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

dsmcFieldsCalc not calculating

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

Like Tree1Likes
  • 1 Post By wyldckat

Reply
 
LinkBack Thread Tools Display Modes
Old   November 14, 2012, 17:23
Default dsmcFieldsCalc not calculating
  #1
New Member
 
Join Date: Aug 2011
Posts: 3
Rep Power: 5
yellowCamel is on a distinguished road
Hello, I am using dsmcFoam to simulate a cold gas thruster that vents to a near vaccum. I used the supersonic wedge as my basis and adjusted the initial conditions for my problem. The geometry is just three concentric cylinders of growing diameter. The first cylinder having a inlet on its face and the final cylinder having an outlet on all faces except the area that interests with the middle cylinder. I am able to intialize and run the program, but when it comes to running the dsmcFieldsCalc, it breaks down. This is the error message that I recieve when I try running the command: Small value (min(mag(rhoNMean)) [0 -3 0 0 0 0 0] 9.99e-301) found in rhoNMean field. Not calculating dsmcFields to avoid division by zero. Has anyone come across this problem before and can explain how they fixed this? Thanks, yc
yellowCamel is offline   Reply With Quote

Old   January 15, 2013, 04:42
Default
  #2
Senior Member
 
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 277
Rep Power: 9
vinz is on a distinguished road
I can't help you much since I have the same problem.
Did you find a solution?
vinz is offline   Reply With Quote

Old   February 14, 2013, 07:14
Default
  #3
T-1
New Member
 
Join Date: Feb 2013
Posts: 1
Rep Power: 0
T-1 is on a distinguished road
Yellow / vinz this happens in the very low density regions. (In paraview you can identify these cells using threshold whilst viewing the density fields.)
I had a similar problem and used some scripting as a quick fix. If you havent resolved the issue since your last message, post your case and i'll check if i can help.
T-1 is offline   Reply With Quote

Old   February 14, 2013, 09:30
Default
  #4
Senior Member
 
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 277
Rep Power: 9
vinz is on a distinguished road
Hello T-1,

The problem looks to be related to the fact that we are simulating wedges which apparently not handled by dsmcFoam so far.
vinz is offline   Reply With Quote

Old   May 1, 2013, 15:47
Default dsmcfield not calculating
  #5
New Member
 
murali
Join Date: Feb 2013
Location: pondicherry
Posts: 10
Rep Power: 4
murali is on a distinguished road
hello T-1

i am also facing same problem, Small value (min(mag(rhoNMean)) [0 -3 0 0 0 0 0] 9.99e-301) found in rhoNMean field. Not calculating dsmcFields to avoid division by zero. calculating averages


can you help me to solve this error
murali is offline   Reply With Quote

Old   February 11, 2014, 05:20
Default same problem :/
  #6
Member
 
Join Date: Jul 2013
Posts: 62
Rep Power: 3
CFDnewbie147 is on a distinguished road
Hello, does anybod fix this problem and have a solution?
Please answer if you know it.

Best regards
CFDNewbie147
CFDnewbie147 is offline   Reply With Quote

Old   February 16, 2014, 11:40
Default
  #7
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,251
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings CFDNewbie147,

I'm sorry to say that everyone who asked about this on this thread, did not follow the basic instructions on How to give enough info to get help

The very most basic question is: what were the exact steps that were taken to reach that message?

Beyond this:
  1. Which OpenFOAM version is being used?
  2. Which tutorial are you using?
  3. If not a tutorial, on which tutorial did you base yourself on?
  4. Can you share a simple test case in which this can be reproduced?
edit: The following thread seems to be a long discussion on a similar topic: dsmcInitialise - dsmcFoam

Best regards,
Bruno

Last edited by wyldckat; February 18, 2014 at 16:14. Reason: see "edit:" | Rephased from "This thread" to "The following thread"
wyldckat is offline   Reply With Quote

Old   February 17, 2014, 02:49
Default
  #8
Member
 
Join Date: Jul 2013
Posts: 62
Rep Power: 3
CFDnewbie147 is on a distinguished road
Hello Bruno,

thank you for answering.

