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

You are not logged in.

#1 2019-02-01 15:01:39

chenghui62000
Member
From: Norway
Registered: 2018-06-19
Posts: 17

Problem:the matrix is singular or almost singular....

Dear all,
I am a new user of code_aster. I am planning to use it to calculate the displacement and deformation of a super flexible structure (fishing net). At the beginning phase, a validation simulation is conducted to test the ability of this FEM solver. The comparative study is liked that:
  FluxBB bbcode test

I have set up the mesh and non-linear static solver, but it breaks out during the calculation. (see the attachment)
Could anyone give advice or help me to fix the problem?


Attachments:
case1.hdf.zip, Size: 273.65 KiB, Downloads: 15

Offline

#2 2019-02-01 23:26:30

dbpatankar
Member
From: Roorkee, Uttarakhand, India
Registered: 2010-05-22
Posts: 166

Re: Problem:the matrix is singular or almost singular....

chenghui62000 wrote:

I am a new user of code_aster.

Welcome!

I have set up the mesh and non-linear static solver, but it breaks out during the calculation. (see the attachment)
Could anyone give advice or help me to fix the problem?

I see that you have modeled the net with bar element. Do you think the net is structurally stable in such a case?
Moreover, the load applied is vertical but all the bar elements are horizontal (initially). How is it going to achieve force equilibrium? I think answering these question will lead you to the solution.

I also feel modelling should be done with cables in this case.

Offline

#3 2019-02-03 07:51:38

konyaro
Member
From: Genève
Registered: 2016-04-02
Posts: 144

Re: Problem:the matrix is singular or almost singular....

Hello,
I found dbpatankar's answer very interesting so I tried to run the analysis with DYNA_NON_LINE in order to overcome instabilities and understand the problem better.

The deformations seem correct with POU_D_T but not with BARRE elements:

POU_D_T vs BARRE

I cannot figure out why the BARRE deformation is so strange, is it because of the vertical loads on horizontal elements? The deformations of the BARRE elements are huge, on the above picture I reduced the forces by 100 in order to be able to display it.

Konyaro

Last edited by konyaro (2019-02-03 07:56:17)


Attachments:
results2.png, Size: 90.65 KiB, Downloads: 237

失敗は成功のもと (L'échec est la base de la réussite)

Offline

#4 2019-02-03 09:10:49

chenghui62000
Member
From: Norway
Registered: 2018-06-19
Posts: 17

Re: Problem:the matrix is singular or almost singular....

Thank you for your answering. 

dbpatankar wrote:

I see that you have modeled the net with bar element.

Sorry, I did not see the reasons why the bar elements cannot be used here. I will try to use the calbe elements to reconduct this simulation again.


konyaro wrote:

The deformations seem correct with POU_D_T but not with BARRE elements

It seems very interesting in your results, I was also planning to use the POU_D_T elements. Maybe it can give the same results with the cable element.

The reference simulation can be found in the flowing article.  It used a spring element to do simulation the deformation of the flexible system. "Physical modeling for underwater flexible systems dynamic simulation" (sorry I could not put the link in the reply)

By administrator, the link:
https://www.sciencedirect.com/science/a … 1804001532

Offline

#5 2019-02-03 09:59:58

jeanpierreaubry
Guru
From: nantes (france)
Registered: 2009-03-12
Posts: 3,316

Re: Problem:the matrix is singular or almost singular....

hello

i have done a few studies like that
it HAS TO BE DONE with CABLE element

i had like to run your case but i cannot find any .comm file in the archive
can you post it here
after that i may explain you why it does not work with BARRE of POU_D_* elements

jean pierre aubry

Offline

#6 2019-02-03 22:53:57

konyaro
Member
From: Genève
Registered: 2016-04-02
Posts: 144

Re: Problem:the matrix is singular or almost singular....

Hello Jean-Pierre,
attached the original comm file, the modified ones and the mesh.

Regards,

Konyaro


Attachments:
barres_poutres.zip, Size: 5.97 KiB, Downloads: 13

失敗は成功のもと (L'échec est la base de la réussite)

Offline

#7 2019-02-04 11:05:31

jeanpierreaubry
Guru
From: nantes (france)
Registered: 2009-03-12
Posts: 3,316

Re: Problem:the matrix is singular or almost singular....

attached is a modified .comm file for CABLE
study it

i have put a gravity preload to make it run
the material is very strange to me, very soft
beware of too short steps in STAT_NON_LINE sometimes it is not good at all

with BARRE we have an assembly with to continuous tangent on the nodes
and the elements remain straight
and probably is the structure is in a plane and loaded perpendicular to it
it does not converge at the very step

with POU we have bending stiffness which is not the truth


Attachments:
cable1.comm, Size: 4.03 KiB, Downloads: 15

Offline

#8 2019-02-04 22:32:13

konyaro
Member
From: Genève
Registered: 2016-04-02
Posts: 144

Re: Problem:the matrix is singular or almost singular....

nice! I tried to remove the gravity at the end of the simulation and it does converge. The gravity is really needed at the very beginning of the simulation, that was a good idea Jean-Pierre!


