About Explicit Dynamic Steps

Advantages of the Explicit Method

The use of small increments (dictated by the stability limit) is advantageous because it allows the solution to proceed without iterations and without requiring tangent stiffness matrices to be formed. It also simplifies the treatment of contact.

The explicit dynamics procedure is ideally suited for analyzing high-speed dynamic events, but many of the advantages of the explicit procedure also apply to the analysis of slower (quasi-static) processes. A good example is sheet metal forming, where contact dominates the solution and local instabilities might form due to wrinkling of the sheet.

The results in an explicit dynamics analysis are not automatically checked for accuracy as they are in Abaqus/Standard (Abaqus/Standard uses the half-increment residual). In most cases this is not of concern because the stability condition imposes a small time increment such that the solution changes only slightly in any one time increment, which simplifies the incremental calculations. While the analysis might take an extremely large number of increments, each increment is relatively inexpensive, often resulting in an economical solution. It is not uncommon for Abaqus/Explicit to take over 105 increments for an analysis. The method is, therefore, computationally attractive for problems where the total dynamic response time that must be modeled is only a few orders of magnitude longer than the stability limit; for example, wave propagation studies or some “event and response” applications.

Time Incrementation

The time increment used in an explicit dynamic analysis must be smaller than the stability limit of the central-difference operator. Failure to use a small enough time increment will result in an unstable solution. When the solution becomes unstable, the time history response of solution variables such as displacements will usually oscillate with increasing amplitudes. The total energy balance will also change significantly. If the model contains only one material type, the initial time increment is directly proportional to the size of the smallest element in the mesh. If the mesh contains uniform size elements but contains multiple material descriptions, the element with the highest wave speed will determine the initial time increment. In nonlinear problems—those with large deformations and/or nonlinear material response—the highest frequency of the model will continually change, which consequently changes the stability limit. Abaqus/Explicit has two strategies for time incrementation control: fully automatic time incrementation (where the code accounts for changes in the stability limit) and fixed time incrementation.

Time Increment Scaling

To reduce the chance of a solution going unstable, you can adjust the stable time increment computed by Abaqus/Explicit by a constant scaling factor. This factor can be used to scale the default global time estimate, the element-by-element estimate, or the fixed time increment based on the initial element-by-element estimate; it cannot be used to scale a fixed time increment specified directly by you.

Automatic Time Incrementation

The default time incrementation scheme in Abaqus/Explicit is fully automatic and requires no user intervention. Two types of estimates are used to determine the stability limit: element by element and global. An analysis always starts by using the element-by-element estimation method and might switch to the global estimation method under certain circumstances, as explained below.

Element-by-Element Estimation

In an analysis Abaqus/Explicit initially uses a stability limit based on the highest element frequency in the whole model. This element-by-element estimate is determined using the current dilatational wave speed in each element. The element-by-element estimate is conservative; it will give a smaller stable time increment than the true stability limit that is based upon the maximum frequency of the entire model. In general, constraints such as boundary conditions and kinematic contact have the effect of compressing the eigenvalue spectrum, and the element-by-element estimates do not take this into account. The concept of the stable time increment as the time required to propagate a dilatational wave across the smallest element dimension is useful for interpreting how the explicit procedure chooses the time increment when element-by-element stability estimation controls the time increment. As the step proceeds, the global stability estimate, if used, will make the time increment less sensitive to element size.

Global Estimation

The stability limit will be determined by the global estimator as the step proceeds unless the element-by-element estimation method is specified, fixed time incrementation is specified, or one of the conditions explained below prevents the use of global estimation. The switch to the global estimation method occurs once the algorithm determines that the accuracy of the global estimation method is acceptable. The adaptive, global estimation algorithm determines the maximum frequency of the entire model using the current dilatational wave speed. This algorithm continuously updates the estimate for the maximum frequency. The global estimator will usually allow time increments that exceed the element-by-element values. Abaqus/Explicit monitors the effectiveness of the global estimation algorithm. If the cost for computing the global time estimate is more than its benefit, the code will turn off the global estimation algorithm and simply use the element-by-element estimates to save computation time.

Fixed Time Incrementation

A fixed time incrementation scheme is also available in Abaqus/Explicit. The fixed time increment size is determined either by the initial element-by-element stability estimate for the step or by a user-specified time increment. Fixed time incrementation might be useful when a more accurate representation of the higher mode response of a problem is required. In this case a time increment size smaller than the element-by-element estimates might be used. The element-by-element estimate can be obtained simply by running a data check analysis (see Abaqus/Standard and Abaqus/Explicit execution). When fixed time incrementation is used, Abaqus/Explicit will not check that the computed response is stable during the step. You should ensure that a valid response has been obtained by carefully checking the energy history and other response variables. Basing the fixed time increment size on the initial element-by-element stability limit You can use time increments the size of the initial element-by-element stability limit throughout a step. The dilatational wave speed in each element at the beginning of the step is used to compute the fixed time increment size.

Output

The element output available for a dynamic analysis includes stress; strain; energies; and the values of state, field, and user-defined variables. The nodal output available includes displacements, velocities, accelerations, reaction forces, and coordinates. All of the output variable identifiers are outlined in Abaqus/Explicit output variable identifiers.