# Output stress dat file **URL:** \ **Category:** Uncategorized\ **Created:** [December 15, 2023, 9:29am UTC](https://calculix.discourse.group/t/output-stress-dat-file/1977 "2023-12-15T09:29:43Z")\ **Posts on this page:** 20\ **Page:** 1
**Author:** ![giucre](https://avatars.discourse-cdn.com/v4/letter/g/90db22/32.png) [@giucre](https://calculix.discourse.group/u/giucre)\ **Post date:** [December 15, 2023, 9:29am UTC](https://calculix.discourse.group/t/output-stress-dat-file/1977/1 "2023-12-15T09:29:43Z")
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 ---
**Author:** ![Calc\_em](https://avatars.discourse-cdn.com/v4/letter/c/43a26b/32.png) [@Calc\_em](https://calculix.discourse.group/u/Calc_em)\ **Post date:** [December 15, 2023, 12:20pm UTC](https://calculix.discourse.group/t/output-stress-dat-file/1977/2 "2023-12-15T12:20:30Z")
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. ---
**Author:** ![giucre](https://avatars.discourse-cdn.com/v4/letter/g/90db22/32.png) [@giucre](https://calculix.discourse.group/u/giucre)\ **Post date:** [December 15, 2023, 4:18pm UTC](https://calculix.discourse.group/t/output-stress-dat-file/1977/3 "2023-12-15T16:18:45Z")
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 ---
**Author:** ![Calc\_em](https://avatars.discourse-cdn.com/v4/letter/c/43a26b/32.png) [@Calc\_em](https://calculix.discourse.group/u/Calc_em)\ **Post date:** [December 15, 2023, 4:52pm UTC](https://calculix.discourse.group/t/output-stress-dat-file/1977/4 "2023-12-15T16:52:59Z")
You need additional keywords to use it: ```auto *USER ELEMENT, TYPE=US3, NODES=3, INTEGRATION POINTS=3, MAXDOF=6 *USER SECTION, ELSET=elset_name, MATERIAL=material_name, CONSTANTS=1 thickness ``` ---
**Author:** ![xyont](https://yyz2.discourse-cdn.com/free1/user_avatar/calculix.discourse.group/xyont/32/3553_2.png) [@xyont](https://calculix.discourse.group/u/xyont)\ **Post date:** [December 15, 2023, 6:16pm UTC](https://calculix.discourse.group/t/output-stress-dat-file/1977/5 "2023-12-15T18:16:57Z")
there’s many example in test file distributed, e.g [`lin_stat_twisted_beam.inp`](https://feacluster.com/CalculiX/ccx_2.18/doc/ccx/input_deck_viewer.php?input_deck=lin_stat_twisted_beam.inp) ![06c9aaabbc721fd22fa79d93e96dff961030354f](https://global.discourse-cdn.com/free1/uploads/calculix/original/2X/4/433b0437912baceb7a9154edbfe2413cb08aea25.png) > [@Missing element US3](https://calculix.discourse.group/t/missing-element-us3/924/3): > > the behavior also the same as user beam element, seems it does not yet supported by CGX. \*\*edited may i corrected, finally i found it how to be working. thanks Guido for implement the improved version of classical shell element, also for some example files at the webs. or, may also thanks to another. did Gil Rama at MTU Aero Engines (et al) contributed directly to CalculiX? ---
**Author:** ![giucre](https://avatars.discourse-cdn.com/v4/letter/g/90db22/32.png) [@giucre](https://calculix.discourse.group/u/giucre)\ **Post date:** [December 15, 2023, 6:28pm UTC](https://calculix.discourse.group/t/output-stress-dat-file/1977/6 "2023-12-15T18:28:02Z")
thanks to all, for the good explanation i will try ---
**Author:** ![giucre](https://avatars.discourse-cdn.com/v4/letter/g/90db22/32.png) [@giucre](https://calculix.discourse.group/u/giucre)\ **Post date:** [December 15, 2023, 7:34pm UTC](https://calculix.discourse.group/t/output-stress-dat-file/1977/7 "2023-12-15T19:34:29Z")
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 ---
