声振论坛

 找回密码
 我要加入

QQ登录

只需一步,快速开始

查看: 3911|回复: 6

[结构分析] ANSYS/LS-DYNA叶片冲击分析

[复制链接]
发表于 2005-11-17 08:09 | 显示全部楼层 |阅读模式

马上注册,结交更多好友,享用更多功能,让你轻松玩转社区。

您需要 登录 才可以下载或查看,没有账号?我要加入

x
  1. fini

  2. /clear

  3. ! blade.inp is a supplement to Chapter 11 (ANSYS/LS-DYNA Seminar)

  4. /title, Implicit-to-Explicit Sequential Solution

  5. ! Stress Initialization to Prescribed Geometry followed by Full Transient

  6. ! This is a simplified attempt to analyze the scenario when a
  7. ! jet engine fan blade snaps off and tears the engine apart

  8. /uis,abort,off ! do not display annoying status boxes...

  9. ! ===========================================================================

  10. /filnam,implicit ! implicit (ANSYS) portion of analysis

  11. /prep7
  12. /view,,1,2,3
  13. /ang,1

  14. ! Note: Only SHELL181 elements are used in this example, but other element
  15. ! types (e.g., SOLID185) can also be used. However, there is a set of
  16. ! companion element types that exist, which make the transition from/to
  17. ! implicit to/from explicit "automatic" (etchg used instead of emodif):
  18. !
  19. ! LINK8 ===> LINK160
  20. ! BEAM4 ===> BEAM161
  21. ! SHELL181 <===> SHELL163 (181 accepts 163 stresses & thicknesses)
  22. ! SOLID185 <===> SOLID164 (185 accepts 164 stresses at 5.6)
  23. ! COMBIN14 ===> COMBI165
  24. ! MASS21 ===> MASS166
  25. ! LINK10 ===> LINK167
  26. !
  27. ! The LS-DYNA link and beam elements require a third node, which is
  28. ! not always used in ANSYS, so these elements must be checked by the
  29. ! user. Also, SHELL181 accepts thickness and stress information from
  30. ! LS-DYNA. Prior to 5.6, it accepted the thicknesses and element
  31. ! force and moment information from SHELL163, which was then used to
  32. ! calculate the stresses that were already determined in LS-DYNA.
  33. ! If more than 5 integration points are used through the thickness
  34. ! (trapezoidal rule), then the old method of force and moment data
  35. ! is used. SOLID185 should have KEYOPT(2)=1 (i.e., uniform reduced
  36. ! integration with hourglass control) to be consistent with SOLID164.

  37. ! It's best to think in terms of "parts" when the model is being created,
  38. ! because ANSYS/LS-DYNA requires part definitions for many of its commands
  39. ! (EDLOAD, EDCGEN, EDREAD, etc). By issuing the EDPART,Create command,
  40. ! ANSYS/LS-DYNA automatically creates parts that are based on unique sets
  41. ! of MAT, REAL, and TYPE numbers used by elements (listed sequentially via
  42. ! the ELIST command). These part lists can be updated after the model has
  43. ! been changed (EDPART,Update) or listed (EDPART,List) at any time before
  44. ! the SOLVE or EDWRITE,ANSYS/TAURUS/both commands are issued, at which
  45. ! point, the part list is set.

  46. et,1,SHELL181 ! implicit shell elements for engine hub
  47. et,2,SHELL181 ! implicit shell elements for blade platform
  48. et,3,SHELL181 ! implicit shell elements for engine blades
  49. et,4,SHELL181 ! implicit shell elements for engine duct
  50. /eshape,1 ! show element thicknesses (to check model)

  51. r,1,0.50 ! thickness of hub (flywheel shape)
  52. r,2,0.50 ! fan blade platform thickness
  53. r,3,0.25 ! fan blade average thickness
  54. r,4,0.75 ! engine duct (housing) thickness

  55. ! Note: Only small strains using linear material properties are allowed
  56. ! in the implicit analysis, since only the resulting displacements
  57. ! will be used in the stress initialization portion (first part)
  58. ! of the explicit analysis. In other words, no path dependent
  59. ! features are allowed in the implicit run.

