Tagged: apdl, modal-analysis, truss
-
-
September 6, 2022 at 1:53 am
victor.mcarv
SubscriberI have been learning ANSYS Mechanical APDL to use it for a paper on the subject of “damage detection based on dynamic properties of structures”.
Currently, I am modeling a benchmark structure to check if my script is working correctly. This structure is a 3D Truss from which I have the 10 first experimental natural frequencies available for comparison.
Unfortunately, my FE model doesn’t seem to be able to extract the correct frequencies, since I am getting numerical results at least 26% and at most 91% higher than the experimental results.
I tried using LINK180 elements, as well as BEAM188 elements (releasing rotation at the joints by using the ENDRELEASE command) for the struts, being each strut represented by a single element, but so far nothing has worked out.
What would be the simplest and yet most correct way to represent a 3D Truss for a Modal analysis?
I can send my script if needed.
-
September 6, 2022 at 7:09 am
Erik Kostson
Ansys EmployeeTruss elements (LINK180) is appropriate – make sure to check all things (dimensions, sections, materials,boundary conditions,…) and have the same as in the physical tests/measurements and so on.
Feel free to post the apdl commands, as other members of the forum might be able to advice.
Erik
-
September 7, 2022 at 1:54 am
victor.mcarv
SubscriberThank you for your reply, Erik. My dimensions, sections and materials seem to be ok. The boundary conditions might not be.
Here's my script.
https://drive.google.com/file/d/1WNkWJu9e5BOacNPlR4uvVCv3jQZHYrg7/view?usp=sharing
Also, here are the real experimental boundary conditions:
"Left" side of the structure": https://imgur.com/HLxhD83
"Right" side of the structure: https://imgur.com/Wez0gHn
On the "Left" side I applied displacements = 0 for X, Y and Z directions, and on the "Right" side I applied displacements = 0 for Y and Z directions.
-
September 7, 2022 at 6:38 am
Erik Kostson
Ansys EmployeeWe (ansys) can not dowwnload attachments. If you want try and add them inline in your message.
Use perhaps beam elements also and work with that.
I would for beam188 definetely use the standard options including keyopt(3) = 3 (cubic shape functions) especially if you have only one element per member when using beam188, and do not release ofcourse if they are welded.
Finally most important since you get higher exp. frequencies (could be that mass is too low in the mass matrix) use the default option for mass matrix (so no lumped methods, no use of LUMPM command).
So just use:
/solution antype,modal modopt,lanb,20 ! Use LANB solver mxpand,,,,yes solve
—
Of course could be that the boundary conditions are wrong. Use springs all the nodes/points with boundary conditions – one spring (COMBIN14) for each direction so you need 3 springs (X,Y,Z) for each node/point where you apply your constraint/displacement boundary conditions. Then you will need to probably tune the spring stiffness to get better agreement between tests and FEA. Finally,
Also in the experiments one should find out the mode shapes (so how do they look like, bending, torsional, etc, and how do points move) corresponding to the frequencies measured, and then compare the same mode/frequency to FEA (also measure the mode shapes near the supports to find out how these points are moving for each mode).
Hope this helps
Erik
-
September 7, 2022 at 3:52 pm
victor.mcarv
SubscriberThank you for the comprehensive reply, Erik. I'm gonna check all of the points you made.
Just to make it available, since you can not download attachments, I'm gonna follow this with my script.
! -------- SCRIPT BELOW -------- !
