CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLOW-3D

Void Array Index Warning

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 4, 2010, 15:21
Default Void Array Index Warning
  #1
New Member
 
Joey
Join Date: Sep 2010
Posts: 7
Rep Power: 6
jfasl is on a distinguished road
I'm trying to run a casting simulation but keep getting this message in the warnings and errors...

warning: void array index exceeds maximum nvor = 28467
at cycle = 12938, time = 0.20113E+01
void region volumes and pressures may be incorrect

I have noticed that my fluid volumes are really off in my casting, anyone know why this happens and what to do to alleviate it?
jfasl is offline   Reply With Quote

Old   November 4, 2010, 23:54
Default
  #2
Senior Member
 
michael barkhudarov
Join Date: Mar 2009
Posts: 331
Rep Power: 9
MuxaB is on a distinguished road
It looks like it is going unstable. Can you look at the results? Does the flow look reasonable?

what version are you running?

By itself this message is not critical, just telling you that it cannot keep track of all voidss in the domain and will join some of them to stay within the maximum allowed number of voids. But the fact that you have so many of them is an indication of a severe breakup of the fluid.
MuxaB is offline   Reply With Quote

Old   November 5, 2010, 10:11
Default
  #3
New Member
 
Joey
Join Date: Sep 2010
Posts: 7
Rep Power: 6
jfasl is on a distinguished road
I can look at the results, they look reasonable flow wise, but the volumes I'm getting are way off for filling. I'm running version 9.4.1.
jfasl is offline   Reply With Quote

Old   November 6, 2010, 20:39
Default
  #4
Senior Member
 
michael barkhudarov
Join Date: Mar 2009
Posts: 331
Rep Power: 9
MuxaB is on a distinguished road
Quote:
Originally Posted by jfasl View Post
I can look at the results, they look reasonable flow wise, but the volumes I'm getting are way off for filling. I'm running version 9.4.1.
How can flow look reasonable but volume be way off? They must both be off.

What kind of filling problem is it? high-pressure die casting, gravity?
MuxaB is offline   Reply With Quote

Old   November 8, 2010, 16:16
Default
  #5
New Member
 
Joey
Join Date: Sep 2010
Posts: 7
Rep Power: 6
jfasl is on a distinguished road
It is a gravity casting, the flow PATTERN looks fine, but I used force windows to measure the volume in each cavity of my mold, and the volumes that the windows are showing are not at all what they should be. Basically, the graphics are showing the cavities full, but after calculating the volume of each cavity and comparing it to what the force window says it is, they dont matchup at all. I was wondering if that error had something to do with it.
jfasl is offline   Reply With Quote

Old   November 8, 2010, 23:13
Default
  #6
Senior Member
 
michael barkhudarov
Join Date: Mar 2009
Posts: 331
Rep Power: 9
MuxaB is on a distinguished road
Quote:
Originally Posted by jfasl View Post
It is a gravity casting, the flow PATTERN looks fine, but I used force windows to measure the volume in each cavity of my mold, and the volumes that the windows are showing are not at all what they should be. Basically, the graphics are showing the cavities full, but after calculating the volume of each cavity and comparing it to what the force window says it is, they dont matchup at all. I was wondering if that error had something to do with it.
I don't think it is an error in the force window integration of fluid volume. What about the total volume in the domain? Does it make sense?
MuxaB is offline   Reply With Quote

Old   November 9, 2010, 11:09
Default
  #7
New Member
 
Joey
Join Date: Sep 2010
Posts: 7
Rep Power: 6
jfasl is on a distinguished road
I'm getting extra volume residing above the cavities after they fill. I tried to measure and match the fluid volume at the beginning (using the preprocessor and the "report" message "fluid at time zero") to the volume of the cavities, but even after doing that I'm getting extra slop on top after the simulation has completed.
jfasl is offline   Reply With Quote

Old   November 15, 2010, 13:31
Default
  #8
Senior Member
 
michael barkhudarov
Join Date: Mar 2009
Posts: 331
Rep Power: 9
MuxaB is on a distinguished road
Quote:
Originally Posted by jfasl View Post
I'm getting extra volume residing above the cavities after they fill. I tried to measure and match the fluid volume at the beginning (using the preprocessor and the "report" message "fluid at time zero") to the volume of the cavities, but even after doing that I'm getting extra slop on top after the simulation has completed.
You mean it overfills? Assuming you are using the velocity bc and the flow rate is constant, there may be a couple of reasons your estimate of the filling time is off. One is the cumulative volume error - the loss or gain of total fluid volume due to the approximations of the numerical scheme. The total volume error is reported during the simulation. You can extract it from the flsgrf file too (in general history data).

The second reason is that not all cells m ay be100% full. If the F-packer is on (default), then most cells should be at least 99% full. However, some may have much less fluid, e.g., the last cells in the cavity to fill. The f-packer tries to 'pack' them but it takes some time during which fluid can spill.

Another possible reason is the open area at the inlet is not what you think it is. The pre-processor reports open areas at mesh boundaries in prpout.
MuxaB 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
latest OpenFOAM-1.6.x from git failed to compile phsieh2005 OpenFOAM Bugs 25 February 9, 2010 05:37
Version 15 on Mac OS X gschaider OpenFOAM Installation 120 December 2, 2009 11:23
Compilation errors in ThirdPartymallochoard feng_w OpenFOAM Installation 1 January 25, 2009 07:59
Axisymmetrical mesh Rasmus Gjesing (Gjesing) OpenFOAM Native Meshers: blockMesh 10 April 2, 2007 14:00
Warning 097- AB CD-adapco 6 November 15, 2004 05:41


All times are GMT -4. The time now is 17:39.