No compression 1d elements in abaqus explicit

[MOZER8]

Hello All,

I want to use no compression 1d elements in abaqus explicit (elements like nastran gap elements). I used hyperelastic material with negative strain and force but it gave unrealistic results.

Basically, I want to model model a mass spring system. The spring has nonlinear stiffness value and it shouldn't carry any load under compression.

I have built a model and experienced negative reaction force in 1D elements. Are there any solution for this? You can check attached model for better understanding.

 

[FEA way]

For linear elastic material you could use truss element and select „No compression” option in the material definition. In your case you can use connector with uniaxial behavior and define tensile behavior only. Force in the compression direction will be zero then. It works only in Abaqus/Explicit but it’s not a problem for you. Maybe connector stop option will work too. Tensile spring (SPRING2 type) with nonlinear behavior is another way.

 

[Erik Panos Kostson]

CGap elements in Nastran are the old and amongst the first type of contacts (point-point) - the equivalent in Abaqus are *GAP See if this is of interest.
As mentioned though this is an old point contact used from my experience many times in facades or civil engineering.

You want a nonlinear spring or a compression only truss (that might work or not in a nonlinear dynamic analysis since it does not have any stiffness in compression, but it could work).
Have in mind that a chain of truss elements are like a chain so they go unstable under compression (think you had made the net model).


36.2.1 Gap contact elements

Product: Abaqus/Standard

References
“Gap element library,” Section 36.2.2

*GAP

 

[FEA way]

What is the actual goal of this analysis ? When I check the attached input file and run it in Abaqus I see wire meshed with truss elements and connected to reference point with dashpot. There’s a prescribed velocity in the X direction and 0 velocities in Y and Z direction. So the whole system is freely flying in the X direction. Shouldn’t this reference node be fixed ?

 

[MOZER8]

FEA way,
The purpose of the analysis is to simulate to pull a 20kg sack with a van. Mass is connected to rope, rope is connected hyperelastic spring, spring is connected to loadcell, loadcell is connected van. Rope is long enough to let the van to reach 25m/s before it pulls the rope. (It is only a simple model, doesn't have static or dynamic friction in the system. I placed a dashpot to see the effect and correlate with the test results)

As for the suggestions from first post,
No compression is out of option not only because of hyperelastic material properties but also because no compression elastic material option can not be used in abaqus explicit.
I defined connector with uniaxial tensile behavior, however I still get negative reaction force.

For the last option, is it possible to define SPRING2 from cae? I looked under springs/dashpots menu but couldn't find spring with nonlinear behavior.


Eric,
Actually, I'm trying to built a model with tension only elements in order to simulate above scenario. The spring that I'm using here is same with the spring that have been used in net analysis.

 

[FEA way]

Unfortunately SPRING2 can’t be used in Explicit too (I forgot about it). Only SPRINGA can be defined in such analysis. Nonlinear behavior must be added through keywords, it’s not supported by CAE.

So it seems that connectors are the best option here. If uniaxial behavior doesn’t work as expected, try connector stop.