- 积分
- 0
- 注册时间
- 2010-7-2
- 仿真币
-
- 最后登录
- 1970-1-1
|
发表于 2010-7-11 20:26:47
|
显示全部楼层
来自 江苏镇江
2. 錐形樑撞擊剛性牆
在本例中要分析錐形樑撞擊一面剛性牆的行為,目的是讓你熟悉以下內容:
1. 如何定義面接觸
2. 如何定義剛性平面,以及怎樣約束它
3. 如何定義物體的初速度(在該例中爲錐形樑)
4. 如何用DMAT出來描寫定義鋼樑及如何用MATRIG卡定義剛性牆
問題及分析模型有關資料如下
我們從在“Geometry”裏建立樑頂端的面開始。不過在此之前先建立三個點:
現在建立兩條線用於建立代表錐形樑頂端的面:
用Curve方法建立面:
Geometry/Create/Surface/Curve/Option=2 Curve
/Starting Curve=2/Ending Curve=3
通過將面1沿Z方向移動-40,同時將其尺寸增加一倍:
Geometry/Transform/Surface/Mscale
/Translation Vector <0 0 -40>/Rotation Matrix {2,0,0/0,2,0/0,0,2}
/Surface List=Surface1
同樣地,將面1沿Z方向移動0.25in,同時將其尺寸增加到原來的3倍,建立代表剛性牆的面3:
Geometry/Transform/Surface/Mscale
/Translation Vector=<0 0 0.25>/Rotation Matrix={3,0,0/0,3,0/0,0,3}
/Surface List=Surface1
在面1與面2之間建立實體1:
Geometry/Create/Solid/Surface/Option:2 Surface
/Starting Surface=1/Ending Surface=2
在樑的兩個端面上建立2×2的網格種子點:
Finite Elements/Create/Mesh Seed/Uniform
/Number of Elements=2/Curve 3 Surface 1.3 2.2 2.1
同樣地,在代表剛性板的面3上建立一個6×6的網格種子點:
Finite Elements/Create/Mesh Seed/Uniform
/Number of Elements = 6/Curve List =Surface 3.2 3.1
然後在樑的縱向建立40個網格種子點:
Finite Elements/Create/Mesh Seed/Uniform
/Number of Elements =40/Curve List = Solid 1.1.3
用Hexa8元素劃分樑的網格:
Finite Elements/Create/Mesh/Solid/Mesher=IsoMesh
/Element Topology=Hex8/Solid 1
用Quad4元素劃分剛性板的網格:
Finite Elements/Create/Mesh/Surface
/Element Topology=Quad4/Mesher=IsoMesh/Surface 3
建立一個名爲“beam”的組,將所有的體元素及其相關節點放入:
Group/Create/New group name=beam
/Add Entity Selection=選擇所有的體元素及其相關節點
同樣地建立一個名爲“Rigid_Plate”的組將所有的板元素及其節點放入:
Group/Create/New Group Name=Rigid_Plate
/Entity Selection=將所有板元素選入
建立一個名爲“vel”的組,將分別處於樑的兩個斷面上的兩個節點放入,用於速度與力的時間歷程輸出:
Group/Create/New Group Name=vel/Entity Selection=Node 5 365
用DMAT材料模型定義樑的材料特性:
Materials/Create/Isotropic/Manual Input/Material name=Steel
/Input Properties/Constitutive Model=ElasPlas(DMAT)
/Element Type=Lagrangian Solid/Yield Model=Von Mises
/Strain Rate Model=None/Failure Model=None
/Spallation Model=Spallation Pressure
用MATRIG材料模型定義剛性板的材料特性:
Materials/Create/Isotropic/Manual Input/Material name=rigid
/Input Properties/Constitutive Model=Rigid(MATRIG)
/Element Type=Shell
/Density=0.00078(密度與質量必須定義其中之一)/Ok/Apply
建立一個名爲“steel_beam”的物理特性用於錐形樑的定義:
Properties/Create/3D/Lagrangian Solid
/Property Set Name=steel_beam/Input properties
/Material Name=steel/OK
/Select Members=選取所有體元素/Add/Apply
建立一個名爲“Rigid_Plate”的物理特性用於板元素網格的定義:
Properties/Create/2D/Type=Shell/Property Set name=Rigid_Plate
/Input Properties/Material Name=rigid/Shell Thickness=1.0/OK
/Select Members=選擇所有的板元素/Add/Apply
定義樑具有10000 in/s的Z方向撞擊速度:
Loads/BCs/Create/Initial Velocity/Nodal
/New Set Name=initial_velocity/Input Data
