What Elements Are Best for Modeling Tensioned Cables in ANSYS?

[rockdogy]

Hi, what sort of elements would you use on a tensioned cable, pinned at either end, that is to have a uniform load across it ?

a single link8/10 element can't work because you can't put a UDL on it, only 2 nodes...Mulitple link elements won't work because there is no stiffness at each node, it just flops around giving a stupid solution. Unless there is something i am missing using link elements.

Any help appreciated, thanks.

 

[CFDFEAGURU]

You should use a 2D beam element and be sure to set the element properties so they include any additional results that you might need.

Thanks
Matt

 

[rockdogy]

Its a 3d problem though. I am using 3node beam elements, but they bend and don't represent a cable properly.

 

[CFDFEAGURU]

I don't understand how a simple cable is a 3D problem. Can you post a picture of your geometry? Also, what is the ANSYS name of the element that you are using?

Thanks
Matt

 

[rockdogy]

sorry its not just a simple cable, its a structure - basically, a vertical mast, with 5 tensioned cables running from the top point of the mast to supports at the ground.
im using beam189 elements for all. its not ideal obviously for the cables, but it may just have to do.

at the moment I am having bigger problems getting a converged solution with non-linear geometry. if i apply too much load to one of the cables, it doesn't converge and aborts. even with sub steps exceeding thousands.

what could the problem be ?? I've tried fully restraining all restraints, or pinning, etc. still doesn't converge with a realistic loading.

could the problem lie at the apex, where all the cables come together with the tip of the mast ? its a single node, each element shares that node. seems fine to me though...

thanks.

 

[CFDFEAGURU]

Sounds like you don't have the geometry connected correctly. Did you build the model using keypoints and lines? If so, type this command into the command line. NUMMRG,kp

This will merge all of the coincident keypoints and lines so that the model is all connected correctly.

Also, make sure that you the large displacement static option turned on in the solution controls.

Also, assuming that you build the geometry in units of inches, make sure you are applying the loads in the correct units.

You can always run a simple modal analysis and watch the first 3 modes and if your model isn't connected properly you will see it flapping around.

Thanks
Matt

 

[nvn]

rockdogy: What type of element on the mast do all the cables attached to at one node? A beam189? Are you greatly overstressing any of your materials anywhere in the model? Are your element properties, material properties, and applied loads valid and input correctly, and did you enter them using consistent units? Have you checked your model for coincident, disconnected nodes? Can you run a linear statics analysis first (after the modal analysis), just to see if the model runs, and to see if something is greatly overstressed in the linear statics results?

 

[rockdogy]

CFDFEAGURU - i built it in solidworks, and imported the sketch. I entered that command anyway. I ran a modal analysis, and as you said, two of my cables are flapping around like maniacs. these are the two that are behind the mast, and that provide reaction to the other front cables which have the loads on them.
but they are still connected at either end ! its just they are deforming like crazy.

nvn - yes, they are all beam189 elements that share the same node at the top. The cable/beam189 that the uniform load is applied deforms quite a bit, realistically about half a meter it will bend.
ive checked nodes, all seems fine. And linear static analysis runs and gives a solution which is expected (plus a huge deformation of the loaded cable , hence requiring nonlinear geometry. although the linear static solution says its like 1000 meters deformed which is more than youde think the linear would do). units and everything else is all good.

So, why does a linear static give a solution, but the modal showed the cables flopping around ? why are they doing that ?

i think ill delete the cables, then rebuild those lines in ansys using key points...try that.

 

[nvn]

rockdogy: The cables can deflect a lot in the modal analysis; no problem. The only thing you want to check for in the modal analysis is to see if any element ends are becoming disconnected. Are any ends becoming disconnected? If not, try the following.

On a temporary copy of your model, reduce your applied loads (and any preloads) to one hundredth of their current value. Then rerun the geometric nonlinear analysis using, say, 1000 time steps.

If the above fails, check your material stress-strain curve. If you are using a bilinear, elastic-perfectly-plastic stress-strain curve, in which the second line is completely horizontal, try changing the second line to a sloped line. Then rerun the analysis mentioned in the second paragraph, above.

If the above fails, and if each cable consists of only one element, change your model to at least ten elements per cable, then rerun the analysis mentioned in the second paragraph, above.

 

[minger]

Simply using BEAM elements will not behave 100% correct for this analysis. BEAMs assume that the element can be loaded in both tension, as well as compression. You're elements cannot. You will need to join your BEAM elements to COMBIN, or more than likely MPC elements in order to simulate this "no-compression" response.

However, I suppose assuming that these cables are preloaded significantly, you "could" assume they are always in tension, but again, you would need to model the preload, which could be done via COMBIN spring elements.

Do you have any images of your deformation or element plots?

