T3D3 Flapping midside node

Analysis issues
1

Based on this example problem , NAFEMS Challenge Problem 5 - The Solution - Dynamic Characteristics of a Truss Structure.

¿Why is the midside node of a T3D3 truss element flapping in my modal analisys? Shouldn’t it be internally constrined to remain colinear.?

Expected:

1st Mode 451Hz

2nd Mode 1050 Hz,

Result:

Mode Frequency
1 11.56978239 ?¿?
2 11.57092652 ?¿?
3 23.13304211 ?¿?
4 23.14029491 ?¿?

*NODE
1,0,1,0
2,1,1,0
3,0,0,0
4,1,1,0
5,0.5,0.5,0
6,0.5,1,0
*ELEMENT,TYPE=T3D3
1,3,5,4
2,1,6,2
*NSET,NSET=HOR
2
*NSET,NSET=TILT
4
*ELSET,ELSET=COMPONENT
1
2
*MATERIAL,NAME=MATERIAL
*ELASTIC,TYPE=ISOTROPIC
210000000000,0.3
*DENSITY
7800
*SOLID SECTION,ELSET=COMPONENT,MATERIAL=MATERIAL
7.853981633974E-05
*BOUNDARY
1,1,,0
1,2,,0
1,3,,0
2,3,,0
3,1,,0
3,2,,0
3,3,,0
4,3,,0
*EQUATION
2
2,1,1,4,1,-1
*EQUATION
2
2,2,1,4,2,-1
*STEP
*FREQUENCY
4
*NODE FILE,GLOBAL=YES
U
*END STEP

imagen
imagen900×716 13.3 KB

2

Same file Imposing colinear midside node.

Expected:

1st Mode 451Hz

2nd Mode 1050 Hz,

Result:

Mode Frequency
1 450 Hz
2 1030 Hz

*NODE
1,0,1,0
2,1,1,0
3,0,0,0
4,0.6666666666667,0.6666666666667,0
5,0.3333333333333,1,0
6,0.6666666666667,1,0
7,0.3333333333333,0.3333333333333,0
8,1,1,0
** Midside nodes
9,0.5,1,0
10,0.5,0.5,0
*ELEMENT,TYPE=T3D3
1,1,9,2
2,3,10,8
*NSET,NSET=HOR
9
*NSET,NSET=TILT
10
*ELSET,ELSET=COMPONENT
1,2
*MATERIAL,NAME=MATERIAL
*ELASTIC,TYPE=ISOTROPIC
210000000000,0.3
*DENSITY
7800
*SOLID SECTION,ELSET=COMPONENT,MATERIAL=MATERIAL
7.853981633974E-05
*BOUNDARY
1,1,,0
1,2,,0
1,3,,0
2,3,,0
3,1,,0
3,2,,0
3,3,,0
4,3,,0
5,3,,0
6,3,,0
7,3,,0
8,3,,0
9,3,,0
10,3,,0
** Horizontal member: local 1 = X, local 2 = Y
*TRANSFORM,NSET=HOR,TYPE=R
1,0,0,0,1,0
** Diagonal member: local 1 along (1,1,0), local 2 transverse
*TRANSFORM,NSET=TILT,TYPE=R
1,1,0,0,1,0
** Horizontal midside node: constrain transverse displacement
*EQUATION
3
9,2,1.,1,2,-0.5,2,2,-0.5
** Diagonal midside node: constrain transverse displacement
*EQUATION
5
10,2,1.,3,1,0.3535533905933,3,2,-0.3535533905933
8,1,0.3535533905933,8,2,-0.3535533905933
** Duplicated end node: node 8 tied to node 2
*EQUATION
2
8,1,1.,2,1,-1.
*EQUATION
2
8,2,1.,2,2,-1.
*STEP,PERTURBATION
*FREQUENCY
2
*NODE FILE,GLOBAL=YES
U
*END STEP

imagen
imagen1184×855 29.6 KB

3

In according to the manual it should stay collinear since T3D3 can’t sustain bending load.

Maybe a foolish question, but just by curiosity, what is the primary purpose by having a mid node located on a truss element with a constant cross section not capable of carry bending ?

