9
Loading
Chapter Chapter 9 - Loading
Overview
Training Manual
INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1
The solution step is where we apply loads on the object and let the solver calculate the finite element solution. Loads are available both in the Preprocessor and Solution menus.
February 7, 2006 Inventory #002268 9-2
Chapter 9 - Loading
A. Define Loads
There are five categories of loads:
DOF Constraints
Training Manual
INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1
Concentrated Loads Surface Loads Body Loads
Inertia Loads
Specified DOF values, such as displacements in a stress analysis or temperatures in a thermal analysis. Point loads, such as forces or heat flow rates. Loads distributed over a surface, such as pressures or convections. Volumetric or field loads, such as temperatures (causing thermal expansion) or internal heat generation. Loads due to structural mass or inertia, such as gravity and rotational velocity.
February 7, 2006 Inventory #002268 9-3
Chapter 9 - Loading
Define Loads
Training Manual
INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1
You can apply loads either on the solid model or directly on the FEA model (nodes and elements).
Solid model loads are easier to apply because there are fewer entities to pick. Moreover, solid model loads are independent of the mesh. You dont need to reapply the loads if you change the mesh.
Pressure on line
Pressures on element faces
Constraint on line Solid model FEA model
Constraints at nodes
Force at keypoint
Force at node
February 7, 2006 Inventory #002268 9-4
Chapter 9 - Loading
Define Loads
Training Manual
INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1
Regardless of how you apply the loads, the solver expects all loads to be in terms of the finite element model. Therefore, solid model loads are automatically transferred to the underlying nodes and elements during solution. Solid Model Loads can be transferred to the finite element mesh manually before solving by using the SBCTRAN command. This can be useful to see all of the loads, both solid model and FE, that have been applied.
For example, if a pressure is applied to an area, a plot of the elements will not show the pressure until the SBCTRAN command is issued or the model is solved.
February 7, 2006 Inventory #002268 9-5
Chapter 9 - Loading
B. Nodal Coordinate System
Training Manual
INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1
All forces, displacements, and other direction-dependent nodal quantities are interpreted in the nodal coordinate system.
Input quantities: Forces and moments FX, FY, FZ, MX, MY, MZ Displacement constraints UX, UY, UZ, ROTX, ROTY, ROTZ Coupling and constraint equations Etc. Output quantities: Calculated displacements UX, UY, UZ, ROTX, ROTY, ROTZ Reaction forces FX, FY, FZ, MX, MY, MZ Etc.
February 7, 2006 Inventory #002268 9-6
Chapter 9 - Loading
...Nodal Coordinate System
Training Manual
INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1
A nodal coordinate system is attached to every node in the model. By default, the nodal CS is parallel to Global Cartesian, i.e, all applied forces and displacement constraints are interpreted in Global Cartesian by default.
Yn
Xn
Yn
Xn Yn
Xn
Y X
Yn
Xn
February 7, 2006 Inventory #002268 9-7
Chapter 9 - Loading
...Nodal Coordinate System
If necessary, you can rotate the nodal CS to a different orientation. For example:
To simulate an inclined roller support. To apply radial forces. To apply radial constraints (perhaps to simulate a rigid, press-fitted pin).
Training Manual
February 7, 2006 Inventory #002268 9-8
INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1
Chapter 9 - Loading
...Nodal Coordinate System
To rotate nodes, use this four-step procedure:
1. Select the desired nodes. 2. Activate the coordinate system (or create a local CS) into which you want to rotate the nodes, e.g, CSYS,1. 3. Choose Main Menu > Preprocessor > Modeling > Move/Modify > Rotate Node CS > To Active CS, then press [Pick All] in the Or picker. issue NROTAT,ALL. 4. Reactivate all nodes.
Training Manual
INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1
Note: When you apply symmetry on anti-symmetry boundary conditions, ANSYS automatically rotates all nodes on that boundary.
Very Important: Nodal Coordinate Systems ALWAYS behave in a Cartesian manner. NROTAT simply aligns the nodal CS with a global or local CS. Consequently, remember that (a) there is no dependency or association of a nodal CS with a global/local CS to which it is rotated and (b) the nodal CS still acts as a Cartesian CS. February 7, 2006
Inventory #002268 9-9
Chapter 9 - Loading
...Nodal Coordinate System
Demo:
Training Manual
INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1
Resume rib.db. Offset working plane to center of bottom circle (using average keypoint location). Create local cylindrical CS at working plane origin. Select nodes at radius = 0.35 and plot them. Rotate all selected nodes into active system. Apply a UX displacement constraint (or an FX force) at all selected nodes. Note the radial direction. Now activate global Cartesian (CSYS,0). Rotate all selected nodes into active system. Replot, and note the new direction of the loads.
February 7, 2006 Inventory #002268 9-10
Chapter 9 - Loading
C. Displacement Constraints
Training Manual
INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1
Displacement constraints are also used to enforce symmetry or antisymmetry boundary conditions.
Symmetry BC: Out-of-plane displacements and in-plane rotations are fixed. Antisymmetry BC: In-plane displacements and out-of-plane rotations are fixed.
Y X
Symmetry Boundary UX=0 ROTY=ROTZ=0
Antisymmetry Boundary UY=UZ=0 ROTX=0
February 7, 2006 Inventory #002268 9-11
Chapter 9 - Loading
D. Concentrated Forces
A force is a concentrated load (or point load) that you can apply at a node or keypoint. Point loads such as forces are appropriate for line element models such as beams, spars, and springs. In solid and shell models, point loads usually cause a stress singularity, but are acceptable if you ignore stresses in the vicinity. Remember, you can use select logic to ignore the elements in the vicinity of the point load.
Training Manual
INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1
February 7, 2006 Inventory #002268 9-12
Chapter 9 - Loading
...Concentrated Forces
Training Manual
INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1
In the 2-D quarter symmetry solid model shown at bottom left, notice that maximum stress SMAX (23,590) is reported at the location of the force. When the nodes and elements in the vicinity of the force are unselected, SMAX (12,281) moves to the bottom left corner, which is another singularity due to the reentry corner. Reflected about x-z plane
half symmetry model
reentry corner
February 7, 2006 Inventory #002268 9-13
Chapter 9 - Loading
Concentrated Forces
Training Manual
INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1
By unselecting nodes and elements near the bottom left corner, you get the expected stress distribution with SMAX (7,945) near the top hole.
February 7, 2006 Inventory #002268 9-14
Chapter 9 - Loading
Concentrated Forces
Note that for axisymmetric models: Input values of forces are based on the full 360. Output values (reaction forces) are also based on the full 360.
Training Manual
INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1
For example, suppose a cylindrical shell of radius r has an edge load of P lb/in. To apply this load on a 2-D axisymmetric shell model (SHELL51 elements, for example), you would specify a force of 2rP.
P lb/in
2rP lb
r
February 7, 2006 Inventory #002268 9-15
Chapter 9 - Loading
E. Verifying Loads
Verifying applied loads Plot them by activating load symbols:
Utility Menu > PlotCtrls > Symbols Commands -- /PBC, /PSF, /PBF
Training Manual
INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1 INTRODUCTION TO ANSYS - Part 1
Or list them:
Utility Menu > List > Loads >
February 7, 2006 Inventory #002268 9-16