forum » ROBOT Millennium » Connection wall to beam moment
Autor
Post
STONEZ

Connection wall to beam moment

Dear ALL

I want to discuss one interesting thing regarding to connection of wall and beam in robot
Almost robot give mee near zero values of moments in connecting nodes of beam with wall.
But what is more interesting, that when i use pin supports on wall moments at connecting nodes of wall with beam are near zero, but when i change support of wall to fix, everything changes, moments in nodes connecting wall with beam, have normal values.
I ask how is posible that changing of suports in base of wall will affect so much redistributing of forces entire whole model.
This happen only in robot, and it has make mee very confuse.

Any comment for this
Regards
Z.G.

STONEZ

bez tytulu

really it seems to be serious.
I belive tat have to be with torsional degrees of fredomm in panel,
To be more specific i have search to find any any information that how robot calculate shells in FEM, but no succes.

stahlbau

Bad structure

There is no problem with beam-shell connection in robot.
Probably You use incorrect structure (almost non-stability geometric)

STONEZ

bez tytulu

stahlbau
i think that is something else.
You can try this yourself
For Example:
Model an wall ( XZ Plae ) and some columns, also beans whic are suported in columns and wall.
Apply pin support at wall, and apply fix support at wall and you will see diferences.
(when put pin supports to wall , to avoid instability you can put lateral supports)
Regards
Z.G.

stahlbau

no problem

Fixed base column, beam supported on column and wall, wall pin supported,
and... moment on end (over wall) looks ok.
Your structure is not correct.

STONEZ

bez tytulu

This have to be noo with type of structure,
otherwise structure is free form,
http://www.4shared.com/photo/_kyBAeyb/RSA_Test_1.html
Look a foto and see results at connection of beam with wall.

Try yourself and u can see.
For example if u have structure in XZ plane and if you define linear support at base of wall ( you fix UX, UY, UZ and RY) and also if you apply full fixed supports, results will bee right.. In other case no.

Regards
Z.G.

STONEZ

Any anfwer from Robot team?

Any anfwer from Robot team?
No Answer
OK

Listen my opinion for this
I thing that in shell model ( Model of FE-shell) in robot something is not going, especially due to torsional degrees of fredom ( rotation in nodes of shell about axis perpendicular to shell), because if you fix base of wall, you get right results. If you pin base of wall you get wrong results (zero moments at connecting nodes of beam with wall), if you suport wall with user defined support ex:( you fix UX, UY, UZ, RY - if u have structure in XZ Plane ) and this mean that torsional degres of freedom are fixed, you also get right results.

I think that this MisterY in shell model of robot is causing many serious errors also in other models.
For example compare horizontal displacements of any building from seismic loads with Robot and Etabs and you get totally diferent results. Displacements from Robot are twice more than displacements from Etabs or any other software, from same seismic case.

I will be happy if im Wrong
Regards
Z.G.

stahlbau

OK

I see now. I used wall in plane XZ and frame in plane YZ, so the moment were correct.
If You use all structure in one plane, there is a problem with torsional degree of freedom of the nodes.
It seems to be enough to fix (for torsion) only one node for panel to receive "correct" moments.
But i agree its not general solution. Probably it is commonly problem for fem programs.
Help do not shown shape functions for shell elements.
It is very important problem. I check this in femap/nastran.

STONEZ

Ya

Dear stahlbau, thank you for reply

I agree to you that something due too torsional degrees is not going.
I have discus this with some friends, and they belive that is problem due to stability.
But problem has not to bee with stability, because you can model all supports pinned ( in wall and in column ) and structure is unstable, but if you fix RY in linear support of wall, also structure is unstable ( possibility to rotate due to X) and you get results.
And one thing, If u define supports at col and wall all pinned , and jou add an small piece of panel perpendicular to waall with no supports otherwise structure is also unstable, and you get right results.
One thing is sure ( if you agree with mee) the problem is not caused due to instability.
By the way i havent check with softwares like FEMAP, nastran, but i have compare with many other softwares like SAP 2000, ETABS, Tower, Scia, and this happen only in Robot. I know that robot for more things is best software in the world, but this problem is confusing mee so much.
As you sed i also have search for concept of shell FE model in robot help and manuals, but nothing.

I think that this MisterY in shell model of robot is causing many serious errors also in other models.
For example compare horizontal displacements of any building from seismic loads with Robot and Many other softwares and you get totally diferent results. Displacements from Robot are twice more than displacements from Etabs or any other software, from same seismic case and same seismic response data.

stahlbau, by the way do you have chech thiswith any earlier version of robot.