  60. mp, ex,1,30.0e6 ! modulus of hub (psi)
  61. mp,dens,1,7.33e-4 ! mass density of hub (lbf-sec^2/in^4)
  62. mp,nuxy,1,0.30 ! Poisson's ratio (unitless)

  63. mp, ex,2,30.0e6 ! modulus of blade platform (psi)
  64. mp,dens,2,7.33e-4 ! mass density of blade platform (lbf-sec^2/in^4)
  65. mp,nuxy,2,0.30 ! Poisson's ratio (unitless)

  66. mp, ex,3,30.0e6 ! modulus of blade (psi)
  67. mp,dens,3,7.33e-4 ! mass density of blade (lbf-sec^2/in^4)
  68. mp,nuxy,3,0.30 ! Poisson's ratio (unitless)

  69. mp, ex,4,30.0e6 ! modulus of engine duct (psi)
  70. mp,dens,4,7.33e-4 ! density of duct not used (lbf-sec^2/in^4)
  71. mp,nuxy,4,0.30 ! Poisson's ratio (unitless)

  72. k,1,0,0,0 ! create simplified jet engine geometry
  73. k,2,0,0,1
  74. l,1,2 ! line #1 used to generate geometry...
  75. lgen,2,1,,,5,0,0 ! inner radius of hub (line #2)
  76. ldiv,2 ! divide line #2 in half into lines #2 and #3
  77. lgen,2,2,3,,5,0,0 ! outer radius of hub (lines #4 and #5)
  78. l,5,7 ! line #6 represents web of hub
  79. local,11,1,0,0,0.5,0,0,90.0 ! local cs to twist blade
  80. lgen,2, 4, 5,,0, -5.0,1.0 ! root of blade (break point at radius = 11")
  81. lgen,2, 7, 8,,0,-12.5,1.5 ! create lines to "skin" blade...
  82. lgen,2, 9,10,,0,-12.5,1.5
  83. lgen,2,11,12,,0,-12.5,1.5
  84. lgen,2,13,14,,0,-12.5,1.5
  85. lgen,2,15,16,,0,-12.5,1.5
  86. lgen,2,17,18,,0,-12.5,1.5
  87. lsel,s,line,,7,20,1
  88. lesize,all,,,2 ! specify esize = 0.25" for blades ("axially")
  89. lsel,all

  90. csys,0 ! return to global coordinate system
  91. kmodif,1,0,0,-2 ! move end-points of origin line for duct
  92. kmodif,2,0,0, 3 ! duct axial length will be 5" for model...
  93. lgen,2, 1,,,21,0,0 ! line #21 at 21" radius (engine duct or housing)
  94. a,6,7,10,9 ! platform at base of blade (area #1)
  95. a,7,8,11,10 ! area #2
  96. askin,7,9,11,13,15,17,19 ! twisting shape of blade "skinned" (area #3)
  97. askin,8,10,12,14,16,18,20 ! area #4

  98. csys,1 ! use global cylindrical cs to copy blades, etc.
  99. lesize,2,,,1 ! specify esize = 0.5" at inner hub radius
  100. lesize,3,,,1 ! specify esize = 0.5" at inner hub radius
  101. arotat,2,3,,,,,1,2,360,4 ! ring at hub inner radius (areas #5 - #12)
  102. lesize,6,,,5 ! specify esize = 1" along hub web (radially)
  103. arotat, 6,,,,,,1,2,360,4 ! hub disk (web) section (areas #13 - #16)
  104. lesize,4,,,2 ! specify esize = 0.25" at hub outer radius
  105. lesize,5,,,2 ! specify esize = 0.25" at hub outer radius
  106. arotat,4,5,,,,,1,2,360,4 ! ring at hub outer radius (areas #17 - #24)
  107. lesize,21,,,5 ! specify esize = 1" for engine duct (axially)
  108. arotat,21,,,,,,1,2,360,4 ! engine housing (duct) ring (areas #25 - #28)
  109. nummrg,kp

  110. type,1 ! engine hub element type
  111. real,1 ! constant hub thickness used throughout
  112. mat,1 ! engine hub material
  113. esize,,9 ! coarse mesh used (hub will become rigid body)
  114. amesh,5,12 ! mesh hub inner ring
  115. amesh,13,16 ! mesh hub web (disk)
  116. amesh,17,24 ! mesh hub outer ring

