Reactions/Model precision

[Rafacascudo]

I´ve been searching similar threads ,but I am not satisfied with the answers.

It´s a model of a large house , pretty basic , with bars ,walls and slabs. Surprisingly I am getting very weird reactions for all load cases(all linear analysis). Checking the controlling values ,I noticed that precision values are way too high , although there is no true error/warnings during model analysis(automatic solver)( one instability type 3)

All loads have precision problems , especially the horizontal ones.

If I increase the number of horizontal supports ,it gets better but far from prefect/acceptable.

Even making all supports fixed( and there are many!!!) results are not perfect.

I tried using all solvers , repair mode , turn Rlink on/off.  Only to notice that they are all reporting different warnings/error(some false) , that adressed ,don´t fix the imprecision

What factors can cause this analysis imprecision? Why there isn´t a warning alerting the user to this BIG analysis error!!!!!

Model attached

[StefanoPasquini6790]

Dear Rafael,

I can't find the issue, to investigate the problem I've isolated the PP condition and also in this case there is a lack of precision of about 34 tons. The lonely think that I can suppose is that in the bars list there is a kind of bar with zero lenght and zero weight, see this picture:

 

Try to investigate in this topic, probably there could be some problems with this bars.

Cheers and Forza Robot

[Rafacascudo]

Thx Stefano for taking the time.

It was a very strange N/A bar with no nodes , no length ,no nothing which only appears on "values" tab on bars table.

Not a single warning. Deleted it but , it remains the same.

Many weird things happening on this RSA 18.

As always I leave the solver on automatic ,as recommended. On my quest to detect what is happenning , I set the solver to any available. To my surprise the Skyline solver detected a serious error that is having a support nodes as a slave node on a rigid link !!!!

How could this pass undetected when having "automatic" solver set???

What else should we be aware????

Very concerned about this!!!!

[mustafahesenow]

Hi @Rafacascudo

I had checked the model also. 

I have few comments on it.

1- There are nodes shown in reaction tables even they are not support.

2-If you check the nodes who is have reactions along x when only gravity loads applied you will find them on one edge of the building where the triangular wall stiffeners exist.

3-The supports under many columns defined as roller ( why ) if you change them to pinned the difference will be much less than before. 

[Rafacascudo]

Thanks  MH ,

1- Could not find these "intruder" nodes. All nodes on the reaction table have force values other than zero ,and the list is the same when I ask to display only the nodes which are support on the nodes table

2 and 3 - Yes ,Those on the edge are the supports for the inclined piles.  This model is for a friend who asked to be like this , because he wants these piles to resist al the horizontal loads from the soil load cases.

Model is still preliminary ,just to check overall reactions.

Anyway , these are design decisions yet to be made . Cannot understand why of these calculation imprecisions!!!

[Rafacascudo]

Well, after many  trials and experiments , the culprit was 0.1581mm!!!!

On top floor , 2 panel slabs with one slab being moment released along the common edge. Also on this common edge there is a large beam which was not aligned by 0.012mm(perpendicular distance).

I would expect Robot to detect this and merge the nodes in the meshing process or  put 1 billion meshed nodes between the bar and the panel edges.

So ,anyway , I corrected this and model ran smooth , with no precision errors in the Reactions table.

   Not sure why this tiny model imprecision caused so large problem , but at least it served to realize that some(many??) errors can go undetected or unreported depending on the solver choice you use, even if it is the most recommended one.

By the way ,model was generated based on an autocad lines drawing . So probably this tiny imprecision came from there.

[Artur.Kosakowski]

Hi @Rafacascudo

As always I leave the solver on automatic ,as recommended. On my quest to detect what is happenning , I set the solver to any available. To my surprise the Skyline solver detected a serious error that is having a support nodes as a slave node on a rigid link !!!!

How could this pass undetected when having "automatic" solver set???

This is actually correct. It is the limitation of rigid links that you cannot have a support in a slave node of the rigid links and as the Skyline solver uses rigid links the corresponding error is displayed. The automatic setting results in having either the multi-threaded or Sparse solver being used which forces modelling rigid links with RLink elements which allow for such support definition.  