Kindly Regards
Z.G.

stahlbau

any best software

Of course. As i said, at first, i did not understand you. If all structure is in one plane, most important is a lack of torsion stiffness of nodes in shell elements.
So: there is not a stability problem, but fem problem for shell elements. Typical nodes in shells have only 5 degree of freedom (without torsion in element plane). For this connection we needs nodes with 6 degree of freedom. There are not information about shape function for shell elements, so we can not say what is wrong - i ask service - results should not be depends on type of supports (constraints) - that mean in statistical mode..
I checked model in nastran. Results did not depends, if wall constraints are fixed or pinned. Moments are
exactly 0! It is not very good information, but solutions do not depends on type of constraints and this is consequent.
By the way, there are not "best" software, especially robot is not best - good for some applications.

STONEZ

bez tytulu

I mean for more things robot is best software in the world, and for almost all things csi is leader. I mean for structural engineering.

As for shell model of robot now im thinking that robot use diferent model of shell from csi, and maybe this is causing some other mismatch results betwen them.

I have read many threads which you have post, and i bet that you are good user of robot.

Im interested to know by your experience, if you have make comparasions of displacements ( ex: lateral displacements) of any with robot and any other software.
By my opinion although i apply fix supports in walls and let isay robot activate "torsional machine" also results does not mech in some aspects with other softs, at structures when shell elements are predominant. This not happen if structure is frame type resisting system.

Regards
Z.G.

stahlbau

fem problem

Robot works very good with beam elements (better than nastran and ansys even, i think). But with shells elements some results match not very good. Please, pay attention that robot use only linear shell elements and more we do not know how many integration point (for interpolation) is used?
However, in most cases the deflecions is good calculated, worse with internal forces and stresses
(ex: let see square plate simply supported only in 4 nodal edge, equal loaded - you receive nonneglectable moments over support).
So, for shell elements should we made very carefully analysis. In other side, it is important what model of shell is used in sci (and other software) - robot uses mindlin theory and it is possible that if you compare results with program using kirchoff theory, the deflections could be smaller.

macjar

bez tytulu

...in my opinion if you want to use rsa in this situation you should model fix of beam by let in beam node into wall.

STONEZ

bez tytulu

@t macjar

You dont need to fix beam
You need to fix base of wall, and than you will have moments differ from zero ( more really ) at connecting nodes ow wall with beam,
But if you apply pin support at base of wall you will get wrong results ( near zero moments at connecting nodes of wall with beam)
I suggest you and other thing. When you use robot to model structure containing walls, and other elements ( beams and columns.... )
I usually put beam inside the wall and anywere ( by my point ) i put columns in edge of walls,
And i have seen that this approach give "good" results, even if you make comparasion with other softwares.

Regards
Z.G.

stahlbau

@STONEZ

I agree, that robot gives not expected moment on end of beam. But I am not sure, the other software gives correct solution. I check again this problem in nastran. Using 4 node elements with additional parametr (k6rot for 6th dof) i can receive moments on end of beam. But there is not exact solution because, there is not exact correlations between parameter for 6th dof and real stiffness of beam fixing. So, in this method works all other software (i think). This parameter probably is constant for other software. They give you moments but only more or less correct. In this situations should be used special fem elements "translation" element beam-shell elements. It is well known in theory of fem, but i do not see this solution in typical software.

STONEZ

Ya

stahlbau

I agree with your point,
I strongly belive that this is not correct way to model connection of beam with wall,
For example If we refer G.A. Rombach - finite element design of concrete structures, it refer many modeling techniques using fem in RC, which one of them is to put the beam inside wall and column in edge of walls.
Regarding to this modeling techniques many softwares(CSI, Robot, Midas, Tower ...) are giving almost same and very accepted results. But im also confuse that if we make model same (node of beam is joined with node of wall) with all softs ( for ex.CSI, Robot, Midas, Tower), and we get same results with all softwares but diferent with robot.
I really dont know which model for shell fem is using Robot.

Stahlbau, i dont know if u agree with mee but i think that for this serious issues robot team must respond and explain because it is really big problem.
And by the way this is not only bug which is happening with robot, but i hope that they know about this bugs, and maybe with an update they will solve and i also hope that they will improve the manuals with more informations, because they really ofer zero informations about analysis and capabylyties of Robot.

Regards

stahlbau

Robot

1. You should not belive, that manual of robot will be more clear or helpful. Please note, that in manual, there are mistakes (f.e. robot will not offer 6 and 8 node shell elements, but in manual you can read this)
Manual do not change during last year any more (almost)

2. I send mail to service with this problem. The answer was not completed. I think, they do not know how exactly this works. Now, robot belong to autodesk, but there are not contact with autodesk, so it is very difficult to explain this. It is not funny but real. If You want, give me your mail, i send you interested article, received from servis. This is problem of 6th dof for shell, probably applied in robot, but it is not clear how it works
in robot.

