I requested stress output in a dat file for S3 and S6 element.
In the dat file I saw 6 stresses sxx syy azz sxy sxz and syz.
First question why for 2D elements we have 6 stresses components and no just 3?
Second question reading the integration points I saw 9 components for s6 element and 2 components for s3 element it is possible to have some pictures for seeing the location of the integration points for the 2 elements.
Thanks Giuseppe
In CalculiX, 2D elements are internally expanded to 3D elements. Details are described in the documentation.
Positions of integration points can be found by requesting the COORD output variable.
Thanks reading the documentation I read that there is US3 element that I a really 2D Elemenent, I am correct?
If would like use that one how can do it?
I try to wrote type=US3 instead of S3 but did not work
You need additional keywords to use it:
*USER ELEMENT, TYPE=US3, NODES=3, INTEGRATION POINTS=3, MAXDOF=6
*USER SECTION, ELSET=elset_name, MATERIAL=material_name, CONSTANTS=1
thickness
there’s many example in test file distributed, e.g lin_stat_twisted_beam.inp
thanks to all, for the good explanation i will try
I try to use your example for calculating the STRESS for a dynamic analysis adding the following steps.
but i did not get the stress results in the dat file. I got the stresses just for the static analysis and for the modal parts.
No stresses for
*STEADY STATE DYNAMICS,HARMONIC=YES
it is my issue or it is a problem of element US3
thanks in advance
** MATERIALS
**
*Material, name=Material-1
*Density
7800.,
*Elastic
2.9e+07, 0.28
*Expansion, Zero=20
1.1E-05
*Conductivity
14
*Specific heat
440000000
*DAMPING,STRUCTURAL=0.06
** Amplitudes ++++++++++++++++++++++++++++++++++++++++++++++
1.,1000.,1100.,1000.
*AMPLITUDE,NAME=A2
1.,1.,1100.,1.
** +++++++++++++++++++++++++++++++++++++++++++++++++++++++++++
*Step,
*Static
1., 1., 1e-05, 1.
*Boundary
Set-2, 1, 1
Set-2, 2, 2
Set-2, 3, 3
Set-2, 4, 4
Set-2, 5, 5
Set-2, 6, 6
**
** LOADS
**
** Name: Load-1 Type: Concentrated force
*Cload
3, 1, 1.
** ccx output
** *NODE PRINT,NSET=Nall
** U
*EL FILE
SNEG,SMID,SPOS
*EL PRINT,ELSET=Eall
S
*NODE FILE
U,RF
*end step
**U,RF,SNEG,SMID,SPOS
** Step-1 ++++++++++++++++++++++++++++++++++++++++++++++++++
**
*Step
*Frequency, Solver=Pardiso, STORAGE=YES
10
**
** Boundary conditions +++++++++++++++++++++++++++++++++++++
*Boundary, op=New
** Name: Incastro
*Boundary
Set-2, 1, 1, 0
Set-2, 2, 2, 0
Set-2, 3, 3, 0
Set-2, 4, 4, 0
Set-2, 5, 5, 0
Set-2, 6, 6, 0
**
** Loads +++++++++++++++++++++++++++++++++++++++++++++++++++
**
**
** Defined fields ++++++++++++++++++++++++++++++++++++++++++
**
**
** History outputs +++++++++++++++++++++++++++++++++++++++++
**
**
** Field outputs +++++++++++++++++++++++++++++++++++++++++++
**
**
** End step ++++++++++++++++++++++++++++++++++++++++++++++++
**
*End step
** Step-2 ++++++++++++++++++++++++++++++++++++++++++++++++++
*Step
*STEADY STATE DYNAMICS,HARMONIC=YES
20.0,1000.0,1,1
**
**
** Boundary conditions +++++++++++++++++++++++++++++++++++++
*BOUNDARY,AMPLITUDE=A2,LOAD CASE = 1
Set-2, 1, 1, 1
**
** Loads +++++++++++++++++++++++++++++++++++++++++++++++++++
**
** Defined fields ++++++++++++++++++++++++++++++++++++++++++
**
**
** History outputs +++++++++++++++++++++++++++++++++++++++++
** *NODE PRINT,NSET=SBALZO
** U
** *NODE PRINT,NSET=CHECK
** U
**EL PRINT,ELSET=barra
** S
** *EL PRINT,ELSET=Shell_part-1
** S
** *EL PRINT,ELSET=el_2D
** S,COORD
**
** Field outputs +++++++++++++++++++++++++++++++++++++++++++
**
** End step ++++++++++++++++++++++++++++++++++++++++++++++++
**
*End step
it has shown some error message, and maybe related to reading eigenfrequency files.
