Preloading a spring element

[GMarsh]

Hi,

I am trying to use a spring element to idealise a bolt in a dynamic (eigenvalue & harmonic) analysis. I read all the associated literature on calculating equivalent spring stiffness to represent a bolt. Now I wonder how can I give preloading to a spring element?

Commercial FEA software have well developed pre-tension elements or some recommend good old method of applying temperature to create preload. But I want to use spring elements due to their simplicity in usage.

One possibility to apply preload in spring seems to be moving, in initial load step, one of the bolted structures by some displacement equivalent to (preload force / spring stiffness). Then perform all subsequent frequency extraction, etc. This would amount to tensioning (stretching) the bolt by preload amount. Is this correct ? Any other suggestions ?

Thank you.

Geoff

 

[GMarsh]

Clarification:

What I meant in my previous post is, in the initial load step, to push both the bolted plates together while connecting spring element onto the outer nodes of plates. This creates compression in bolted plates and tension in spring element. I would like to know if this is correct.

Thanks, Geoff

 

[Drej]

Not sure which code you're using, but I've quickly looked at the COMBIN14 spring in the ANSYS manual, and the user can apply a preload to this element in a couple of ways.

"A preload in the spring may be specified in one of two ways, either through an initial (force-free) length (ILENGTH) or an initial force (IFORCE) input. Only 2-D or 3-D springs support this input (KEYOPT(2) = 0). Only one of the input options may be used to define the preload. If the initial length is different than the input length defined by the nodal coordinates, a preload is presumed to exist. If an initial force is given, a negative value indicates the spring is initially in compression and a positive value indicates tension. "




------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[GMarsh]

Hi Drej,

Many thanks for your mail.

I am using Abaqus in which there are only three types of Spring elements - Spring1, Spring2 and SpringA. Basically they differ in the connection direction and nodes. For e.g. Spring1 connects a node and ground, Spring2 connects two nodes. And finally SpringA acts along a line of action instead of a fixed direction like Z-axis, etc.

I wonder if it is available in Ansys, it must be there in some form in Abaqus as this is a very simple element.

If you know something on this, please update. I will also check on this.

Thank you for your help.

Regards
Geoff

 

[GMarsh]

Drej,

One issue with ANSYS COMBIN14 element is ambiguity in their definition of damping coefficient.

Here is what it says in Element library:

The damping portion of the element contributes only damping coefficients to the structural damping matrix. The damping force (F) or torque (T) is computed as:
Fx = - cvdux/dt or Tθ = - cvd θ/dt 

They say damping coefficient adds to structural damping matrix (which means damping force should be proportional to displacement) and then gives the formula showing proportionality to velocity (which shows it like a viscous damping coefficient). I am not sure what it does actually. Any idea what this means?

Generally structural damping is good to simulate bolts.

Thank you

Geoff

 

[GregLocock]

I suggest you check this on a simple model, but preload should make no difference to the frequencies you obtain in a linear analysis.

That's because preload is a non linear phenomenon

Cheers

Greg Locock


New here? Try reading these, they might help FAQ731-376

http://eng-tips.com/market.cfm?

 

[Drej]

Just a note that preload may make some difference, since you can carry out a pre-stressed modal analysis which locks in the stiffening from a previous analysis. In ANSYS, use the PSTRES command and ANTYPE,STATIC prior to a modal analysis to achieve this.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[GMarsh]

Hi Drej, Greg,

Thank you for your response. I searched all possible literature on ANSYS and found that the COMBIN14/7/37/40 elements take only viscous damping coefficient. For a detailed review of various damping types and their specification in ANSYS, I found the attached document very useful. Hope anyone visiting this thread may find it useful.

As mentioned in the attached file, there is one alternative by specifying betaj parameter for different materials (but not for elements defined without geometry, such as a spring element).

Summary - in ABAQUS for a spring element we can give either viscous or structural damping, but cannot give preload; in ANSYS we can give preload to spring but can only specify viscous damping not structural damping.

Regards
Geoff