Engineering analysis + design software

User Area > Advice

Using joints: Spring stiffnesses

Using Joints: Mesh  |  Geometric attributes  |  Material attributes  |  Spring stiffnesses  |  Supports  |  Loadcase properties

A spring stiffness is required in the definition of joint or spring support attributes in LUSAS.

Spring stiffness, k, is as defined in Hooke's law, viz. F=k*x where F is an applied force and x is the resulting displacement. It follows that where a known displacement (x) for a known force (F) is available, the spring stiffness entered in the dialog box, k = F/x.  Similarly, the spring stiffness for any rotational stiffnesses required should be based on a Hookean model, viz. M = k, and rotational spring stiffness will be specified in moment/ radians.  

In many cases the joint represents a specific medium in the structure and the stiffnesses should be calculated accordingly.  Derivations of spring stiffnesses appropriate to a "modulus of subgrade reaction" or other specialised theorem, are not considered in this article.

In other cases, the joint represents a part of the structure.  In such a case, engineering theory can be used to derive equations for k based on the structural member which the spring is intended to model (appropriate to each degree of freedom in the joint material attribute).  The notes below are intended as an example considering a specific (but common) case. 

Sometimes it is necessary to use a joint element to model a "fixed" or "free" condition (e.g. to mimic the action of a tension-only member or contact).   However, for a "fixed" condition, you cannot enter a stiffness of infinity, so you should use a high stiffness.  For a "free" condition, you may not be able to enter a stiffness of zero, so you may use a low stiffness. Zero may be entered but may cause numerical instability, depending on the solution method selected.  

In the case of modelling contact for example (lift-off support/connection), the joints do not model a structural element and so there is no associated length, they just model the contact interface the stiffness is input directly and the joints should ideally be meshed with coincident end nodes.  If the joint is modelling something arbitrarily stiff or flexible (in the case of modelling contact or a hinge connection for example) then the key is to make the joint stiffness much stiffer or much more flexible relatively speaking to the elements it connects to.  

The notes below give further guidance to model a "fixed" or "free" condition using simple and approximate calculations for the stiffness of an adjacent element as a basis for deciding what order of magnitude of stiffness in the joint would be considered very stiff or very flexible in comparison.  The use of precise numbers to carry out a precise calculation is therefore not necessary; the approximate values determined are then factored arbitrarily up or down by something like 1E3 or 1E6 to get something relatively very stiff or very flexible respectively. The reason for this approach is to avoid extreme high/low stiffnesses as these may cause ill-conditioning and convergence problems in a nonlinear solution.

Note that in the case of modelling a bearing, connector or connection arrangement, the question is not what the length of the joint is, but what is the geometry and material of the connection component/arrangement it is to represent.  If a joint is simply representing a connector of constant section and a given length, then the axial stiffness can be calculated as F/x = EA/L, where L is the length of the member rather than the joint element.  If the joint represents something more complex, then the calculations below would not suffice a component like a bearing may have stiffnesses published by the manufacturer for example.

Spring stiffnesses for joints between point features or at line ends

If the spring stiffnesses were intended to model a thin beam (assuming beam theory):

Axial: Ka = EA/L, (typical units kN/m, N/mm etc)

Lateral: (one end fixed and the loaded end guided): Kh = 12EI/L   (typical units kN/m, N/mm etc)

Rotational: Km = EI/L    (typical units kNm/rad, Nm/rad etc)

Torsional: Kt = GJ/L   (typical units kNm/rad, Nm/rad etc)

In a case where the stiffness specified is to model a "fixed" or "free" condition, in principle, the stiffnesses should be high or low relative to the rest of the structure, in particular adjacent members. A good starting point for the estimation of a suitable spring stiffness might therefore be:

  • For a "fixed" condition, first use approximate calculations for Ka, Kh, Km and Kt (using the above equations for example) to determine the stiffnesses of the most stiff adjacent member, then factor each stiffness by a large number such as 1E3 or 1E6 to be input for the joint to ensure that it is much stiffer.
  • For a "free" condition,  first use approximate calculations for Ka, Kh, Km and Kt (using the above equations for example) to determine the stiffnesses of the least stiff adjacent member, then factor each stiffness by a small number such as 1E-3 or 1E-6 to be input for the joint to ensure that it is much less stiff.
 

