Atom topic feed | site map | contact | login | Protection des données personnelles | Powered by FluxBB | réalisation artaban

You are not logged in.

- Topics: Active | Unanswered

**Penta****Member**- Registered: 2023-04-18
- Posts: 8

Hello,

Im currently working on the simulation of a belt (20 m long, 1.6m large, 1.5 mm thick) which is suspended between two edges. I used DKT element, and im using N/mm/s/ton unit system. The DZ displacement computed is way too large (around 8e5 mm, so about 800m which is 40 the total length). Im not sure what I've done wrong, but I tried unit test:

- Estimate the mass of the part, seems ok

- test pesanteur on one single element, seems ok

- Test a cantilever configuration with low linear effort, seems ok

However, when running mumps solver, I need to increase a little the tolerated error to make it run (3e-6 instead of 1e-6). I also tried non-linear solving, I have the same Issue. I tried to use membrane, but never succeed to make it run because the matrix is singular.

I enclosed the .comm file and the HDF too. I'd be happy if someone could provide some insight, comment or advice for my case.

Thank in advance,

Penta

*Last edited by Penta (2023-04-19 02:02:09)*

Offline

**jonas loenartz****Member**- Registered: 2021-10-01
- Posts: 69

Can you post the .comm-file and the mesh?

Jonas

Offline

**Penta****Member**- Registered: 2023-04-18
- Posts: 8

Sorry about that, here they are. Also Im quite a new Code_Aster user, there might be some reflexes I wont have. Im using Salome-Meca interface to run thing too.

Offline

**jonas loenartz****Member**- Registered: 2021-10-01
- Posts: 69

I couldn't find any abvious mistakes on a first glance. I will further look into this, when I'm home.

Offline

**Penta****Member**- Registered: 2023-04-18
- Posts: 8

Thank you for your time!

I ran some other tests like increasing the thickness, and it gace a plausible result. I might have an idea of whats going on but I'm not sure at all. My guess relies on those assumption:

- Gravity is computed using volume (surface x thickness) multiplied by density

- Gravity is estimated at each step

- The element deforms and the thickness doesn't change

So basically the gravity force on each element can increase as the overall volume, and so the mass of the element increases too (bad Poisson coeff estimation on the shell element). If the stiffness cannot maintain balance it just deforms to very large values. Do you think this could happen?

Thanks again for your help and your time,

Offline

**miib****Member**- From: Near Goethe's Palm (Padua).
- Registered: 2021-03-23
- Posts: 363

please give me back this values :

young_mod = 205e3

grav = 9810

density = 7.9e-9

# Thickness of the belt in mm

thick = 1.5

in I.S. (International Standard) and write the units near to them right.

Mechanical Engineer.

CAD 3D designer with 15 years of experience. I use Code_Aster since 2019, initially for curiosity, sequentially with enthusiasm ( during COVID-19 period permitted to me a re-study of my university notions). Also Nastran user (leaved), Inventor Simulation user (leaved).

Offline

**Penta****Member**- Registered: 2023-04-18
- Posts: 8

Hi Miib, here are the values in IS:

young_mod = 205e9 #Pa

grav = 9.810 #m/s²

density = 7900 # kg/m³

# Thickness of the belt in mm

thick = 1.5e-3 #m

*Last edited by Penta (2023-04-19 20:29:01)*

Offline

**miib****Member**- From: Near Goethe's Palm (Padua).
- Registered: 2021-03-23
- Posts: 363

Penta wrote:

Hi Miib, here are the values in IS:

young_mod = 205e9 #Pa

grav = 9.810 #m/s²

density = 7900 # kg/m³

# Thickness of the belt in mm

thick = 1.5e-3 #m

Thank you

it is steel

in the next days (i haven't wife/girlfriend ) i will study (gratis) your case.

Stay tuned .

Mechanical Engineer.

CAD 3D designer with 15 years of experience. I use Code_Aster since 2019, initially for curiosity, sequentially with enthusiasm ( during COVID-19 period permitted to me a re-study of my university notions). Also Nastran user (leaved), Inventor Simulation user (leaved).

