B32-beam elements

bruno.zilli · December 15, 2022, 7:19am

Hello.

I’m a ccx user and I’m using it almost daily for steel industry with satisfaction. I solved many problems with ccx, and I compliment with the team for this great work.
Now I’m experiencing an issue with B32 elements. I’m doing some tests, but I don’t find my mistake.
There is a simple beam column. I did sone tests but It doesn’t converge. I checked b.c and loads, section, but it doesn’t want to land to a useful result.
Please let me know.
Model in Newton-meters [N-m].
E=2.06e+11 N/m2

Thank you.
Kindest Regards

files:

main
*INCLUDE, INPUT=allinone.inp
*INCLUDE, INPUT=add_material.inp
*INCLUDE, INPUT=add_sections.inp
*INCLUDE, INPUT=add_support.inp
*INCLUDE, INPUT=add_contact.inp

*STEP,NLGEOM

*STATIC

*INCLUDE, INPUT=add_concload.inp
*INCLUDE, INPUT=add_boundary.inp
*NODE FILE
U,
*EL FILE,Output=3d
S,
*NODE PRINT,NSET=BC
RF
*END STEP

sections

*BEAM SECTION,MATERIAL=STEEL,ELSET=WCLM,OFFSET1=0.0000E+00,OFFSET2=0.0000E+00,SECTION=rect
0.8000E-01,6.0000E-03
1.0000E+00,0.0000E+00,0.0000E+00

allinone
*NODE, NSET=Nall
1,0.000000000000e+00,0.000000000000e+00,0.000000000000e+00
2,0.000000000000e+00,0.000000000000e+00,1.000000000000e+00
3,0.000000000000e+00,0.000000000000e+00,5.000000000000e-01
4,0.000000000000e+00,0.000000000000e+00,2.500000000000e-01
5,0.000000000000e+00,0.000000000000e+00,7.500000000000e-01
*ELEMENT, TYPE=B32, ELSET=Eall
1, 1, 4, 3
2, 3, 5, 2
** Names based on LX
*NSET,NSET=LX
2,
** Names based on BC
*NSET,NSET=BC
1,
** Names based on B32
*ELSET,ELSET=WCLM
1,
2,

material
*MATERIAL,NAME=STEEL
*ELASTIC
2.1000E+11,0.3

*DENSITY
0.0000E+00
*EXPANSION
0.0000E+00

Calc_em · December 15, 2022, 8:01am

Can you share the whole input file (paste it here in a preformatted text block or use some hosting website) ? The most important part (boundary conditions and loads) is missing.

Did you try running it without NLGEOM ?

bruno.zilli · December 15, 2022, 11:57am

Hello,
yes I used NLGEOM, please see the main in the message.
The cloads are one force

*CLOAD
LX,1,1.0000E-01

there are BC

*BOUNDARY
BC,1,1,0
BC,2,2,0
BC,3,3,0

JuanP74 · December 15, 2022, 9:17pm

your problem is a cantilever beam with a tip load alog X and pinned at the root so it’s a mechanism. Just fix the six degrees of freedom at the root and will work:
*BC,1,6,0

bruno.zilli · December 16, 2022, 7:10am

of course.
Sorry for my trivial question.

I did a little bit more, a composite section.

Thank you.

Bruno

bruno.zilli · December 17, 2022, 9:28am

dear colleagues,

I noticed a difference in the displacement values, something like 15%. It is possible due to the mesh I did. But I can’t understand another thing. The value of the moments seems to be unlikely as the true. Is Syy the section force Myy? It is from the manuals.
Force(x) = 1000 N. lenght 1 m. Moment (yy) = 1000 Nm. I did the same model with 2d options (SECTION FORCES), and the result doesn’t seem to be confortable (Syy = Myy)=262 Nmm. Did I do some mistakes? Thank you in advance. I write here the main, the section and the results (jpeg). Model in N-m.