*WARNING reading *STEADY STATE DYNAMICS:
number of data points: 1
is smaller than 2;
2 data points are taken instead
Setting a higher number of data points should eliminate this warning message:
*STEADY STATE DYNAMICS,HARMONIC=YES
20.0,1000.0,20,3
That’s the default setting.
hello i think that there somenthing in the element and firing setting.
because in the same model i swap the element type from US3 to S3 and modified the firing setting
from:
set CCX_NPROC_RESULTS=8
set CCX_NPROC_STIFFNESS=8
set OMP_NUM_THREADS=8
set MKL_NUM_THREADS=8
set CCX_PATH=C:\Dynamic_Analysis
cmd /k %CCX_PATH%\ccx_dynamic.exe test_S3
to
set CCX_NPROC_RESULTS=1
set CCX_NPROC_STIFFNESS=1
set OMP_NUM_THREADS=1
set MKL_NUM_THREADS=1
set CCX_PATH=C:\Dynamic_Analysis
cmd /k %CCX_PATH%\ccx_dynamic.exe test_S3
and i got the results for the 2 frequency:
20
doing the same for the element US3 i got the stress just for the first frequency
i have the same experiences also, when request output of displacement everything seems okay. However, it crash when i request stress output, this usually does not happen in dynamic analysis of expanded shell element.
maybe the problem need to be reproduced by simple model and small number of element first, studying discrepancy and solver behavior using shell element type S3, S6 and US3.
I used the model lin_stat_twisted_beam.inp and I add the dynamic step.
If I modify the element from US3 to S3 and I got the STRESS results from the dynamic parts instead using the US3 element i did not get the stresses.
So my question is anybody find some bugs with US3 element in a dynamic analysis? or work fine?
Do you mean *DYNAMIC (dynamic implicit) ? I get stress results also with US3 elements in this step.
No I mean
*STEADY STATE DYNAMICS,HARMONIC=YES
Do you get stress results in this case?
If it runs to completion (“Job finished”), paste the content of this file (apart from the mesh definition since it’s available in the original file that you linked) here. We must know the exact setup to look for errors and SSD analyses are really picky in CalculiX.
below example of cantilever plates subjected to static distributed and concentrated loads
*Heading
shell element (US3) test, Unit system: N_MM_TON_S_C
*Node
1, 0.00000000E+000, 1.00000000E+002, 0.00000000E+000
2, 0.00000000E+000, 5.00000000E+001, 0.00000000E+000
3, 5.00000000E+001, 1.00000000E+002, 0.00000000E+000
4, 5.00000000E+001, 5.00000000E+001, 0.00000000E+000
5, 1.00000000E+002, 1.00000000E+002, 0.00000000E+000
6, 1.00000000E+002, 5.00000000E+001, 0.00000000E+000
7, 1.50000000E+002, 1.00000000E+002, 0.00000000E+000
8, 1.50000000E+002, 5.00000000E+001, 0.00000000E+000
9, 2.00000000E+002, 1.00000000E+002, 0.00000000E+000
