[SOLVED] Deeper understanding of shell models

k_zurawski

Hi,

I replicated a simple linear study to which I had all information. If someone could help me understanding by referring to the attached study. I'd like to dive deeper into it.

First thing - at first I used DKT and TRIA3 elements just to start. If there's a bending introduced to a model is DKT formulation proper or should COQUE3D be always used?

Second thing - if there's no node or nodal group specified as an initial point to start of VECTEUR propagation along adjacent shells in shell group how this is resolved by C_A? At this point I'm changing VECTEUR values by trial and error to run the simulation.

I have more questions, but lets stick to those for now.

BTW modelisation in attached study is already changed to COQUE3D. I used the same linear mesh as in case of DKT and changed it to TRIA9 in *.comm file.

k_zurawski

attached study

Attached file:
088-case02.zip, 851293kb

k_zurawski

HDF file

Attached file:
Case02-HDF.zip, 1414690kb

jeanpierreaubry

hello

i do not really understand what you are exactly trying to to do

the mesh seems to me quite unnecessarily large, complicated and refined to test differences between element types

i would stick to something much simpler where an analytical or reference solution is known

and i would clearly split in plane and out of plane bending

there are quite a few examples in the test case section of the install

with this hints to understand the title

SSLS**

S for Structural analysis

S for Static

L for Linear analysis

S for Surface elements 2D

these tests generally have an analytical solution and are for most of them described in an old (in the eighties) and thick french book "Guide de validation des progiciels de calcul de structures"

jean pierre aubry

k_zurawski

What I'm trying to do is to get approximately the same results from a study prepared and calculated in Femap/Nastran. The 3D model is divided in that complex manner simply because I wanted to mesh it with QUAD4 as in the case mentioned above. But from my understanding instead of DKT/DST I should use COQUE_3D, which requires QUAD9 or TRIA7 topology. At first I wanted to focus on comm file to obtain any results. Now I have 5x difference in stress results but the deflection is about the same as in Femap/Nastran. This matter I'd like to park for now and focus on other things. Later I'll change the mesh to QUAD4. I'll share the results from Nastran as soon as I get permission to do that.

So in case of local shell orientation. The goal is to show i.e. SIXX for whole model, by pointing local axes to the same direction.

I plotted how X and Y local axes are located on my model using IMPR_CONCEPT (red - local X, yellow - local Y) I wanted all local x axes pointing in the same direction (in global Z in this case). I understand how to setup local X pointing in required direction by VECTEUR, but I can only do it for that beam section. In case of C section there's no error reported if local X axes point in global Y direction. So I'm not able to show let's say SIXX for the whole model. This will differ if local axes are not pointing in the same direction. Am I right?

and i would clearly split in plane and out of plane bending

could you describe this more in detail?

Thank you for pointing to the examples. Are they described anywhere else than in the book you've mentioned?

Attached file:
2023-11-28_150543.png, 756903kb

jeanpierreaubry

lets concentrate on your model at first

please post a view of the result as displayed in FEMAP

for code_aster

i suggest you try and concentrate on TRIA3 with DKT at first

one important point is that the local axis you define are necessary for 2D elements they are use to calculate the stress at Gauss point ELGA

then some averaging is done and criterion like von Mises are calculated

either at NOde for ELement ELNO

then at node NOEU

in your model, at the junction where the the vertical member is fixed to the horizontal one you have one node with nearby elements lying on 3 planes orthogonal one to each other they cannot share the same axis

at this node corner the SIEQ_NOEU is meaningless in my opinion

SIEQ_ELNO is more representative of some physical things

look at the two attached pictures for SIEQ_NOEU and SIEQ_NOEU (in Gmsh) the difference is quite large 450 to 580

i do not remember the name of all the components in Nastran, it is almost 20 years aback now, but the same discrepancies appeared as far as i remember

Thank you for pointing to the examples. Are they described anywhere else than in the book you've mentioned?

more about this later

Attached file:
sieq_noeu.png, 157496kb

jeanpierreaubry

SIEQ_ELNO view

Attached file:
sieq-elno.png, 53662kb

k_zurawski

I'll post the view from Femap as soon as I get permission. I asked for it and I'm still waiting. I paid for a general FEM training some time ago. Now I'm back to C_A (this time for real) and I wanted to replicate the study.

I'll change back to TRIA3 or QUAD4 (if I manage to mesh it correctly) and I'll paste results.

Johannes mentioned the difference between SIEQ_ELNO and SIEQ_NOEU several times and I additionally read documentation regarding this matter. I understand the difference how the fields are obtained but still I don't understand why are those two fields present instead of just one. The values represent the same place in space, but since the values are obtained differently they must differ. So which one is "true"? For instance If you're using less advanced software and you choose von Mises stress you are presented with only one field. Why NOEU in this case is meaningless for you? Is it related to singularity in this region?

I changed the model back to what was before.

