Discussion Groups

Robot Structural Analysis

Reply
Contributor
annecy-structures
Posts: 12
Registered: ‎11-15-2011
Accepted Solution

Barre de treillis / traction compression vs séisme

1497 Views, 7 Replies
12-07-2011 02:51 AM

Bonjour,

 

suite à une solution évoquée sur le forum, j'ai modélisé mes montants d'ossature bois et le panneau OSB qui permet de reprendre la stabilité horizontale est modélisé grâce à des barres treillis travaillant uniquement en traction.

Le logiciel réalise donc un calcul non linéaire sur la structure et cela fonctionne bien sous charges permanentes, neige et vent.

A partir du moment où j'intègre un calcul sismique, toutes les barres treillis reprenant uniquement de la traction (j'ai également des tirants métalliques définis de la même façon) semblent ne plus intervenir dans le calcul. Dans le tableau des efforts, les valeurs pour ces barres sont nulles. Du coup, ma structure n'est plus stable ou se déplace de manière importante.

 

Que dois-je faire pour avoir un modèle de calculs cohérent?

 

Cordialement,

Jean Gay-Lancermin

 

 

AS74 Jean
Please use plain text.
Product Support
Rafal.Gaweda
Posts: 5,596
Registered: ‎04-26-2010

Re: Barre de treillis / traction compression vs séisme

12-07-2011 02:56 AM in reply to: annecy-structures

Nonlinear seismic - why not :

 


1. Stiffness matrix for modal analysis is taken from the last calculated case
before modal case so some tension members "are not working" in this case and
this state will be fixed for next modal case(s)
2. Modes should (may) activate \ deactivate some different tension bars depending
on direction they are acting but this effect can not be considered due to point 1
3. Even if we calculate model after combining results for most tension bars it may
appear that results are "not existing" because combining "not existing" results
and some value results gives "not existing" finally
4. Spectral/seismic analyse is based on assumption of harmonic vibrations which
is not true for nonlinear model. In such case you should use time history instead.
One have to convert time - acceleration data into time - displacement data and
finally apply them to the supports of your structure (to model movement of the ground).

 


More complete explanations related to above points:


Existence of tension-only members (or any other nonlinear objects like cables, uplift supports, etc) results in non-linear behaviour of the structure and in such case the precise approach to seismic analysis is using non-linear time history analysis. It is possible in Robot but:
1/ it is necessary to input time history of ground motion
2/ non-linear time history is the type of analysis requiring significant hardware resources and requiring quite a long time


Another possibility (applicable in some cases) is using standard modal and seismic analysis (response spectra) which is a linear dynamic analysis (with constant stiffness) – in such case model is linearized. Such approach is not recommended for users without significant experience in seismic design and it can be used for rather regular structures with regular arrangement of tension-only bracings.
Generally when model contains nonlinear objects (including tension-only members) and dynamic modal analysis is defined in it this modal analysis is performed for the stiffness of model resulting from the static load case directly preceding the modal load case.
So for instance if this static load case results on all tension-only bracings not working then modal (and seismic) analysis will be performed without influence of these bracings.
If the preceding static load case results in all tension-only bracings working then modal (and seismic) analysis will be performed with influence of all bracings. And so on – generally depending on static loads applied in preceding load case the vibration frequencies and other results of modal and seismic analysis performed for the same model can be completely different.
Of course it is not corresponding to the real behaviour of the structure.
But in case of for instance regular model with X bracings it is possible to define a preceding static load case with some notional horizontal load resulting in half of bracings working (one arm of each X bracing) so the stiffness of these bracings will be used in modal and seismic analysis. In real structure the active bracings are changing during vibrations – in the structure like this or one half or another half of bracings is active. In linearized model this change cannot be done but in case of X bracing it may be assumed that this simplification results in local change limited to each X bracing field.
In case of using such simplified approach it is also important to remember about combinations – combinations of static load cases in nonlinear models are iterated individually – superposition principle is not used for them. In case of linearization performed for seismic load cases the results for them are combined with static loads using superposition principle – as linear combinations.



Rafal Gaweda
Please use plain text.
Contributor
StuartRogers
Posts: 25
Registered: ‎03-07-2012

Re: Barre de treillis / traction compression vs séisme

10-24-2012 07:54 AM in reply to: Rafal.Gaweda

Rafel,

 

Appologies for adding this onto an existing thread, but seemed like a good place for it.