10, 2.00000000E+002, 5.00000000E+001, 0.00000000E+000
11, 0.00000000E+000, 0.00000000E+000, 0.00000000E+000
12, 5.00000000E+001, 0.00000000E+000, 0.00000000E+000
13, 1.00000000E+002, 0.00000000E+000, 0.00000000E+000
14, 1.50000000E+002, 0.00000000E+000, 0.00000000E+000
15, 2.00000000E+002, 0.00000000E+000, 0.00000000E+000
*Element, Type=US3, Elset=Shell_part-1
1, 1, 2, 3
2, 3, 2, 4
3, 3, 4, 5
4, 5, 4, 6
5, 5, 6, 7
6, 7, 6, 8
7, 7, 8, 9
8, 9, 8, 10
9, 2, 11, 4
10, 4, 11, 12
11, 4, 12, 6
12, 6, 12, 13
13, 6, 13, 8
14, 8, 13, 14
15, 8, 14, 10
16, 10, 14, 15
*Nset, Nset=Node_Set-1
1, 2, 11
*Nset, Nset=Internal_Selection-1_Concentrated_Force-1
10
*Nset, Nset=Internal_Selection-1_Concentrated_Force-2
9, 15
*Nset, Nset=Internal-1_Surface-1
1, 2, 3, 4, 5, 6, 7, 8, 9, 10, 11, 12, 13, 14, 15
*Elset, Elset=Element_Set-1
1, 2, 3, 4, 5, 6, 7, 8, 9, 10, 11, 12, 13, 14, 15, 16
*Elset, Elset=Internal-1_Surface-1_S2
1, 2, 3, 4, 5, 6, 7, 8, 9, 10, 11, 12, 13, 14, 15, 16
*Surface, Name=Surface-1, Type=Element
Internal-1_Surface-1_S2, S2
*Material, Name=S235
*Density
7.8E-09
*Elastic
210000, 0.28
*Expansion, Zero=20
1.1E-05
*Conductivity
14
*Specific heat
440000000
*USER ELEMENT,TYPE=US3,NODES=3,INTEGRATION POINTS=3,MAXDOF=6
*USER SECTION,ELSET=Shell_part-1,MATERIAL=S235,CONSTANTS=1
10
*Step
*Static, Solver=Spooles
*Boundary
Node_Set-1, 1, 3
Node_Set-1, 5
*Cload
Internal_Selection-1_Concentrated_Force-1, 3, -100
*Cload
Internal_Selection-1_Concentrated_Force-2, 3, -50
*Dload
Internal-1_Surface-1_S2, P2, -0.5
*Node file
RF, U
*EL FILE
SNEG,SMID,SPOS
*End step
it can be extended to thermal, frequency and dynamic analysis.
frequency analysis, displacement and stress output request.
*Step
*Frequency, Solver=Spooles
6
*Boundary
Node_Set-1, 1, 3
Node_Set-1, 5
*Node file
RF, U
*EL FILE
SNEG,SMID,SPOS
*End step
Steady state dynamics, loading scheme and input was simple taken from this link.
*Heading
shell element (US3) test, Unit system: N_MM_TON_S_C
*Node
1, 0.00000000E+000, 1.00000000E+002, 0.00000000E+000
2, 0.00000000E+000, 5.00000000E+001, 0.00000000E+000
3, 5.00000000E+001, 1.00000000E+002, 0.00000000E+000
4, 5.00000000E+001, 5.00000000E+001, 0.00000000E+000
5, 1.00000000E+002, 1.00000000E+002, 0.00000000E+000
6, 1.00000000E+002, 5.00000000E+001, 0.00000000E+000
7, 1.50000000E+002, 1.00000000E+002, 0.00000000E+000
8, 1.50000000E+002, 5.00000000E+001, 0.00000000E+000
9, 2.00000000E+002, 1.00000000E+002, 0.00000000E+000
10, 2.00000000E+002, 5.00000000E+001, 0.00000000E+000
11, 0.00000000E+000, 0.00000000E+000, 0.00000000E+000
12, 5.00000000E+001, 0.00000000E+000, 0.00000000E+000
13, 1.00000000E+002, 0.00000000E+000, 0.00000000E+000
14, 1.50000000E+002, 0.00000000E+000, 0.00000000E+000
