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

Error in initializing solution (invalid float)

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 10, 2013, 10:23
Default Error in initializing solution (invalid float)
  #1
New Member
 
Michael
Join Date: Nov 2013
Posts: 8
Rep Power: 5
myaero is on a distinguished road
Hi everyone!

I am currently analyzing an airfoil on Fluent (incompressible flow).
When initializing the solution I get this error:

Error: Domainvar_Get_Float: invalid float
Error Object: -1.#ind

I don't know what it means. I saw a topic of 2005 saying that it was probably the boundary conditions or the mesh but I don't see what is wrong in my case.

My mesh consists of an inflation (smallest layer about 1e-7 m) and triangles around.
My BC are simply the lower and upper sides of the airfoil which are considered as walls (no slip, etc), a farfield with a gauge pressure of 95000, M=0.28, Xcomp= 0.99963, Ycomp= 0.02705 and I also have two other BC ("fff-surface" and "interior_fff-surface") that I suppose come from the geometry that I created during the first stage in space claim and are defined as an "interior" type.

Can you help me?

cheers!
myaero is offline   Reply With Quote

Old   December 10, 2013, 12:38
Default
  #2
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,311
Rep Power: 22
flotus1 will become famous soon enoughflotus1 will become famous soon enough
What is the output when you click on "mesh->check" ?
flotus1 is offline   Reply With Quote

Old   December 11, 2013, 12:05
Default
  #3
New Member
 
Michael
Join Date: Nov 2013
Posts: 8
Rep Power: 5
myaero is on a distinguished road
Hi, thanks for the reply!

Here it is:

Domain Extents:
x-coordinate: min (m) = -3.999947e+01, max (m) = 4.000050e+01
y-coordinate: min (m) = -3.897546e+01, max (m) = 4.097702e+01
Volume statistics:
minimum volume (m3): 3.381924e-10
maximum volume (m3): 1.471395e+01
total volume (m3): 5.021998e+03
Face area statistics:
minimum face area (m2): 5.555087e-07
maximum face area (m2): 6.414105e+00
Checking mesh.................
WARNING: The mesh contains high aspect ratio quadrilateral,
hexahedral, or polyhedral cells.
The default algorithm used to compute the wall
distance required by the turbulence models might
produce wrong results in these cells.
Please inspect the wall distance by displaying the
contours of the 'Cell Wall Distance' at the
boundaries. If you observe any irregularities we
recommend the use of an alternative algorithm to
correct the wall distance.
Please select /solve/initialize/repair-wall-distance
using the text user interface to switch to the
alternative algorithm.
........
Done.

I don't know why it says something about "volume area" because I am working in 2D.
And then well it is just a warning. I used high aspect ratio cells (quadrilaterals) for the boundary layer, I think it is a correct algorithm...
myaero is offline   Reply With Quote

Old   December 11, 2013, 12:12
Default
  #4
New Member
 
Michael
Join Date: Nov 2013
Posts: 8
Rep Power: 5
myaero is on a distinguished road
BTW I also noticed that my orthogonal quality is very low: 4e-3.
But my mesh is alerady extremely refined around the airfoil:

The "element size" is about 2e-3 m
My first layer thickness around the airfoil is 5.5e-7 m

Only the farfield has cells of size 6 m (but they are at 50 or 70 m from my airfoil so I don't think it is a problem...).
myaero is offline   Reply With Quote

Old   December 11, 2013, 12:29
Default
  #5
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,311
Rep Power: 22
flotus1 will become famous soon enoughflotus1 will become famous soon enough
Concerning the high aspect ratio cells, this is a common warning message for simulations at high Reynolds numbers. Nevertheless, I recommend that you do what the warning message says and have a look at the cell wall distance computed by fluent.
You might simply produce a xy plot of the cell normal distance along the wall.
Never mind the "volume" statistics for a 2d mesh, the output is always the same no matter if the mesh is 2d or 3d.

Since your mesh quality is extremely low, you should consider that this might cause the errors. Keep in mind that a "fine" mesh does not equal a mesh with good quality.
With some pictures of the mesh and more info on how (which software, settings) it was created we should be able to give you a hint on how to improve it.

Since you get the error on initialization: is there anything special about your initialization values?
Do you still get the same error when using a velocity boundary condition instead of the far field bc?
flotus1 is offline   Reply With Quote

Old   December 12, 2013, 06:09
Default
  #6
Member
 
vidyanand
Join Date: Nov 2011
Location: bangalore,india
Posts: 66
Rep Power: 10
Vidyanand Kesti is on a distinguished road
this error we got usually for boundary condition, please check the bc and units, sometime i face the problem in periodic model, try to use smooth and swap option to increase the quality
Vidyanand Kesti is offline   Reply With Quote

Old   December 13, 2013, 06:43
Default
  #7
New Member
 
Michael
Join Date: Nov 2013
Posts: 8
Rep Power: 5
myaero is on a distinguished road
Hi,

I uploaded some pictures.

