Member
 
Join Date: Mar 2009
Posts: 138
Rep Power: 8
camoesas is on a distinguished road
Hey Glenn,

thats interesting, but after a lot of searching and aimless clicking in Ansys I still don't know where to choose compressible / incompressible solver!

I can't remember ever seen such a menu


Could you please lift the fog! Thanks
camoesas is offline   Reply With Quote

Old   May 21, 2010, 04:10
Default
  #7
New Member
 
Arsene Noume
Join Date: May 2010
Posts: 4
Rep Power: 7
energic is on a distinguished road
Hello!
I'm simulating a centrifugal compressor and i have the same problem (a wall has been placed at portion of an outlet boudary condition...)
I tried by setting a static pressure as outlet boundary condition but the situation persist.
I just want to know if your problem has been solve, and how? it could help me.
Thankyou
energic is offline   Reply With Quote

Old   May 21, 2010, 06:35
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Quote:
where to choose compressible / incompressible solver!
Unfortunately everybody in the world calls them incompressible and compressible solvers, but CFX is different. In CFX to activate the compressible solver you have to have a compressible fluid model chosen (such as ideal gas) and select the total energy equation option for heat transfer. If you select an incompressible material (eg constant density gas) or "thermal energy" heat transfer model you will be using the incompressible solver.
ghorrocks is offline   Reply With Quote

Old   May 21, 2010, 08:52
Default
  #9
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
Quote:
Hello!
I'm simulating a centrifugal compressor and i have the same problem (a wall has been placed at portion of an outlet boudary condition...)
I tried by setting a static pressure as outlet boundary condition but the situation persist.
I just want to know if your problem has been solve, and how? it could help me.
Thankyou
This occours at higher PR, when for example separations reach the outlet face (in my experience). You should switch to opening.
Attesz is offline   Reply With Quote

Old   May 22, 2010, 06:53
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Quote:
You should switch to opening.
A better approach is to move the outlet boundary downstream so there is no reverse flow. Reverse flow at the outlet (whether it is an outlet or an opening) is harder to converge than one with no reverse flow.
ghorrocks is offline   Reply With Quote

Old   May 28, 2010, 04:59
Default
  #11
Senior Member
 
Join Date: Mar 2009
Posts: 138
Rep Power: 8
camoesas is on a distinguished road
Hello Everybody,

Thank you for trying to help me.

Now me Simulation is just running fine! It was the mesh indeed. I got a new one and now everything s fine!
camoesas 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
Fluent3DMeshToFoam simvun OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 48 May 14, 2012 05:20
Errors running allwmake in OpenFOAM141dev with WM_COMPILE_OPTION%3ddebug unoder OpenFOAM Installation 11 January 30, 2008 21:30
AMG versus ICCG msrinath80 OpenFOAM Running, Solving & CFD 2 November 7, 2006 16:15
Multicomponent fluid Andrea CFX 2 October 11, 2004 05:12
help with wall functions Nick Georgiadis Main CFD Forum 4 February 20, 2000 18:07


All times are GMT -4. The time now is 15:15.