Abaqus/Explicit forming analysis

The goal of the forming process is to quasi-statically form a channel with a punch displacement of 0.03 m. In selecting loading rates for quasi-static analyses, it is recommended that you begin with faster loading rates and decrease the loading rates as necessary to converge on a quasi-static solution more quickly. However, if you wish to increase the likelihood of a quasi-static result in your first analysis attempt, you should consider step times that are a factor of 10 to 50 times slower than that corresponding to the fundamental frequency. In this analysis you will start with a time period of 0.007 s for the forming analysis step, which is based on the frequency analysis performed in Abaqus/Standard, which shows that the blank has a fundamental frequency of 140 Hz, corresponding to a time period of 0.00714 s. This time period corresponds to a constant punch velocity of 4.3 m/s. You will examine the kinetic and internal energy results carefully to check that the solution does not include significant dynamic effects.

This page discusses:

Creating the Abaqus/Explicit forming analysis

Copy the Standard model to a model named Explicit. Make all subsequent model changes to the Explicit model. To begin, edit the Steel material definition to include a mass density of 7800 kg/m3.

A concentrated force will be applied to the blank holder. To compute the dynamic response of the holder, a point mass must be assigned to its rigid body reference point. The actual mass of the holder is not important; what is important is that the mass should be of the same order of magnitude as the mass of the blank (0.78 kg) to minimize noise in the contact calculations. Choose a point mass value of 0.1 kg. To assign the mass, expand Engineering Features underneath the Holder in the Parts container in the Model Tree. In the list that appears, double-click Inertias. In the Create Inertia dialog box that appears, enter the name PointMass and click Continue. Select the reference point of the holder, and assign it a mass of 0.1 kg.

For the first attempt of this metal forming analysis, you will use tabular amplitude curves with the default smoothing parameter for both the application of the holder force and the punch stroke. Create a tabular amplitude curve for application of the holder force named Ramp1 using the data in Table 1. Define a second tabular amplitude curve for the punch stroke named Ramp2 using the data in Table 2.

Table 1. Ramp amplitude data for Ramp1 and Smooth1.
Time (sec) Amplitude
0.0 0.0
0.0001 1.0
Table 2. Ramp amplitude data for Ramp2 and Smooth2.
Time (sec) Amplitude
0.0 0.0
0.007 1.0

As with the Abaqus/Standard analysis, you will need two steps for the Abaqus/Explicit analysis. In the first step the holder force is applied; in the second step the punch stroke is applied. Delete the step named Move punch. Replace the step named Holder force with an explicit dynamics step, and specify a time period of 0.0001 s. This time period is appropriate for the application of the holder force because it is long enough to avoid dynamic effects but short enough to prevent a significant impact on the run time for the job. Enter Apply holder force as the step description. Create a second explicit dynamics step named Move punch with a time period of 0.007 s. Enter Apply punch stroke as the step description.

To help determine how closely the analysis approximates the quasi-static assumption, the various energy histories will be useful. Especially useful is comparing the kinetic energy to the internal strain energy. The energy history is written to the output database file by default. Modify the history output request for the punch reference node to request output at 200 evenly spaced intervals.

Open the Load Manager, and modify the concentrated force named RefHolderForce in the step named Holder force so that the amplitude definition for this load is set to Ramp1.

Change the displacement boundary condition RefPunchBC in the Move punch step so that U2 is set to –0.03 m in the step. Use the amplitude curve Ramp2 for this boundary condition.

Monitoring the value of a degree of freedom

In this model you will monitor the vertical displacement (degree of freedom 2) of the punch's reference node throughout the step. Because the DOF Monitor was set to monitor the vertical displacement of RefPunch in the Abaqus/Standard forming analysis, you do not need to make any changes.

Mesh creation and job definition

Change the family of the elements used to mesh the blank to Explicit, and specify enhanced hourglass control.

Create a job named Forming-1. Give the job the following description: Channel forming -- attempt 1.

Before you run the forming analysis, you may wish to know how many increments the analysis will take and, consequently, how much computer time the analysis requires. You can use the Verify Mesh tool to obtain an estimate of the stable time increment (the option is located in the Size Metrics tabbed page of the Verify Mesh dialog box). Knowing the stable time increment, which in this case does not change much from increment to increment, you can determine how many increments are required to complete the forming stage. Once the analysis begins, you can get an idea of how much CPU time is required per increment and, consequently, how much CPU time the analysis requires.

The stable time increment for this analysis is approximately 3.8 × 10−8 s. Therefore, the forming stage requires approximately 185,000 increments for a step time of 0.007 s.

Save your model to a model database file, and submit the job for analysis. Monitor the solution progress; correct any modeling errors that are detected, and investigate the cause of any warning messages.

Once the analysis is underway, an X–Y plot of the values of the degree of freedom that you selected to monitor (the punch's vertical displacement) appears in a separate viewport. From the main menu bar, select Viewport DOF Monitor: Forming-1 to follow the progression of the punch's displacement in the 2-direction over time as the analysis runs.