*INCLUDE, INPUT=allinone.inp
*INCLUDE, INPUT=add_material.inp
*INCLUDE, INPUT=add_sections.inp
*INCLUDE, INPUT=add_support.inp
*INCLUDE, INPUT=add_contact.inp

*STEP,NLGEOM
*CONTROLS,PARAMETERS=TIME INCREMENTATION
1,2,3,40,2,2,2
0.5,0.5,0.75,0.85

*STATIC

*INCLUDE, INPUT=add_concload.inp
*INCLUDE, INPUT=add_boundary.inp
**NODE FILE
**U,
**EL FILE,Output=3d
**S,
**NODE PRINT,NSET=BC
**RF
**END STEP

*NODE FILE,OUTPUT=2D
U,RF

*EL FILE,SECTION FORCES
S

*NODE PRINT,NSET=Nall
RF

*END STEP

*BEAM SECTION,MATERIAL=STEEL,ELSET=WCLM,OFFSET1=0.0000E+00,OFFSET2=0.0000E+00,SECTION=rect
0.8000E-01,6.0000E-03
1.0000E+00,0.0000E+00,0.0000E+00

*BEAM SECTION,MATERIAL=STEEL,ELSET=PL1CLM,OFFSET1=0.0000E+00,OFFSET2=4.5,SECTION=rect
1.0000E-01,1.0000E-02
0.0000E+00,1.0000E+00,0.0000E+00

*BEAM SECTION,MATERIAL=STEEL,ELSET=PL2CLM,OFFSET1=0.0000E+00,OFFSET2=-4.5,SECTION=rect
1.0000E-01,1.0000E-02
0.0000E+00,1.0000E+00,0.0000E+00

bruno.zilli · December 19, 2022, 4:24pm

I found out the same situation in a similar file, composite section. The value of Syy (Myy)section force is not likely the real value expected. Thank you in advance for any answer or feedback.
** Structure: cantilever beam.
** Test objective: B32 elements, composite beam.
**
*NODE, NSET=Nall
1, -1.49012e-08, 0.00000e+00, 0.00000e+00
2, 1.00000e+00, 0.00000e+00, 0.00000e+00
3, 5.00000e-01, 0.00000e+00, 0.00000e+00
4, 2.00000e+00, 0.00000e+00, 0.00000e+00
5, 1.50000e+00, 0.00000e+00, 0.00000e+00
*ELEMENT, TYPE=B32, ELSET=Eall
1, 1, 3, 2
2, 2, 5, 4
3, 1, 3, 2
4, 2, 5, 4
*BOUNDARY
1,1,6
*MATERIAL,NAME=EL1
*ELASTIC
206000000000,.3
*MATERIAL,NAME=EL2
*ELASTIC
206000000000,.3
*ELSET,ELSET=SET1
1,2
*ELSET,ELSET=SET2
3,4
*BEAM SECTION,ELSET=SET1,MATERIAL=EL1,SECTION=RECT,OFFSET2=-.5
0.05, 0.05
0.d0,1.d0,0.d0
*BEAM SECTION,ELSET=SET2,MATERIAL=EL2,SECTION=RECT,OFFSET2=.5
0.05, 0.05
0.d0,1.d0,0.d0
*STEP,NLGEOM
*STATIC
*CLOAD
4,3,1000
**NODE PRINT,NSET=Nall
**U
**EL PRINT,ELSET=Eall
**S
**EL FILE
**U,S
**END STEP
*NODE FILE,OUTPUT=2D
U,RF

*EL FILE,SECTION FORCES
S

*NODE PRINT,NSET=Nall
RF

*END STEP

JuanP74 · December 20, 2022, 7:37am

The value in that output set is not what you expected, from the manual:

If OUTPUT=2D the fields in the expanded
elements are averaged to obtain the values in the nodes of the original 1d and
2d elements. In particular, averaging removes the bending stresses in beams
and shells.