15, 2.00000000E+002, 0.00000000E+000, 0.00000000E+000
*Element, Type=US3, Elset=Shell_part-1
1, 1, 2, 3
2, 3, 2, 4
3, 3, 4, 5
4, 5, 4, 6
5, 5, 6, 7
6, 7, 6, 8
7, 7, 8, 9
8, 9, 8, 10
9, 2, 11, 4
10, 4, 11, 12
11, 4, 12, 6
12, 6, 12, 13
13, 6, 13, 8
14, 8, 13, 14
15, 8, 14, 10
16, 10, 14, 15
*Nset, Nset=Node_Set-1
1, 2, 11
*Nset, Nset=Internal_Selection-1_Concentrated_Force-1
10
*Nset, Nset=Internal_Selection-1_Concentrated_Force-2
9, 15
*Material, Name=S235
*Density
7.8E-09
*Elastic
210000, 0.28
*Expansion, Zero=20
1.1E-05
*Conductivity
14
*Specific heat
440000000
*USER ELEMENT,TYPE=US3,NODES=3,INTEGRATION POINTS=3,MAXDOF=6
*USER SECTION,ELSET=Shell_part-1,MATERIAL=S235,CONSTANTS=1
10
*AMPLITUDE,NAME=A1
0, 30,
0.000451178595332783, 33.8268343236509,
0.000902357190665565, 37.0710678118655,
0.00135353578599835, 39.2387953251129,
0.00180471438133113, 40,
0.00225589297666391, 39.2387953251129,
0.0027070715719967, 37.0710678118655,
0.00315825016732948, 33.8268343236509,
0.00360942876266226, 30,
0.00406060735799504, 26.1731656763491,
0.00451178595332783, 22.9289321881345,
0.00496296454866061, 20.7612046748871,
0.00541414314399339, 20,
0.00586532173932618, 20.7612046748871,
0.00631650033465896, 22.9289321881345,
0.00676767892999174, 26.1731656763491,
0.00721885752532453, 30,
*BOUNDARY
Node_Set-1, 1, 3
Node_Set-1, 5
*STEP
*FREQUENCY,SOLVER=Spooles,STORAGE=YES
10,0.01
*END STEP
*STEP
*STEADY STATE DYNAMICS,HARMONIC=NO
128.53,148.53,2,1,20,0.,0.00721885752532453
*MODAL DAMPING
1,10,0.01
*CLOAD, AMPLITUDE=A1
Internal_Selection-1_Concentrated_Force-1,3,1.
*NODE FILE
U
** *EL FILE
** SNEG,SMID,SPOS
*END STEP
only displacement output request is succeeded, stress output lead to program crash.
really thanks for your deep investigation!
So we can say that US3 element have a BUG, what do you think?
i take your simply model and switch to S3 element and I got the results (disp and stress) for *STEADY STATE DYNAMICS,HARMONIC=YES analysis
*Heading
shell element (S3) test, Unit system: N_MM_TON_S_C
*Node
1, 0.00000000E+000, 1.00000000E+002, 0.00000000E+000
2, 0.00000000E+000, 5.00000000E+001, 0.00000000E+000
3, 5.00000000E+001, 1.00000000E+002, 0.00000000E+000
4, 5.00000000E+001, 5.00000000E+001, 0.00000000E+000
5, 1.00000000E+002, 1.00000000E+002, 0.00000000E+000
6, 1.00000000E+002, 5.00000000E+001, 0.00000000E+000
7, 1.50000000E+002, 1.00000000E+002, 0.00000000E+000
8, 1.50000000E+002, 5.00000000E+001, 0.00000000E+000
9, 2.00000000E+002, 1.00000000E+002, 0.00000000E+000
10, 2.00000000E+002, 5.00000000E+001, 0.00000000E+000
11, 0.00000000E+000, 0.00000000E+000, 0.00000000E+000
12, 5.00000000E+001, 0.00000000E+000, 0.00000000E+000
13, 1.00000000E+002, 0.00000000E+000, 0.00000000E+000