  117. type,2 ! blade platform element type
  118. real,2 ! platform thicker than adjoining blade
  119. mat,2 ! blade platform material
  120. esize,,4 ! 4 divisions along length of blade platform
  121. amesh,1,2 ! mesh platform at base of blade (copy below)

  122. type,3 ! fan blade element type
  123. real,3 ! constant fan blade thickness used (I know ...)
  124. mat,3 ! fan blade material (only linear properties here)
  125. esize,,36 ! 36 divisions (esize = 0.25") along blade length
  126. amesh,3,4 ! mesh fan blade (copy below)

  127. agen,36,1,4,1, 0,10.0,0 ! generate all of the engine blades and platforms

  128. type,4 ! engine duct element type (not used here...)
  129. real,4 ! constant thickness cylindrical shape used
  130. mat,4 ! engine duct material
  131. esize,,9 ! use 36 element divisions circumferentially
  132. amesh,25,28 ! mesh the engine housing (duct or shroud)
  133. nummrg,kp

  134. csys,0 ! return to global coordinate system
  135. nummrg,node ! clean up any "loose ends" in the model...
  136. nummrg,kp

  137. ! Note: No nodes or elements may be introduced for the first time in the
  138. ! explicit portion of an implicit-to-explicit sequential analysis.
  139. ! All entities must be pre-defined in the implicit portion of the run,
  140. ! even if they are not used there. All of these elements in question
  141. ! must have all of the degrees of freedom (DOFs) of all of their
  142. ! nodes set to zero in the implicit run. Then, in the explicit run,
  143. ! the elements are converted to the companion type and the DOFs from
  144. ! the implicit run are deleted (and re-specified, as necessary). In
  145. ! this example, the pressure loading on the engine duct (100 psi?) is
  146. ! a second order effect and, is therefore, not modeled in the implicit
  147. ! part of the sequential solution. Another example would be the
  148. ! bird in a bird-strike analysis, which would probably best be modeled
  149. ! with SOLID185 elements and then completely restrained here. In the
  150. ! explicit run, the SOLID185 elements would be converted to SOLID164
  151. ! elements and the DOFs would be deleted. The corresponding keyopts,
  152. ! real constants, material properties, boundary conditions, and
  153. ! loading would still need to be defined in the explicit analysis...

  154. esel,s,type,,4 ! engine housing elements
  155. nsle ! engine housing nodes
  156. d,all,all,0.0 ! fix all DOFs of unused entities
  157. nsel,all
  158. esel,all

  159. fini
  160. /solu
  161. antype,static

  162. ! outpr,all,all
  163. outres,all,all

  164. omega,,,420.0 ! engine spin load (420.0 rad/sec = 4,010.7 rpm)
  165. esel,s,type,,1 ! engine hub elements (rigid body in explicit run)
  166. nsle ! engine hub nodes (not concerned with hub)
  167. d,all,all,0.0 ! fix engine hub to allow loading of fan blades
  168. nsel,all
  169. esel,all

  170. save
  171. eplot
  172. solve ! default solver used, but others OK, too
  173. fini

  174. /post1
  175. set,last
  176. /eshape,0
  177. /graphics,full
  178. /dscale,,1
  179. shell,bottom ! results for bottom layer of shell element
  180. plnsol,s,eqv ! blade maximum von Mises stress at root
  181. shell,top ! results for top layer of shell element
  182. plnsol,s,eqv ! blade maximum von Mises stress at root
  183. fini

  184. ! ===========================================================================

  185. /filnam,explicit ! explicit (LS-DYNA) portion of analysis

  186. /prep7
  187. etchg,ite ! convert SHELL181 elements to SHELL163 elements
  188. ! default settings automatically specified...

  189. ! Note: The EMODIF command may be used instead of the ETCHG command, but
  190. ! the latter is more automatic for "companion" elements (refer to the
  191. ! ANSYS/LS-DYNA User's Guide - Release 5.6 for details). In both cases,
  192. ! the shell element thicknesses, etc. still need to be re-specified...