the output from your test example:

forces (fx,fy,fz) for set NALL and time 0.1000000E+01

     1  4.760012E-05  8.901917E-12 -1.000000E+03
     2 -1.182220E-03 -7.126103E-11 -4.492205E-06
     3 -7.118512E-04 -1.964509E-10 -3.951682E-06
     4  4.025537E-03  4.375274E-10  1.000000E+03
     5 -2.179066E-03 -2.019078E-10 -6.011425E-06

bruno.zilli · December 20, 2022, 7:51am

Hello Juan
thank you for your feedback. My goal is to get out the bending moments and the section forces in B32 beam elements with composite sections. Is it possible to get it out with cgx visualtization?
Thank you in advance.
Bruno

JuanP74 · December 20, 2022, 8:47am

I usually don’t use beams in ccx as they’re not true structural elements. The manual reads:

6.2 Element Types 123
the stresses in the beam nodes are replaced by the section forces. They are
calculated in a local coordinate system consisting of the 1-direction n1, the 2-
direction n2 and 3-direction or tangential direction t (Figure 74). Accordingly,
the stress components now have the following meaning:
• xx: Shear force in 1-direction
• yy: Shear force in 2-direction
• zz: Normal force
• xy: Torque
• xz: Bending moment about the 2-direction
• yz: Bending moment about the 1-direction
The section forces are calculated by a numerical integration of the stresses
over the cross section. To this end the stress tensor is needed at the integration
points of the cross section. It is determined from the stress tensors at the nodes
belonging to the cross section by use of the shape functions. Therefore, if the
section forces look wrong, look at the stresses in the expanded beams (omitting
the SECTION FORCES and OUTPUT=2D parameter).

If you look at the stresses in the expanded model they look correct so maybe section forces still needs some improvements.

bruno.zilli · December 20, 2022, 9:26am

Juan, thank you.

Yes, bending moment in 2-direction is Sxz, but If I generate Sxz in cgx in my little test, it shows unlikely numbers.

It is as I thought. At the moment, ccX still needs some serious improvements for the beam elements.

I warmly suggest the developers to fix this serious gap.

Thank you again.

Bruno

xyont · February 23, 2023, 9:40am

can you share a complete single files input? interesting to know since the case mention is cantilever (fixed support)

commonly it’s related to element type, meshing or fiberized by user defined.

previously i found, only at simple supported has little problems due to over constraining at node of expanded element.

bruno.zilli · February 27, 2023, 5:20am

Hello.
concentrated loads
*CLOAD
LX,1,1.0000E-01

material
*MATERIAL,NAME=STEEL
*ELASTIC
2.1000E+11,0.3
*DENSITY
0.0000E+00
*EXPANSION
0.0000E+00

sections
*BEAM SECTION,MATERIAL=STEEL,ELSET=WCLM,OFFSET1=0.0000E+00,OFFSET2=0.0000E+00,SECTION=rect
0.8000E-01,6.0000E-03
1.0000E+00,0.0000E+00,0.0000E+00

*BEAM SECTION,MATERIAL=STEEL,ELSET=PL1CLM,OFFSET1=0.0000E+00,OFFSET2=4.5,SECTION=rect
1.0000E-01,1.0000E-02
0.0000E+00,1.0000E+00,0.0000E+00

*BEAM SECTION,MATERIAL=STEEL,ELSET=PL2CLM,OFFSET1=0.0000E+00,OFFSET2=-4.5,SECTION=rect
1.0000E-01,1.0000E-02
0.0000E+00,1.0000E+00,0.0000E+00