14, 1.50000000E+002, 0.00000000E+000, 0.00000000E+000
15, 2.00000000E+002, 0.00000000E+000, 0.00000000E+000
*Element, Type=S3, Elset=Shell_part-1
1, 1, 2, 3
2, 3, 2, 4
3, 3, 4, 5
4, 5, 4, 6
5, 5, 6, 7
6, 7, 6, 8
7, 7, 8, 9
8, 9, 8, 10
9, 2, 11, 4
10, 4, 11, 12
11, 4, 12, 6
12, 6, 12, 13
13, 6, 13, 8
14, 8, 13, 14
15, 8, 14, 10
16, 10, 14, 15
*Nset, Nset=Node_Set-1
1, 2, 11
*Nset, Nset=Internal_Selection-1_Concentrated_Force-1
10
*Nset, Nset=Internal_Selection-1_Concentrated_Force-2
9, 15
*Nset, Nset=Internal-1_Surface-1
1, 2, 3, 4, 5, 6, 7, 8, 9, 10, 11, 12, 13, 14, 15
*Elset, Elset=Element_Set-1
1, 2, 3, 4, 5, 6, 7, 8, 9, 10, 11, 12, 13, 14, 15, 16
*Elset, Elset=Internal-1_Surface-1_S2
1, 2, 3, 4, 5, 6, 7, 8, 9, 10, 11, 12, 13, 14, 15, 16
*Surface, Name=Surface-1, Type=Element
Internal-1_Surface-1_S2, S2
*Material, Name=S235
*Density
7.8E-09
*Elastic
210000, 0.28
*Expansion, Zero=20
1.1E-05
*Conductivity
14
*Specific heat
440000000
*DAMPING,STRUCTURAL=0.06
** Amplitudes ++++++++++++++++++++++++++++++++++++++++++++++
*AMPLITUDE,NAME=A2
1.,1.,1100.,1.
** +++++++++++++++++++++++++++++++++++++++++++++++++++++++++++
*SHELL SECTION,MATERIAL=S235,ELSET=Shell_part-1
10
*Step
*Frequency, Solver=Pardiso, STORAGE=YES
10
**
** Boundary conditions +++++++++++++++++++++++++++++++++++++
*Boundary, op=New
** Name: Incastro
*Boundary
Node_Set-1, 1, 1, 0
Node_Set-1, 2, 2, 0
Node_Set-1, 3, 3, 0
Node_Set-1, 4, 4, 0
Node_Set-1, 5, 5, 0
Node_Set-1, 6, 6, 0
**
** Loads +++++++++++++++++++++++++++++++++++++++++++++++++++
**
** Defined fields ++++++++++++++++++++++++++++++++++++++++++
**
** History outputs +++++++++++++++++++++++++++++++++++++++++
**
** Field outputs +++++++++++++++++++++++++++++++++++++++++++
**
** End step ++++++++++++++++++++++++++++++++++++++++++++++++
**
*End step
** Step-2 ++++++++++++++++++++++++++++++++++++++++++++++++++
*Step
*STEADY STATE DYNAMICS,HARMONIC=YES
20.0,1000.0,1,3
**
**
** Boundary conditions +++++++++++++++++++++++++++++++++++++
*BOUNDARY,AMPLITUDE=A2,LOAD CASE = 1
Node_Set-1, 1, 1, 1
**
** Loads +++++++++++++++++++++++++++++++++++++++++++++++++++
**
** Defined fields ++++++++++++++++++++++++++++++++++++++++++
**
** History outputs +++++++++++++++++++++++++++++++++++++++++
*NODE PRINT,Nset=Internal-1_Surface-1
U
*EL PRINT,ELSET=Shell_part-1
S
** Field outputs +++++++++++++++++++++++++++++++++++++++++++
**
** End step ++++++++++++++++++++++++++++++++++++++++++++++++
**
*End step
instead using US3 element I can confirm your results if I request only the DISPLACENT no issue instead if I add the stress output no results are available
It should be reported in the CalculiX GitHub repository (Issues · Dhondtguido/CalculiX · GitHub) as a bug or undocumented limitation.
