S8-1PAT301, Section 8, October 2003 SECTION 8 LOAD & BOUNDARY CONDITIONS. - презентация

1 S8-1PAT301, Section 8, October 2003 SECTION 8 LOAD & BOUNDARY CONDITIONS

2 S8-2PAT301, Section 8, October 2003

3 S8-3PAT301, Section 8, October 2003 LOAD AND BOUNDARY CONDITIONS n Loads and boundary conditions are analysis code specific n They can be applied to geometry or finite elements u Loads and boundary conditions associated to geometry will be re-applied to new mesh after re-meshing the geometry, editing, etc. n Fields are used to define variations in loads or boundary conditions n Can use imported results from previous analysis – FEM field

4 S8-4PAT301, Section 8, October 2003 TYPES OF LOAD/BOUNDARY CONDITIONS n Some of the Load and Boundary Conditions that are supported u Displacement u Initial velocity u Inertial load u Force u Pressure u Distributed load u CID distributed load u Total load u Inflow u Outflow u Contact u Temperature u Heat source u Heat flux u Convection u Radiation l Also, view factor

5 S8-5PAT301, Section 8, October 2003 STRUCTURAL LOAD/BOUNDARY CONDITIONS SELECTION TEMPLATES n Load and boundary condition choices are dependent upon the specified analysis preference

6 S8-6PAT301, Section 8, October 2003 CREATING LOAD/BOUNDARY CONDITIONS n Select the appropriate Load/BC from the Object option box(i.e. Pressure, Temperature, Inflow, …) n Select the Load Case applicable to this load/boundary condition n We recommend not using more than 31 characters for set names n Enter Target Element Type if required (1-D, 2-D, or 3-D) n Input the appropriate data on the Input Data form n Specify region (Application Region) to apply the Load/BC to

7 S8-7PAT301, Section 8, October 2003 n Displacement boundary condition syntax u Translation and rotation LOAD/BCs INPUT DATA SYNTAX n The correct syntax is shown above the databoxes Null= free degree-of-freedom 0= fixed degree-of-freedom Non-zero number = enforced o or o Example -- : U x = U z = 0, U y = free

8 S8-8PAT301, Section 8, October 2003 EXAMPLE NODAL CONSTRAINTS n Markers displayed at visualization lines when Loads/BCs are applied to geometry Constraints for nodes on edge Translation Rotation

9 S8-9PAT301, Section 8, October 2003 APPLICATION REGION INPUT METHODS n Loads may be applied to FEM or Geometry entities n The Select Geometry Entities box and the Add button are used to select various application regions of the model n Clicking on Add will add the contents of the Select box to the Application Region n The contents of the Application Region can be edited using standard databox editing features n Clicking on OK will accept the entities in the Application Region box and close the form

10 S8-10PAT301, Section 8, October 2003 PRESSURE LOADING USING SPATIAL FIELDS n Specify pressure load as *COSR(T) in cylindrical coordinate system 1 u Create the spatial field using coordinate system 1 u Specify the field in Load/Boundary Conditions

11 S8-11PAT301, Section 8, October 2003 TIME DEPENDENT LOAD EXAMPLE 1. Create a time dependent field 2. Time dependent load case must first be defined prior to creating the load under Loads/BCs Time Pressure

12 S8-12PAT301, Section 8, October 2003 TIME DEPENDENT LOAD EXAMPLE (Cont.) 3. Create the load set The spatial and time dependence functions are multiplied

13 S8-13PAT301, Section 8, October 2003 FORCES IN AN ALTERNATIVE COORDINATE SYSTEM n Forces in radial direction of 100 are applied using Coordinate Frame Coord 3 n Coordinate Frame Coord 3 is cylindrical

14 S8-14PAT301, Section 8, October 2003 THERMAL LOAD & BOUNDARY CONDITIONS n Load & boundary conditions form is analysis code and analysis type sensitive. Shown are the load & boundary condition sets supported by MSC.Patran Thermal.