!! UNITS: N,kg,m,s!!-------------------------------------------------------------------------!!****_ 1. CLEARING _****!!-------------------------------------------------------------------------!!! 1.1 Clearing the modelFINISH/CLEAR,NOSTART!!-------------------------------------------------------------------------!!****_ 2. INPUT _****!!-------------------------------------------------------------------------!!! 2.1 MaterialEMOD = 6.964E+10 ! [N/m^2] Young's modulusNU = 0.33 ! [adm] Poisson's ratioDEN = 2714.47 ! [kg/m^3] Density!! 2.2 Cross sections! 2.2.1 Primary elements (PRI)REP = 0.07620 ! [m] External radiusESP = 8.300E-3 ! [m] ThicknessRIP = 0.06790 ! [m] Internal radiusARP = 3.757E-3 ! [m^2] Cross-sectional areaIXXP = 9.785E-6 ! [m^4] Moment of inertiaJP = 1.957E-5 ! [m^4] Polar moment of inertia! 2.2.2 Secondary elements (SEC)RES = 0.03810 ! [m] External radiusESS = 6.300E-3 ! [m] ThicknessRIS = 0.03180 ! [m] Internal radiusARS = 1.383E-3 ! [m^2] Cross-sectional areaIXXS = 8.518E-7 ! [m^4] Moment of inertiaJS = 1.704E-6 ! [m^4] Polar moment of inertia! 2.2.3 Tertiary elements (TER)RET = 0.02540 ! [m] External radiusEST = 4.800E-3 ! [m] ThicknessRIT = 0.02060 ! [m] Internal radiusART = 6.937E-4 ! [m^2] Cross-sectional areaIXXT = 1.855E-7 ! [m^4] Moment of inertiaJT = 3.709E-7 ! [m^4] Polar moment of inertia!!-------------------------------------------------------------------------!!****_ 3. PRE-PROCESSING _****!!-------------------------------------------------------------------------!!/PREP7!/VIEW,1,1,2,3/REP,FAST!! 3.1 Adding materialMP,EX,1,EMODMP,PRXY,1,NUMP,DENS,1,DEN!! 3.2 Adding element typeET,1,LINK180!! 3.3 Adding sectionsSECTYPE,1,LINK,,PRISECDATA,ARP,!SECTYPE,2,LINK,,SECSECDATA,ARS,!SECTYPE,3,LINK,,TERSECDATA,ART,!! 3.4 Creating nodes! 3.4.1 Bottom front chordN,1,0.00,0.00,0.00N,2,1.73,0.00,0.00N,3,3.46,0.00,0.00N,4,5.19,0.00,0.00N,5,6.92,0.00,0.00N,6,8.65,0.00,0.00N,7,10.53,0.00,0.00N,8,12.32,0.00,0.00N,9,13.96,0.00,0.00N,10,15.60,0.00,0.00N,11,17.24,0.00,0.00! 3.4.2 Top front chordN,12,0.00,1.98,0.00N,13,1.73,1.98,0.00N,14,3.46,1.98,0.00N,15,5.19,1.98,0.00N,16,6.92,1.98,0.00N,17,8.65,1.98,0.00N,18,10.53,1.98,0.00N,19,12.32,1.98,0.00N,20,13.96,1.98,0.00N,21,15.60,1.98,0.00N,22,17.24,1.98,0.00! 3.4.3 Bottom back chordN,23,0.00,0.00,-1.83N,24,1.73,0.00,-1.83N,25,3.46,0.00,-1.83N,26,5.19,0.00,-1.83N,27,6.92,0.00,-1.83N,28,8.65,0.00,-1.83N,29,10.53,0.00,-1.83N,30,12.32,0.00,-1.83N,31,13.96,0.00,-1.83N,32,15.60,0.00,-1.83N,33,17.24,0.00,-1.83! 3.4.4 Top back chordN,34,0.00,1.98,-1.83N,35,1.73,1.98,-1.83N,36,3.46,1.98,-1.83N,37,5.19,1.98,-1.83N,38,6.92,1.98,-1.83N,39,8.65,1.98,-1.83N,40,10.53,1.98,-1.83N,41,12.32,1.98,-1.83N,42,13.96,1.98,-1.83N,43,15.60,1.98,-1.83N,44,17.24,1.98,-1.83!/PNUM,NODE,1 ! Show node numbers!! 3.5 Creating elements! 3.5.1 Primary elementsTYPE,1MAT,1SECNUM,1! 3.5.1.1 Bottom front chordEN,1,1,2EN,2,2,3EN,3,3,4EN,4,4,5EN,5,5,6EN,6,6,7EN,7,7,8EN,8,8,9EN,9,9,10EN,10,10,11! 3.5.1.2 Top front chordEN,11,12,13EN,12,13,14EN,13,14,15EN,14,15,16EN,15,16,17EN,16,17,18EN,17,18,19EN,18,19,20EN,19,20,21EN,20,21,22! 3.5.1.3 Bottom back chordEN,21,23,24EN,22,24,25EN,23,25,26EN,24,26,27EN,25,27,28EN,26,28,29EN,27,29,30EN,28,30,31EN,29,31,32EN,30,32,33! 3.5.1.4 Top back chordEN,31,34,35EN,32,35,36EN,33,36,37EN,34,37,38EN,35,38,39EN,36,39,40EN,37,40,41EN,38,41,42EN,39,42,43EN,40,43,44! 3.5.2 Secondary elementsTYPE,1MAT,1SECNUM,2! 3.5.2.1 Front in-panel diagonalsEN,41,1,13EN,42,3,13EN,43,3,15EN,44,5,15EN,45,5,17EN,46,7,17EN,47,7,19EN,48,9,19EN,49,9,21EN,50,11,21! 3.5.2.2 Bottom in-panel diagonalsEN,51,2,23EN,52,2,25EN,53,4,25EN,54,4,27EN,55,6,27EN,56,6,29EN,57,8,29EN,58,8,31EN,59,10,31EN,60,10,33! 3.5.2.3 Top in-panel diagonalsEN,61,12,35EN,62,14,35EN,63,14,37EN,64,16,37EN,65,16,39EN,66,18,39EN,67,18,41EN,68,20,41EN,69,20,43EN,70,22,43! 