  193. r,1,,3,0.50 ! hub (3 int. pts. through 0.5" thickness)
  194. r,2,,3,0.50 ! blade platform (same as above)
  195. r,3,,5,0.25 ! blades (5 int. pts. through 0.25" thickness)
  196. r,4,,5,0.75 ! duct (5 int. pts. through 0.75" thickness)

  197. edint,5 ! saves data for all 5 layers (blades and duct)

  198. esel,s,type,,1 ! hub elements
  199. nsle ! hub nodes
  200. ddele,all,all ! remove imposed displacements from implicit run
  201. edmp,rigid,1,7,4 ! convert hub to rigid body (only rotz = free)
  202. nsel,all
  203. esel,all

  204. ! Simulate one blade snapping off by unselecting a row of elements along the
  205. ! root. Alternatively, areas #1 and #2 could have been cleared (ACLEAR,1,2).

  206. asel,s,area,,1,2 ! blade platform areas of blade #1
  207. esla ! elements of first platform
  208. nsle ! corresponding nodes
  209. nsel,r,loc,x,10.7,11.1 ! reselect nodes of outer row of elements
  210. esln,s,1 ! select elements with all nodes active
  211. cm,esnap,elem ! row of elements to be unselected before SOLVE

  212. asel,s,area,,3,4 ! blade #1 (projectile)
  213. esla ! elements of first blade
  214. cm,eproj,elem ! element component for EDHIST command
  215. nsle ! nodes of first blade
  216. cm,nproj,node ! node component for EDHIST command
  217. asel,all
  218. nsel,all
  219. esel,all

  220. ! Use nonlinear (plastic) material properties for the fan blades:

  221. ! Note: First convert engineering stress versus engineering strain data
  222. ! into true stress versus true (hencky) strain data. Then subtract
  223. ! off the elastic true strain from the total true strain to find
  224. ! the plastic true strain, which is used with the total true stress
  225. ! in LS-DYNA *MAT_PIECEWISE_LINEAR_PLASTICITY material model #24.

  226. !--------------------------------------------------------------------------
  227. ! Stress-Strain Data used with Piecewise Linear Plasticity (Power Law 8):
  228. !--------------------------------------------------------------------------
  229. ! Total Total Total Total Elastic Plastic
  230. ! Stress/ Eng. Eng. True True True True
  231. ! Strain Stress Strain Stress Strain Strain Strain
  232. ! Point (psi) (in/in) (psi) (in/in) (in/in) (in/in)
  233. !--------------------------------------------------------------------------
  234. ! 1 0 0.0000 0 0.0000 0.0000 0.0000
  235. ! 2 60,000 0.0020 60,120 0.0020 0.0020 0.0000
  236. ! 3 77,500 0.0325 80,020 0.0320 0.0027 0.0293
  237. ! 4 83,300 0.0835 90,260 0.0802 0.0030 0.0772
  238. ! 5 98,000 0.1735 115,000 0.1600 0.0038 0.1562
  239. ! 6 98,300 0.2710 124,940 0.2398 0.0042 0.2356
  240. ! 7 76,400 1.2255 170,030 0.8000 0.0057 0.7943
  241. !--------------------------------------------------------------------------

  242. ! Note: The first point on the stress/strain curve is NOT entered.
  243. ! Start with the second point (where ordinate = yield stress).
  244. ! Also, please follow the limits imposed by the *SET command.

  245. *dim,strn,,6 ! define array for effective plastic true strain data
  246. *dim,strs,,6 ! define array for effective total true stress data

  247. strn(1)= 0.0, 0.0293, 0.0772, 0.1562, 0.2356, 0.7943 ! strain (in/in)
  248. strs(1)= 60120., 80020., 90260., 115000., 124940., 170030. ! stress (psi)

  249. edcurve,add,1,strn,strs ! load curve #1: abscissa=strain & ordinate=stress
  250. tb,plaw,3,,,8 ! specify power law #8 for material (MAT) #3
  251. tbdata,1,60120.0 ! yield stress, psi
  252. tbdata,3,0.30 ! set material failure at 30% true plastic strain
  253. tbdata,6,1 ! use load curve #1 for stress/strain data

  254. ! Note: Strain rate effects can be included by specifying the necessary
  255. ! strain rate parameters and the load curve defining the strain rate
  256. ! scaling effect on the yield stress. Please refer to Chapter 7
  257. ! (Material Models) of the ANSYS/LS-DYNA User's Guide for a complete
  258. ! description of this material model.

