Non-linear analysis, P-delta analysis

[PatrickEC]

These settings are described in two places in the help:

http://docs.autodesk.com/RSA/2013/ENU/index.html?url=filesROBOT/GUID-539BF9B3-3DA5-4E07-8BC6-15284F8...

http://docs.autodesk.com/RSA/2013/ENU/index.html?url=filesROBOT/GUID-FB3C86D3-0E30-43A6-82D6-6C50F42...

I always use Non-linear analysis, because I tested that this is in fact what is usually called a second order or P-Δ analysis. I tested this on:

• a cantilever column with axial load and horizontal load applied at the top
• a column with pinned support at the bottom and a horizontal support at the top

In both cases the additional bending moments were as I expected.

Now, the second option is called P-delta analysis and it is supposed to account for third-order effects, so I am confused why it is called P-delta.

From the help:

"P-delta analysis - takes account of the third-order effects, such as the additional lateral rigidity and stresses resulting from deformation. This effect considers additional forces arising in a deformed structure such as a beam with fixed supports on both ends, loaded by a vertical load, longitudinal forces arise and the deflection decreases."

I modeled such a beam described above, see the attached file, but I do see any longitudinal forces.

[Pawel.Pulak · Accepted solution]

Hi Patrick,

as concerns misleading names of analysis it was already explained there:

http://forums.augi.com/showthread.php?141487-Assorted-queries-non-linear-analysis-for-part-braced-fr...

Repeating here: resulting from backward compatibility with previous versions of the software:(

As concerns not observing the 3rd order geometrical non-linear effects in your model it is necessary to divide the beam in at least 2 parts - to have one node free to move. Attached modified model corresponding to the sceen capture below. It was also discussed in this post:

http://forums.autodesk.com/t5/Autodesk-Robot-Structural/problem-in-analysis-with-zero-displacements/...

The precision of this type of analysis depends on the number of divisions of bars.

---------------------------------------------
If this post answers your question please click "Accept as Solution". It will help everyone to find answer more quickly!

Best regards,

[Gotzman]

Hello

I want to continue the theme of nonlinear analysis in the robot. if possible otvette how you can use the length of the bar elements relultatam obtained from non-linear analysis to the robot in the selection of sections of steel structures. If you can step.

[Pawel.Pulak]

Helllo,

your question is not clear for me.

When I have applied some  "reverse engineering" using Google Translate in English-Russian direction I have received more clear message:

"если это возможно ответте, как можно использовать длины стержневых элементов relultatam получена из нелинейного анализа роботу в выборе участков стальных конструкций."

Do you mean something similar to the point 5.2.2(7)a) of EN 1993-1-1 (Eurocode 3)?:

If second order effects in individual members and relevant member imperfections (see 5.3.4) are totally accounted for in the global analysis of the structure, no individual stability check for the members according to 6.3 is necessary

Or do you mean using Robot to calculate buckling lengths of individual members to be used in steel design?

Regards,

[Gotzman]

---

Or do you mean using Robot to calculate buckling lengths of individual members to be used in steel design?

Regards,

---

Yes it is
Hello, Yes poorly translated the question.

Yes, I was referring to the lengths of derived for the design of steel structures. can be either manual or have a robot

[Pawel.Pulak]

Hello,

in such case it has nothing to do with non-linear P-delta analysis.

The automatic buckling length in steel design is discussed in this forum topic:

http://forums.autodesk.com/t5/Autodesk-Robot-Structural/Robot-2013-buckling-length-calculation/m-p/3...

There were also some discussions related to using buckling analysis to calculate buckling lengths of individual members. The general conclusion is that buckling analysis is suitable for global stability (buckling) of whole structure. Using it for individual members is difficult and inefficient. See these forum topics:

http://forums.autodesk.com/t5/Autodesk-Robot-Structural/Buckling-Analysis/m-p/3299643/highlight/true...

http://forums.autodesk.com/t5/Autodesk-Robot-Structural/Bucking-analysis-of-column/m-p/3709322/highl...

---------------------------------------------
If this post answers your question please click "Accept as Solution". It will help everyone to find answer more quickly!

Regards,

[Gotzman]

Thanks, Pawel, we probably each other misunderstood

The calculation is carried out on the deformed scheme (2nd order theory) on a given combination (RSN). In this calculation, an initial imperfection laid schemes (OBLI), resulting, for example, the analysis of buckling (task Buckling Eigenvalues, EIGE). This technique, to my knowledge, is given in the Eurocodes for steel structures.
In fact, in this calculation indirectly addressing the real flexibility and a gauge length of the elements according to their place in the design scheme.
To determine the safety factor in this case there is a possibility of the iterative selection of the critical load (ULTI). In SOFiSTiK it works. In Robot???

