General Mechanical

General Mechanical

  1. All Channels
  2. General Mechanical
  3. Modal analysis of a 3D Truss

Modal analysis of a 3D Truss

Tagged: , ,

    • September 6, 2022 at 1:53 am
      victor.mcarv
      Subscriber

      I 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 Employee

       

       

       

      Truss 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
      Subscriber

      Thank 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 Employee

       

       

       

       

       

       

       

      We (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
      Subscriber

      Thank 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 model
      FINISH
      /CLEAR,NOSTART
      !
      !-------------------------------------------------------------------------!
      !****_                    2. INPUT                                   _****!
      !-------------------------------------------------------------------------!
      !
      ! 2.1 Material
      EMOD = 6.964E+10 ! [N/m^2] Young's modulus
      NU = 0.33 ! [adm] Poisson's ratio
      DEN = 2714.47 ! [kg/m^3] Density
      !
      ! 2.2 Cross sections
      ! 2.2.1 Primary elements (PRI)
      REP = 0.07620 ! [m] External radius
      ESP = 8.300E-3 ! [m] Thickness
      RIP = 0.06790 ! [m] Internal radius
      ARP = 3.757E-3 ! [m^2] Cross-sectional area
      IXXP = 9.785E-6 ! [m^4] Moment of inertia
      JP = 1.957E-5 ! [m^4] Polar moment of inertia
      ! 2.2.2 Secondary elements (SEC)
      RES = 0.03810 ! [m] External radius
      ESS = 6.300E-3 ! [m] Thickness
      RIS = 0.03180 ! [m] Internal radius
      ARS = 1.383E-3 ! [m^2] Cross-sectional area
      IXXS = 8.518E-7 ! [m^4] Moment of inertia
      JS = 1.704E-6 ! [m^4] Polar moment of inertia
      ! 2.2.3 Tertiary elements (TER)
      RET = 0.02540 ! [m] External radius
      EST = 4.800E-3 ! [m] Thickness
      RIT = 0.02060 ! [m] Internal radius
      ART = 6.937E-4 ! [m^2] Cross-sectional area
      IXXT = 1.855E-7 ! [m^4] Moment of inertia
      JT = 3.709E-7 ! [m^4] Polar moment of inertia
      !
      !-------------------------------------------------------------------------!
      !****_                    3. PRE-PROCESSING                          _****!
      !-------------------------------------------------------------------------!
      !
      /PREP7
      !
      /VIEW,1,1,2,3
      /REP,FAST
      !
      ! 3.1 Adding material
      MP,EX,1,EMOD
      MP,PRXY,1,NU
      MP,DENS,1,DEN
      !
      ! 3.2 Adding element type
      ET,1,LINK180
      !
      ! 3.3 Adding sections
      SECTYPE,1,LINK,,PRI
      SECDATA,ARP,
      !
      SECTYPE,2,LINK,,SEC
      SECDATA,ARS,
      !
      SECTYPE,3,LINK,,TER
      SECDATA,ART,
      !
      ! 3.4 Creating nodes
      ! 3.4.1 Bottom front chord
      N,1,0.00,0.00,0.00
      N,2,1.73,0.00,0.00
      N,3,3.46,0.00,0.00
      N,4,5.19,0.00,0.00
      N,5,6.92,0.00,0.00
      N,6,8.65,0.00,0.00
      N,7,10.53,0.00,0.00
      N,8,12.32,0.00,0.00
      N,9,13.96,0.00,0.00
      N,10,15.60,0.00,0.00
      N,11,17.24,0.00,0.00
      ! 3.4.2 Top front chord
      N,12,0.00,1.98,0.00