**Author:** ![xyont](https://yyz2.discourse-cdn.com/free1/user_avatar/calculix.discourse.group/xyont/32/3553_2.png) [@xyont](https://calculix.discourse.group/u/xyont)\ **Post date:** [December 15, 2023, 9:07pm UTC](https://calculix.discourse.group/t/output-stress-dat-file/1977/8 "2023-12-15T21:07:47Z")
it has shown some error message, and maybe related to reading eigenfrequency files. ```auto *WARNING reading *STEADY STATE DYNAMICS: number of data points: 1 is smaller than 2; 2 data points are taken instead ``` ---
**Author:** ![Calc\_em](https://avatars.discourse-cdn.com/v4/letter/c/43a26b/32.png) [@Calc\_em](https://calculix.discourse.group/u/Calc_em)\ **Post date:** [December 15, 2023, 9:46pm UTC](https://calculix.discourse.group/t/output-stress-dat-file/1977/9 "2023-12-15T21:46:32Z")
Setting a higher number of data points should eliminate this warning message: ```auto *STEADY STATE DYNAMICS,HARMONIC=YES 20.0,1000.0,20,3 ``` That’s the default setting. ---
**Author:** ![giucre](https://avatars.discourse-cdn.com/v4/letter/g/90db22/32.png) [@giucre](https://calculix.discourse.group/u/giucre)\ **Post date:** [December 15, 2023, 11:50pm UTC](https://calculix.discourse.group/t/output-stress-dat-file/1977/10 "2023-12-15T23:50:34Z")
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 ![image](https://global.discourse-cdn.com/free1/uploads/calculix/original/2X/3/367280d4a4724a801da6d591016a44f7f5a18638.png) and 1000 ![image](https://global.discourse-cdn.com/free1/uploads/calculix/original/2X/f/f0e1706ced7a134fbb58215a1841abb9bfbcac7c.png) doing the same for the element US3 i got the stress just for the first frequency ![image](https://global.discourse-cdn.com/free1/uploads/calculix/original/2X/e/e69db1c28aae6e3fc88c29779a4d4a14c0ac99f7.png) anybody know the correct setting? probably insert the correct setting I will get the results also for the second frequency. any suggestion? is element bugs or I did some mistake? Thanks ---
**Author:** ![xyont](https://yyz2.discourse-cdn.com/free1/user_avatar/calculix.discourse.group/xyont/32/3553_2.png) [@xyont](https://calculix.discourse.group/u/xyont)\ **Post date:** [December 16, 2023, 1:04am UTC](https://calculix.discourse.group/t/output-stress-dat-file/1977/11 "2023-12-16T01:04:37Z")
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. ---
**Author:** ![giucre](https://avatars.discourse-cdn.com/v4/letter/g/90db22/32.png) [@giucre](https://calculix.discourse.group/u/giucre)\ **Post date:** [December 16, 2023, 1:39pm UTC](https://calculix.discourse.group/t/output-stress-dat-file/1977/12 "2023-12-16T13:39:44Z")
I used the model [`lin_stat_twisted_beam.inp`](https://feacluster.com/CalculiX/ccx_2.18/doc/ccx/input_deck_viewer.php?input_deck=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? ---
**Author:** ![Calc\_em](https://avatars.discourse-cdn.com/v4/letter/c/43a26b/32.png) [@Calc\_em](https://calculix.discourse.group/u/Calc_em)\ **Post date:** [December 16, 2023, 5:34pm UTC](https://calculix.discourse.group/t/output-stress-dat-file/1977/13 "2023-12-16T17:34:00Z")
> [@giucre](#): > > dynamic step Do you mean `*DYNAMIC` (dynamic implicit) ? I get stress results also with US3 elements in this step. ---
**Author:** ![giucre](https://avatars.discourse-cdn.com/v4/letter/g/90db22/32.png) [@giucre](https://calculix.discourse.group/u/giucre)\ **Post date:** [December 16, 2023, 8:15pm UTC](https://calculix.discourse.group/t/output-stress-dat-file/1977/14 "2023-12-16T20:15:14Z")
No I mean \*STEADY STATE DYNAMICS,HARMONIC=YES Do you get stress results in this case? ---
**Author:** ![Calc\_em](https://avatars.discourse-cdn.com/v4/letter/c/43a26b/32.png) [@Calc\_em](https://calculix.discourse.group/u/Calc_em)\ **Post date:** [December 16, 2023, 8:52pm UTC](https://calculix.discourse.group/t/output-stress-dat-file/1977/15 "2023-12-16T20:52:48Z")
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. ---