15 S8-15PAT301, Section 8, October 2003 CONVECTION HEAT TRANSFER EXAMPLE n Simulate a steady-state temperature distribution across an aluminum plate n Create a spatially varying convection coefficient along one edge using the field directive n Convection coefficient is specified under Loads/BCs m q=3000 W/m2 Aluminum Plate T=300K h=(1.5*y)+10 (W/m 2 K) Tambient=300 K 1 m

16 S8-16PAT301, Section 8, October 2003 THERMAL LOAD & BOUNDARY CONDITIONS n Varying edge Convection Coefficient is specified n The Application Region is determined by using the select menu (element, element edge, or free edges)

17 S8-17PAT301, Section 8, October 2003 PLOTTING LOADS/BCs n Fringe plots of any Loads/BCs can be plotted such as: u Temperatures u Components of a vector n The desired vector must be selected from the Select Data Variable box n The vectors must now be used to create a scalar for plotting n The plot can be applied to all of the groups in the current viewport n To display Loads/BCs set, applied to geometry, on the FEM, first, activate Show on FEM Only toggle in Display/Load/BC/El. Props form, then Plot Markers in the Loads/BCs form

18 S8-18PAT301, Section 8, October 2003 n Created load and boundary conditions can be verified using u Marker plots showing created Loads/BCs icons l Displacement l Rotation l Displacement and rotation l Temperature l Force u Contour plots of any scalar data quantity (fringe and element fill) u Display tables showing the Loads/BCs in a spreadsheet format SHOWING LOADS/BCs

19 S8-19PAT301, Section 8, October 2003 PLOTTING LOADS/BCs - EXAMPLE n Fringe plot of varying force is rendered for the elements in group FA_gp while the other elements in default_group are plotted with null data

20 S8-20PAT301, Section 8, October 2003 DISPLAY OF LOAD/BCs n Applied Loads/BCs become part of the graphics display. Screen refreshes and view changes will not remove them. n Control of all or individual Loads/BCs display is done through the Display/Load/BC/El. Props form n Allows color coding of Loads/BCs Markers n Evaluate load & boundary condition sets applied to geometry on finite elements by selecting Show on FEM Only n Labeling and scaling of vectors are adjusted in the Vectors/Filters section

21 S8-21PAT301, Section 8, October 2003 ASSOCIATION OF FINITE ELEMENTS TO GEOMETRY When geometry (i.e. curve, surface, solid) is meshed (i.e. IsoMesh, Paver) the mesh (finite elements) is associated automatically to the geometry If a mesh is imported onto geometry (i.e. File/Import, Finite Elements/Transform) it is not automatically associated to the geometry; it must be associated manually using Finite Elements: Associate It is important to have mesh associated to geometry if the Load/BCs are applied to the geometry and remeshing will be done later.

22 S8-22PAT301, Section 8, October 2003

23 S8-23PAT301, Section 8, October 2003 LOAD CASES

24 S8-24PAT301, Section 8, October 2003

25 S8-25PAT301, Section 8, October 2003 LOAD CASE CREATION n Group multiple load/boundary conditions n Static or time dependent n Priorities to add or overwrite load/boundary condition sets can be specified

26 S8-26PAT301, Section 8, October 2003 LOAD CASE CREATION (Cont.) n Load cases may be created prior to the creation of load/boundary conditions n Specify a load case name (not more than 31 characters) n Current load case is what Loads/BCs are assigned to n Select load case type u To specify time dependent load/boundary conditions it is necessary to first create time dependent load case n Resolving intersecting load/boundary conditions is done under Assign/Prioritize Loads/BCs

27 S8-27PAT301, Section 8, October 2003 ASSIGN/PRIORITIZE LOADS/BCs n Select the desired load/boundary conditions in Select Individual Loads/BCs section n Specify the scale factor for each LBC by clicking in a cell under Scale Factor, then input data in Scale Factor box n Prioritize intersecting load/boundary conditions by clicking in a cell under Priority, then enter the priority (e.g. 1)in Priority box

28 S8-28PAT301, Section 8, October 2003 EXERCISE Perform Workshop 11 Anchor Loads and Boundary Conditions Using a Field in your exercise workbook.