Force vs. Displacement data for a Flat Spring

[jongyonkim]

Hi,

I'm running a simulation of unrolling a flat spring made of silicon to obtain the system's reaction force (spring force) vs. displacement graph.

See the picture at :

http://i102.photobucket.com/albums/m97/jongyonkim/flatspring.jpg

http://i102.photobucket.com/albums/m97/jongyonkim/flatspring3D.jpg

I am currently using ABAQUS/Explicit to run the stretching analysis. Basically, I apply a constant force on either end of the spiral and stretch it until it completely unwinds.

Before I can dive into postprocessing, I need to know how to calculate the (spring reaction) force vs. (spiral end) displacement of this particular structure.

Does anyone know how to do the calculation of my flat spring? Any recommendation on online sources / books regarding a similar spring structure?

Also, ABAQUS/Explicit can spit out a number of data including nodal displacement, External Work, Kinetic Energy, Internal Energy, etc.

I tried differentiating Internal Energy (of the entire structure) with respect to displacement to get force, but that seems wrong somehow...

Thank you.

 

[xerf]

ABAQUS can output the reaction forces, too.
You can obtain 2 sets of pairs of values (i.e. two XY Data):
-end displacement vs. time
-reaction force vs. time
You can match the two XY Data (for example by copy-pasting the data into Excel) to obtain
reaction force vs. end displacement
and then try to best fit a curve.

 

[jongyonkim]

Hi xerf,

Every time I try to plot "RF" reaction force from history output, I get a flat zero line (meaning no useful data).

Since I'd like to measure the spirng reaction force, I request history output (RF) on the surface that I also apply the force to pull the spiral.

Is there something wrong with the surface that I requested RF output on? Where/how should I request history output of RF so that it actually produces nonzero data?

I tried partitioning a surface within the structure parallel and next to the pulling surface, but it still gave me a flat zero line...

Thanks.

 

[brep]

How have you requested the output?

RF is a nodal quantity so you'll have to provide a Set as the "domain" in the history output request dialog. Then you can choose RF (or whatever) as the output data to be created. Plot as for any history data in Viewer.

Alternatively you can create XY data in the Visualization module (Viewer) based on Field Output. You do this by: Tools - XY Data - Create - ODB Field Data. Select unique nodal data and then whatever variable (RF) you need, then in the next tab you choose a node or nodes (pick from viewport, choose a node set, or type in the node label). Plot.

 

[jongyonkim]

Hi brep,

Yes, I've tried the above, but it still gives me flat zero lines.

I noticed that if I fix a boundary condition (ENCASTRE) to one end of the spiral and pull the other one, the reaction force (of the encastred region) magically spits out nonzero data.

So I am wondering why Reaction Force is only "present" when the structure is bounded to some external body.

What I really need is the reaction forces happening within the elements/nodes in the spiral arms while the arms are unrolling. (Hence successfully obtaining spring force vs. distance data of the whole flat spring structure)

How would I go about doing this? It's basically isolating the internal nodes and looking at their "free body diagram" to extract reaction forces.

Thanks.

 

[xerf]

The reaction forces are provided only at the fixed nodes.

In Abaqus Standard you can output the nodal forces NFORC due to stresses. (
I think this is not available with Explicit.)

If you have the stress distribution within a cross section you can integrate it to obtain the nodal forces.

 

[jongyonkim]

Thank you for all the feedback, but I would like to make clear something.

I spent a lot of time trying to figure out this seemiingly simple problem of finding the spring force of my structure, however, I am still in need of help.

In order to clarify what I need, I've made a simple model of a cantilever shown in the following online photo (link)

http://i102.photobucket.com/albums/m97/jongyonkim/reactionforce.jpg

I would like to obtain data for the red-colored vector Reaction Force.

I've tried the following:
1) use Boundary Condition (fix the velocity/displacement) to pull and extract "RF1"
-Apparently, one can extract "Reaction Forces" only if the surfaces are bounded under a BC. My original structure, when subject to such BC, experiences too much inertia (the heavy centerpiece mass rotates faster than the spirals unroll, forcing the centerpiece to push the spirals out : undesirable) for it to give accurate results.

2) use Force to pull and extract Stress, which then you can integrate to find the force.
-There are so many kinds of stress (Mises, Equivalent Pressure Stress, Stress Components, etc) that I don't know which of them is appropriate for my calculation.
-If I get stress from the surface which I pull with some fixed amt of force, how do I go about finding the "reaction force"? This should be pointing the other direction, because the more the spirals unroll, the greater the spring/reaction force becomes...

*I got "Section Integrated Output" to find out the total amount of force on a surface, but unfortunately it only gives you the values of the load, not the reaction force pointing the other direction. For example, If I have 100N in the four corners of the surface, Section Integrated Output Total Force gives me 400N, which is an obvious result, but this is not what I need.
So this isn't very useful to me...

 

[Tamlin]

Hi jongyonkim,

maybe it's helpful if you assume your problem as static.

Use Abaqus/Standard and apply several different loads to the spiral ends and measure the specific displacement (use nlgeom).
So you get an diagramm force versus displacement.
Hope I haven't misunderstood your problem.

Greetings Tamlin

 

[koetue]

Hallo Jongkim,
you can use the output variable nodal force NF.
cheers
Koe

 

[jongyonkim]

It looks like rather than /Explicit, /Standard is recommended.

However, I have no experience with using /Standard, because the biggest reason why I considered /Explicit was its automatic stability.

I tried using /Standard (Dynamic, Implicit), but to my horror, the structure failed to converge due to many "negative eigenvalue" problems.

Judging from the geometry and nonlinear stretching behavior of the structure, I don't think I can succeed with /Standard.

1) Any more suggestions with /Explicit? If I use Force to pull the ends, I can't get the "reaction force" output/vectors... If I use BC (fix velocity/displacement), the centerpiece inertia messes up the unwinding...

Also, the "reaction force" vectors seem to point the opposite way...when looking at RF, does it mean "reaction force ON the structure by the external entity" or "reaction force caused BY the structure on the external entity?" It seems like ABAQUS is showing the former, but the latter is what I need since I'm measuring the spring reaction force. If it's the former, can I simply flip the sign (change the direction of the vector) and consider it as the spring reaction force?

2) If you have experience dealing with this kind of coil structure using /Standard, how do you stabilize the simulation (i.e. not get "negative eigenvalue" error messages)?

Thank you for showing interest in my inquiry.
I appreciate your help.

 

[Tamlin]

Hello jongyonkim,

when I mentioned Abaqus/Standard I assumed that you use a STATIC general step, not a dynamic implicit.

My suggestion is :
fix the spring in the center, apply your loads at the end of the spiral ends and measure the displacement.

Greetings Tamlin