Tension only members in software packages 6

[atee001]

Hi,

I've found that some software packages have an option of specifying a particular member as a "Tension only" member.

However,I've never used this functionality in my practise so far (though I am relatively new to the field!).

I am curious to know what is the advantage of specifying a member as a "Tension only" member?

Also,I found that this functionality of "Tension only" member is found in the Non-linearity option corresponding to structural analysis in some packages.

Could anyone shed some light on this functionality of Tension only members and cite some situations wherein you have used this option and in what context?

Thanks in advance.

 

[Grahammachin]

I have used tension only members in the analysis of steel frames where the cross bracing is steel flats. The steel flats are good in tension but next to useless in compression. Hence specifying them as tension only members.

 

[asixth]

Bascially, after performing the analysis, the software you are using will search to see whether specified tension only members are under a compression. If they are, then that element will be deleted from the analysis and the analysis is re-run.

Design elements such as angle and rod bracing is typically specified as tension only.

I have run into problems when analysis a pin jointed truss which tension only diagonals such as a roof frame. If the truss is symmetrical and symmetrically loaded, the two internal diagonals are switch of from the analysis and an instability occurs.

 

[EdR]

Also useful for modeling cable components.....

Ed.R.

 

[271828]

...and good for modeling contact--just put the tension-only member in on the opposite side of the member.

Just be sure to run lots of simple test cases for which you know the answer. I've tried tension-only members on several packages over the years and several didn't work correctly. SAP2000's current cable elements work fine, best I can tell.

 

[jhardy1]

"Also,I found that this functionality of "Tension only" member is found in the Non-linearity option corresponding to structural analysis in some packages."

Using Tension-Only members is by definition non-linear, because the structural stiffness matrix must be modified whenever a Tension-Only member is added or deleted from the structural model, and an iterative analysis is required until a converged solution is obtained for all load cases. If you are running several load cases, it is very possible that some Tension-Only members will be in tension for some load cases (e.g. wind from north, say), but compression for others (e.g. wind from south), so each such load case will conceivably have a different set of active members, each of which requires its own solution.

If you specify Tension-Only members, but run a Linear Analysis, most software packages would include ALL Tension-Only members in ALL load cases, regardless of whether they are in Tension or Compression.

 

[atee001]

Hi all,

In an analysis, if a member is specified as tension-only,but during first analysis found in compression,then (As said by asixth) in the reanalysis(second time) that member would be deleted from the calculation and reanalysis carried out.This would thus modify the structural stiffness matrix (as pointed out by JulianHardy).

But,JulianHardy,I do not get your point when you say that-

"If you specify Tension-Only members, but run a Linear Analysis, most software packages would include ALL Tension-Only members in ALL load cases, regardless of whether they are in Tension or Compression"

Can you kindly shed some light on this statement?

In any case even in linear analysis each load case would require its own solution and when the user generates combinations he could superimpose the laod cases to get the effects for combinations.Right?>

I am trying to say that superposition is still valid even in Tension only members??Then,why include it in Non-linear analysis when superposition is valid?

 

[asixth]

Some packages will only calculate one stiffness matrix for one freedom case for all load cases.

So if an element defined as "Tension-only" goes into compression for any load case than that element will be removed from the analysis. This isn't ideal and the developer producing the software should be notified.

 

[enginerding]

RISA-3D has a pretty good option for tension-only members. They call it an Euler Buckling member. These members can take compression up to their critical buckling load. After the compression exceeds this value, it shuts it off and eliminates it from the stiffness matrix. This helps with model convergence.

Sometimes with true tension-only members you can get a situation like asixth was discussing where the model will not converge because when the model shuts the member off and re-runs the analysis, the would-be strain in the member is a tensile one and the program will turn the member back on again. Next run off, next run on, and the solution will never converge. If you allow the member to take some small compressive force the model will be able to converge - hence the Euler Buckling member in RISA-3D

 

[blackmaddog]

One reason to use tension on only is to avoid the seismic compactness criteria of AISC 341-05 Seismic Provisions section 14.2 for OCBF's.

Also, sometimes a tension member that gets incidental compression in certain load cases gives high code checks. These can be avoided by using tension only.

 

[IFRs]

I use both tension only and compression only elements to mimic chains/cables and foundation supports, respectively. Seems to work nicely (in Cadre).

 

[jhardy1]

@ ate001:

But,JulianHardy,I do not get your point when you say
that-

"If you specify Tension-Only members, but run a
Linear Analysis, most software packages would include
ALL Tension-Only members in ALL load cases,
regardless of whether they are in Tension or
Compression"

Can you kindly shed some light on this statement?

For a linear analysis, most packages will simply assemble the stiffness matrix for the whole structure, including all tension-only members, compression-only members, and any other elements which have any kind of non-linear behaviour specified (e.g. non-linear stress-strain curve, if the package supports this capability). It will then solve the equations for the basic linear stiffness matrix in a single pass for all load cases, including all members.


In any case even in linear analysis each load case
would require its own solution and when the user
generates combinations he could superimpose the laod
cases to get the effects for combinations.Right?>

I am trying to say that superposition is still valid
even in Tension only members??Then,why include it in
Non-linear analysis when superposition is valid?

For a linear analysis, you can use superposition to produce combinations from primary load cases, and you only need to solve the equations once, in a single pass.

However, for a non-linear analysis, superposition does NOT apply, and every load case and combination has to be solved independently, using an iterative approach. If you want to produce a load combination from two or more primary load cases, you can NOT use superposition, you MUST assemble the equations and solve them for each and every load combination independently.

For example, consider a frame with some tension-only bracing. These members might go into compression under dead load, so would be removed from the stiffness matrix for the dead load case. Some might go into tension under lateral wind load or seismic load (depending on the direction of application of the load), while others remain in compression, so each such load case needs to be considered independently, as they each potentially have a different structure stiffness matrix. Finally, if we want to consider a combination of dead load plus wind load, we cannot use superposition to determine the loads in the members, because the load factor at which they switch from compression into tension (and thus get reactivated in the stiffness matrix) is a non-linear relationship.

Hope this helps!

 

[apsix]

I would hope that analysis software packages are sophisticated enough to realise that a reversal of load direction could reverse the force acting on a tension-only member and treat all load casas separately, mine certainly does.

On the subject of cables; they are not modelled well using tension-only members. T-O members have flexural, torsional and shear capacity while cables don't. My software warns against using T-O for cables and has a separate cable member type to use.

 

[IFRs]

For my tention only cables I include an appropriate area and a very small, almost zero flexural, torsional and shear property values. The forces and moments in the results data reflect these choices.