1. I use the OpenFOAM version 2.2.1
2./3. I use the the wedge15Ma5 dsmc tutorial as base for my simulations
I took the simulation case and adapted it to an extern built mesh which I've imported to OpenFOAM without any failures in checkMesh. It looks like a windtunnel with inlet, outlet, walls and the geometry inside the windtunnel. As in the wedge15Ma5 tutorial i made the sides of the windtunnel to the "flow" region with "patch" and the geometry itself as the "obstacle".

With this i do the dsmcInitialise where particles are inserted and then I do dsmcFoam. But when doing the dsmcFieldsCalc there's always the mentioned failure message.

4. It's "only" a windtunner with an object inside it. So yes I can or anybody can built it quickly. (e.g from motorbike tutorial)

I hope this will be enough information.

Best regards
CFDNewbie147
CFDnewbie147 is offline   Reply With Quote

Old   February 22, 2014, 11:30
Default
  #9
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,251
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi CFDnewbie147,

I'm not very familiar with these solvers. But I've found the file "discreteMethods/dsmcFoam/README" in the "tutorials" folder, which has some crucial information on what fields are used by this solver.

Beyond this, please provide a simple case that reproduces this problem. That way it'll take me considerably little time to try and diagnose the problem. Otherwise, don't expect me to give any answers on this before July 2014

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   February 27, 2014, 03:11
Default
  #10
Member
 
Join Date: Jul 2013
Posts: 62
Rep Power: 3
CFDnewbie147 is on a distinguished road
Hello again,

I think I solved the problem. When you look at the file "discreteMethods/dsmcFoam/README" as you've said: [...]"setting zeroGradient boundary conditions on walls" [...] for iDof, internalE, linearKe, momentum, rhoM and rhoN.
I changed the originally "calculated" for my wall to zeroGradient and the dsmcFields-calculation works and i get overallT, UMean and so on...

I don't know exactly why there was calculated because these parameters are only relevant for cell data but now it works. If anybody does have some hints, please answer

Best regards
CFDNewbie148
CFDnewbie147 is offline   Reply With Quote

Old   March 1, 2014, 06:26
Default
  #11
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,251
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi CFDnewbie147,

Quote:
Originally Posted by CFDnewbie147 View Post
I changed the originally "calculated" for my wall to zeroGradient and the dsmcFields-calculation works and i get overallT, UMean and so on...

I don't know exactly why there was calculated because these parameters are only relevant for cell data but now it works. If anybody does have some hints, please answer
It's somewhat simple to explain:
  • "zeroGradient" means that the patch imposes that the derivative must be zero, therefore there is a constraint in the boundary that will make the field values in cells adjacent to the patch to bend the flow in order to make the first derivative equal to zero. Note: this is usually necessary in situations where the equations need a constraint on a boundary, in order to be able to find a solution.
  • "calculated" means that anything that goes through the patch is inferred from the adjacent cells, without further restrictions. As you've mentioned, this is usually used in situations where either only the cell data is relevant or if the fields are fully calculated based on other fields.
Best regards,
Bruno
CFDnewbie147 likes this.
wyldckat is offline   Reply With Quote

Reply

Tags
calc, dsmc, dsmcfieldscalc, dsmcfoam, error

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
calculating buoyancy of a floating body raghav777 CFX 0 June 27, 2011 02:57
Calculating forces on a non-closed surface ScottN FLUENT 0 March 1, 2011 18:18
Problems in calculating the fluid traction on the current structure frame in 3D models fw407 OpenFOAM Running, Solving & CFD 0 August 6, 2008 12:04
Calculating time thuy FLUENT 5 April 10, 2008 04:23
How to update polyPatchbs localPoints liu OpenFOAM Running, Solving & CFD 6 December 30, 2005 18:27


All times are GMT -4. The time now is 23:45.