Attachments:
cable_jp_mod.comm, Size: 4.09 KiB, Downloads: 9

失敗は成功のもと (L'échec est la base de la réussite)

Offline

#9 2019-02-05 09:29:54

jeanpierreaubry
Guru
From: nantes (france)
Registered: 2009-03-12
Posts: 3,316

Re: Problem:the matrix is singular or almost singular....

konyaro wrote:

nice! I tried to remove the gravity at the end of the simulation and it does converge. The gravity is really needed at the very beginning of the simulation, that was a good idea Jean-Pierre!

yes the very first steps may be a headache with cable structure without a preload more than ever if the load is pependicular i guess

Offline

#10 2019-02-11 10:47:10

chenghui62000
Member
From: Norway
Registered: 2018-06-19
Posts: 17

Re: Problem:the matrix is singular or almost singular....

Dear all,

Thank you for your help!
Sorry, I am a little to get back this topic because of my Ph.D courses.

1.

Jeanpierreaubry wrote:

i have done a few studies like that
it HAS TO BE DONE with CABLE element

Thank you very much for this information. It saves my time to try different elements. I think that the element's names can be different in software. I had done a similar simulation in ANSYS using beam or bar elements.

2.

Jeanpierreaubry wrote:

the material is very strange to me, very soft

I have changed the density of the material in the new .comm file to make it more realistic (see in the attachment). This material is wildly used in the fishing industry. It is a twine rope in Nylon material, and it is very flexible compared to the metal cable.

3.

Jeanpierreaubry wrote:

with BARRE we have an assembly with to continuous tangent on the nodes
and the elements remain straight
and probably is the structure is in a plane and loaded perpendicular to it
it does not converge at the very step

Thank you for explaining why BARRE cannot be used here. But I am still a little confused that: are the motion equations of the discrete elements is different between CABLE and BARRE? From my point of view, it is may because of the nonlinear behaviour we apply in the cable (see the below code) makes it can solve this problem.

                        COMPORTEMENT=_F(DEFORMATION='GROT_GDEP',
                                        GROUP_MA=('twines', ),
                                        RELATION='CABLE'),

 

4.

konyaro wrote:

The gravity is really needed at the very beginning of the simulation,

Thank you very much for your contributions to this topic. Both yours and jean pierre's comm file helps me a lot to understand the simulation process. I think I got the same results as you.
resultsimage

There are some questions I would like to put out here:
5. Is the thermal dilation coefficient is necessary during the material definition? I have deleted this parameter, and the simulation can still give the same results.
6. The initial load (pre-tension, I think) is important for the simulation because it can avoid the singular matrix. But, it won't bring overestimation in the final results?

elemprop = AFFE_CARA_ELEM(CABLE=_F(GROUP_MA=('twines', ),
                                   N_INIT=10.0,
                                   SECTION=3.14159265359e-06),
                          MODELE=model)

7. There only two forces on the nodes are actually applied to the simulation, I could find the reason why. because I think I have applied all the three node forces in my comm file.

Thank you very much again and best regards,
Hui Cheng

Last edited by chenghui62000 (2019-02-11 20:06:50)


Attachments:
case1_new.tar.gz, Size: 4.28 KiB, Downloads: 12

Offline

#11 2019-02-13 20:50:42

konyaro
Member
From: Genève
Registered: 2016-04-02
Posts: 144

Re: Problem:the matrix is singular or almost singular....

chenghui62000 wrote:

5. Is the thermal dilation coefficient is necessary during the material definition? I have deleted this parameter, and the simulation can still give the same results.

Useless because no thermal load.

chenghui62000 wrote:

6. The initial load (pre-tension, I think) is important for the simulation because it can avoid the singular matrix. But, it won't bring overestimation in the final results?

According to U4.42.01 §16.3:
"This keyword makes it possible to define an initial pre-tensioning allowing the convergence of
calculation into nonlinear (it is thus useless into linear). It is applied only to the first step of time. "
Therefore it does'nt affect the final result, you can try to modify this value, it has no effect.

chenghui62000 wrote:

7. There only two forces on the nodes are actually applied to the simulation, I could find the reason why. because I think I have applied all the three node forces in my comm file.

The force F3 is applied to the GROUP_NO F2.

Last edited by konyaro (2019-02-13 21:09:47)


失敗は成功のもと (L'échec est la base de la réussite)

Offline

#12 2019-02-13 22:32:42

chenghui62000
Member
From: Norway
Registered: 2018-06-19
Posts: 17

Re: Problem:the matrix is singular or almost singular....

Konyaro, Thank you so much!

Konyaro wrote:

The force F3 is applied to the GROUP_NO F2.

Sometimes, I could not find this kind of mistake by myself.

Offline

Board footer