[Artur.Kosakowski]

Hi @Rafacascudo

You may try to use this option:

What I personally often do with models like yours is instead of the above option is to use this one prior to model generation or often even for selection after local meshing of some panels:

If you find your post answered press the Accept as Solution button please. This will help other users to find solutions much faster. Thank you.

[Rafacascudo]

Hi Artur,

Are you saying that in "automatic" solver(Sparse or multithread) RSA allows  , for example , a fixed support being a slave to a "regular" node ,considering it correct , or just not issueing a warning/error??

[Rafacascudo]

Artur ,

    Investigating further I found out that the real trigger to the  imprecision errors  were the linear releases applied to one of the slabs along that whole edge. Deleting the releases for this edge makes the model run without imprecision ,despite the beam not supporting the slab for just  3.05m in a total edge length of 14m due to the tiny misaligment. How can the the linear releases cause so much harm? I could understand if the whole edge was without support from the beam , but it was just around 20% of the whole edge length.

  And the most important ,Why doesn´t Robot give an error warning telling the user that there´s something wrong with your model, check reactions precision!!!????

   Results were pretty much wrong and unacceptable and despite of that robot ran it to the end without a single glitch or error message.

[Refaat]

Hi @Rafacascudo

And the most important ,Why doesn´t Robot give an error warning telling the user that there´s something wrong with your model, check reactions precision!!!????

Robot doesn’t give such like this message . even if the structures a absolutely unstable (Pic 1) .

In your case the instability warning was happened at calculation node Not at standard node which should have nodal support (Pic 2) .

But really it is very serious issue should be considered soonly as error message not as instability warning .

Refaat

[Rafacascudo]

Hi @Refaat

The warning type 3 instability keeps appearing even for the corrected model . I believe its due to many rigid links , causing large differences on elements stiffness.

So I think , the type 3 warning was not an indication that something was wrong with model/reaction precision. That ,passed undetected.

What scared me is that I was already extracting results ,and had to make minor corrections in the model(local panel direction) And noticed that the reaction results changed dramatically for loads without relation with that minor change.

[Refaat]

Dear Rafacascudo ,

I think there is something should be corrected. Because as we know these calculation nodes are created due to using of linear releases.

So, once I deleted the mesh and all the linear releases then many isolated nodes were appeared (Pic 1) .

After that I deleted all of these isolated nodes  and remeshing the model again then running the analysis.

So incoherent mesh error in some panels also was appeared (Pic2).

Perhaps all of these due to inaccuracy when the model build up (Autocad lines) .

Refaat

[Artur.Kosakowski]

Hi @Rafacascudo

I agree that Robot could indicate the situation where the sum of applied forces differs from the sum of reaction for linear static analysis however I'd also say that checking this is as well as displacements/rotations of nodes and shape of deformation is the first thing to be done after running the analysis.

[Rafacascudo]

Artur, Sorry for the delay but,
Of course I always check displacements , reactions and Forces on bars and panels. But for reactions The 1st check is mainly graphically. And graphically it was not possible/easy to detect the error. It looked ok for a 1st glance, because values were not absurd as in type 1, 2 instabilities errors.
I have been reading this forum almost from its beginning , and I don't remember many or constants posts stressing that reactions precision should always be checked. I suppose that this a very rare error to occur during Model analysis, isn't it?
Robot gives warnings for so many things, some of them that almost always are of no importance as type 3 instability and " load not distributed on claddings..." which can be fake ,that I wonder why this error has never been addressed with at least a warning.
Because to me this is one kind of error that can never be ignored or be considered as a fake!!
Isn't it??

[Artur.Kosakowski]

Hi @Rafacascudo

I do understand your point. I will create a request for adding the corresponding warning on your behalf and forward it to the development team.

[mustafahesenow]

Hi @Rafacascudo

This is really very important point. and it should be there is a warring message related to this matter appear when will occurs.

Many thanks for this important note.