support
*BOUNDARY
BC,1,6,0

allinone
*node, nset=Nall
1, 0.000000e+00, 0.000000e+00, 0.000000e+00
2, 0.000000e+00, 0.000000e+00, 1.000000e+00
3, 0.000000e+00, 0.000000e+00, 6.666667e-02
4, 0.000000e+00, 0.000000e+00, 1.333333e-01
5, 0.000000e+00, 0.000000e+00, 2.000000e-01
6, 0.000000e+00, 0.000000e+00, 2.666667e-01
7, 0.000000e+00, 0.000000e+00, 3.333333e-01
8, 0.000000e+00, 0.000000e+00, 4.000000e-01
9, 0.000000e+00, 0.000000e+00, 4.666667e-01
10, 0.000000e+00, 0.000000e+00, 5.333333e-01
11, 0.000000e+00, 0.000000e+00, 6.000000e-01
12, 0.000000e+00, 0.000000e+00, 6.666667e-01
13, 0.000000e+00, 0.000000e+00, 7.333333e-01
14, 0.000000e+00, 0.000000e+00, 8.000000e-01
15, 0.000000e+00, 0.000000e+00, 8.666667e-01
16, 0.000000e+00, 0.000000e+00, 9.333333e-01
17, 0.000000e+00, 0.000000e+00, 3.333333e-02
18, 0.000000e+00, 0.000000e+00, 1.000000e-01
19, 0.000000e+00, 0.000000e+00, 1.666667e-01
20, 0.000000e+00, 0.000000e+00, 2.333333e-01
21, 0.000000e+00, 0.000000e+00, 3.000000e-01
22, 0.000000e+00, 0.000000e+00, 3.666667e-01
23, 0.000000e+00, 0.000000e+00, 4.333333e-01
24, 0.000000e+00, 0.000000e+00, 5.000000e-01
25, 0.000000e+00, 0.000000e+00, 5.666667e-01
26, 0.000000e+00, 0.000000e+00, 6.333333e-01
27, 0.000000e+00, 0.000000e+00, 7.000000e-01
28, 0.000000e+00, 0.000000e+00, 7.666667e-01
29, 0.000000e+00, 0.000000e+00, 8.333333e-01
30, 0.000000e+00, 0.000000e+00, 9.000000e-01
31, 0.000000e+00, 0.000000e+00, 9.666667e-01
*nset, nset=BC
1,
*nset, nset=LX
2,
*element, elset=B32,type=B32
1, 1, 17, 3,
2, 3, 18, 4,
3, 4, 19, 5,
4, 5, 20, 6,
5, 6, 21, 7,
6, 7, 22, 8,
7, 8, 23, 9,
8, 9, 24, 10,
9, 10, 25, 11,
10, 11, 26, 12,
11, 12, 27, 13,
12, 13, 28, 14,
13, 14, 29, 15,
14, 15, 30, 16,
15, 16, 31, 2,
16, 1, 17, 3,
17, 3, 18, 4,
18, 4, 19, 5,
19, 5, 20, 6,
20, 6, 21, 7,
21, 7, 22, 8,
22, 8, 23, 9,
23, 9, 24, 10,
24, 10, 25, 11,
25, 11, 26, 12,
26, 12, 27, 13,
27, 13, 28, 14,
28, 14, 29, 15,
29, 15, 30, 16,
30, 16, 31, 2,
31, 1, 17, 3,
32, 3, 18, 4,
33, 4, 19, 5,
34, 5, 20, 6,
35, 6, 21, 7,
36, 7, 22, 8,
37, 8, 23, 9,
38, 9, 24, 10,
39, 10, 25, 11,
40, 11, 26, 12,
41, 12, 27, 13,
42, 13, 28, 14,
43, 14, 29, 15,
44, 15, 30, 16,
45, 16, 31, 2,

*elset, elset=WCLM
1, 2, 3, 4, 5, 6, 7,
8, 9, 10, 11, 12, 13, 14, 15,
*elset, elset=PL1CLM
16, 17, 18, 19, 20, 21, 22,
23, 24, 25, 26, 27, 28, 29, 30,
*elset, elset=PL2CLM
31, 32, 33, 34, 35, 36, 37,
38, 39, 40, 41, 42, 43, 44, 45,

main
*INCLUDE, INPUT=allinone.inp
*INCLUDE, INPUT=add_material.inp
*INCLUDE, INPUT=add_sections.inp
*INCLUDE, INPUT=add_support.inp
*INCLUDE, INPUT=add_contact.inp

*STEP,NLGEOM

*STATIC

*INCLUDE, INPUT=add_concload.inp
*INCLUDE, INPUT=add_boundary.inp
**NODE FILE
**U,
**EL FILE,Output=3d
**S,
**NODE PRINT,NSET=BC
**RF
**END STEP
*NODE FILE,OUTPUT=2D
U,RF

*EL FILE,SECTION FORCES
S

*NODE PRINT,NSET=Nall
RF

*END STEP

thank you for your attention to this case.