  259. ! Use nonlinear (plastic) material properties for the engine duct, to

  260. tb,plaw,4,,,8 ! specify power law #8 for material #4 (duct)
  261. tbdata,1,60120.0 ! yield stress, psi
  262. tbdata,3,0.50 ! set material failure at 50% true plastic strain
  263. tbdat,6,1 ! use load curve #1 for stress/strain data
  264. esel,s,type,,4 ! engine duct elements
  265. nsle ! engine duct nodes
  266. ddele,all,all ! remove imposed displacements from implicit run
  267. nsel,all
  268. esel,all

  269. ! Allow GUI to recognize batch-defined material input

  270. mpmod,1,7
  271. mpmod,2,1
  272. mpmod,3,28
  273. mpmod,4,28

  274. edcgen,ag ! automatic general contact

  275. fini
  276. /solu
复制代码
回复
分享到:

使用道具 举报

 楼主| 发表于 2005-11-17 08:10 | 显示全部楼层
  1. ! Using the REXPORT command, write the displacements (and rotations
  2. ! and temperatures) determined in the ANSYS implicit analysis to the
  3. ! ASCII "drelax" file. This command also sets the "m=drelax" option
  4. ! in the lsdyna script, prompting LS-DYNA to read the drelax file in.

  5. rexport,dyna,,,,,implicit,rst

  6. ! By issuing the EDDRELAX command, a stress initialization to a
  7. ! prescribed geometry analysis is requested. In a sequential
  8. ! implicit-to-explicit run, a "dynamic relaxation" analysis is
  9. ! performed in the pre-transient portion of the explicit analysis
  10. ! to preload the structure by imposing the deformed geometry over
  11. ! 101 time steps (with damping). The time during these 101 time
  12. ! steps can be thought of as "pseudo" time, since the time interval
  13. ! for the transient event begins at time equal to zero. Please
  14. ! note that, although the temperatures are being written to the
  15. ! "drelax" file, they are not currently being used. They will be
  16. ! supported in a later release. The remaining fields of the
  17. ! EDDRELAX command are ignored in an implicit-to-explicit analysis.

  18. eddrelax,ansys ! request stress initialization analysis...

  19. ! Impart initial spin velocity to nodes after stress initialization done

  20. esel,s,type,,1,3,1 ! spinning engine components
  21. nsle ! nodes of hub, blade platforms, and blades
  22. cm,nrots,node ! nodes initially spinning at 420.0 rad/sec

  23. edivelo,nrots, 0,0,0, 420, 0,0,0, 90,90,0 ! Phase field set automatically

  24. nsel,all
  25. esel,all

  26. ! Continue spinning load on hub (converted to a rigid body now).

  27. *dim,etime,,2 ! dimension explicit time array
  28. *dim,spin,,2 ! dimension spin loading array
  29. etime(1)=0.00 ! run time array out past termination time...
  30. etime(2)=0.02 ! time array duration = 0.02 seconds
  31. spin(1)=0.00 ! extending load curves facilitates restarts...
  32. spin(2)=8.40 ! 8.4 radians in 0.02 seconds = 420 rad/sec

  33. ! Note: The EDPART command is used to create, update, and list part IDs
  34. ! needed by the EDLOAD, EDCGEN, etc. commands. Please see Chapter
  35. ! 3 of the ANSYS/LS-DYNA 5.6 User''s Guide for more information
  36. ! concerning this topic.

  37. edpart,create ! create and list parts (part #1 = rigid body
  38. ! hub, #2=platforms, #3=blades, and #4=duct)

  39. ! Below, "rbrz" is used to apply a rigid body rotation about the z-axis,
  40. ! since there is no straight-forward method to apply an omega to the rigid
  41. ! body at 5.6 (without editing the explicit.k input file). The load curve
  42. ! specified is the equivalent of a constant omega of 420 radians per second.