1 Like
4

Good question! Abaqus also has 3-node truss elements and describes them this way:

The 3-node truss element available in Abaqus/Standard is often useful for modeling curved reinforcing cables in structures, such as prestressed tendons in reinforced concrete or long slender pipelines used in the off-shore industry.

So you could try modeling cable sag with it, but it may not work 100% correctly in CalculiX: Simulation of cables with tension-only materials

2 Likes
5

Hi fgr,

Thanks for looking at this.

In the context of this particular benchmark, the 3 node Truss is needed to properly extract the axial modes. The two node truss delivers the wrong values. If a truss framework is intended to be computed using dynamics based on modal superposition you need to extract the right modes.

Mode Frequency
1 12.67347097
2 12.67527377
3 25.33732515
4 25.34875591

1 Like
6

so it’s capable of taking more complex deformations along its axis without resorting to increasing the number of elements. You can take bending with a 2 node beam element, right?

2 Likes
7

NAfems document states the solution can be improved increasing the number of intermediate nodes. That requires imposing collinearity to avoid hinges inbetween trusses. I have done it, but I can’t see improvement. in fact, second mode looks less accurate.

imagen
imagen960×658 23.2 KB

8

convergence depends on the problem, I do not know how many linear trusses are need to obtain the same solution as with parabolic elements, but if everything is right at some mesh density it will converge.

Do not forget mass distribution is different.

2 Likes
9

the manual description of the element:

6.2.36 Three-node 3D truss element (T3D3) This element is similar to the B32 beam element except that it cannot sustain bending. This is obtained by inserting hinges in each end node of the element.

so I guess making it behave as a real truss is a job on the analyst side…if the truss cross section is too thin then the truss will behave as a beam.

1 Like
10

But then don’t call it Truss. If the software doesn’t constrain midside node of T3D3 to be colinear it is not a truss. It is a beam with ends release (and rotational constrain I guess).

11

Yes, that’s pretty much what CalculiX offers as truss elements. And you are right that they aren’t really trusses, just hinged beams.

1 Like
12

well, it is closer to a real truss, right? if you want to simulate idealized trusses just have to consider a beam with very big bending stiffness, maybe that’s what is wrong in the element, the bending stiffness of the cross section does not take into account the element length so the value can be inapropriate.

1 Like
13

Appart from the fact that T3D3 should not transfer bending moment to their neightbours which actually works, I think it should not bend itself ¿right?.

The main issue I see right now is that 2nd order “Truss” can bend itself , those modes will populate the modal analisys as they are tipically smaller than axial modes.

imagen
imagen910×367 21.2 KB

Chat GPT about T3D3 self bending:

“In Finite Element Analysis (FEA) software like Abaqus, T3D3 stands for a Truss, 3D, 3-node quadratic displacement element. Despite having three nodes (which might intuitively suggest it can capture a curved or bent shape), its internal mathematical formulation fundamentally prevents it from experiencing or displaying bending.”

No way to solve this . 100,200, 300 modes requested. There is always a lower bending mode

imagen
imagen875×780 45.6 KB

14

Maybe *EQUATION could eliminate this behavior. CalculiX also has MPC STRAIGHT, but:

Since the 3-D expansion of standard beam, shell, plane stress, plane strain and axisymmetric elements frequently involves the use of extra linear equations and/or nonlinear MPC’s such as knots, the additional application of nonlinear MPC’s to such elements is problematic. Therefore, it is not allowed to apply STRAIGHT, PLANE, BEAM and MEANROT MPC’s to any node belonging to such elements.

1 Like
15

Tested. MPC STRAIGHT can’t be used with 1D/2D elements.

Equation works as shown in my workarround but I guess that should be hard coded internally for T3D3.

16

Yeah, apart from cable sag modeling maybe. But it may require beam elements in CalculiX anyway. Perhaps a GitHub request would be in place here ?

1 Like
17

After colinear midside nodes. Everybody happy and dancing.

After colinear midside nodes.mpeg [video-to-gif output image]

2 Likes