[Pawel.Pulak]

Hello,

I have searched some documentation of SOFiSTiK and it seems (see close to page 53 and then chapter 5.7 of this document) that it is the approach I have mentioned before: similar to the point 5.2.2(7)a) of EN 1993-1-1 (Eurocode 3):

If second order effects in individual members and relevant member imperfections (see 5.3.4) are totally accounted for in the global analysis of the structure, no individual stability check for the members according to 6.3 is necessary

In case of Robot such approach can be used when 2nd order analysis ("Non-linear analysis" check-box active for appropriate design combinations) is used and local and global imperfections are considered in the structure. Global imperfections can be considered using for instance Buckling Deformation (last tab of Analysis Type window) or changing horizontal coordinates of nodes.

Regards,

[legar]

Pawel wrote:

"In case of Robot such approach can be used when 2nd order analysis ("Non-linear analysis" check-box active for appropriate design combinations) is used and local and global imperfections are considered in the structure. Global imperfections can be considered using for instance Buckling Deformation (last tab of Analysis Type window) or changing horizontal coordinates of nodes."

Question is:

Can we use in Robot 2013, Global Imperfections from Buckliong Deformation (last tab of Analysis Type window) together with local imperfections on bars.

It didn't work correctly in Robot 2012 - on January 2012 KW  from Robobat wrote me that problem was signed as RM-26704.

JC - Legar

[Pawel.Pulak]

@JC

Unfortunately RM-26704 is not fixed yet 😞

But it is related to SIMULTANEOUS use of buckling deformation and local imperfections.

Point 5.3.2(11) of EN 1993-1-1 states that buckling deformation is used for global AND local imperfection, so there is no need to additionally define local imperfections:

Regards,

[legar]

Pawel,

In theory we can use p. 5.3.2(11) of EN 1993-1-1, but I have no idea how to use these formulas:

in such a frame:

BTW

As you can see in the model there are 37 parametric bars. Then you can understand my proposal (wishlist for future...) for new parametric members with possibility to change web and flanges prperties on their length . By use of proposed new parametric members there will be max 15 different parametric member types.

JC - Legar

[Tuctas]

  I would like to add something similar to this issue.

  It would be useful if Robot was calculating the Alpha_cr coefficient (αcr) that is defined in EC3 (chapter 5.2) in order to be able to decide if it is necessary to take in to account second order effects or not. 

  Regards

[Pawel.Pulak]

@Tuctas

Calculation of Alpha_cr is registered on our wish list for about 2 year. As I remember your requested for it:)

@Legar

I will have to look in more detail in this Eurocode procedure to give some advices. It can take some time:(

As concerns your "side" topic: implementation of "multi-segment" parametric sections would result in increasing the complexity of New Section window. It would be necessary to add definition of appropriate segments (in absolute and relative way?), section dimensions for appropriate segments. Moreover in such case section labels will be umbiguous - the same section label would correspond to different sections for different segments. Connecting it with the existing possibility to assign sections in the direction coherent or opposite to local X would result in real puzzle.

And it would be necessary to support such way of definition in steel design modules. And here showing results of design for such sections in clear way would be also very difficult.

Regards,

[legar]

Hi Pawel,

Thanks for reply - I am waiting impatiently for advices to Eurocode 3 procedure :).

Regarding to implementation of "multi-segment" parametric sections... hard to say if it is not impossible if we not try to do it :).

BTW

I was using for few years specialized software to design steel frames with tapered sections and in this software it worked perfectly. Modelling of such a frames in specialized software was very easy, because engineer draw structure in SL (steel lines = external flange of girts or purlins) from joint to joint (base plate --> knee --> connection between roof rafters --> ridge... and so on). It was not necessary to calculate coordinates of many points which is necessary in Robot :(... Please remember that after every change of profiles height (during optimization) we must to recalculate all points coordinates :(.

JC-Legar

[t.sautierr]

Pawel, I have made some extra examples of 2nd order and Pdelta (so called in RSA, but we know that it is more 2dn order and 3rd ordre).

Could please confirm that my conclusions are right :

For cantilever and beams aver two supports :

When I increase that loading, at the beginning, no influence or very small between 2 and 3rd order, but for the biggest loads, then the difference is huge -> due to constraint effect.

For beams : between 2nd and third order -> takes into account that the delfected beam "pulls" the support

Thefore, if I could sum up in my mind the main difference between these two analysis :

2nd order : RSA is updating the efforts only, taking into account the pdelta effect and at each iteration it is starting from non deformed chape (common pdelta effect and that's all).

3order : RSA iis updating the efforts and deformed shape, taking into account the pdelta effect and can even add "new" type of effort according to the deformed ahsape, at each iteration it is starting from  deformed chape calculated at the previous step. (geometrical effect).

3order can also highligh effect when loading becomes big (cosntraint effect).

Question : do you have an example of code stiulation 3rd order as to be taken into account? To me global analysis in Eurocodes doesn't ask for that except for very particuliar structure (antenna, ..)

Thanks a lot.

[Pawel.Pulak]

Thomas,

your conclusions are correct.

Also the attached test model is very good and it gives a comprehensive demonstration of geometrical non-linear effects.

