Tagged: lsdyna, LSDYNA Suite, lsdyna, R13.x, structuralmechanics


March 17, 2023 at 8:59 amFAQParticipant
LSDYNA offers a number of keywords for imposing loads on structures. For example, *LOAD_NODE_OPTION can be used for applying nodal forces and moments, *LOAD_SEGMENT_OPTION can be used for defining distributed loads over segments, while *LOAD_RIGID_BODY can be used for applying a concentrated force or moment at the center of mass of a rigid body. The load value is usually specified as a function of time through a load curve (*DEFINE_CURVE) that is referenced by the field LCID. However, this may not be convenient when a load is described by an analytical function of time or if the load also depends on other variables, such as the nodal coordinates. In such cases, the load can be specified by referencing a *DEFINE_FUNCTION or a *DEFINE_CURVE_FUNCTION card through the field LCID. As explained in the manual, *DEFINE_FUNCTION can be referenced by a limited number of keywords between which the arguments of the function can differ. For example, in *LOAD_NODE, the *DEFINE_FUNCTION card can be used with 7 arguments, namely the time, the three current coordinates of the node, and the three initial coordinates of the node at which the load is applied. On the other hand, in *LOAD_SEGMENT, the function has 10 arguments: the time, the current and initial coordinates at the segment centroid, and the three translational velocities at the segment centroid. Unless stated otherwise, the function arguments should be included in the correct order as stated in the manual. One of the common usages of *DEFINE_FUNCTION in *LOAD_SEGMENT is the application of hydrostatic or soil pressure. The example below applies a nodal force at nodes 2 and 4 which is proportional to the resultant displacement at node 2 and node 4, respectively. *LOAD_NODE_SET 1,1,1,1.0 *SET_NODE_LIST 1 2,4 *DEFINE_FUNCTION 1 f(t,x,y,z,x0,y0,z0)=5.0*sqrt((xx0)*(xx0)+ (yy0)*(yy0)+(zz0)*(zz0)) Functions that cannot be described with a simple arithmetic expression can be provided in the form of a script instead. The script is written in a Clike programming language and needs to be appended in the *DEFINE_FUNCTION card as shown below. The following example is used for applying a force that is equal to the product of a constant k times the X displacement at the node if this product is negative, else the force is set equal to zero. *DEFINE_FUNCTION 1 float force(float t, float x, float y, float z, float x0, float y0, float z0) { float result, k; k = 5.0; result = k*(xx0); if (result >= 0.0) result = 0.0; return result; } *DEFINE_CURVE_FUNCTION can be used in place of *DEFINE_CURVE. The curvefunction can reference other curve definitions, kinematic and force response quantities, intrinsic functions, and other quantities that are listed in the Manual Vol I. To output the value of the curve, *DATABASE_CURVOUT can be used. The curvefunction below is interpreted as follows. The function contains an expression that has a component proportional to the X displacement at node 2 and a second component proportional to the X velocity at the same node. The applied force is set equal to the result of the expression if that is negative, otherwise the applied force is set equal to zero. *LOAD_NODE 2,1,1,1.0 *DEFINE_CURVE_FUNCTION 1 IF(5.0*DX(2)0.01*VX(2),5.0*DX(2)0.01*VX(2),0.0,0.0)

Introducing Ansys Electronics Desktop on Ansys Cloud
The Watch & Learn video article provides an overview of cloud computing from Electronics Desktop and details the product licenses and subscriptions to ANSYS Cloud Service that are...
How to Create a Reflector for a Center HighMounted Stop Lamp (CHMSL)
This video article demonstrates how to create a reflector for a center highmounted stop lamp. Optical Part design in Ansys SPEOS enables the design and validation of multiple...
Introducing the GEKO Turbulence Model in Ansys Fluent
The GEKO (GEneralized KOmega) turbulence model offers a flexible, robust, generalpurpose approach to RANS turbulence modeling. Introducing 2 videos: Part 1Â provides background information on the model and a...
Postprocessing on Ansys EnSight
This video demonstrates exporting data from Fluent in EnSight Case Gold format, and it reviews the basic postprocessing capabilities of EnSight.
 The warning message is: “The maximum contact stiffness is too big. This may affect the accuracy of the results.” Why does large contact stiffness affect results accuracy?
 Contact Definitions in ANSYS Workbench Mechanical
 After Workbench crashes, how can I recover the project from a .mechdb file?
 Model has a large number of contacts – how to reduce them?
 How to resolve “Error: Invalid Geometry”?
 How to display the color of each body based on the material in Mechanical?
 Please explain the warning message “coefficient ratio exceeds 10e8” ?
 How to locate an element of a particular ID number in Mechanical?
 How to Connect Excel to Workbench
 How can I plot bodies colored by material property in Workbench?
Â© 2023 Copyright ANSYS, Inc. All rights reserved.