      N,13,1.73,1.98,0.00
      N,14,3.46,1.98,0.00
      N,15,5.19,1.98,0.00
      N,16,6.92,1.98,0.00
      N,17,8.65,1.98,0.00
      N,18,10.53,1.98,0.00
      N,19,12.32,1.98,0.00
      N,20,13.96,1.98,0.00
      N,21,15.60,1.98,0.00
      N,22,17.24,1.98,0.00
      ! 3.4.3 Bottom back chord
      N,23,0.00,0.00,-1.83
      N,24,1.73,0.00,-1.83
      N,25,3.46,0.00,-1.83
      N,26,5.19,0.00,-1.83
      N,27,6.92,0.00,-1.83
      N,28,8.65,0.00,-1.83
      N,29,10.53,0.00,-1.83
      N,30,12.32,0.00,-1.83
      N,31,13.96,0.00,-1.83
      N,32,15.60,0.00,-1.83
      N,33,17.24,0.00,-1.83
      ! 3.4.4 Top back chord
      N,34,0.00,1.98,-1.83
      N,35,1.73,1.98,-1.83
      N,36,3.46,1.98,-1.83
      N,37,5.19,1.98,-1.83
      N,38,6.92,1.98,-1.83
      N,39,8.65,1.98,-1.83
      N,40,10.53,1.98,-1.83
      N,41,12.32,1.98,-1.83
      N,42,13.96,1.98,-1.83
      N,43,15.60,1.98,-1.83
      N,44,17.24,1.98,-1.83
      !
      /PNUM,NODE,1 ! Show node numbers
      !
      ! 3.5 Creating elements
      ! 3.5.1 Primary elements
      TYPE,1
      MAT,1
      SECNUM,1
      ! 3.5.1.1 Bottom front chord
      EN,1,1,2
      EN,2,2,3
      EN,3,3,4
      EN,4,4,5
      EN,5,5,6
      EN,6,6,7
      EN,7,7,8
      EN,8,8,9
      EN,9,9,10
      EN,10,10,11
      ! 3.5.1.2 Top front chord
      EN,11,12,13
      EN,12,13,14
      EN,13,14,15
      EN,14,15,16
      EN,15,16,17
      EN,16,17,18
      EN,17,18,19
      EN,18,19,20
      EN,19,20,21
      EN,20,21,22
      ! 3.5.1.3 Bottom back chord
      EN,21,23,24
      EN,22,24,25
      EN,23,25,26
      EN,24,26,27
      EN,25,27,28
      EN,26,28,29
      EN,27,29,30
      EN,28,30,31
      EN,29,31,32
      EN,30,32,33
      ! 3.5.1.4 Top back chord
      EN,31,34,35
      EN,32,35,36
      EN,33,36,37
      EN,34,37,38
      EN,35,38,39
      EN,36,39,40
      EN,37,40,41
      EN,38,41,42
      EN,39,42,43
      EN,40,43,44
      ! 3.5.2 Secondary elements
      TYPE,1
      MAT,1
      SECNUM,2
      ! 3.5.2.1 Front in-panel diagonals
      EN,41,1,13
      EN,42,3,13
      EN,43,3,15
      EN,44,5,15
      EN,45,5,17
      EN,46,7,17
      EN,47,7,19
      EN,48,9,19
      EN,49,9,21
      EN,50,11,21
      ! 3.5.2.2 Bottom in-panel diagonals 
      EN,51,2,23
      EN,52,2,25
      EN,53,4,25
      EN,54,4,27
      EN,55,6,27
      EN,56,6,29
      EN,57,8,29
      EN,58,8,31
      EN,59,10,31
      EN,60,10,33
      ! 3.5.2.3 Top in-panel diagonals
      EN,61,12,35
      EN,62,14,35
      EN,63,14,37
      EN,64,16,37
      EN,65,16,39
      EN,66,18,39
      EN,67,18,41
      EN,68,20,41
      EN,69,20,43
      EN,70,22,43
      ! 3.5.2.4 Back in-panel diagonals
      EN,71,23,35
      EN,72,25,35
      EN,73,25,37
      EN,74,27,37
      EN,75,27,39
      EN,76,29,39
      EN,77,29,41
      EN,78,31,41
      EN,79,31,43
      EN,80,33,43
      ! 3.5.3 Tertiary elements
      TYPE,1
      MAT,1
      SECNUM,3
      ! 3.5.3.1 Front panel orthogonal elements
      EN,81,1,12
      EN,82,2,13
      EN,83,3,14
      EN,84,4,15
      EN,85,5,16
      EN,86,6,17
      EN,87,7,18
      EN,88,8,19
      EN,89,9,20
      EN,90,10,21
      EN,91,11,22
      ! 3.5.3.2 Bottom panel orthogonal elements