**Author:** ![xyont](https://yyz2.discourse-cdn.com/free1/user_avatar/calculix.discourse.group/xyont/32/3553_2.png) [@xyont](https://calculix.discourse.group/u/xyont)\ **Post date:** [December 17, 2023, 2:35am UTC](https://calculix.discourse.group/t/output-stress-dat-file/1977/16 "2023-12-17T02:35:39Z")
> [@xyont](#): > > maybe the problem need to be reproduced by simple model and small number of element first, below example of cantilever plates subjected to static distributed and concentrated loads ```auto *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 ``` ![2023-12-17 09_32_51-CalculiX GraphiX](https://global.discourse-cdn.com/free1/uploads/calculix/original/2X/4/47be757cb41e6dd9623c6fd63cefc180c0c99112.png) ![2023-12-17 09_24_06-CalculiX GraphiX](https://global.discourse-cdn.com/free1/uploads/calculix/original/2X/0/009daf6816c0fa1b38c75eb3cc9863669d2f4243.png) ![2023-12-17 09_28_33-CalculiX GraphiX](https://global.discourse-cdn.com/free1/uploads/calculix/original/2X/c/cf8b734997a164b48ce2cbee32de4a296769979d.png) it can be extended to thermal, frequency and dynamic analysis. ---
**Author:** ![xyont](https://yyz2.discourse-cdn.com/free1/user_avatar/calculix.discourse.group/xyont/32/3553_2.png) [@xyont](https://calculix.discourse.group/u/xyont)\ **Post date:** [December 17, 2023, 2:50am UTC](https://calculix.discourse.group/t/output-stress-dat-file/1977/17 "2023-12-17T02:50:21Z")
frequency analysis, displacement and stress output request. ```auto *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 ``` ![2023-12-17 09_47_28-CalculiX GraphiX](https://global.discourse-cdn.com/free1/uploads/calculix/original/2X/c/c5e80cfbbfc2f80eaa7ed4e4d8ab08f31bbfd2b6.png) ![2023-12-17 09_47_52-CalculiX GraphiX](https://global.discourse-cdn.com/free1/uploads/calculix/original/2X/5/52dea688d630cc747150a72094a6ec586f8f77a9.png) ---
**Author:** ![xyont](https://yyz2.discourse-cdn.com/free1/user_avatar/calculix.discourse.group/xyont/32/3553_2.png) [@xyont](https://calculix.discourse.group/u/xyont)\ **Post date:** [December 17, 2023, 3:33am UTC](https://calculix.discourse.group/t/output-stress-dat-file/1977/18 "2023-12-17T03:33:57Z")
Steady state dynamics, loading scheme and input was simple taken from this [link](https://github.com/suleymanmuti/CalculiX-Examples/tree/master/steady_state_dynamics/beam_harmonic_as_non_harmonic). ```auto *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 ``` ![2023-12-17 10_28_50-CalculiX GraphiX](https://global.discourse-cdn.com/free1/uploads/calculix/original/2X/f/f214fb1a56d8a95622330f43f8fabe639d0b3fdf.png) only displacement output request is succeeded, stress output lead to program crash. ---
**Author:** ![giucre](https://avatars.discourse-cdn.com/v4/letter/g/90db22/32.png) [@giucre](https://calculix.discourse.group/u/giucre)\ **Post date:** [December 17, 2023, 9:15am UTC](https://calculix.discourse.group/t/output-stress-dat-file/1977/19 "2023-12-17T09:15:33Z")
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 ---
**Author:** ![Calc\_em](https://avatars.discourse-cdn.com/v4/letter/c/43a26b/32.png) [@Calc\_em](https://calculix.discourse.group/u/Calc_em)\ **Post date:** [December 17, 2023, 9:26am UTC](https://calculix.discourse.group/t/output-stress-dat-file/1977/20 "2023-12-17T09:26:21Z")
It should be reported in the CalculiX GitHub repository ([Issues · Dhondtguido/CalculiX · GitHub](https://github.com/Dhondtguido/CalculiX/issues)) as a bug or undocumented limitation. [Next page](https://calculix.discourse.group/t/output-stress-dat-file/1977.md?page=2)