Attached file:
ResMoy_SIEQ_ELNO-DKT_TRIA3.png, 859197kb

jeanpierreaubry

So which one is "true"?

none of them! (private joke)

strictly speaking

it depends what you mean by true

generally speaking all this averaging mathematics has to be taken with a pinch of salt the most "true" values are at Gauss point ELGA

with a node at which arrives 3 elements in different planes

the sum of the values about the X axis is meaningless

this sum is true in a 3D model

I understand the difference how the fields are obtained but still I don't understand why are those two fields present instead of just one

according to what you are doing one of them may be more useful than the other

remember code_aster supposes you are grown boy who knows what he is doing (unlike most of the push button software whose commercial people claim you can do finite element analysis even if you do not know about it)

k_zurawski

with a node at which arrives 3 elements in different planes

the sum of the values about the X axis is meaningless

this sum is true in a 3D model

You were referring to what I have written before about SIXX? Yes, this is meaningless if we take under consideration the results I printed to med file. This thought was rather chaotic, sorry for that. Let's leave that for now.

I understood that SIEQ_NOEU values are meaningless in this particular example.

remember code_aster supposes you are grown boy who knows what he is doing

well, when it comes to Code_Aster I feel rather like a small girl. The problem with FEA is that there are basically little to none useful books about it unless you want to write your own software. I think the only way is to learn it from someone else and/or by checking real structures under real load.

Despite understanding how SIEQ_ELNO and SIEQ_NOEU are calculated one might have no clue how to deal with this information.

k_zurawski

von Mises stress from Femap/Nastran

Attached file:
2023-11-28_204034.png, 1225760kb

k_zurawski

zoom to connected beam to C channel, why there's a discontinuity in stress propagation between beam and c channel?

Attached file:
2023-11-28_205643.png, 1349534kb

k_zurawski

displacement

Attached file:
2023-11-28_203940.png, 742566kb

jeanpierreaubry

it looks like we are looking at different problems

first there seems to be a trouble with units

k_zurawski

The study he created is in m, Pa etc. So that beam lenght is 0,7m. The study I created is in mm, MPa etc. Beam is 700mm. They are both the same models. I doublechecked the values. There was a slight difference, he set E=205GPa (205e9) whereas I set E=210GPa (210 000 as is in your book on page 56 for models in mm)

Total displacement at the end of the beam in his case is 0,0019m and in my case with E=205GPa is 2,595mm, so first information is that my model is less stiff in some way.

He applied 1000N to the edge of the beam, I setup FORCE_ARETE = 37.037037 on 27mm edge, which gives us in total 999,999999N. Could you tell me where else I could make an error?

The difference is that he used QUAD4 and I'm not sure how many dofs he set to 0 for "DIS_TR". It might be the case he set all to 0 and I only translations. I'll check that later.

Attached file:
displacement.png, 776864kb

jeanpierreaubry

I'm not sure how many dofs he set to 0 for "DIS_TR". It might be the case he set all to 0 and I only translations. I'll check that later.

i cannot see any stiffness, K_TR_D_L assigned to the discrete element in your command file only mass assignement, M_TR_D_N, in that case the stiffness are set to zero by default, a warning is printed in the .mess file

and in any case a stiffness assigned to an element sitting on a node that is fixed is not taken into account

k_zurawski

I'm aware of that. M_TR_D_N is used to apply DDL_IMPO only. Johannes told me during training that I'll get this error in mess file and in this case I may omit that. I don't see any other things in my comm file that could lead to different results. I don't understand why Nastran's and C_A's results differ so much. I'm curious why there's a discontinuity in stress propagation between beam and c channel? Especially if they share the same node where the singularity may occur. I can only guess.

jeanpierreaubry

I'm aware of that. M_TR_D_N is used to apply DDL only. Johannes told me during training that I'll get this error in mess file and in this case I may omit that.

M_TR_D_N is to apply mass only, hence the M however it does not make any difference in your calculation

I don't see any other things in my comm file that could lead to different results. I don't understand why Nastran's and C_A's results differ so much.

quite a few years ago i made benchmarks on a model with beams and plates with code_aster Nastran and Samcef i had scatter of results for stress at nodes or in element in a much wider range than what we can see here

if i remem ber well it was around 2.5 times as much

the structure was much larger and more complicated than here

with very simple models the scatter was very reduced

I'm curious why there's a discontinuity in stress propagation between beam and c channel? Especially if they share the same node where the singularity may occur. I can only guess.

this discontinuity exist in true life

make a model with beam or simply make a hand calculation with beam theory

the bending stress are different in the two members

k_zurawski

OK, so since this discontinuity is ok, why do we see different plot in Paraview? He in the same area has below 60MPa and my results vary from 152 to 251 MPa for elements depending on the layer.

Attached file:
Untitled.png, 1802165kb

k_zurawski

I changed the mesh to QUAD4 and made it almost exactly the same as the "original" from training (except for 4 triangles). I named the groups as in case of TRIA3 study and run the simulation. Now I'm getting error, that some edge elements were created but they are not attached to any with the stiffness. This information is new for me and I don't know how to deal with it. Please look at line 174 in mess file. The element, and next few to which the error refers to are at the far end of the RHS beam. I attach the mesh, comm, export and mess file. Could you explain what I did wrong?

Attached file:
088-case02-QUAD4.zip, 112116kb