ADINA Dynamic Impact Analysis of a Linear Spring-Damper and Mass System
Model Definition
This article demonstrates the ability of ADINA to analyze a dynamic impact event and yield results that converge to an analytic solution. A general discussion on convergence and contact modeling is provided.
Mass, Stiffness, and Damping
The model consists of a 50 lbs mass supported by a linear spring-damper. The linear spring-damper has a stiffness of 75 lbs/in and a damping rate of 2.5 lbs-s/in. It is modeled using a Nastran CBUSH1D element. The lower end of the spring-damper element is rigidly connected to a contact sphere. The contact sphere is modeled with massless shell elements that are sufficiently thick such that it behaves like a rigid body. The ground surface is also modeled with massless shell elements.
Loads and Boundary Conditions
All nodes on the ground are assigned a fixed constraint. The mass node is assigned a 12456 constraint, to provide stability to the model where only the Z-degree of freedom is relevant. All nodes of the spring-damper and mass system are assigned an initial velocity of -92.16 in/s, which is consistent with the system being dropped from a height of 11 inches above the ground surface. Gravity is modeled as a body load with a z-acceleration of -386.09 in/s^2.
Time Step and Integration Settings
A time step of 0.002 seconds is used for this analysis. Default parameters are used for time integration and nonlinear solution settings.
Ground Contact Definition
A contact connection is defined between the ground surface elements and the contact sphere elements. The connection property is shown in the image below. The connection property is defined in Femap using the 'Adv Nonlin (601)' tab on the Connection Property dialog. The 'Type' is set to '0. Contact'; the 'Contact Type' is set to '0. Constrain Function'; and the 'Compliance Factor' is set at 0.00075. Some discussion on the impacts and sensitivities of the contact parameters are discussed below. Please note that any friction settings are irrelevant here, since this problem is constrained as a single degree of freedom analysis.
Analysis Results
Comparison of ADINA Results to the Analytic Solution
The results below illustrate good correlation between the time histories of the analytic solution and the ADINA solution. The time histories shown are of the strut length (8 inches undeformed), velocity of the supported mass element, system load factor, and ground penetration (distance that the contact sphere nodes overlap ground surface nodes).
ADINA predicts the strut length at peak compression to be 5.29 inches (-0.44% error) and the peak load factor to be 5.38 g's (0.59% error). ADINA predicts the steady state condition exactly (0% error).
The amplitudes of two peaks in the response can be used to calculate the system damping. This calculation, shown below, matches the input 2.5 lbs-s/in damping rate.
Contact Parameters and Convergence
Many analysis parameters can impact solution convergence, but a couple key ones for dynamic contact problems are the time step and the contact parameters. The sensitivity to time step size is not studied here. In general, a smaller time step will help aid model convergence while increasing run time. The time step of 0.002 seconds used in this analysis seems sufficient to accurately capture the response of the system and resolve the peak load factor.
Compliant contact (constraint function type) is used in this analysis. The compliance factor is a numerical value that allows the contact nodes to overlap by some amount. A lower compliance factor means less overlap (penetration) is allowed. In effect, a lower compliance factor means a more rigid contact condition.
In general, increasing the compliance factor can aid model convergence. Allowing the contact nodes to penetrate offers more time for contact forces to develop, which reduces numerical noise and oscillations. The image below shows what happens to the system accelerations and forces when the compliance factor is decreased. Additionally, using the default settings for a 'Rigid Target' contact results in significant high-frequency oscillations. The solution is still able to converge, but that is not always the case for practical applications and more detailed models.
When using compliant contact, it is important to look at the resulting penetration. Ideally the penetration is small relative to the global displacements of the system. It is best practice to find the smallest compliance factor that allows the model to converge with minimal high-frequency oscillations in the acceleration and force output. ADINA offers several other solution parameters that can be used to aid model convergence, such as contact force damping, a nonlinear line search algorithm, and time integration coefficients.
Related Articles
ADINA Structures TRANSOR for Femap Menu: Run and Monitor Analysis
Run an ADINA Analysis Access the ADINA Analyze menu as shown below. Use the Analyze menu to control the analysis filename headings and file locations; control the allocated memory; and initiate an analysis using one of the menu buttons indicated ...ADINA Structures and Appropriate Model Fidelity for Dynamic Analysis
What is ADINA Structures? ADINA (Automatic Dynamic Incremental Nonlinear Analysis) Structures is a finite element solver that provides state-of-the-art stress capabilities for the analysis of solids and structures. The analysis can be linear or ...ADINA Dynamic Analysis Using Femap
What is in this webinar? SDA Engineer Tyler Chetto presents this webinar on ADINA Dynamic Analysis Using FEMAP v2022.2. During this webinar you will learn about: Creating dynamic finite element models (FEMs) Setting up and running dynamic analysis ...ADINA Structures TRANSOR for Femap Menu: Analysis Settings
ADINA Structures Analysis Settings Menu Access the Analysis Settings menu as shown below. This menu is where the ADINA Structures analysis type is defined. The menu options do vary based on which analysis type is selected. For the dynamic analyses, ...ADINA Structures TRANSOR for Femap Menu: Output Requests
ADINA Structures Output Requests Access the Output Requests menu as shown below. Use this menu to control the output file format and which output data is included. Note that Velocities and Accelerations are not included by default, but these are ...