I hope that it would be possible to improve the beam element performances.

Bruno

xyont · February 27, 2023, 5:51am

the model discretization or fiberized of Wide Flange section seems not adequate, only one member along web depth. also the intersection of web and flange plates.

someone can improve the models by refining something like figure below to capable to captured in both strong and weak axis.

it’s nature finite element behavior, minimum two element along thickness also required for better results in plasticity and local buckling.

bruno.zilli · February 28, 2023, 5:37am

Hello, thank you anyway for your good advise.

The problem still exists, because the point is not on the tension state, but on the section forces.

Juan explained the problem, please read all the discussion. The construction of the beam element in ccX, at the moment. is made in a such way that it is not reliable to get out the section forces in a correct way. If you would like to check it, please consider the teoretical bending moment by the concentrated load at the tip, and the fem results. Thank you.

Section forces are fundamental parameters for working with eurocodes (e.g. EC3).

Thank you anyway, I hope that the developers will improve this important part in a next future.

Bruno

xyont · February 28, 2023, 10:53am

what percentage of different? right it’s not exact, if that goal someone need to set to user beam element U1 with classical formulation.

it’s a finite element with solid not classical ones, much depend on user models and constructed of member meshing or section discretization.

please posted sketch of problem, hand calculation or references, input files and tabulated output report.

bruno.zilli · February 28, 2023, 1:04pm

Hello,

yes we know about the ccX B32 beam philosofy.

The difference is far more the 100%. E.g.: with the model in mm, the lenght of the cantilever beam is 1000 mm, the force is 1000 N, I expect a moment of 1E+6 Nmm. The results are very far from it.

Differently, the values of the displacement are in the range of what is expected by the theory.

I’m a long life user of open source, with other software. I my opinion, ccX is a powerful and well designed software.

At the moment it lacks in workable beam elements only.

If you think that it could be worth, a good improvement of beam elements, in my opinion, would be to joint the section mesh (2D) to the analysis (as other open source software is doing in a reliable way).

Thank you very much indeed, just for the part of the software that is very useful and good.

I’m still using it, I post a picture of hertz contact, one example I did

for steel industry.

Best Regards

Bruno

xyont · February 28, 2023, 3:11pm

strange, i took some simple test and i can confirm. but this does not happen in previous versions (2016) i’ll check later. it seems some code has been changes, output in 3D still shown as expectable.

but it’s not as in 2D output, shown unexpected result values along the beam length.

bruno.zilli · February 28, 2023, 8:13pm

Yes, the bending moment is unlikely.

Regards

Bruno

xyont · March 1, 2023, 5:21am

previously i only investigate at stress and deflection, found some disadvantage of beam composed model

knot generation makes over-stiffen the beam element (in example above is ~33% lower)
stress existed at simple supported due to over-constraining of expanded nodes.

this condition also has been notify in document manuals, it similar to shell element by duplicating element. fortunately the codes treat the condition and applied with *Composite keyword, but not available yet for beam element. it need different codes to eliminate knot generates at every nodes.

regarding to section forces along the beam, i really hope some fixes to be working properly also. even limited, user beam U1 with classical currently available and it can be use as alternative.

Topic		Replies	Views
Is contact of beam and shell allowed in CCX?	11	1835	October 24, 2020
Beam not reconstructed properly	15	468	October 31, 2022
Wrong beam model results	4	514	November 19, 2020
Problem using U1 element (general beam section)	9	1709	August 1, 2023
TIED contact and beam won't converge in CCX 2.17+	6	191	April 29, 2024

B32-beam elements

Related Topics