  43. edload,add,rbrz,,1,etime,spin,0 ! Phase = 0 for sequential run (on part #1)

  44. ! The phase parameter on the EDLOAD command was added at ANSYS/LS-DYNA 5.4.
  45. ! The default value of zero is used for explicit transient loading in both
  46. ! a sequential implicit/explicit analysis and in an explicit-only analysis.
  47. ! In these cases, the load curve is applicable to the LS-DYNA transient
  48. ! portion of the run. The other two phase options are not valid in a
  49. ! sequential analysis. They are used for explicit-only cases of stress
  50. ! initialization by dynamic relaxation (phase=1) OR stress initialization
  51. ! by dynamic relaxation followed by a transient analysis (phase=2).

  52. nsel,s,loc,y,20.1,21.1 ! nodes on duct at wing attachment point
  53. d,all, ux,0.0,,,, uy, uz ! fix duct in translation to wing
  54. d,all,rotx,0.0,,,,roty,rotz ! fix duct in rotation to wing
  55. nsel,all
  56. esel,all

  57. cmsel,u,esnap ! unselect row of elements to "snap off" blade

  58. time,0.010 ! termination time (can continue with EDSTART)
  59. edrst,50 ! write data to results file 52 times (50+2)
  60. edhtime,50 ! write data to history file 52 times (50+2)
  61. edhist,eproj ! elements belonging to snapped off blade
  62. edhist,nproj ! nodes belonging to snapped off blade
  63. edenergy,1,1,1,1 ! output energies (hourglass, sliding interface ...)
  64. edout,glstat ! output LS-DYNA global energy file (ASCII)
  65. !!!edopt,add,,both ! write results for both ANSYS and LS-TAURUS/LS-POST
  66. edopt,add,,ansys ! write results for just ANSYS

  67. !!!edwrite,both,,k ! create LS-DYNA input file (explicit.k)
  68. edwrite,ansys,,k ! create LS-DYNA input file (explicit.k)

  69. save

  70. /eof

  71. ! Note: If the LS-DYNA solver is run directly (from outside of ANSYS),
  72. ! issue: /ansys56/bin/lsdyna56 i=explicit.k m=drelax

  73. solve ! overwrites the existing "explicit.k" input file and solves ...

  74. fini
  75. /post1
  76. /dscale,,1 ! set displacement magnification to one
  77. /view,,0.1,-0.75,0.65
  78. set,first
  79. layer,5 ! top layer of shell element
  80. plnsol,s,eqv ! von Mises equivalent stress plot
  81. layer,1 ! bottom layer of shell element
  82. plnsol,s,eqv ! von Mises equivalent stress plot

  83. andata,0.5,,2,1,33,2,0,1 ! animate every other frame up to substep 33 ...

  84. fini
  85. /exit

  86. !2345678901234567890123456789012345678901234567890123456789012345678901234567890

  87. ! Note: Stress data is available for each layer. For the fan blades and
  88. ! engine duct, five integration points are used (real constant NIP)
  89. ! and the results are saved for each layer (EDIMT,5). However,
  90. ! strain data is only available for the top and bottom layers.
  91. ! Although the LAYER,1 command gives both stress and strain data
  92. ! for the bottom layer, the LAYER,2 command gives stress data for
  93. ! the second layer, but gives strain data for the top layer (#5).
  94. ! To get stress data for the top layer, issue LAYER,5. Also, the
  95. ! explicit results are for the integration point locations, which
  96. ! are at the midplane of a given layer. To approximate surface
  97. ! stresses and strains, a sufficient number of integration points
  98. ! (layers) must be used through the thickness...
复制代码
发表于 2011-3-29 09:56 | 显示全部楼层
发表于 2011-3-29 19:28 | 显示全部楼层
介似嘛?
发表于 2011-3-29 20:00 | 显示全部楼层
大哥,编辑一下再发上来啊。。。
发表于 2011-4-1 16:28 | 显示全部楼层

这是论坛版本转换造成的,早期的帖子不少出现这种情况,不是编辑问题
发现这种情况联系管理员修复一下就好了
发表于 2011-7-20 14:26 | 显示全部楼层
这个要参考
您需要登录后才可以回帖 登录 | 我要加入

本版积分规则

QQ|小黑屋|Archiver|手机版|联系我们|声振论坛

GMT+8, 2024-11-26 09:29 , Processed in 0.079689 second(s), 18 queries , Gzip On.

Powered by Discuz! X3.4

Copyright © 2001-2021, Tencent Cloud.

快速回复 返回顶部 返回列表