cable design

[AJA14]

In analysis of cables via robot, a pretension value has to be inserted and then iterations have to be made. I was wondering if there was a way to predetermine a good judgement for the pretension to be used for the cable which eliminates the need for doing many iterations. This may not be a pure robot question but I would appreciate the help nevertheless.

[Pawel.Pulak]

For preliminary analysis of models containing many cables it is much more efficient to define cables not by pretension but by elongation or length:

In such case when specifying for instance zero relative elengation the unloaded cable length equal to the distance of end nodes will be used. For instance +0.01 relative elongation corresponds to unloaded cable length 1 percent longer than the distance of end nodes.

In case of defining cables by pre-tension it is sometimes very difficult to predict what unloaded cable lengths may be necessary to obtain it and moreover there is a risk that equilibrium and convergence is not possible with reasonable lengths of cables. See:

http://docs.autodesk.com/RSA/2012/ENU/filesROBOT/GUID-DCDD6D6E-D1BA-4535-9A21-AA28C9277CF-243.htm 

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

Best regards,

[fmp999]

I am having the following problem with a guyed tower (17 m) and 4 guys, when i try to run the analysis with the non-linearities on=non-linear analysis +P-d (figure below), the program gives me a error:

  

The cables are defined with pre-tension F0, should i change to relative elongation?

And if with a relative elongation of 1%, still does not converge, should i try to reduce the elongation to 0,1%?

I already saw the thread http://forums.autodesk.com/t5/Autodesk-Robot-Structural/Disproportionate-Collapse-and-Catenary-Actio... in wich you sugests to do some modifications to the algorithm solver, so i dont know if i should try to do my analysis with the non-linearities options turned on or off.

And after i find the cable elongation, the pre-tension F could be obtained from F=A*dl*E ?

with A=area of section; E= modulus of elasticity and dl=elongation and F=pre-tension

Thank you,

[Pawel.Pulak]

The message "Matrix is not positive definite..." may result from 2 reasons:

1/ tower not stifff enough or tension forces in cables too high - resulting in buckling of the tower

2/ sometimes such message is resulting from the instability of the structure - in case of guyed towers it is very easy to forget about fixing RZ rotation at the bottom of the tower and defining only pinned support there

It is also important to remember about using full Newton_Raphson method - see message 6 of http://forums.autodesk.com/t5/Autodesk-Robot-Structural/Disproportionate-Collapse-and-Catenary-Actio...

If still problems please attach the model.

Regards,

[fmp999]

Hello,

I am still having problems, i changed the cross sections of the tower to the highest angles availables in Robot and i still had the error of critical load excedeed for the case of only selfweight acting on the structure. Than i changed the cables from F0 to relative elongation to 0.0001 and just in this case i the program did not show any error.

The support of the tower is defined with RZ fixed and also all the translations degrees are fixed too.

Is there any way to send the model just to you?

Thanks,

[Pawel.Pulak]

Your description suggests that the reason of problems was corresponding to point 1 of my previous answer: "1/ tower not stifff enough or tension forces in cables too high - resulting in buckling of the tower"

When defining the cables by Fo=0 Robot is in reality using zero elongation so it can result in "short" cables, big tension forces in them thus big compression force in the mast - thus buckling of it.

Using 0.0001 relative elongation the length of cables was increased, tension forces in them reduced, compression force in the mast reduced too - thus no buckling.

Later today I will look closer at your model sent using PM.

Regards,

[Pawel.Pulak]

Additional remarks related to the model received by PM:

F0 force in cable definition was not  Fo=0 but Fo=1 kN 

The model was slightly unsymmetrical and this connected with the existence of interacting cables defined by the same tension force resulted in problems.

As already suggested on this forum recommended to define cables by elongations. In such case forces can be indirectly controlled modifying the values of elongations.

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

Regards,

[Jummybear]

Hi,

I ask my question here instead of creating new topic.

Just want to make clear one thing about cables. In my pic i simple model, distance between support = 30m, cable length L=30m. Why I get the sag of ~244mm? It means that cable length is something else, not 30m, where it is fixed in my cable defenition. I supposed that I will get huge FX forces at support nodes with cable length of 30m which is also the support node distance...

Or such sag of 244mm is due to cable elongation caused by selfweight?

Thanks.

[Pawel.Pulak]

Yes, this sag is caused by the cable elongation caused by selfweight.

30m is the unloaded length of cable (unloaded = under no loads)

As you can see the horizontal reactions in the top cable are 3.6 kN - they are approximately equal (neglecting inclination resulting from sag) to the tension force in the cable. For the area of 1cm2=100mm2 it corresponds to the stress of 36 MPa. For S 355 steel it corresponds to the strain of 1.7e-4 and for 30m length of the cable it corresponds to increase of length of about 5mm.

244mm sag is quite reasonable for 5mm increase of length for 30m long cable.

In the bottom cable the sag is bigger and horizontal reactions are smaller because of the influence of horizontal displacement of columns the cable is connected to.

Best regards,

[fmp999]

Hello, another question related with the topic.

I am trying to run a modal analisys, in just a simple cable, pinned at the ends... but i got the following error: dynamic degrees of freedom equal to 0.

So is it possible to run a modal analysis with cable elements?? I already tried to divide the cable in n elements, but the program does not converge.

[Pawel.Pulak · Accepted solution]

Dynamic modal analysis is a linear analysis assuming constant stiffness.

Cables are non-linear objects and their stiffness can change very significantly.

So here is the first incoherence.

Generally in case of modal analysis of structures containing non-linear objects (cables, tension-only members, uplift supports, etc....) Robot linearizes the model, i.e. runs modal analysis using constant stiffness resulting from the static loads case directly preceding the modal load case. It means that small vibrations from the deformed shape of the static case are analysed.

If you want to analyse anything else than small vibrations for such model then it is necessary to run nonlinear time history analysis

Now as concerns your observations:

1/ cables have no rotation degrees of freedom so a single cable element with supports on both ends (pinned or fixed) will report 0 dynami degrees of freedom

2/ after dividing the cable in n elements to obtain convergence it is necessary to: a/ activate "Non-linear" + "P-delta", b/ define the cable by elongation or by length instead of the default definition by force (impossible to find solution for the  deflected shape of cable with precisely the same tension in all elements of the cable chain)

After solving a/ and b/ and obtaining convergence the modal analysis can give results - but they will be for the linearized model as I mentioned at the beginning.

Regards,

[Jummybear]

Thanks Pawel, now its clear.