Modeling of Cable in a bridge

  • 1.3K Views
  • Last Post 28 April 2019
mradwan posted this 25 April 2019

Hello

I have to model a cable stayed bridge on Ansys workbench , I have a lot of difficulties in modeling the cables , I have tried using springs and links but I couldn't get it to work. Either the solution doesn't converge or I got a solver pivot error.

Kindly, any suggestions.

 

Order By: Standard | Newest | Votes
jj77 posted this 26 April 2019

I assume then that it might be the connection between columns and links/cables.

Ok, use the edit mesh and insert marge node group. This will work if you split your column which I assume is a 3D body into slices so that at every start/end of a line body there is one vertex on the column. In that way we can merge the nodes between the ends of the links and the column nodes using the merge nodes function.

 

To see this look at the image below from a small example - two columns, and two cables going across - one is located at the vertices on the columns and the one below it is not - thus there is a pivot error. Now if the bottom one was connected at column vertices, which can be created by splitting the column there, then it would have been OK, and it would have solved.

  • Liked by
  • mradwan
jj77 posted this 25 April 2019

Cables can modelled with link180 element.

 

We have had quite a few discussions about that, so have a look (typically one needs amount of pre-stress to stabilise them).

 

See here how to do that:

https://studentcommunity.ansys.com/thread/transmission-line-simulation/

 

mradwan posted this 25 April 2019

Thank you for answering my question but I have a problem in connecting the cables to the column I always have these list of errors even for a line model for the bridge. I tried to use joint and contact but nothing is working

Solver pivot warnings or errors have been encountered during the solution.  This is usually a result of an ill conditioned matrix possibly due to unreasonable material properties, an under constrained model, or contact related issues.  Check results carefully.

The model dimensions in the solver unit system were determined to be very large.  This may lead to numerical accuracy issues.  Check results carefully.

A solver pivot warning or error has been detected in the UY degree of freedom of node 525 located in SYS-5\Beam (beam). This is usually a result of an ill conditioned matrix possibly due to unreasonable material properties, an under constrained model, or contact related issues.  Check results carefully. You may select the offending object and/or geometry via RMB on this warning in the Messages window.

Solver pivot warnings or errors have been encountered during the solution.  This is usually a result of an ill conditioned matrix possibly due to unreasonable material properties, an under constrained model, or contact related issues.  Check results carefully.

One or more MPC contact regions or remote boundary conditions may have conflicts with other applied boundary conditions or other contact or symmetry regions. This may reduce solution accuracy. Tip: You may graphically display FE Connections from the Solution Information Object for non-cyclic analysis. Refer to Troubleshooting in the Help System for more details.

Joints are being used in the current analysis with Large Deflection turned Off.  Thus, only linearized joint behavior will be considered.  If finite rotation and large deflection effects are to be considered, please turn on Large Deflection.

One or more beams with user-defined mesh cross sections have been sent to the solver as pre-integrated sections. Beam section results will not be available for these bodies. If these results are desired, please change the Cross Section (For Solver) property for those bodies.

One or more parts were found to be unmodified so smart updated.

 

mradwan posted this 27 April 2019

That solves the connection problem but only for beam elements and only for small loads, if I apply the self weight of the structure or change the type of element to links I will have the same error.I tried to prestress the cables by the code you provided in the link above but still there's a problem.

Kindly, can you help me with this issue and how to properly prestress the cables?

Thank you very much

----------------------------------

code used 

INISTATE,SET,CSYS,-2    ! LOCAL ELEMENT SYSTEM FOR PRE-STRAINS 
INISTATE,SET,DTYP,EPEL   ! STRAIN
INISTATE,DEFINE,,,,,1E-7      ! STRAIN VALUE

jj77 posted this 28 April 2019

Hard to say what happens without looking into the model.

 

I would say start with adding the above inistate snippet for all line bodies are converted from beams to links - this adds a low randow pre-strain for solver/convergence stability only. You might need to change that to a pre-stress as it is in reality by saying:

INISTATE,SET,CSYS,-2    ! LOCAL ELEMENT SYSTEM FOR PRE-STRAINS 
INISTATE,SET,DTYP,STRE  ! STRESS
INISTATE,DEFINE,,,,,1      ! STESS of 1 unit (say if SI it is 1 PA)

- have in mind what you are trying to do is vert complex and if you are student I would recommend studying and doing basic FEA not bridge analysis which is something you will learn after many years of working with bridges as bridge engineer. (cable tension is also a type of optimisation problem)

 

Try that and use auto time stepping as ON, and say with 20 initial 20 minimum and 100 maximum.

See this for details:http://www.padtinc.com/blog/the-focus/you-dont-wanna-step-to-this-breaking-down-loadsteps-and-substeps-in-ansys-mechanical

 

No I am travelling away for work teaching engineers FEA, so I will not be able to look into this, so good luck and remember try to learn basic solid and beam mechanics and make sure you take a course in FE and understand the different type of elements before doing complex things - take it in steps. 

 

Close