As concerns the 3rd order effects the Eurocode does not mention it directly but for instance some points in 5.2.1 chapter can be interpreted in such way that they should be considered - even if it is called there "second-order analysis":

The "pseudo-cable" effects observed for heavily loaded slender beams (bars 22to25 in your test model), where under flexural load significant tension forces can be observed, fits the description of point (2).

Considering these effects "increase the action effects significantly or modify significantly the structural behaviour".

Additional note:

When checking your test model I have noticed some anomalies of results. The reason was in changing the tolerance of iterations from the default value of 0.0001 to 0.001. After restoring the original values the anomalies are not observed. It is shown in this video:

Best regards,

[t.sautierr]

Very interesting to see the difference what huge difference when setting the tolerance to loose ... !

Do you have explanation for such a difference in force results : I assume as the criterion is for the whole structure, you may have difference less than 0.001 on the whole matrix of results between step X-1 and final matrix step X, but a big difference in two points -> support of the columns with the heavy load?

In the first model I put a the tolerance to 0.001 because 0.0001 wasn't converging with such a load this particuliar bar and I mus confess that I found these results ok because it is non linear so I wasn't shocked to multiply the load by 2 or 3 and have the forces multiplied by 4-5-6 whatever.

i assume the same can happen regarding displacement.

[Pawel.Pulak]

Unfortunately the more separated the model (composed of more separate parts) the more sensitive is the nonlinear algorithm to the tolerance values during iterations - tolerances are checked "globally" and in may results in local fluctuations.

When leaving in your original model only bars 21to25  then there is no anomaly in bar 25 even for the tolerance of 0.001.

Using this tolerance for the model composed from 30 separate parts and from 5 separate parts makes the difference.

I will discuss it with developers to confirm.

Regards,

[Tuctas]

I hope that some time the titles of the two options of non-linear analysis in Robot will be at last corrected...(this is the only way to stop confusing the users...).  

I think that he picture that Artur had uploaded in the 9th post of an other related discussion (http://forums.autodesk.com/t5/Robot-Structural-Analysis/Geometric-non-linear-analysis/m-p/4429165/hi... gives many answers.

t.sautier, when you say: "2nd order : RSA is updating the efforts only, taking into account the pdelta effect and at each iteration it is starting from non deformed chape (common pdelta effect and that's all)" obviously you mean pDelta effects and not pdelta (actually the correct symbol of these effects is P-Δ, and P-δ respectively, as the come out from the Greek letters). When you say that at each iteration the analysis is starting from non-deformed shape, you mean the deformed shape of the elements and not the deformed shape of the structure (the later is generated because of the displaced nodes of columns) don't you? 

[t.sautierr]

---

Tuctas wrote:

I hope that some time the titles of the two options of non-linear analysis in Robot will be at last corrected...(this is the only way to stop confusing the users...).  

I hope also .... I think many engineer using RSA performed 3rd order analysis without knowing it!

t.sautier, when you say: "2nd order : RSA is updating the efforts only, taking into account the pdelta effect and at each iteration it is starting from non deformed chape (common pdelta effect and that's all)" obviously you mean pDelta effects and not pdelta (actually the correct symbol of these effects is P-Δ, and P-δ respectively, as the come out from the Greek letters).

this big delta and small delta still confuses me ... I meant the effect of creating a moment beause of non centered own weight due to deformation. I don't remember which delta big or small we are talking about for this effect 🙂

When you say that at each iteration the analysis is starting from non-deformed shape, you mean the deformed shape of the elements and not the deformed shape of the structure (the later is generated because of the displaced nodes of columns) don't you?

Hummm, I'am not sure what I meant 🙂 as my example was with one element (one bar). In my mind, this applies also to a whole structure : 2nd order ->

For one increment of loading :

iterations 

step 1 : RSA calculate deformed shape 1st order,

step 2 : then second step calculates induced moment because of non centered own weight,  

step 3 : retstard from non deformed structure and applies ow weight + above moment 

step 4 : new deformed shape new moment etc ....

iterates till difference between effort of iteration n-(n-1) < tolerance

Next increment starting from non deformed shape + effort from previous increment.

But Pawel has to confirm 😉

For third order, much more complicated ..... because stress matrix in addition, updating of this matrix, stiffness matrix also updated, the two matrices are linked stiness is inluenced by stresses, .... etc .... I would say that as everything is updated at each iteration, then its like the calculations is made using the deformed shape at each iteration;

But Pawel has to confirm 😉

thanks Pawel for your explanations and look forward if you have news from the development team. But I'm not sure something can be done except choosing another measure of the solution rest .... I keep in mind my this effect happens when structures is made of part of sub structure with a complete or partially independent behavior -> the criterion doesn't detects these difference because it average at the whole structure scale. Maybe we could have the same effect for example with a building with one floor very loose compared to other floor very stiff -> one shall not play with tolerance espacially in this case 🙂