      EN,92,1,23
      EN,93,2,24
      EN,94,3,25
      EN,95,4,26
      EN,96,5,27
      EN,97,6,28
      EN,98,7,29
      EN,99,8,30
      EN,100,9,31
      EN,101,10,32
      EN,102,11,33
      ! 3.5.3.3 Top panel orthogonal elements
      EN,103,12,34
      EN,104,13,35
      EN,105,14,36
      EN,106,15,37
      EN,107,16,38
      EN,108,17,39
      EN,109,18,40
      EN,110,19,41
      EN,111,20,42
      EN,112,21,43
      EN,113,22,44
      ! 3.5.3.4 Back panel orthogonal elements
      EN,114,23,34
      EN,115,24,35
      EN,116,25,36
      EN,117,26,37
      EN,118,27,38
      EN,119,28,39
      EN,120,29,40
      EN,121,30,41
      EN,122,31,42
      EN,123,32,43
      EN,124,33,44
      ! 3.5.3.5 Out of panel diagonals
      EN,125,1,34
      EN,126,24,13
      EN,127,3,36
      EN,128,26,15
      EN,129,5,38
      EN,130,28,17
      EN,131,7,40
      EN,132,30,19
      EN,133,9,42
      EN,134,32,21
      EN,135,11,44
      !
      GPLOT ! Multiplot
      !
      ! 3.6 Boundary conditions
      ALLSEL,ALL  
      D,1,UX,0
      D,1,UY,0
      D,1,UZ,0
      D,23,UX,0
      D,23,UY,0
      D,23,UZ,0
      D,11,UY,0
      D,11,UZ,0
      D,33,UY,0
      D,33,UZ,0
      !
      !-------------------------------------------------------------------------!
      !****_                    4. PROCESSING                              _****!
      !-------------------------------------------------------------------------!
      !
      /SOLU
      !
      ! 4.1 Defining solution parameters
      ANTYPE,2 ! Modal analysis
      MODOPT,LANB,10,1E-1,100,,ON ! Block Lanczos, 10 modes, minimum frequency, maximum frequency, mode normalization
      EQSLV,SPARSE ! Sparse solver
      MXPAND,10,,,0 ! Expanding 10 modes
      LUMPM,1 ! Lumped mass approximation
      !
      ! 4.2 Solving
      SOLVE
      FINISH
      !
      !-------------------------------------------------------------------------!
      !****_                    5. POST-PROCESSING                         _****!
      !-------------------------------------------------------------------------!
      !
      /POST1
      SET,LIST
      !
      !-------------------------------------------------------------------------!
      !****_                     END OF SCRIPT                             _****!
      !-------------------------------------------------------------------------!
    • September 7, 2022 at 4:08 pm
      Erik Kostson
      Ansys Employee

      No 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
        Subscriber

        Do 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
      Subscriber

      Thank you very much. I'm going to try it.

    • September 8, 2022 at 8:19 am
      Erik Kostson
      Ansys Employee

      See the help manual (element reference) for more info on combin14 - also there are examples (e.g., VM197 - in the verification manual).

Viewing 7 reply threads
  • You must be logged in to reply to this topic.
Ansys Innovation Space

Simulation World 2022

Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.

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.

© 2022 Copyright ANSYS, Inc. All rights reserved.