[SOLVED] Deeper understanding of shell models

k_zurawski

I changed also the way DKT is assigned to mesh from TOUT=OUI to GROUP_MA=('THK3','THK4'). Then I got the information that there are no elements attached to LOADD_EL group.

I prepared model and mesh again, the result is the same. Please help.

jeanpierreaubry

try this

model = AFFE_MODELE(AFFE=(_F(MODELISATION='DKT',


                            PHENOMENE='MECANIQUE',
                            GROUP_MA=('THK3','THK4','LOADD_EL',),
                            #TOUT='OUI',

),

and try to avoid using TOUT='OUI', as much as possible

as it looks like you have ghost or unused GROUP_MA in the mesh for example Group_14

why do you keep assigning mass and not assigning stiffness to elements P1 to P4?

k_zurawski

...so for LOADD_EL as well, I'll check that. I thought that DKT applies to 2D elements only, not their "border". LOADD_EL is group containing line elements.

Geometrical Group_14 was used to control submesh, it landed in the mesh group automatically, and I didn't notice that it's there. I'll delete it from final mesh.

As for the M_TR_D_N, this is taken from an example I was given during training. Since I'm not using PESANTEUR this, as stiffness, would not be taken into account. I don't know how else I could create LIASON_SOLIDE. I tried using nodal group without POI1 element, but solver reported orphan mesh. Then it was explained to me, that I need any sort of element in that central node (which was kind of obvious, when it was pointed out). I don't know how to simplify it.

k_zurawski

No success yet, I obviously overlooked something, but still don't see it. I attach mess file.

I don't know why it run flawlessly when I had TRIA3 mesh and now with QUAD4 there's problem after a problem. Study didn't change that much. So this has to be something with mesh. I've been using Salome 9.7 to mesh it.

Attached file:
Case02.mess, 32993kb

k_zurawski

It seems that there's a rigid body motion, but I don't know why. Every connection seems all right.

I attach the most recent files. I changed mesh, changed M_RT_D_N to K_TR_D_N with all 6 stiffness components equal 1. I'll get back to it in the evening.

Line 345 in mess file "à la ligne 1640 qui correspond au degré de liberté" - ligne 1640 reffers to SEG2 element number 1640?

Attached file:
088-case02a.zip, 107888kb

StanislavPavlica

Hello Krzystof,

088-case02-QUAD4.zip ...

remove elemets 1 2 3 4 next to P2 and elements 1291 1292 1293 1294 next to P1.

And put back DRX=0.0, DRY=0.0, DRZ=0.0, for GROUP_NO=('P1','P2','P3','P4',)

Stano

jeanpierreaubry

Line 345 in mess file "à la ligne 1640 qui correspond au degré de liberté" - ligne 1640 reffers to SEG2 element number 1640?

1640 is an internal number in the solving process

what is important is

Degré de liberté physique associé au noeud N161 et à la composante DRZ.

which is a rigid body motion

it is very difficult for me to follow what you are doing

the mesh is changing every time

in 088-case02-QUAD4 the group HE4 contains 24 elements while only 18 in 088-case02a

and a few other things

the attached .comm file runs well on my computer on the mesh of 088-case02-QUAD4

Attached file:
Case02.comm, 5671kb

k_zurawski

Thank you Stanislav, I'll check it in the evening

Jean Pierre,

Sorry for changing mesh all the time.

First mesh was based on model edited in Shaper. Shaper cuts hole arc even if it's not asked to, which is annoying. I had to cut model more to have the same arc length so that I could define one submesh hypothesis. That's why there were more elements in that group than in Case02a.

Since model didn't run and there was a mess in shaper results tree I decided to prepare final model again CAD system and import it to geom module. So after importing it from CAD had to mesh it once more. I run the simulation and had rigid body motion problem again. Case02a is the most recent and I won't be changing it again.

Again sorry for the chaos I introduced.

jeanpierreaubry

i said

in 088-case02-QUAD4 the group HE4 contains 24 elements while only 18 in 088-case02a

what about that?

there is not only the geometry but the way it is meshed!

k_zurawski

I'm sorry, I didn't fully understand the first time.

Yes, you're right, I picked only 3/4 of hole edge to that HE4 group.

k_zurawski

Mesh 088-case02-QUAD4 plus comm file shared by you works perfectly. Thank you.

Unfortunately stress propagation still is different than in the study from the course. I don't know Femap/Nastran so maybe I'm trying to compare pears to apples? Are there any other fields than SIEQ_ELNO and SIEQ_NOEU for shells from which can we display Von Mises stress?

Attached file:
ResSup_SIEQ_ELNO.png, 946448kb

k_zurawski

Stanislav Pavlica wrote:
Hello Krzystof,

088-case02-QUAD4.zip ...

remove elemets 1 2 3 4 next to P2 and elements 1291 1292 1293 1294 next to P1.

And put back DRX=0.0, DRY=0.0, DRZ=0.0, for GROUP_NO=('P1','P2','P3','P4',)

Stano

I see what you mean. It's weird, but I did not specify any modelisation to SEG2, so those elements should be "transparent" for the solver. Correct me please if I'm wrong.