Offline

**k_zurawski****Member**- From: Gdansk (Poland)
- Registered: 2010-03-13
- Posts: 186

JDC.py : ERREUR A L'EXECUTION - INTERRUPTION

>> JDC.py : DEBUT RAPPORT

CR d'execution de JDC en MIXTE

!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!

! <S> Exception utilisateur levee mais pas interceptee. !

! Les bases sont fermees. !

! Type de l'exception : error !

! !

! Solveur MUMPS : !

! La solution du système linéaire est trop imprécise : !

! Erreur calculée : 2.63157e-06 !

! Erreur acceptable : 1e-06 (RESI_RELA) !

! !

! Conseils : !

! On peut augmenter la valeur du mot clé SOLVEUR/RESI_RELA. !

!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!

fin CR d'execution de JDC en MIXTE

well, it's quite deformed for linear elastic

*Last edited by k_zurawski (2023-04-19 22:35:18)*

regards,

Krzysztof

Offline

**Penta****Member**- Registered: 2023-04-18
- Posts: 8

Hi everyone,

Thanks again for your help and your time. I've done few more test, especially mass estimation at initila state (that i've done before) but also after deformation: The mass actually increases during computation from 3.79200E-01 ton (379.2 kg) to 3.13166E+01 ton (31 316 kg)!

The more I look at it, the more I think there is a loop between element deformation that increases the volume and the element mass, and weight estimation that increases element length. What do you think, is this something that have been seen somewhere?

Thank you all

Offline

**jonas loenartz****Member**- Registered: 2021-10-01
- Posts: 69

Hello, I have run your case, and I got the same strange results. I checked your mesh and your input-data and there is nothing wrong with it. I built the exact same model with Altair Hypermesh and ran the analysis using the mechanical solver "optistruct". The results are practically identical. Max DZ is around 8e5mm.

So this is not a problem of code_aster specifically, but rather lies in the nature of the mathematics behind FEM in general. I have to admit that my knowledge of the theory of the finite element method does not go beyond the basics.

I think this could be a case fo a nonlinear-analysis with large displacement. I think the initially calculated matrix of rigidity for the flat belt is just wrong and does not represent the state of the belt hanging through at all (maybe someone with more knowledge about the theory of FEM can explain this a little better).

Jonas

Offline

**jonas loenartz****Member**- Registered: 2021-10-01
- Posts: 69

Penta wrote:

Hi everyone,

Thanks again for your help and your time. I've done few more test, especially mass estimation at initila state (that i've done before) but also after deformation: The mass actually increases during computation from 3.79200E-01 ton (379.2 kg) to 3.13166E+01 ton (31 316 kg)!

The more I look at it, the more I think there is a loop between element deformation that increases the volume and the element mass, and weight estimation that increases element length. What do you think, is this something that have been seen somewhere?

Thank you all

That is 100% not the case. You are doing a linear static analysis. You have a matrix of rigidity and vector of external forces. The basic equation of linear elasticity is rigidity * displacement = external forces. The solver solves this equation for the displacements. The matrix of rigidity is calculted for the initial geometry as is the gravity load (based on volume * density, spread on the nodes of the mesh). In non-linear analysis, the matrix of rigidity is recalculated for the deformed geometry after a given number of iterations.

Edit: Think about the belt like a tightrope. In its initial state, a tiny force in the middle between its two ends is enough to make it sag, because the rope has no angle to counter the force in the center. The more the rope sags and the greater the angle gets, the greater the force has to be, to push the center further down. In your analysis the calculation is done with the rigidity of this initial state, where a tiny force is enough to bend your belt to infinity.

Try the following: Make the belt slightly v-shaped, just to test for plausibility. I bet you won't see these large DZ-values anymore

*Last edited by jonas loenartz (2023-04-20 11:56:26)*

Offline

**jonas loenartz****Member**- Registered: 2021-10-01
- Posts: 69

Ok, I tested the v-shaped geometry and this gets even weirder. I attached screenshots of the displacement-field. In the wedge of the v-shape the displacement is small, but in the two straight parts left and right of it, we have the same problem as before. This is getting interesting

But I stand with my explanation until someone corrects me. I think theres something wrong with the rigidity.