 

Mesh attributes for joints between line features (or edges of surfaces)

When assigned to line features, which have a calculable length, forces in the equation F=k*x are per unit length and spring stiffnesses should be likewise (typical units therefore kN/m, N/mm etc).  If the spring stiffnesses were intended to model a cantilevering "slab":

  • In plane of slab: Kx = EA/L. A is per unit length of cantilever tip, viz. A=thickness t
  • Lateral (along edge of slab): Ky = Gt/L based on shear deformation. For isotropic elastic materials, Shear modulus G=E/[2(1+v)]
  • Lateral (normal to slab): Kz = 12EIyy/L. Iyy is per unit length of cantilever tip viz. Iyy=t/12
  • Torsion about local x: KTHx = CG/L where C=t/6 generally
  • Rotation about local y: KTHy = EIyy/L I is per unit length
  • Rotation about local z: KTHz = EIzz/L I is per unit length

In a case where the stiffness specified is to model a "fixed" or "free" condition, in principle, the stiffnesses should be high or low relative to the rest of the structure, in particular adjacent members. A good starting point for the estimation of a suitable spring stiffness might therefore be:

  • For a "fixed" condition, first use approximate calculations for Kx, Ky, Kz, KTHx, KTHy and KTHz (using the above equations for example) to determine the stiffnesses of the most stiff adjacent member, then factor each stiffness by a large number such as 1E3 or 1E6 to be input for the joint to ensure that it is much stiffer.
  • For a "free" condition,  first use approximate calculations for Kx, Ky, Kz, KTHx, KTHy and KTHz (using the above equations for example) to determine the stiffnesses of the least stiff adjacent member, then factor each stiffness by a small number such as 1E-3 or 1E-6 to be input for the joint to ensure that it is much less stiff.
 

 

 

Mesh attributes for joints between surface feature faces

When assigned to surface features, which have a calculable face area, forces in the equation F=k*x are per unit area and spring stiffnesses should be likewise (typical units therefore kN/m, N/mm etc).  If the spring stiffnesses were intended to model a cantilevering "slab":

  • Perpendicular to joint: Ka = EA/L based on in-plane ("axial") deformation. Since Ka will be per unit area, assigned to a surface feature, 'A' may be taken as unity in many cases. 
  • Parallel to joint: Kh = 3EI/L based on flexural deformation of slab (minor bending axis). Since Kh will be per unit area, assigned to a surface feature, 'A' should be divided through. An effective area may need to be assumed.
  • Lateral to joint: KL = Gt/L based on shear deformation. For isotropic elastic materials, Shear modulus G=E/[2(1+v)]. Since KL will be per unit area, assigned to a surface feature, 't' may be taken as unity in many cases.

In a case where the stiffness specified is to model a "fixed" or "free" condition, in principle, the stiffnesses should be high or low relative to the rest of the structure, in particular adjacent members. A good starting point for the estimation of a suitable spring stiffness might therefore be: 

  • For a "fixed" condition, first use approximate calculations for Ka, Kh, and KL (using the above equations for example) to determine the stiffnesses of the most stiff adjacent member, then factor each stiffness by a large number such as 1E3 or 1E6 to be input for the joint to ensure that it is much stiffer.
  • For a "free" condition,  first use approximate calculations for Ka, Kh, and KL (using the above equations for example) to determine the stiffnesses of the least stiff adjacent member, then factor each stiffness by a small number such as 1E-3 or 1E-6 to be input for the joint to ensure that it is much less stiff.
 

 

 

How do I check joint stiffnesses entered are suitable?

The joint strain (relative displacement between its nodes) can be checked (using a Contours or Values post-processing layer).  

View > Drawing Layers > Contours > choose "Entity" as "Strain - " following by the joint type used, and then select the appropriate "Component" as Ex, Ey or Ez depending on which direction is the lift-off/contact contact direction

For strain in a direction that was intended to be "fixed" the amount of strain should be checked as being negligible for each direction (for contact or for a rigid connection or bond for example). Where modelling contact, the strain in the normal direction between contacting surfaces would represent a penetration between those surfaces and so the stiffness can be adjusted if required to reduce this. In the case of a gap, you can check that the joint strain does not exceed the gap (meaning that the gap has closed but with negligible penetration) and increase the contact stiffness if it does. 

The image below shows a check for the contact stiffness where there is too much penetration and the contact stiffness needs to be increased:

The joint force/moment in a direction that was intended to be "free", can be similarly checked as being negligible in the case of lift-off or for a hinge rotation for example (or other freedom intended to have low/zero stiffness) and again the stiffness adjusted if required to reduce that spurious force/moment for the relevant freedom. 

View > Drawing Layers > Contours > choose "Entity" as "Force/Moment - " following by the joint type used, and then select the appropriate "Component" as Fx, Fy or Fz depending on which direction is the lift-off/contact contact direction

The image below shows a check for the lift-off stiffness where there is too much tensile force in the joint and the lift-off stiffness needs to be reduced:

The image below shows both contact and lift-off stiffnesses corrected to give little tensile force in the lift-off direction and little penetration in contact:


How do I model lift off supports? (main page)

How do I model tension only members? (main page)

How do I model a hinged connection between shell meshed surfaces? (main page)


innovative | flexible | trusted

LUSAS is a trademark and trading name of Finite Element Analysis Ltd. Copyright 1982 - 2022. Last modified: November 29, 2022 . Privacy policy. 
Any modelling, design and analysis capabilities described are dependent upon the LUSAS software product, version and option in use.