/Trans Veloc=<0.,0.,10000>/OK/Select Application Region/FEM
/Select all beam nodes/Add/OK/Apply
定義板與樑之間的主從接觸(板爲主,樑爲從):
Loads/BCs/Create/Contact/Element Uniform
/Option=Master-Slave Surface/New Set Name=contact
/Select Application Region/Type=Master/Element Type=2D
/Surface=Both/Geometry Filter=FEM
/Select Entities=點擊滑鼠拖動游標將所有殼元素框入/Add
現在將類型改爲從屬型:
/Type=Slave/Element Type=3D/FEM/Application Region=Select the Face of the Solid Elements on the tip of the beam only
/Add/OK/Apply
(提示:爲了更方便的選取,只顯示出“beam”組。)
定義剛性板的約束:
Loads/BCs/Create/Rigid Body Object
/New Set Name=rigid_constraint/Input Data
/選擇UX UY UZ RX RY RZ/Select Application Region
/點擊滑鼠任選板上一節點/OK/Apply
現在我們可以定義輸出要求了。你可以從定義執行控制參數開始:
Analysis/Analyze/Input Deck/Translate
/Job name=tapered_beam/Execution Controls
/Execution Control Parameters…
要求輸出樑的等效應力,壓力與等效塑性應變:
Analysis/Analyze/Input Deck/Translate/Output Request
/Result Name=BEAM/File Type=Archive
/Result Type=Element Output/Steps for Output=0 thru end by 50
/Step Frequency for saving=10000/Add
/Select Groups for Output=beam/Entity Type=Lagrangian
/Result Types=Effective Stress/Pressure/Effective Plastic Strain
/Apply
(提示:按下Ctrl鍵後用滑鼠左鍵可作多項選擇)
同樣地,建立一個Archive文件儲存板的輸出資料:
Analysis/Analyze/Input Deck/Translate/Output Request
/Result Name=PLATE/File Type=Archive
/Result Type=Element Output/Steps for Output=0 thru end by 50
/Step Frequency for Saving=10000/Add
/Select Groups for Output=Rigid_Plate/Entity Type=Dummy
/Result Types=User_Specified
要求輸出樑端面上節點速度與力的時間歷程:
Analysis/Analyze/Input Deck/Translate/Output Request
/Result Name=VEL/File Type=Time History
/Result Type=Grid Point Output/Steps for Output=0 thru end by 2
/Step Frequency for saving = 10000/Add
/Select Groups for Output=vel
/Result Types=X,Y & Z Translational Velocities and Z-Force/Apply
要求材料總結的輸出:
Analysis/Analyze/Input Deck/Translate/Output Request
/Result Name=Energy/File Type=Material Summary
/Steps for Output=0 thru end by 2/Add/OK
/Apply(To Translate the Input Deck)
(提示:當你點擊“Apply”鍵,MSC.Patran圖形介面暫時消失,而在你的工作目錄下將産生一個名爲tapered_beam.dat的Dytran輸入檔。)
產生的Dytran輸入檔爲“tapered_beam”,儲存在你的目錄中。
在Unix平臺上進行作業,在你的工作目錄下鍵入以下命令:
dytran jid=tapered_beam
在NT平臺上則用MSC.Dytran圖形介面進行作業:
作業完成後,關閉原來的Patran資料庫,打開一個新的資料庫用於做後處理。這樣就不會損壞原來的資料庫。
將Archive文件“BEAM”與“PLATE”讀入:
Analysis/Read Archive File/Model And Results/Translate
/Select Archive File/選擇ARC文件“BEAM”與“PLATE”/Add/Apply
/Apply
看最終變形的Quick Plot:
Results/Create/Quick Plot/Select Result Cases=選擇最後一步/Select Fringe Result=Displacement
/Select Deformation Result=Displacement(將“Deform Attributes”下的“Scale Factor”設爲“True Scale”並且關閉“Show Max/Min Label”)
/Apply
接著看變形的動畫:
Results/Create/Deformation
/Select Result Case=選擇所有情況
