Hi
As part of a validation of a bigger model, I'm trying to calculate the work done in deforming two Truss Elements (T3D2). One end of these elements is ENCASTRED, while the other end is linked to a Reference Point through a Linear Equation constraint. Both elements are Wires, one with cross section 1 and the other with 5 units. The same material properties (density=1E-12; Young's modulus=1) are applied to both. The equation coefficients are in the input file. I've called them 'SPRINGS' everywhere.
Now, I've run two different cases.
Case 1: The two elements are modeled in the same part.
Result 1: Reaction forces RF2 are equal (0.3343 units)
External work ALLWK = 0.335 units
Displacements U2 in the elements are 1.67172 and 0.3343 units.
Case 2: The two elements are modeled as different parts and brought into an assembly.
Result 2: Reaction forces RF2 are equal (0.22305 units)
External work ALLWK = 0.25467 units
Displacements U2 in the elements are 1.761 and 0.232 units.
I'm unable to understand where the difference is coming from, and would appreciate some light on that.
Also, when I equate the forces in the two elements and try to solve by hand, my answer matches the results from Case 1. But when I simulations separately on the two elements and add ALLWK from the two, I get the ALLWK from Case 2. Could someone help with that too, please?
Hi Anish Janakiraman,
One linear equation (constraint) UY(2)+UY(4)=2*UY(RP) has infinite number of possible solutions UY(2) and UY(4). Therefore, both your solutions are correct.
Well looking at the input files I don't see an obvious difference. What you can try to do is to get the model which is the assembly and change it to write a "flat" input file, so without separate parts, but everything in one. You should check that it gives you the same answer as the one with parts. If not, then there is something wrong, and probably you need to contact support.
If they give the same results, you can compare the two "flat" input files and spot the difference, there should be something.
Hope this helps you get started with solving the problem.
In one file you run it with nlgeom = on and the other is off. From my experience Abaqus/explicit behaves very sensitive to it.
Yes, Christian Willberg is right. The difference in results is caused by NLGEOM. For NLGEOM=YES Hooke's law instead of σ=E*e becames σ=E*ln(1+e), where e is deformation of truss. Moreover, Abaqus manual says that "when truss elements are used in large-displacement analysis, the updated cross-sectional area is calculated by assuming that the truss is made of an incompressible material, regardless of the actual material definition." Therefore, S=S0/(1+e), where S0 and S are initial and updated cross-sectional areas respectively.
Lagrangian multipliers method ensures the uniqueness of solution.
- Badges
- Science topic