Preprocessing—creating the model with Abaqus/CAE

Create a three-dimensional, deformable, planar wire part. (Remember to use an approximate part size that is slightly larger than the largest dimension in your model.) Name the part Pipe, and use the Create Lines: Connected tool to sketch a horizontal line of length 5.0 m. Dimension the sketch as needed to ensure that the length is specified precisely.

The pipe is made of steel with a Young's modulus of 200 × 10⁹ Pa and a Poisson's ratio of 0.3. Create a linear elastic material named Steel with these properties. You must also define the density of the steel material (7800 kg/m³) because eigenmodes and eigenfrequencies will be extracted in this simulation and a mass matrix is needed for this type of procedure.

Next, create a Pipe profile. Name the profile PipeProfile, choose Thin-walled as the formulation, and specify an outer radius of 0.09 m and a wall thickness of 0.02 m for the pipe.

Create a Beam section named PipeSection. In the Edit Beam Section dialog box, specify that section integration will be performed during the analysis and assign material Steel and profile PipeProfile to the section definition.

Finally, assign section PipeSection to the pipe. In addition, define the beam section orientation with the approximate ${\mathbf{n}}_{\mathbf{1}}$-direction as the vector (0.0, 0.0, –1.0) (the default). In this model the actual ${\mathbf{n}}_{\mathbf{1}}$-vector will coincide with this approximate vector.

Create a dependent instance of the part named Pipe. For convenience, create geometry sets that contain the vertices at the left and right ends of the pipe and name them Left and Right, respectively. These regions will be used later to assign loads and boundary conditions to the model.

In this simulation you need to investigate the eigenmodes and eigenfrequencies of the steel pipe section when a 4 MN tensile load is applied. Therefore, the analysis will be split into two steps:

Create a general static step named Pull I with the following step description: Apply axial tensile load of 4.0 MN. The actual magnitude of time in this step will have no effect on the results; unless the model includes damping or rate-dependent material properties, “time” has no physical meaning in a static analysis procedure. Therefore, use a time period of 1.0. Include the effects of geometric nonlinearity, and specify an initial increment size that is 1/10 the total step time. This causes Abaqus/Standard to apply 10% of the load in the first increment. Accept the default number of allowable increments.

You need to calculate the eigenmodes and eigenfrequencies of the pipe in its loaded state. Thus, create a second analysis step using the linear perturbation frequency extraction procedure. Name the step Frequency I, and give it the following description: Extract modes and frequencies. Although only the first (lowest) eigenmode is of interest, extract the first eight eigenmodes for the model.

The default output database output requests created by Abaqus/CAE for each step will suffice; you do not need to create any additional output database output requests.

To request output to the restart file, select OutputRestart Requests from the main menu bar of the Step module. For the step labeled Pull I, write data to the restart file every 10 increments.

In the first step create a load named Force that applies a 4 × 10⁶ N tensile force to the right end of the pipe section such that it deforms in the positive axial (global 1) direction. Forces are applied, by default, in the global coordinate system.

The pipe section is clamped at its left end. It is also clamped at the other end; however, the axial force must be applied at this end, so only degrees of freedom 2 through 6 (U2, U3, UR1, UR2, and UR3) are constrained. Apply the appropriate boundary conditions to sets Left and Right in the first step.

In the second step you require the natural frequencies of the extended pipe section. This does not involve the application of any perturbation loads, and the fixed boundary conditions are carried over from the previous general step. Therefore, you do not need to specify any additional loads or boundary conditions in this step.

Seed and mesh the pipe section with 30 uniformly spaced second-order, pipe elements (PIPE32).

Before continuing, rename the model to Original. This model will later form the basis of the model used in the example discussed in Example: restarting the pipe vibration analysis.

Create a job named Pipe with the following description: Analysis of a 5 meter long pipe under tensile load.

Save your model in a model database file, and submit the job for analysis. Monitor the solution progress; correct any modeling errors and investigate the source of any warning messages, taking corrective action as necessary.