By Michelle Hayes,2014-10-05 07:13
5 views 0

    Answers 8

    Quasi-Static and Import Analysis

    Keywords Version

    Question W81: What analysis procedure is used in this input file? Answer: The analysis procedure is a natural frequency extraction

    (;FREQUENCY). The procedure option must immediately

    follow the ;STEP option.

    Question W82: In Abaqus a distinction is made between linear perturbation

    analysis steps and general analysis steps. What type of

    procedure is the analysis procedure in this input file? Answer: The ;FREQUENCY option is a linear perturbation procedure.

    Question W83: In an analysis with more than one step in the same input file,

    what influence does the result of a linear perturbation step

    have on the base state of the model for the following analysis


    Answer: None. Only general analysis steps change the base state of the


    Question W84: How does the order of the line segments affect the ability of

    Abaqus to resolve the contact condition?

    Answer: The order of the line segments determines the direction of the

    outward normal vector of the rigid surface. If the outward

    normal points in the wrong direction, Abaqus cannot establish

    the contact between the surfaces and, therefore, cannot find a


    ? Dassault Systèmes, 2008 Introduction to Abaqus/Standard and Abaqus/Explicit


    Question W85: What effect will an increase in friction have on the solution? Answer: An increased friction coefficient will increase the critical shear

    stress at which sliding of the blank begins. Thus, the crit

    material will be stretched more, causing further thinning of the

    material and increasing the stresses.

    Question W86: In Abaqus the input data are classified as either model or

    history data. What type of data is the contact pair definition in

    Abaqus/Explicit? What type of data is the contact pair

    definition in Abaqus/Standard?

    Answer: The contact pair definition is history data in Abaqus/Explicit

    and model data in Abaqus/Standard.

Question W87: When entering plasticity data with the ;PLASTIC option,

    what are the stress and strain measures that Abaqus uses? Answer: Abaqus uses true (Cauchy) stress and log strain.

    Question W88: What effects would a higher damping coefficient have? Answer: A higher damping coefficient would reduce the stable time

    increment. In general, damping should be chosen such that

    high frequency oscillations are smoothed or eliminated with

    minimal effect on the stable time increment. Figure WA81

    shows a plot of the kinetic energy with and without damping.

    Note the high frequency oscillations in the analysis without


    ? Dassault Systèmes, 2008 Introduction to Abaqus/Standard and Abaqus/Explicit


    Figure WA81. Kinetic energy with and without damping

    Question W89: What is the slope of the curve at the beginning and end, and

    why is this important?

    Answer: The slope of the amplitude curve at the beginning and end of

    the step is zero. This is important because it prevents

    discontinuities in the punch displacement that lead to

    oscillations in an Abaqus/Explicit analysis.

    Question W810: How would the results change if a linear amplitude definition

    were used instead?

    Answer: With a linear amplitude definition the displacement of the

    punch will be applied suddenly at the beginning of the step

    and stopped suddenly at the end of the step, causing

    oscillations in the solution.

    A linear amplitude definition results in large spikes in the

    kinetic energy, especially at the beginning of the step. As a

    result, the kinetic energy may be large compared to the

    internal energy and the early solution may not be quasi-static.

    The preferred approach is to move the punch as smoothly as

    possible. Figure WA82 compares the kinetic energy history

    ? Dassault Systèmes, 2008 Introduction to Abaqus/Standard and Abaqus/Explicit


    when a linear amplitude definition is used and when the

    smooth step amplitude definition is used.

    Figure WA82. Kinetic energy plot with and without SMOOTH STEP

    Question W811: How do you determine if an analysis that includes mass

    scaling produces acceptable results?

    Answer: The kinetic energy should be a small fraction of the internal


    As the kinetic energy increases, inertia effects have to be

    considered and the solution is no longer quasi-static.

    Figure WA81 shows the internal and kinetic energy for mass

    scaling factors of 10 (used in our simulation), 100, and 900,

    10which correspond to a solution speedup of , 10, and 30,


    ? Dassault Systèmes, 2008 Introduction to Abaqus/Standard and Abaqus/Explicit


    Figure WA83. Energies with different mass scaling

    Question W812: How does mass scaling affect the solution time? Answer: The stable time increment is calculated according to

    e ,(L!;?;tmin,stable!;cd,,

    ewhere L is a characteristic element length and c is the d

    dilatational wave speed. An increase in density decreases c, d

    which in turn increases t. stable

    Question W813: What elements are used to model the blank, and does this

    element type have an hourglass deformation mode? Answer: The analysis uses SAX1 elements. These elements have no

    hourglass modes. Consequently, hourglassing is not of

    concern in the analysis.

    Question W814: To what value should the UPDATE parameter on the

    ;IMPORT option be set if the total Mises stresses are to be

    plotted at the end of the springback analysis?

    ? Dassault Systèmes, 2008 Introduction to Abaqus/Standard and Abaqus/Explicit


    Answer: The UPDATE parameter should be set to NO. When the

    UPDATE parameter is set to YES, the deformed configuration

    of the previous analysis is used as the reference configuration

    for the import analysis. All stresses, strains, displacements, etc.

    are reported relative to the updated reference configuration

    and not as total values.

    Question W815: Where do you find the information to define the STEP and

    INTERVAL parameters on the ;IMPORT option?

    Answer: The status (.sta) file gives an overview of the progression on

    the analysis. Information about the number of steps and the

    number of increments completed in each step can be obtained

    from this file.

    In this analysis we wish to model the springback of the can

    after the forming of the can bottom is complete: this is


    Question W816: Why is it advantageous to choose Abaqus/Standard for the

    springback analysis?

    Answer: A true static procedure is the preferred approach for modeling

    springback. The imported model will not be in static

    equilibrium at the beginning of the step. Thus,

    Abaqus/Standard applies a set of artificial internal stresses to

    the imported model state and then gradually removes these

    stresses. This leads to the springback deformation. In

    Abaqus/Explicit the removal of the contact between the blank

    and the tools represents a sudden load removal, which leads to

    low frequency vibrations of the blank. While these vibrations

    will eventually dissipate, this approach leads to lengthy

    computation times.

    ? Dassault Systèmes, 2008 Introduction to Abaqus/Standard and Abaqus/Explicit

Report this document

For any questions or suggestions please email