Search Contact information
University of Cambridge Home Department of Engineering
University of Cambridge >  Engineering Department >  computing help

The ABAQUS FAQ


12. Output

Q12.1 : How do I suppress output being written to the *.dat file?

By default no output is written to the *.dat file. This is equivalent to specifying the following statements in the abaqus input file (*.inp). Notice the FREQUENCY is set to 0 causing the output to be suppressed.
*EL PRINT, POSITION=INTEGRATION POINTS, FREQUENCY=0
**
*EL PRINT, POSITION=CENTROIDS, FREQUENCY=0
**
*EL PRINT, POSITION=NODES, FREQUENCY=0
**
*NODE PRINT, FREQUENCY=0 
This will suppress any element or nodal output being written to the printed output file (*.dat).

Q12.2 : I want to print element stresses averaged at nodes as well as the Gauss points. How do I do that?

Use the following statements in the abaqus input file (*.inp).
*EL PRINT, POSITION=INTEGRATION POINTS, FREQUENCY=n
S
*EL PRINT, POSITION=AVERAGED AT NODES, FREQUENCY=n
S

This will print separate tables consisting of the stresses at Gauss points and the values averaged at the nodes for every nth increment.

Q12.3 : I want to print a single table with stresses and strains at Gauss points. How do I do that?

Use the following statements in the abaqus input file (*.inp).
*EL PRINT, POSITION=INTEGRATION POINTS, FREQUENCY=n
 S,E

This will print a single table which contains the stresses and strains at the Gauss Points.
For 2D problems this should be OK. However for 3D problems it is not possible to fit the many components in a single line across the page.

Q12.4 : I would like to print the displacements w.r.t. local co-ordinates. How do I do that?

First of all you need to specify the local co-ordinate system using the *TRANSFORM keyword. This is then applied on a selected set of nodes.
*TRANSFORM, TYPE=C, NSET=CID1
          0.,          0.,          0.,          0.,          0.,          1.
**
*NSET, NSET=CID1
       1,       2,       3,       4,       5

The implication of the use of *TRANSFORM is that any input concentrated force and moment you apply to this node set will be interpreted in the local co-ordinate system.
Then use the following statement in the ABAQUS input file.
*NODE PRINT, GLOBAL=NO, FREQUENCY=n
 U

This in fact is the default output option. If necessary the displacements w.r.t. the global axes can be obtained by using GLOBAL=YES in the *NODE PRINT statement.
However if you want to use the displacements w.r.t local co-ordinates in some graphical output (ie drawing contour of one component of displacement w.r.t. local co-ordinate) then it will not be possible even if you specify the following data in the ABAQUS input file.
*NODE FILE, GLOBAL=NO, FREQUENCY=n
 U

The reason is *NODE FILE controls the data written to the *.fil (results) file and changing this has no effect on any contours. Contours are produced from the *.res (restart) file which is always written in global coordinates. PATH plots are also generated from the *.res file and so will again will always be in the global coordinate system.
However you can use FEMGV to produce contour plots of displacements w.r.t local co-ordinates because FEMGV reads the results from the *.fil for post processing. So depending on whether you included GLOBAL=YES or NO the contours of the displacements will be different if using FEMGV.

Q12.5 : I would like to print the element stresses and strains w.r.t. a local co-ordinate system. How do I do that?

This is done using the ORIENTATION option in the *SOLID SECTION keyword and the specification for the *ORIENTATION keyword as illustrated below :
**
** square_plate
**
*SOLID SECTION, ELSET=SQUARE_P, MATERIAL=STEEL,ORIENTATION=CYL
          5.,
**
*ORIENTATION,SYSTEM=CYLINDRICAL,NAME=CYL
0., 0., 0., 0., 0., 1.
3, 0
Here a local cylindrical co-ordinate system is specified. Then use of the following output option :
**
*EL PRINT, POSITION=INTEGRATION POINT, FREQ=1
S
produces the following output in the (*.dat) file. Note the presence of OR next to the integration point which indicates use of the local co-ordinate system with the *ORIENTATION option.
 ELEMENT  PT FOOT-       E11         E22         E12         
             NOTE 
 
       1   1  OR    -2.9537E-08 -2.7172E-09  3.5417E-08
       1   2  OR    -3.4626E-08  6.6933E-09  7.9072E-09
       1   3  OR    -5.5444E-09 -1.3702E-08  3.0689E-08
       1   4  OR    -1.2208E-08 -2.7172E-09  2.6730E-08


 OR: *ORIENTATION USED FOR THIS ELEMENT


Q12.6 : In running a ABAQUS analysis I can't find the *.msg file?