 

I am running a THA on a non-linear system. The model is for a structure which includes x-bracing.

 

For the linear simplification, a Modal analysis is run. It is my understanding that ROBOT then uses the results from this modal analysis for the THA. Is this correct?

 

When I change the analysis to a non-linear analysis (set the x-bracing members to tension only members), does ROBOT automatically change the analysis from a modally decomposed analysis to a different time-stepping method? Or should I be careful to remove the modal analysis from the model also?

 

With regard to your previous answers “modal analysis is defined in it this modal analysis is performed for the stiffness of model resulting from the static load case directly preceding the modal load case” and “generally depending on static loads applied in preceding load case the vibration frequencies and other results of modal and seismic analysis performed for the same model can be completely different” - am I right in thinking that this is not an issue for a THA analysis?

 

I am concerend that I am unintensionally doubling (or halving) the lateral stiffness of the structure depending on the loadcase preceeding the modal analysis.

 

Thank you for your help,

 

Regards,

 

Stuart

Please use plain text.
Product Support
Rafal.Gaweda
Posts: 5,596
Registered: ‎04-26-2010

Re: Barre de treillis / traction compression vs séisme

10-25-2012 05:08 AM in reply to: StuartRogers
 

For the linear simplification, a Modal analysis is run. It is my understanding that ROBOT then uses the results from this modal analysis for the THA. Is this correct?

 

Yes. 

 

When I change the analysis to a non-linear analysis (set the x-bracing members to tension only members), does ROBOT automatically change the analysis from a modally decomposed analysis to a different time-stepping method?

 

Stiffness matrix for modal analysis is taken from the last calculated case before modal case so some tension members "are not working" in this case and this state will be fixed for next modal case(s)

 

Or should I be careful to remove the modal analysis from the model also?

 

Remove Modal? Modal must be defined before THA.

 

With regard to your previous answers “modal analysis is defined in it this modal analysis is performed for the stiffness of model resulting from the static load case directly preceding the modal load case” and “generally depending on static loads applied in preceding load case the vibration frequencies and other results of modal and seismic analysis performed for the same model can be completely different” - am I right in thinking that this is not an issue for a THA analysis?

 

IN such case THA takes mass matrix from Modal case and this matrix is not changed during THA calculations but stiffeness matrix is updated (depending on structure state during each increment for each timestep) in case of nonlinear THA



Rafal Gaweda
Please use plain text.
Contributor
StuartRogers
Posts: 25
Registered: ‎03-07-2012

Re: Barre de treillis / traction compression vs séisme

10-25-2012 06:43 AM in reply to: Rafal.Gaweda

Rafel,

 

Thank you again for your help.

 

I don't fully understand what ROBOT is doing for a non-linear dynamic analysis.

 

You say 'Stiffness matrix for modal analysis is taken from the last calculated case before modal case'

 

and that the modal analysis must be defined before the THA.

 

BUT, 'stiffeness matrix is updated (depending on structure state during each increment for each timestep) in case of nonlinear THA'

 

Is the stiffness matrix updated following each timestep or only calculated once?

 

Also, is the solver implicit or explicit? Are there any solver parameters that need to be considered for this type of analysis?

 

Kind Regards,

 

Stuart

Please use plain text.
Product Support
Rafal.Gaweda
Posts: 5,596
Registered: ‎04-26-2010

Re: Barre de treillis / traction compression vs séisme

10-25-2012 07:41 AM in reply to: StuartRogers

 

Is the stiffness matrix updated following each timestep or only calculated once?

 

 

My mistake I copied part of explanations concerning linear calculations and spectral seismic cases.

Yes, stiffeness matrix is updated in nonlin THA case in each increment in each timestep.



Rafal Gaweda
Please use plain text.
Active Contributor
PatrickSt-Louis5310
Posts: 41
Registered: ‎09-19-2010

Re: Barre de treillis / traction compression vs séisme

11-05-2012 07:48 AM in reply to: Rafal.Gaweda

Why not making a tutotarial video, or an article which show it by a step by step procedure to show to users how to manage this kind of analysis with ARSA ?

 

Please use plain text.
Active Contributor
patkson
Posts: 30
Registered: ‎11-17-2013

Re: Barre de treillis / traction compression vs séisme

09-19-2014 01:54 AM in reply to: annecy-structures
Yh I think it will be nice to show the step by step procedure.
Regards
Please use plain text.