3. The book of Rombach is very interested, but i am not sure, that autor is a designer. Some proposed solutions are very "academic", however some problems are not exact or complete (f.e. the influence of mesh quality on the results, the influence of creep).

4. Besides, i think, that this type of frame is not common in practise (in Poland there is not earthquake zone). Only a few frames in object has directly connections with concrete wall (stairs tower, i think). So, it is probably, designer use pinned connections in this situation (the wall stop only horizontal deflection).
So, this is only "theoretical" problem and autodesk have not questions from users in this subject.
But I agree, this situation is strange and uncomfortable.

B.R.

STONEZ

Thanks

Ok,
I'm interested to see that article and my mail is: zg.stonez@gmail.com
I agree to you that robot is in autodesk company, but i dont know if the developing team is same or has changed.

I tell you an other thing regarding to displacement of shells due to seismic loading
Robot does not take into consideration behaviour factor in calculating of displacements.
To be more specific, displacements in robot due to seismic loads are computed due to spectrum data with q=1 ( behaviour factor q=1)OTHERWISE YOU CHANGE q, you have no diferences in displacements due to seismic, but for forces M,V,N everything is ok.
I dont know if this is bug, or if this vorks in this way with robot.

Kindly Regards


macjar

bez tytulu

...trochę się na tym zastanawiałem i wpadłem chyba na sposób jak zrealizować połączenie belka - ścian, metoda polega na tym żeby w węźle łączącym belkę i ścianę wstawić panel prostopadły do ściany o kształcie odpowiadającym przekrojowi belki i bardzo dużej sztywności..."podobną" metodę stosuje się przy projektowaniu układów płytowo słupowych żeby uzyskać poprawną sztywność połączenia płyta słup oraz w przypadku oparcia tarczy żelbetowej na słupie. Metoda bardzo dobrze się sprawdza przy modelowaniu oparcia tarczy żelbetowej na słupie...nie ma pików w tarczy i dodatkowo otrzymuje się poprawne momenty w słupie, co nie jest bez znaczenia przy wymiarowaniu tych elementów.

to Stonez
sorry stonez my english is low so I describe briefly
...I thought bit about this problem and I hope... I have way how to model the conection beam and wall, We should use PARPENDICULAR shell in node of conection beam-wall. Shell must has big stiffnes and shape similar to beam section.

stahlbau

do macjar

Nie o to chodzi. Jest kilka sposobów połączenia belki i tarczy (powłoki) w jednej płaszczyźnie. Problem polega na tym, że teoretycznie w robocie powinien być obługiwany 6 stopień swobody dla obrotów w płaszczyźnie panela.
Istnieje więc bezpośrednie połączenie węzłów belki i powłoki. Sztywność tego połączenia nie może jednak zależeć od ilości i rodzaju podpór (przynajmniej jeśli połączenie belka-powłoka nie jest w bezpośrednim jego sąsiedztwie). Wartości momentów utwierdzenia belki nie mogą być tak silnie od tego uzależnione, a tak jest. Coś więc w zastosowanym modelu sztywności "w planie" jest nie w porządku. Inne, zastępcze sposoby modelowania tego styku nie są przedmiotem dyskusji.

macjar

bez tytulu

ok rozumiem ... ale czy udało ci się uzyskać informacje z serwisu na ten temat bo jakoś nie kwapią się do podjęcia dyskusji
pozdrawiam

stahlbau

macjar

Serwis zrobił co mógł, dostałem nawet namiar na źródło podstaw teoretycznych rozwiązania tego problemu w robocie, ale to niczego nie rozwiązuje bo dalej nie wiadomo jak to zostało zaimplementowane. Natomiast w praktyce działa to wątpliwie. Trzeba by mieć kontakt z kimś z programistów z autodesku, a właściwie z kimś, kto sprawuje nadzór merytoryczny nad zagadnieniami mechanika+MES w robocie (pytanie czy ktoś taki w ogóle jest?)

 
forum » ROBOT Millennium » Connection wall to beam moment



GRAITEC Advance Design jest w pełni rozwiniętym i łatwym w obsłudze oprogramowaniem do analizy strukturalnej MES, dedykowanym inżynierom konstruktorom pracującym w środowisku BIM. Daje możliwość projektowania każdego typu konstrukcji, kompleksowych obliczeń statycznych, wraz z wymiarowaniem elementów żelbetowych, stalowych i drewnianych. Wszystko to zgodnie z Eurokodami (posiada Polskie Załączniki Krajowe do Eurokodów) - EC0, EC1, EC2, EC3, EC5 oraz EC8.

CADKON+ BASIC jest skutecznym narzędziem CAD do edycji i przeglądania rysunków, posiada pełną kompatybilność ze wszystkimi formatami DWG. Zapewnia użytkownikom proste, naturalne i ekonomiczne rozwiązanie umożliwiające tworzenie oraz edycję rysunków.