Determining an appropriate step time

You can determine an appropriate step time.

Loading rates discusses the procedures for determining the appropriate step time for a quasi-static process. We can determine an approximate lower bound on step time duration if we know the lowest natural frequency, the fundamental frequency, of the blank. One way to obtain such information is to run a frequency analysis in Abaqus/Standard. In this forming analysis the punch deforms the blank into a shape similar to the lowest mode. Therefore, it is important that the time for the forming stage is greater than or equal to the time period for the lowest mode if you wish to model structural, as opposed to localized, deformation.

  1. Copy the existing model to a model named Frequency. Make all of the following changes to the Frequency model. In the frequency extraction analysis you will replace all existing steps with a single frequency extraction step. In addition, you will delete all of the rigid body tools and contact interactions; they are not necessary for determining the fundamental frequency of the blank.
  2. Add a density of 7800 to the material model Steel.
  3. Delete the die, holder, and punch part instances. These rigid parts are not necessary for the frequency analysis.

    Tip: You can delete any part instance using the Model Tree by expanding Instances underneath the Assembly container, clicking mouse button 3 on the instance name, and selecting Delete from the menu that appears.

  4. Replace the existing steps with a single frequency extraction step.
    1. Delete the step Move punch.
    2. In the Model Tree, click mouse button 3 on the step Holder force and select Replace from the menu that appears.
    3. In the Replace Step dialog box, select Frequency from the list of available Linear perturbation procedures. Enter the step description Frequency modes; select the Lanczos eigensolver option; and request five eigenvalues. Rename the step Extract Frequencies.
    4. Suppress the DOF Monitor.

    Note:

    Since the frequency extraction step is a linear perturbation procedure, nonlinear material properties will be ignored. In this analysis the left end of the blank is constrained in the x-direction and cannot rotate about the normal; however, it is not constrained in the y-direction. Therefore, the first mode extracted will be a rigid body mode. The frequency of the second mode will determine the appropriate time period for the quasi-static analysis in Abaqus/Explicit.

  5. Delete all contact interactions.
  6. Open the Boundary Condition Manager, and examine the boundary conditions in the Extract Frequencies step. Delete all boundary conditions except the boundary condition named CenterBC. This leaves the blank constrained with a symmetry boundary condition applied to the left end.
  7. Remesh the blank if necessary.
  8. Create a job named Forming-Frequency with the following job description: Channel forming -- frequency analysis. Submit the job for analysis, and monitor the solution progress.
  9. When the analysis is complete, enter the Visualization module and open the output database file created by this job. From the main menu bar, select PlotDeformed Shape; or use the tool in the toolbox.

The deformed model shape for the first vibration mode is plotted (it is a rigid body mode). Advance the plot to the second mode of the blank. Superimpose the undeformed model shape on the deformed model shape.

The frequency analysis shows that the blank has a fundamental frequency of 140 Hz, corresponding to a period of 0.00714 s. Figure 1 shows the displaced shape of the second mode. We now know that the shortest step time for the forming analysis is 0.00714 s.

Figure 1. Second mode of the blank from the Abaqus/Standard frequency analysis.