Strange Truss elements aligned with the X direction

Hi ,

I have set up a simple rectangular plate of 10 x 10 x 0.1 inches and with a circular hole in the center Diameter 3 inch.

Additionally, I have connected the perimeter with a set of Truss elements *ELEMENT,TYPE=T3D2 which share a common node (Vertex) .

The Vertex is at the center of the hole but slightly elevated in the Z direction 1 inch.

The rectangular plate is clamped on two sides and I’m pulling in the perpendicular direction to the plate with a force F=100lb applied to the Vertex.

The result shows that the truss elements aligned with the X direction do not release their Rotational DOFs as all the other ones have.

See Pictures.

Inp file attched

hi,

i’m not really sure why the problem exist. but, firstly you need to plot the axial force of all truss element to understand is this has been distributed properly or not.

i see quickly from Mises stress, the distribution is not smoothed as expected. concerning at mid side nodes of shell element, may this is another causes of problems.

you can try to remove the truss element were connected to midside node of shell element and see the results.

Hi Xyont and thanks for giving attention.

I have reviewed all the orientations, mesh , set Ux and Uy =0 for the vertex node to see if that helped. Stress distribution is clearly not homogeneous because the truss doesn’t allow the lip to rotate.
There is something else which may help to identify the problem. The model is not invariant under rotation . It Is not the truss , the problem is with the elements aligned with the X axis.
I can see you have reproduced the model . ¿Could you give it a try and rotate it 90º around Z.?

Regards and Thanks again.

You can fix all four sides to make it clear. I did it and the issue is at X axis.
Both images represent the same model but rotated 90º around Z.

i’m interested in axial force distribution of truss element before viewing at stress of shell element.

I’ve seen this too. The displacement is wrong and the truss is transferring moment to the shell where it should have a hinge.

Edit: Looks like it’s not really transferring moment but simply fixing the rotation of the shell to 0.

restraining rotation of shell edge around the holes only make unreasonable results since naturally truss element did not allow to transmitted.

it seems the problem is not related to the axes, knot exist at there due to expansion of element and connection nodes.

reduce truss dimensions with higher stiffness eliminate the problems, however i’m not yet to check further in axial force distribution of truss element.

@xyont @Victor Thank for your response

@xyont That’s the point. Nobady has restrain the rotation of the LIP. There is a bug on Trusses aligned with the X axis that makes them not to behave as truss.

We would need a circular plate with a perfect radial mesh to do that ¿isn’t it?

Same problem. This is not a force distribution problem. The Rotation degree of freedom of the truss is not released.

again, try reduced truss dimension or area with higher modulus of elasticity to be equivalent in stiffness as previous models.

Reducing truss cross-sectional area by 10000 doesn’t help. Rotation of the shell is still fixed to 0 when the truss is within a few degrees of the X axis. Also with E increased by a few orders of magnitude.

maybe, but the spurious deformation at the areas previously shown is eliminated.

if this only related to axes and dimension of the truss does not affected, the spurious should always the same and still exist.

I don’t understand your example, but I think it’s actually a problem of the shells, not the trusses. Here’s an example that shows the problem. It depends on one of the shell nodes (7) having a strange x-coordinate.

``````*NODE
1,1.5,0,-1
2,2.55,0,-1
3,1.85,0,-1
4,0,-0.3,0
5,2.2,-0.3,-1
6,2.55,-0.3,-1
7,1.495,-0.3,-1
8,0,0,0
9,2.2,0,-1
10,1.85,-0.3,-1
*ELEMENT,TYPE=T3D2,ELSET=Dandelion_Truss
1,1,8
4,7,4
*ELEMENT,TYPE=S4,ELSET=Shell_Plate
2,9,3,10,5
3,3,1,7,10
5,2,9,5,6
*MATERIAL,NAME=Material
*ELASTIC,TYPE=ISOTROPIC
200000000000,0
*SHELL SECTION,ELSET=Shell_Plate,MATERIAL=Material
0.0001
*SOLID SECTION,ELSET=Dandelion_Truss,MATERIAL=Material
1E-08
*BOUNDARY
2,1,6,0
4,1,2,0
6,1,6,0
8,1,2,0
*STEP
*STATIC
*BOUNDARY
4,3,,2.54E-05
8,3,,2.54E-05
*NODE FILE
U
*END STEP
``````

i did not create an example, only modified Trus_Bug.inp posted by Disla in the beginning of discussion, small modification in truss apply as i described.

thanks for new example, could it be post similar model in Y as you mentions which known to be working.

That file’s gone. @Disla, could you please share it again?

Here’s the good version that’s the same but rotated 90 degrees.

``````*NODE
1,0,1.5,-1
2,0,2.55,-1
3,0,1.85,-1
4,0.3,0,0
5,0.3,2.2,-1
6,0.3,2.55,-1
7,0.3,1.495,-1
8,0,0,0
9,0,2.2,-1
10,0.3,1.85,-1
*ELEMENT,TYPE=T3D2,ELSET=Dandelion_Truss
1,1,8
4,7,4
*ELEMENT,TYPE=S4,ELSET=Shell_Plate
2,9,3,10,5
3,3,1,7,10
5,2,9,5,6
*MATERIAL,NAME=Material
*ELASTIC,TYPE=ISOTROPIC
200000000000,0
*SHELL SECTION,ELSET=Shell_Plate,MATERIAL=Material
0.0001
*SOLID SECTION,ELSET=Dandelion_Truss,MATERIAL=Material
1E-08
*BOUNDARY
2,1,6,0
6,1,6,0
8,1,2,0
4,1,2,0
*STEP
*STATIC
*BOUNDARY
4,3,,2.54E-05
8,3,,2.54E-05
*NODE FILE
U
*END STEP
``````

I have attached the original file and the version with circular plate.
Regards

right it seems your example model (aligned to X) has detected as unstable structure, try move node 4&8 in direction-Y coordinates by incrementally.

given expected when moving at least 0.081 (‘m’ units i guess), may this is due to some tolerances setting inside the solver? how about the model in ‘mm’ units, also in quadratic shell element.

Yea, it’s starting to look like this already known problem of shells borking with certain very specific geometries. Fixing this case isn’t useful since its more of a general bug.

I noticed that it gave a different but still wrong result with the Pastix solver, so maybe the stiffness matrix is becoming ill-conditioned.

switch the truss element to beam (B31R, truss like) not an issue, but i did not investigate further about clamping condition around holes of connected element.

1 Like