[SOLVED]Problem:the matrix is singular or almost singular....

chenghui62000 · 2019-02-01 15:01:39

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?

Last edited by chenghui62000 (2019-02-23 23:33:26)

Attachments:
case1.hdf.zip, Size: 273.65 KiB, Downloads: 57

dbpatankar · 2019-02-01 23:26:30

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.

konyaro · 2019-02-03 07:51:38

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: 468

chenghui62000 · 2019-02-03 09:10:49

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

jeanpierreaubry · 2019-02-03 09:59:58

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

konyaro · 2019-02-03 22:53:57

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: 54

jeanpierreaubry · 2019-02-04 11:05:31

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 no continuous tangent on the nodes
and the elements remain straight
and probably if 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

Last edited by jeanpierreaubry (2019-02-21 14:34:11)

Attachments:
cable1.comm, Size: 4.03 KiB, Downloads: 69

konyaro · 2019-02-04 22:32:13

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: 65

jeanpierreaubry · 2019-02-05 09:29:54

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

chenghui62000 · 2019-02-11 10:47:10

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: 61

konyaro · 2019-02-13 20:50:42

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)

chenghui62000 · 2019-02-13 22:32:42

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.

chenghui62000 · 2019-02-20 21:10:26

Hello, Thank you all for your kindly help.

There is one more question for this case: Can I use the DYNA_NON_LINE solver to do the same simulation?
Assume the same boundary condition, it should get the same result?
I have tried to modify the .comm file, but the outcome seems wrong (at least not same with the STAT_NON_LINE simulation).
Could you please help me to check the .comm file?

Thank you in advance.
Hui Cheng

Last edited by chenghui62000 (2019-02-21 08:52:55)

Attachments:
astk2.tar.gz, Size: 4.29 KiB, Downloads: 50

jeanpierreaubry · 2019-02-21 09:36:06

i will answer your question with a question

what is the difference between DYNA_NON_LINE and STAT_NON_LINE?

chenghui62000 · 2019-02-21 10:07:09

Hi, Jean Pierre Aubry,

From my point of view, the distinction between the dynamic and the static analysis on the basis of whether the applied load has enough acceleration in comparison to the structure's natural frequency. If a load is applied sufficiently slowly, the inertia forces (Newton's first law of motion) can be ignored and the analysis can be simplified as static analysis.

Dynamic analysis can be used to find dynamic displacements, time history, and modal analysis. A dynamic analysis is also related to the inertia forces developed by a structure when it is excited by means of dynamic loads applied suddenly (e.g., wind blasts, explosion, water current forces).

Best regards,
Hui Cheng

jeanpierreaubry · 2019-02-21 10:21:13

to keep going with the argument

you are generally right
but i cannot see any initial speed or acceleration in your comm file

i have never done a DYNA_NON_LINE analysis whose .comm file was a direct translation of STAT_NON_LINE .comm file

chenghui62000 · 2019-02-21 12:15:55

Hi Jean Pierre Aubry,

Thank you for your reply. Please forgive my knowledge gap, did you mean I need to define an initial speed or acceleration in the .comm file? or I need to define time-dependent load using AFFE_CHAR_MECA_F? Or I need to change the element? I have seen a case in the forum (a cable-coque connection case), there seems no initial definition for speed or acceleration in the .comm file.

BTW, the reason why I want to use the DYAN_NON_LINE: I want to see how the net is deformed in the real-time domain.

Thank you very much,
Hui Cheng

Last edited by chenghui62000 (2019-02-21 14:32:33)

jeanpierreaubry · 2019-02-21 15:18:05

what i do usually

perform a first STAT_NON_LINE that will set an initial state with the only static load, not varying with time
for example gravity due to the own weight

then perform the DYNA_NON_LINE with it as ETAT_INIT

dynanl=DYNA_NON_LINE(
	.......
	ETAT_INIT=(
		_F(
			VITE= vitini, 
			#some initial speed given to some nodes, 
			#if the load condition call for that, 
			#for example an object falling on
			#may not be necessary
		 	EVOL_NOLI= statnl, #the previous STAT_NON_LINE analysis concept name
		),
	),
	......

AFFE_CHAR_MECA_F is not necessary here
there is an example of what AFFE_CHAR_MECA_F can be used for in my book

time steps where the load is applied has to be representative of the truth

konyaro · 2019-02-22 17:29:40

Hello,
You can transform your STAT_NON_LINE to DYNA_NON_LINE keeping exactly the same boundary conditions and adding, for instance:

SCHEMA_TEMPS=_F(SCHEMA='HHT',
                ALPHA=-0.3,
                FORMULATION='DEPLACEMENT',),

All the initial velocities and accelerations will be automatically set to zero.
Without damping your net will be oscillating forever so it will be hard to compare the results with the static analysis.
You can add damping either in the materials or use a dissipative scheme, for instance HHT with a low alpha-value, for instance -0.3. That should stabilize the net after a few oscillations.

Konyaro

Last edited by konyaro (2019-02-22 17:30:18)

jeanpierreaubry · 2019-02-22 17:56:17

@konyaro
you are absolutely right

may i had that setting a
load FONC_MULT 0,0, 1.1 and a INCREMENT of the same value
or
load FONC_MULT 0,0, 100.1 and a INCREMENT of the same value
will produce the same results in STAT_NON_LINE
but
may produce radically different ones in DYNA_NON_LINE

chenghui62000 · 2019-02-23 23:33:02

Thank you Konyaro and Jean Pierre Aubry,
It is your kindly help makes me feel confident in this software.

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

[SOLVED]Problem:the matrix is singular or almost singular....

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

Re: [SOLVED]Problem:the matrix is singular or almost singular....

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

Re: [SOLVED]Problem:the matrix is singular or almost singular....

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

Re: [SOLVED]Problem:the matrix is singular or almost singular....

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

Re: [SOLVED]Problem:the matrix is singular or almost singular....

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

Re: [SOLVED]Problem:the matrix is singular or almost singular....

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

Re: [SOLVED]Problem:the matrix is singular or almost singular....

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

Re: [SOLVED]Problem:the matrix is singular or almost singular....

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

Re: [SOLVED]Problem:the matrix is singular or almost singular....

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

Re: [SOLVED]Problem:the matrix is singular or almost singular....

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

Re: [SOLVED]Problem:the matrix is singular or almost singular....

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

Re: [SOLVED]Problem:the matrix is singular or almost singular....

#13 2019-02-20 21:10:26

Re: [SOLVED]Problem:the matrix is singular or almost singular....

#14 2019-02-21 09:36:06

Re: [SOLVED]Problem:the matrix is singular or almost singular....

#15 2019-02-21 10:07:09

Re: [SOLVED]Problem:the matrix is singular or almost singular....

#16 2019-02-21 10:21:13

Re: [SOLVED]Problem:the matrix is singular or almost singular....

#17 2019-02-21 12:15:55

Re: [SOLVED]Problem:the matrix is singular or almost singular....

#18 2019-02-21 15:18:05

Re: [SOLVED]Problem:the matrix is singular or almost singular....

#19 2019-02-22 17:29:40

Re: [SOLVED]Problem:the matrix is singular or almost singular....

#20 2019-02-22 17:56:17

Re: [SOLVED]Problem:the matrix is singular or almost singular....

#21 2019-02-23 23:33:02

Re: [SOLVED]Problem:the matrix is singular or almost singular....

Board footer