 

[CFDFEAGURU]

Yes, now that you are supplying us with more information on the problem we can help you better. Please show the actual geometry and material props/real constants then we can help guide you to the right solution.

Always, put as much information in your questions as possible.

Thanks
Matt

 

[minger]

After a quick RTFM, it appears as if the proper way of modeling cables/wires are the user of LINK10 elements, which allow for tension or compression only spars.

LINK10s should only be used when elements 'can' go slack. If the final configuration is known to be always taut, then LINK8 should be used. No bending stiffness is included in either configuration, but may be added by superimposing a beam element with a small area on each LINK element.

See the verification manual, VM31 for a Cable Supporting Hanging Loads using LINK10 elements.

p.s. LINK167 can also be used in your case.

p.p.s. It would still be a good idea to show your problem sketch.
The initial strain is entered via real constant.

 

[nvn]

rockdogy wants to apply a UDL; see post 1. I think his beam189 elements should work fine for this application; that is not the problem.

He doesn't need to worry about whether any cables are currently going into compression or not; that isn't causing the model to fail. He can deal with that later (if he has cables in compression), after he gets the model running, by adding one short tension-only link10 at one end of each cable, I think.

rockdogy: For now, remove preload, don't change element types nor make the model more complicated yet, see post [strike]10[/strike] 9, and let us know what happens.

 

[rockdogy]

Thanks Minger, your right, but I am just going to stick with beam elements, it should do for the moment. ill might try those things you mentioned later, when i focus more on the details of the problem.

i attached a model pic. that's with 10 nodes selected, with 100 N force in x-direction. and all DOF restraints.
(i want to be applying a 3000N uniform load really, so wat I am doing is much less)

material is linear elastic. no real constants, just two sections i created which i select when meshing.

Okay, so post 10, with 100N at 10 nodes, i selected large displacement, with 1000 sup steps. ran it, didnt converge. Changed it to 400 sub steps, and it converged...change it back to 1000 and it converges, lol.

bumped the load up to 200 at each node...cant get it to converge. tried 6000, tried 400 steps. won't converge.
strange thing is sometimes it will work, then most time it doesnt. when i get a solution, with the lower loads, it deforms as expected.

 

[nvn]

With 100 N at 10 nodes, and 400 substeps, what are the maximum stresses in your model? And what is the modulus of elasticity (E) and tensile yield strength in your model for that material? And what are the maximum displacements?

 

[rockdogy]

max displacement is the centre of loaded cable, at 340mm. Max stress is about 100mpa in that cable.
the cable properties are 10mm diameter, elastic moduls is 193gpa, poissons ratio 0.3. no yield stress , its just linear elastic.
Just now, i tryed to re-run it at 400 steps, and it didnt work. 200 did though...

 

[rockdogy]

btw the modulus of the mast is 60gpa. i put it up to 600gpa now, and the solution solved for a 3kn load on the cable. after fiddling with time steps still.

 

[nvn]

rockdogy: See my question in the first paragraph of post 9, and let us know the answer to that question. Did you turn on the large displacement static option, mentioned by cfdfeaguru in post 6?

You said the cable stress is 100 MPa. And what is the maximum stress in the mast?

Perhaps set 10 time substeps on the time control menu, and perhaps try the arc-length method. On the Arc-Length Options menu, set Max multiplier (maxarc) to 1.0, and Min multiplier (minarc) to 0.1.

Also, perhaps try hand calculations, using the force the cable is applying to the mast, to attempt to ensure the mast is not trying to buckle.

And maybe cfdfeaguru, minger, or someone has additional advice.

 

[CFDFEAGURU]

Well, for a problem this simplistic, ANSYS shouldn't have a problem. If we assume that all of the loading is correct, the material constants are correct, the real properties are correct, the geometry is connected correctly and the solution is still chaotically converging depending on the solver settings then I would have to say that the loading on the cables is just too great.

What are you trying to calculate? The displacement of the entire structure, the reactions at the cable supports, the stress distribution down the length of the cable, ... ?

Also, save all of the time steps and view them as the solution proceeds. Primarily look at the last converged time step and see what the elements are doing.

Thanks
Matt

 

[rockdogy]

nvn, i think cfdfeaguru is right in saying ansys shouldn't have a problem. I switched "line search" to "on", and max equilibrium iterations to 1000, based on a nonlinear buckling example i was just reading, and the solution works like a charm.
btw i am looking at all you mentioned, displacement, reactions, stresses...

Thanks very much for working through this with me guys, at least now I've got a better understanding of debugging models.
I might have a crack at what minger was going on about a bit further down the track, so expect me back here, lol.
cheers.

 

[CFDFEAGURU]

Sounds good. Debugging models is what makes you learn ANSYS.

Ask me any questions that you might have in the future.

Thanks
Matt