/Select Deformation result=Displacement/Animate/Apply
建立關於等效應力雲形圖的動畫:
Results/Create/Fringe/Select Result Case=選擇所有情況
/Select Fringe Result=EFFSTS/Animate/Apply
現在來畫時間歷程曲線,先要讀入THS(Time History)文件:
Analysis/Read History File/Result/Translate/Select History File
/選擇所要的THS文件/Add/Apply/Apply
畫出樑頂端上的中心節點的Z方向的速度:
XY Plot/Action=Create/Object=Window/Name Window=w1/Apply
XY Plot/Action=Post/Object=Curve
/Post Curve=選擇“ZVEL_gp_5.curve”
同樣地畫出Z方向的力:
XY Plot/Action=Post/Object=Curve
/Post Curve=選擇“ZFORCE_gp_5.curve”
MSC.Dytran輸入檔 ex2_beam.dat
START
TIME=99999
CEND
ENDTIME=99999.99
ENDSTEP=1200
CHECK=NO
TITLE= Jobname is: beam
TLOAD=1
TIC=1
SPC=1
$ Output result for request: BEAM
TYPE (BEAM) = ARCHIVE
ELEMENTS (BEAM) = 1
SET 1 = 101 THRU 260
ELOUT (BEAM) = EFFSTS PRESSURE EFFPLS
STEPS (BEAM) = 0 thru end by 50
SAVE (BEAM) = 10000
$ Output result for request: ENERGY
TYPE (ENERGY) = MATSUM
STEPS (ENERGY) = 0 thru end by 2
$ Output result for request: PLATE
TYPE (PLATE) = ARCHIVE
ELEMENTS (PLATE) = 2
SET 2 = 1 THRU 36
ELOUT (PLATE) = ZUSER
STEPS (PLATE) = 0 thru end by 50
SAVE (PLATE) = 10000
$ Output result for request: VEL
TYPE (VEL) = TIMEHIS
GRIDS (VEL) = 3
SET 3 = 105 465
GPOUT (VEL) = XVEL YVEL ZVEL ZFORCE
STEPS (VEL) = 0 thru end by 2
SAVE (VEL) = 10000
$------- Parameter Section ------
PARAM,INISTEP,1e-7
PARAM,MINSTEP,1e-9
$------- BULK DATA SECTION -------
BEGIN BULK
$ --- Define 418 grid points ---
GRID 1 -3 3 0
......
GRID 469 2 -2 -40.25
$ --- Define 196 elements
$ -------- property set rigid_wall ---------
CQUAD4 1 1 1 2 9 8
......
CQUAD4 36 1 41 42 49 48
$ -------- property set steel_beam ---------
CHEXA 101 2 101 102 105 104 110 111+A000001
+A000001 114 113
......
CHEXA 260 2 456 457 460 459 465 466+A000160
+A000160 469 468
$ ========== PROPERTY SETS ==========
$ * rigid_wall *
PSHELL1 1 DUMMY
$ * steel_beam *
PSOLID 2 1
$ ========= MATERIAL DEFINITIONS ==========
$ -------- Material steel id =1
DMAT 1 .00783 1 1 1 1
EOSPOL 11.64e+09
SHREL 18.18e+08
YLDVM 1 1.4e+07
PMINC 1-3.8e+07
$ ======== Load Cases ========================
$ -------- Contact : contact
CONTACT 3 SURF SURF 1 2 +A000161
+A000161 V2 BOTH +A000162
+A000162 +A000163
+A000163 ON
$ Slave contact surface for contact
$
SURFACE 1 SEG 1
CFACE 1 1 101 1
CFACE 2 1 102 1
CFACE 3 1 103 1
CFACE 4 1 104 1
$
$ Master contact surface for contact
$
SURFACE 2 SEG 2
CFACE 5 2 1 1
......
CFACE 40 2 36 1
$
$ ------- Initial Velocity BC initail_velocity -----
SET1 4 101 THRU 469
TICGP 1 4 ZVEL 10000
$
$ add these manually
$
TLOAD1,1,2,,12
FORCE,2,2,,0.,0.,0.,0
$
RIGID,2,2,50.,,0.,0.,0.,,+
+,,0.,0.,0.,,,,,+
+,,1E20,,,1E20,,1E20
$
ENDDATA |
|