Welcome to the forums. Please post in English or French.

You are not logged in.

#1 2011-02-05 00:01:23

rcbsimoes
Member
Registered: 2010-12-09
Posts: 41

simple frame

Hi forum!!

could same one explain why does my simulation ends with:

!------------------------------------------------------------------!
   ! <EXCEPTION> <FACTOR_21>                                          !
   !                                                                  !
   ! (Solveur linéaire LDLT ou MULT_FRONT) Matrice non factorisable ! !
   !   On sait en plus que:                                           !
   !     - pivot est vraiment nul à la ligne 241                      !
   !     - pour le noeud N37 et la composante DX                      !
   !------------------------------------------------------------------!

this should be a realy easy problem...

i'm posting my med, comm, and mess files. just in case...

thanks in advance,
rui


Attachments:
mesa_princ.tar.gz, Size: 7.73 KiB, Downloads: 258

Offline

#2 2011-02-05 01:36:07

tcdonley
Member
From: Virginia, USA
Registered: 2010-11-24
Posts: 94

Re: simple frame

Hello Rui,

Your mesh has coincident nodes which are not actually connected. I have no idea how this would have happened as you built the model, but here's how you can fix it. Well, first I'll tell how I found it:

Using Salome - Mesh module, go to Mesh - Mesh Element Info.

Now click on some of your linear elements along the lines which connect to your fixed nodes, and which you think are connected to the big X.

If you look at the node numbers listed for each element, you'll see the X is not connected to anything!

Here's the fix in Salome Mesh:

Go to Modification- Transformation - Merge Nodes - and use the default tolerance to merge coincident nodes. Now your study will run with very pretty results!

Best regards,

Tim D.

Offline

#3 2011-02-05 13:13:22

rcbsimoes
Member
Registered: 2010-12-09
Posts: 41

Re: simple frame

thanks tcdonley,
that did it!

but does the error indicates that??

i would expect, "orphelis nodes" or "rigid body motion" for this mesh error.

rui

Offline

#4 2011-02-05 14:28:08

ppeetteerr
Member
Registered: 2009-06-30
Posts: 234

Re: simple frame

I believe orphaned nodes are nodes not part of a mesh. All of your nodes are part of a mesh. You simply do not have enough constraints to solve your problem.

Offline

#5 2011-02-05 15:35:02

rcbsimoes
Member
Registered: 2010-12-09
Posts: 41

Re: simple frame

any way, here's how i generated the geometry:
P1 = geompy.MakeVertex(0, 0, 0)
P2 = geompy.MakeVertex(165, 0, 0)
P3 = geompy.MakeVertex(409, 0, 0)
P4 = geompy.MakeVertex(575, 0, 0)
P5 = geompy.MakeVertex(575, 336, 0)
P6 = geompy.MakeVertex(409, 336, 0)
P7 = geompy.MakeVertex(165, 336, 0)
P8 = geompy.MakeVertex(0, 336, 0)
P9 = geompy.MakeVertex(287, 168, 0)
Line_1 = geompy.MakeLineTwoPnt(P1, P2)
Line_2 = geompy.MakeLineTwoPnt(P2, P3)
Line_3 = geompy.MakeLineTwoPnt(P3, P4)
Line_4 = geompy.MakeLineTwoPnt(P8, P7)
Line_5 = geompy.MakeLineTwoPnt(P7, P6)
Line_6 = geompy.MakeLineTwoPnt(P6, P5)
Line_7 = geompy.MakeLineTwoPnt(P2, P9)
Line_8 = geompy.MakeLineTwoPnt(P9, P6)
Line_9 = geompy.MakeLineTwoPnt(P3, P9)
Line_10 = geompy.MakeLineTwoPnt(P7,P9)
   
then i meshed and created the groups in SMESH module,

rui

Offline

#6 2011-02-05 17:24:05

apalazzi
Member
Registered: 2010-05-11
Posts: 283

Re: simple frame

rcbsimoes wrote:

any way, here's how i generated the geometry:
[...]
Line_1 = geompy.MakeLineTwoPnt(P1, P2)
[...]
then i meshed and created the groups in SMESH module,

rui

Hi,

I think that your problem is in MakeLineTwoPnt: with this function you'll generate a line, that will translate in a segment and two nodes when meshing; so, if you make two lines, you'll have two segments and *four* points, that most probably is not what you wanted.
Use MakeEdge instead, this will just create the edge without the ending nodes.

Bye

Andrea

Offline

#7 2011-02-05 18:03:56

tcdonley
Member
From: Virginia, USA
Registered: 2010-11-24
Posts: 94

Re: simple frame

Rui, the error you saw is Code-Aster's way of saying, "you've got rigid body motion because your model is unconstrained in direction X." It tells you the node where the solver found the problem, which is usually helpful because it helps you find the mesh section that is "floating around." In this case, your model was also unconstrained in Y and Z but the solver didn't get past the X component.

The opposite error is a message about DDLS surabondante, which indicates an overconstrained condition, with too many known components.

Good to hear Andrea figured out how to avoid the mesh problem in future.

Have fun!
- Tim

Offline

#8 2011-02-06 15:36:02

rcbsimoes
Member
Registered: 2010-12-09
Posts: 41

Re: simple frame

Yes Apalazzi!! you are right.
I did it the way you say and it works as well.


thanks forum for your help!
rui

Offline