Department of Engineering

IT Services

The ABAQUS FAQ


10. ABAQUS - Analysis

Q10.1 : What is the difference between "General" and "Perturbation" steps?

Most complex analysis are likely to have a sequence of steps. For example consider an analysis with four steps (see figure below). In step 1 the structure could be subjected to a static loading. Step 2 could be a frequency step. Step 3 could be further loading and step 4 another frequency step. The frequency steps 2 and 4 would be dependent on the state reached at the end of the previous steps (namely 1 and 3). This is generally true for any type of analysis with more than one step. The behaviour of the structure is dependent on the state at the end of the previous step.

An analysis step during which the response is nonlinear is called general analysis step. An analysis step during which the response is linear is called a linear perturbation step. A linear perturbation analysis step provides the linear response of the system about the base state ie the state at the end of the last nonlinear analysis step prior to the linear perturbation step. In the above example the state at the end of step 1 forms the base state for the frequency response in step 2.
Also because the step 2 is a perturbation step it has no influence on the response in step 3 which only depends on the results at the end of step 1. Similarly for step 5 the base state is the state at the end of step 3.

The following procedures are purely linear perturbation procedures (The references made are to the User's manual version 6.3):
  • BUCKLE (Section 6.2.3)
  • FREQUENCY (Section 6.3.4)
  • MODAL DYNAMIC (Section 6.3.5)
  • RANDOM Response (Section 6.3.9)
  • RESPONSE SPECTRUM (Section 6.3.8)
  • STEADY STATE DYNAMICS (Section 6.3.6)

A STATIC step could be made into a perturbation step by including the PERTURBATION parameter on the *STEP keyword.
*STEP, PERTURBATION
*STATIC 

Omitting this parameter implies that a general *STATIC analysis is required.
Each step has step time. The total time is the accumulation of the step times of all the general steps in an analysis. The step times of all perturbation steps are omitted from this.
Similarly all results quantities are accumulated values from all the general steps in an analysis. The results output in the perturbation steps are incremental values about the base state.


Q10.2 : How do I carry out a non-linear analysis where there is a possibility of instability?

Geometrically nonlinear static problems frequently involve buckling or collapse behaviour, where the load-displacement response shows a negative stiffness. The static equilibrium states during the unstable phase of the response can be found by using the ``modified Riks method''. This method is selected by including the RIKS parameter on the *STATIC keyword (Section 6.2.4 of the User's manual version 6.3).

In a large deformation analysis the effect of geometric nonlinearity can be significant. Use the NLGEOM option with the *STEP keyword to take into account the changes in geometry during the analysis. Then the stiffness matrix is calculated using the current configuration ie using the current position of the nodes.
The Riks method cannot be used when the only loading is by applied moments and/or applied rotations. However the bending moment can be represented by a couple ie set of point loads acting in the opposite direction, separated by a suitable distance.
A Riks step cannot be followed by another step in the same run. Subsequent steps must be analysed using the *RESTART option (Section 7.1.1 User's manual version 6.3).

*STEP, INC=10, NLGEOM 
*STATIC, RIKS 



Q10.3 : In trying to restart an analysis from a step which did not complete I am getting the same error message?

In the *RESTART keyword line add the END STEP parameter. Example :
 *RESTART, READ, STEP=2, INC=10, END STEP, WRITE 



Q10.4 : I am interested in the dynamic response (ie oscillations) due to heating of a thermocouple. How do I go about analysing this problem?

This analysis has to be carried out in 2 parts. First part is a heat transfer analysis. Then carry out a dynamics analysis with the temperatures from the first analysis as input. The element types for the 2 analyses will be different.


Q10.5 : I have carried out a static analysis with the RIKS method and I find that the time at the end of the step exceeds the step time. What do I do?

Check the dataline for the *STATIC keyword includes the load proportionality factor. This is the 5th parameter in the data line. This should be set to 1.



Q10.6 : What is the significance of the "minimum" and "maximum" time increments in a step?