I also tried to do as the warning says but:
1/ I cannot compute the cell-wall-distance because to do so I need to initialize the solution (with standard values). But when I do that I get the same error of invalid float...
2/ I entered solve/initialize/repair in the text user interface. But it said that wall distance repair wasn't needed. Here is what I got:

> / solve initialize repair-wall-distance

repair-wall-distance doesn't seem to be required; proceed anyway? [no] yes

Enabled correction of wall distance at high aspect ratio
quadrilateral, hexahedral, and polyhedral cells.
Warning: compute-wall-distance: wall distance not required by enabled models.


I don't think my values for the initialize have something special. I just say "standard initialization" and compute from "farfield". The values are automatically set up.

And well for the BC I cannot use a velocity BC because my domain is a sphere so I cannot really set somethine like inlet/outlet (if that is what you mean).
My BC are quite simple actually. The detail of them is in my first post, but tell me if you need to know somehting else!
As for the software I used "ANSYS meshing". What I did is:
1/ upload the airfoil with the domain (from spaceclaim, which is like Design Modeler). My arifoil is surrounded by two quadrilateral domains. I also added straight lines at the trailing edge to divide it in several sections (easier for inflation). You can see it in the pictures.
2/ Set up a method with triangles
3/ Set up two "Sizing" around my airfoil to get more accurate data (elements of size 2mm and 5 mm)
4/ Set up an inflation to capture the boundary layer. My first layer is about 5.5e-7 mm and I have 70 of them with a growth ratio of 1.1

Mesh1.jpg

Mesh2.jpg

Mesh3.jpg

DomainAroundAirfoil.jpg

TrailingEdge.jpg

Thanks a lot for your comments!
myaero is offline   Reply With Quote

Old   December 13, 2013, 06:55
Default
  #8
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,311
Rep Power: 22
flotus1 will become famous soon enoughflotus1 will become famous soon enough
Are you using double precision in Fluent? I highly recommend that.
flotus1 is offline   Reply With Quote

Old   December 13, 2013, 07:10
Default
  #9
Senior Member
 
Join Date: Jan 2010
Location: Germany
Posts: 268
Rep Power: 9
Zaktatir is on a distinguished road
Double Precision!

But your quality is poor!

Enhance quality and try again
Zaktatir is offline   Reply With Quote

Old   December 13, 2013, 08:48
Default
  #10
New Member
 
Michael
Join Date: Nov 2013
Posts: 8
Rep Power: 5
myaero is on a distinguished road
Why do you mean by double precision?

And how do you see that my quality is poor? Is it because of the huge cells far from the airfoil?
myaero is offline   Reply With Quote

Old   December 13, 2013, 10:38
Default
  #11
New Member
 
Michael
Join Date: Nov 2013
Posts: 8
Rep Power: 5
myaero is on a distinguished road
Or maybe this part is not very good (see attached picture)... I removed some lines at the TE (now I only have two, starting at the vertical part of the TE) because I had some problems with the inflation.

When I click on "meshing" this is what I get if I zoom on the TE:

TrailingEdgeMesh.jpg

When I check my mesh quality, it says that the minimum orthogonal quality is about 5e-3 (which is too low). I think it comes from this part of the mesh. Is that what you were refering to whan you talked about my mesh quality?

But then I am not really sure how to improve that, the TE is what it is... the sharp angle ("bottom" of the TE) is always going to be there.
myaero is offline   Reply With Quote

Old   December 17, 2013, 07:12
Default
  #12
New Member
 
Michael
Join Date: Nov 2013
Posts: 8
Rep Power: 5
myaero is on a distinguished road
Well in the end I think I fixed the problem.

I just set the Flow Courant Number to 1 (it was set to 5 before) and I also ticked the box "pseudo-transient" which is recommanded when you have high aspect ratio cells. Then I just set up the length scale to 1 (length of my airfoil).
And it worked! The solution converges where what seems to be proper values.

Thank you for your help, all of you!
myaero is offline   Reply With Quote

Reply

Tags
error, float, fluent, initialization

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
Pressure outlet boundary condition rolando OpenFOAM Running, Solving & CFD 59 January 26, 2016 22:01
grid dependancy gueynard a. Main CFD Forum 19 June 27, 2014 21:22
Problems building Paraview 3.12 on Gentoo Linux pajot OpenFOAM Installation 11 April 11, 2013 08:09
CFL Condition Matt Umbel Main CFD Forum 14 January 12, 2001 15:34
Wall functions Abhijit Tilak Main CFD Forum 6 February 5, 1999 02:16


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