Jonas

*Last edited by jonas loenartz (2023-04-20 12:29:26)*

Offline

**Penta****Member**- Registered: 2023-04-18
- Posts: 8

Wow, ok right, thats weird haha. Thanks for the explanation, Im trying to redo simulation of the gravity using nodal reaction. This would confirm your idea I guess as nodal forces should be independent from any geometry variable.

Offline

**jeanpierreaubry****Guru**- From: nantes (france)
- Registered: 2009-03-12
- Posts: 3,974

hello all

i wonder what you guys find strange in here

a MECA_STATIQUE analysis gives exactly the same results as a quick analytic with beam theory

the contrary would be strange

jean pierre aubry

consider reading my book

freely available here https://framabook.org/beginning-with-code_aster/

Offline

**jonas loenartz****Member**- Registered: 2021-10-01
- Posts: 69

jeanpierreaubry wrote:

hello all

i wonder what you guys find strange in here

a MECA_STATIQUE analysis gives exactly the same results as a quick analytic with beam theorythe contrary would be strange

jean pierre aubry

You are right of course. I rarely have to use the analytical approach, so when it is a good idea to use it, I don't think about it at all ... So Beam-theory and MECA_STATIQUE give results, that don't match reality... STAT_NON_LINE is the way to go then, or do you have another, easier idea, M. Aubry?

Offline

**jeanpierreaubry****Guru**- From: nantes (france)
- Registered: 2009-03-12
- Posts: 3,974

jonas loenartz wrote:

STAT_NON_LINE is the way to go then, or do you have another, easier idea, M. Aubry?

oh yes i have an idea!

as an engineer i would never build something with these figures after a quick analytical approach

that is all

the result is so far out that a STAT_NON_LINE will not proove the structure to be feasible

consider reading my book

freely available here https://framabook.org/beginning-with-code_aster/

Offline

**Penta****Member**- Registered: 2023-04-18
- Posts: 8

Hi,

Im not trying to build anything, just understanding a case of a belt under its own weight. I'll take a look at the elastic catenary equation to see if it match the order of magnitude.

Thanks

Edit: The nodal force give the same result, so I think you were right Jonas.

*Last edited by Penta (2023-04-20 16:19:39)*

Offline

**miib****Member**- From: Near Goethe's Palm (Padua).
- Registered: 2021-03-23
- Posts: 363

Penta wrote:

Hi,

Im not trying to build anything

pity you could build a plate on the rolls of a rolling mill before it is cut and coiled

(in the pic the scale factor is multiplied "x 50")

*Last edited by miib (2023-04-20 18:53:23)*

Mechanical Engineer.

CAD 3D designer with 15 years of experience. I use Code_Aster since 2019, initially for curiosity, sequentially with enthusiasm ( during COVID-19 period permitted to me a re-study of my university notions). Also Nastran user (leaved), Inventor Simulation user (leaved).

Offline

**Penta****Member**- Registered: 2023-04-18
- Posts: 8

miib wrote:

pity you could build a plate on the rolls of a rolling mill before it is cut and coiled

Yep this is the kind of stuff, but a lot more thinner haha.

Offline

**miib****Member**- From: Near Goethe's Palm (Padua).
- Registered: 2021-03-23
- Posts: 363

nyprohutni.cz/deleni-ocelovych-svitku

CAD 3D designer with 15 years of experience. I use Code_Aster since 2019, initially for curiosity, sequentially with enthusiasm ( during COVID-19 period permitted to me a re-study of my university notions). Also Nastran user (leaved), Inventor Simulation user (leaved).

Offline

**jonas loenartz****Member**- Registered: 2021-10-01
- Posts: 69

Have you found a solution for your problem. For I am currently facing a rather similar challenge and I am interested in calculating the bending line of an elastic rope or band. The catenary curve doesn't apply here, because it is for untightened and unelastic ropes only.

Offline