This is explained with reference to the figure for question 10.5 above.
In the above example the maximum time increment allowed is 0.2. This will not be exceeded in any increment in this step. By default automatic time stepping will be used. This means that the ABAQUS program will choose the largest time increment on efficiency and other grounds.
In a given increment if convergence is not possible it will re-solve with a reduced time step. ABAQUS will repeat this procedure until convergence is reached in a given increment. However the analysis will be terminated if ABAQUS has to reduce the time step to a value less than the minimum time step (0.01 for this example). These parameters sets limits and are means of controlling what happens in a given step. If any one of the limits is reached the step is terminated. Irrespective of which limit is reached first the step will be terminated.

Q10.7 : In carrying out a frequency analysis I am getting warning messages about negative eigenvalues. What do I do?

Check the boundary conditions if any are specified. Check the material properties.
Check that original shape of the elements in the mesh are reasonable. Triangular elements must be nearly equilateral (and aspect ratios should not exceed 3). Similarly quadrilateral elements should not exceed an aspect ratio of 10.
If no errors are detected then draw the different eigenmodes and check that the mode shapes are realistic. If so the warning messages can be ignored. However in general warning messages should not be routinely ignored. These may have some implications on the results from the analyses.

Q10.8 : Can I apply any loading in a frequency step?

Any applied loading during a frequency step (using *FREQUENCY procedure) will be ignored.
However if *STEP, NLGEOM is used in a general analysis then the initial stress stiffness effect of any loading applied in a prior step will be taken into account in the eigenvalue extraction.
Therefore to include the effect of any pre-loading apply the loading in the first step with *STEP, NLGEOM option.
If initial stresses prescribed by *INITIAL CONDITIONS, TYPE=STRESS are to be considered in the frequency extraction then include this in a static step (step 1) which includes the NLGEOM option. Specify the appropriate boundary conditions and loading in the same step. Then use *FREQUENCY in step 2.


Q10.9 : I want to use the displacement obtained from one analysis to modify the geometry (to change the nodal position) and carry out a separate analysis. Is this possible?

Yes it is possible. This is catered for by the *IMPERFECTION keyword.
Let us assume that the analysis-ID of the analysis from which the displacements (to be used as imperfection) is "static1". This could be anything and used here for illustrative purposes. Run this analysis and this will create the results file static1.res among other output files.
The second analysis should have the following input. Only the essential ones are shown.
*HEADING
Second analysis which uses the displacement from the previous analysis
as an imperfection.
*NODE
Data lines to define the initial "perfect" geometry
.....
*IMPERFECTION, FILE=static1, STEP=< step>, INC=< inc>, NSET=< node-set-name>
1, < scale-factor>
....
**
*STEP, NLGEOM
*STATIC, RIKS
...
*CLOAD and/or *DLOAD
data lines to specify loading
*END STEP
In the above specify the < step> as the STEP number and the < scale factor> if the displacements from the previous analysis are to be scaled. Otherwise specify it as 1.
INC and NSET are the other optional parameters. If the displacements at the end of particular increment rather than the end of the step (from the previous analysis) is to be considered then set the INC parameter. Similarly if the displacements of only a subset of the nodes in the mesh is to be considered as the imperfection then define a node set and specify it using the NSET parameter.
If the previous analysis is a buckling or a frequency analysis then the *IMPERFECTION key word is as follows :
*IMPERFECTION, FILE=buckle1, STEP=< step>, NSET=< node-set-name>
< mode-number-1>, < scale-factor-1>
< mode-number-2>, < scale-factor-2>
as many lines as required modes to be used.
In this case the imperfection is a linear combination of the selected mode shapes.

Q10.10 : In an axisymmetric analysis are there any restrictions in the choice of the axis of symmetry?

Yes, Only the z axis can be the axis of symmetry. In an axisymmetric analysis r-z-theta forms the 1-2-3 axes. The radial axis is considered to be horizontal going from left to right. The z-axis (the axis of symmetry) is the axis pointing vertically upwards. The 3rd-axis is directed towards the user, normal to the rz plane.