3.5.2.4 Back in-panel diagonalsEN,71,23,35EN,72,25,35EN,73,25,37EN,74,27,37EN,75,27,39EN,76,29,39EN,77,29,41EN,78,31,41EN,79,31,43EN,80,33,43! 3.5.3 Tertiary elementsTYPE,1MAT,1SECNUM,3! 3.5.3.1 Front panel orthogonal elementsEN,81,1,12EN,82,2,13EN,83,3,14EN,84,4,15EN,85,5,16EN,86,6,17EN,87,7,18EN,88,8,19EN,89,9,20EN,90,10,21EN,91,11,22! 3.5.3.2 Bottom panel orthogonal elementsEN,92,1,23EN,93,2,24EN,94,3,25EN,95,4,26EN,96,5,27EN,97,6,28EN,98,7,29EN,99,8,30EN,100,9,31EN,101,10,32EN,102,11,33! 3.5.3.3 Top panel orthogonal elementsEN,103,12,34EN,104,13,35EN,105,14,36EN,106,15,37EN,107,16,38EN,108,17,39EN,109,18,40EN,110,19,41EN,111,20,42EN,112,21,43EN,113,22,44! 3.5.3.4 Back panel orthogonal elementsEN,114,23,34EN,115,24,35EN,116,25,36EN,117,26,37EN,118,27,38EN,119,28,39EN,120,29,40EN,121,30,41EN,122,31,42EN,123,32,43EN,124,33,44! 3.5.3.5 Out of panel diagonalsEN,125,1,34EN,126,24,13EN,127,3,36EN,128,26,15EN,129,5,38EN,130,28,17EN,131,7,40EN,132,30,19EN,133,9,42EN,134,32,21EN,135,11,44!GPLOT ! Multiplot!! 3.6 Boundary conditionsALLSEL,ALLD,1,UX,0D,1,UY,0D,1,UZ,0D,23,UX,0D,23,UY,0D,23,UZ,0D,11,UY,0D,11,UZ,0D,33,UY,0D,33,UZ,0!!-------------------------------------------------------------------------!!****_ 4. PROCESSING _****!!-------------------------------------------------------------------------!!/SOLU!! 4.1 Defining solution parametersANTYPE,2 ! Modal analysisMODOPT,LANB,10,1E-1,100,,ON ! Block Lanczos, 10 modes, minimum frequency, maximum frequency, mode normalizationEQSLV,SPARSE ! Sparse solverMXPAND,10,,,0 ! Expanding 10 modesLUMPM,1 ! Lumped mass approximation!! 4.2 SolvingSOLVEFINISH!!-------------------------------------------------------------------------!!****_ 5. POST-PROCESSING _****!!-------------------------------------------------------------------------!!/POST1SET,LIST!!-------------------------------------------------------------------------!!****_ END OF SCRIPT _****!!-------------------------------------------------------------------------! -
September 7, 2022 at 4:08 pm
Erik Kostson
Ansys EmployeeNo worries - I would take away the LUMPM, but perhaps that will not do it. Most likely if material dimensions are OK, it is the Boundary conditions.
Use springs on all the nodes/points with boundary conditions – one spring (COMBIN14) for each direction so you need 3 springs (X,Y,Z) for each node/point where you apply your constraint/displacement boundary conditions. Then you will need to probably tune the spring stiffness to get better agreement between tests and FEA. Finally make sure you measure the mode shapes experimentally.
-
September 7, 2022 at 10:10 pm
victor.mcarv
SubscriberDo you have any examples of an application of the COMBIN14 element as a boundary condition? I see it needs 2 nodes as inputs, so would I need to create some extra nodes in order to apply this element?
-
-
September 7, 2022 at 6:48 pm
victor.mcarv
SubscriberThank you very much. I'm going to try it.
-
September 8, 2022 at 8:19 am
Erik Kostson
Ansys EmployeeSee the help manual (element reference) for more info on combin14 - also there are examples (e.g., VM197 - in the verification manual).
-
- You must be logged in to reply to this topic.

Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.

Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.

Ansys Blog
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- whether have the difference between using contact and target bodies
- What is the difference between bonded contact region and fixed joint
- How to calculate the residual stress on a coating by Vickers indentation?
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
-
2726
-
2146
-
1357
-
1150
-
462
© 2023 Copyright ANSYS, Inc. All rights reserved.