The other weird thing is that my last mesh doesn't contain any additional SEG2 elements in those holes and I'm still getting rigid body motion. Well I should have sticked to one mesh and make adjustments where needed.

What is even weirder:

Degré de liberté physique associé au noeud N2212 et à la composante DZ.

This node is in the middle of RHS beam.

k_zurawski

I attach screenshot with marked node from the error.

Attached file:
Screenshot_2023-12-01_222222.png, 25951kb

StanislavPavlica

Hello Krzysztof,

sorry for error in my last comment, DRX=0.0, DRY=0.0, DRZ=0.0, for GROUP_NO=('P1','P2','P3','P4',) are not needed, removing elements it's enough.

k_zurawski wrote:

It's weird, but I did not specify any modelisation to SEG2, so those elements should be "transparent" for the solver. Correct me please if I'm wrong.

To be honest I don't now. From approach of jeanpierreaubry I see, that you can have more elements in mesh and in AFFE_MODELE define model just on part of the mesh.

It is writen in 4.41.01 (Operator AFFE_MODELE): This operator allows to affect modelings on whole or part of the grid. To this I never pay attention.

Some tests for using TOUT='OUI' with 088-case02-QUAD4.zip:

for

model = AFFE_MODELE(AFFE=(_F(MODELISATION='DKT',
                            PHENOMENE='MECANIQUE',
                            TOUT='OUI'),
                          _F(GROUP_MA=('P1','P2','P3','P4',),
							PHENOMENE='MECANIQUE',
							MODELISATION='DIS_TR',),
                          ),
                    MAILLAGE=Mesh)

and mesh without removed elements you have in .mess file (after AFFE_MODELE):

Modélisation Formulation Type maille Élément fini Nombre _ _ SEG2 MEBODKT 1294 DIS_TR _ POI1 MECA_DIS_TR_N 4 DKT _ QUAD4 MEDKQU4 8640

DKT _ TRIA3 MEDKTR3 4

So there are 1294 SEG2 MEBODKT elements.

Finite elements of type SEG2 MEBODKT (used for application of loadings - see U3.12.01 part 1.3) are created for all edges of the elements of plate.

Same model = AFFE_MODELE definition and mesh with removed elements:

Modélisation Formulation Type maille Élément fini Nombre _ _ SEG2 MEBODKT 1286 DIS_TR _ POI1 MECA_DIS_TR_N 4 DKT _ QUAD4 MEDKQU4 8640

DKT _ TRIA3 MEDKTR3 4

So there are 8 SEG2 MEBODKT fewer. Obviously with option TOUT='OUI' are SEG2 MEBODKT elements created not only for edges of the elements of plate but on beams outside of plate too.

Original mesh (no removed elements) with jeanpierreaubry .comm file:

Modélisation Formulation Type maille Élément fini Nombre _ _ SEG2 MEBODKT 8 DIS_TR _ POI1 MECA_DIS_TR_N 4 DKT _ QUAD4 MEDKQU4 8640

DKT _ TRIA3 MEDKTR3 4

Just 8 elements are created needed for 'LOADD_EL' !

It seems like using TOUT='OUI' in AFFE_MODELE can create a unexpected problem. I learned something :).

k_zurawski wrote:
The other weird thing is that my last mesh doesn't contain any additional SEG2 elements in those holes and I'm still getting rigid body motion.

You mean Case02.med? It runs well on my computer?

Stano

k_zurawski

I meant mesh from Case02a not Case02. Jean Pierre's comm file plus mesh from 088-case02-QUAD4.zip (Case02) works without modification. It seems that removing TOUT='OUI', adding 2D mesh groups and LOADD_EL to DKT formulation does the job. I have never added 1D element group to DKT formulation. But I understand that this will create SEG2 elements on LOADD_EL edge. A neat way to create less elements in the study.

From *.mess file you referred to you can find in "Modelisation" column "-", which means that that despite MEBODKT being applied to "hollow 1D mesh" no stiffness is added to SEG2.

I've always used TOUT="OUI" in "Modelisation" and took advantage of overwriting rule. I have never thought that it might make any difference. So I leaned something new also.

k_zurawski

Thank you guys.

jeanpierreaubry

as stated in my book

using TOUT='OUI' can be very harmful if one does not know what one is doing

k_zurawski

Apparently I'm one of those users. I think even if someone reads your book few times, will have to go through some of the problems to have this "aha" moment.

...small remark, using C_A in comparison to commercial codes... For example in case of Abaqus, you simply have less insight into all what's under the hood.

echo6

For femap results, you should turn off all averaging. Hit shift-f5, then click on contour options. Use level colors, uncheck corner data, and check the no averaging check mark. This should give you the raw elemental result from nastran. Also you can use the list menu and list the output vectors for a particular element. This should compare two the gauss point results from aster.

k_zurawski

Hi echo6,

I don't have access either to original study or Femap itself. The owner does much more complicated studies on a daily basis. He doesn't store studies of this complexity and size.

« Previous Page Next Page »