The radial distance is measured from the z axis and r=0 at the z axis. Only the radial section is meshed and ABAQUS integrates this section through 360 degrees for any calculation which involves the volume.
So only the radial section should be considered. It is wrong to consider even the diametral section.

Q10.11 : I How do I stop and re-start an analysis job?

Input file for the first run dynam.inp Include the line
*RESTART, WRITE, FREQ=1
in the second step of this input file and this will write the results of every increment (FREQ = 1) to the re-start file.
The job is run from the command line as follows :
abaqus j=dynam
In this example the 2nd step is not completed.
Lets assume that in the re-started run the analysis is to be continued from the end 10th increment of the second step.
This is done by including the following line after the *HEADING statement.
*RESTART, READ, STEP=2, INCREMENT=1, END STEP, WRITE
Failing to include the END STEP parameter would result in the re-started run repeating the second step exactly and failing to complete in the same way as the first run.
Note that since this is a re-start run all the model data part of the input (F.E.Mesh data material properties etc) is omitted. The next statement after the *RESTART statement consists of a *STEP statement.
Input file for the re-started run dynamr.inp
The job is submitted from the command line as follows :
abaqus oldjob=dynam j=dynamr
The following extract taken from dynamr.dat shows that the results are read from the restart file up to the 10th increment and the analysis continuing with the next step (STEP 3).
  *HEADING
           BISSHOPP AND DRUCKER -- SMALL DISPLACEMENT ANALYSIS  B21        

          STEP    1  INCREMENT    1  HAS BEEN FOUND ON THE RESTART FILE

          STEP    2  INCREMENT    1  HAS BEEN FOUND ON THE RESTART FILE

          STEP    2  INCREMENT    2  HAS BEEN FOUND ON THE RESTART FILE
....

          STEP    2  INCREMENT    8  HAS BEEN FOUND ON THE RESTART FILE

          STEP    2  INCREMENT    9  HAS BEEN FOUND ON THE RESTART FILE

          STEP    2  INCREMENT   10  HAS BEEN FOUND ON THE RESTART FILE
The analysis continuing wth the next step (STEP 3). Following is the extract from the status file : dynamr.sta
 Abaqus/Standard 6.9-1                  DATE 01-Sep-2009 TIME 15:31:01
 SUMMARY OF JOB INFORMATION:
 MONITOR NODE:      11  DOF:  2
 STEP  INC ATT SEVERE EQUIL TOTAL  TOTAL      STEP       INC OF       DOF    IF
               DISCON ITERS ITERS  TIME/    TIME/LPF    TIME/LPF    MONITOR RIKS
               ITERS               FREQ
   3     1   1     0     1     1  1.11       0.0100     0.01000     19.3     
   3     2   1     0     1     1  1.12       0.0200     0.01000     10.1     
   3     3   1     0     1     1  1.13       0.0300     0.01000     0.116    
   3     4   1     0     1     1  1.14       0.0400     0.01000    -10.7     
   3     5   1     0     1     1  1.15       0.0500     0.01000    -20.5     
   3     6   1     0     1     1  1.16       0.0600     0.01000    -26.7     
   3     7   1     0     1     1  1.17       0.0700     0.01000    -29.3     
.....
   3    97   1     0     1     1  2.07       0.970      0.01000    -11.6     
   3    98   1     0     1     1  2.08       0.980      0.01000    -1.12     
   3    99   1     0     1     1  2.09       0.990      0.01000     9.46     
   3   100   1     0     1     1  2.10       1.00       0.01000     18.8     
                          
 THE ANALYSIS HAS COMPLETED SUCCESSFULLY
If the ODB files from the first run and the re-started run needs to be combined into a single ODB file for post-processing purposes, this is achieved by typing the following line from the command line :
Execution procedure for joining output database (.odb) files from restarted analyses
abaqus restartjoin originalodb=odb-file-name restartodb=odb-file-name [copyoriginal].
© Cambridge University Engineering Dept
Information provided by abaqus-support
Last updated: 18 December 2011