This would indicate that data errors must have been detected during the pre (data checking) stage of the ABAQUS run. The detected errors can be found in the printed output file (*.dat). For confirmation look at the *.log file. If you use the interactive option then this information will be printed on the screen (instead of the *.log file).


Q12.7 : In running a ABAQUS analysis the *.dat file has terminated abruptly. What is wrong?

When ABAQUS completes a run irrespective of whether it had detected any errors or not there will always be a summary at the end of the printed output file (*.dat). The last statement lists the CPU time used for the particular stage (pre, analysis). If you find that the *.dat file has come to an abrupt end then the most likely reason is that in creating the various output files your disk quota has been exceeded.
Use the following command to check your disk quota in the Teaching System.
df
If you find that there is a difference between the usage and allocation of disk quota you need to remember that one of the ABAQUS files (*.023) is created in the directory from which ABAQUS is run and gets deleted when it completes its run. This could explain the discrepancy.


Q12.8 : How do I generate a customised output file?

If none of the *NODE PRINT and *EL PRINT input statements with its option cater for your requirement (example : you want the nodal displacements printed to a greater accuracy than it is printed in the *.dat file) then you can
  1. Write a post processing program to read the *.fil file and write out the results to a separate file after the ABAQUS run has completed. A typical post processing routine is listed in section 5.1.3 of the ABAQUS User's manual titled Accessing the results file information (Version 6.5).
  2. Use one of the user subroutines (example : USDFLD or UVARM) to write the required results to a separate file during the ABAQUS run. Here be careful to specify the fully qualified name of the file in the Teaching System. See the answer to the question "12.12".


Q12.9 : How do I monitor the progress of a long analysis?

A useful output file is the status file (*.sta). This is useful in checking the progress of a long ABAQUS run and also to monitor the state of the analysis, while it is running. There is one line of output for each increment of each step which is written to the status file at the end of each increment.
By including the following statement in the *.inp file one can monitor the progress of a single variable (d.o.f) at a single node.
*MONITOR, NODE=11, DOF=2

Then the y-displacement (uy) at node 11 will be written to the *.sta file so that the user can monitor its progress during a ABAQUS run. The contents of a typical status file is listed below.
SUMMARY OF JOB INFORMATION:
STEP  INC ATT SEVERE EQUIL TOTAL  TOTAL    STEP       INC OF      DOF    IF
              DISCON ITERS ITERS  TIME/  TIME/LPF    TIME/LPF   MONITOR RIKS
              ITERS               FREQ

   1    1   1     0     1     1   1.00     1.00       1.000    
 MONITOR NODE:      11 DOF:  2
   2    1   1     0     1     1   1.01    1.000E-02  1.0000E-02  -27.9    
   2    2   1     0     1     1   1.02    2.000E-02  1.0000E-02  -21.7    
   2    3   1     0     1     1   1.03    3.000E-02  1.0000E-02  -14.0    
   2    4   1     0     1     1   1.04    4.000E-02  1.0000E-02  -4.05    
   2    5   1     0     1     1   1.05    5.000E-02  1.0000E-02   7.47    
   2    6   1     0     1     1   1.06    6.000E-02  1.0000E-02   17.7    
   2    7   1     0     1     1   1.07    7.000E-02  1.0000E-02   24.4    
   2    8   1     0     1     1   1.08    8.000E-02  1.0000E-02   28.6    
   2    9   1     0     1     1   1.09    9.000E-02  1.0000E-02   30.0    
   2   10   1     0     1     1   1.10     .100      1.0000E-02   26.7    

Type tail -10 analysis-id.sta and this will display the last 10 lines of the status file. Example : tail -10 plate.sta.
You can also use the the following command which will display the contents of the status file as it gets updated. You need to use the CTRL/C to quit when the analysis is completed.
tail -10f plate.sta.
To get a visual plot which is updated automatically can be obtained using ABAQUS/CAE.
Choose Step module and select Output menu and choose the monitor option. Select the Dof to monitor and select the Node as a point in the model and set the frequency of output and click on OK.
Once the job is created and submitted choose the Viewport and choose the monitor variable. This should display the plot.

Q12.10 : I have run an analysis and the *.res file has not been created. What is wrong?

Check whether the following statement has been included in the *.inp file.
*RESTART,WRITE,FREQUENCY=n



Q12.11 : In running a ABAQUS analysis using the user subroutine option the printed output is terminated after the datacheck stage and there are no report of any errors?

This can happen if the user subroutine you have written had syntax or some other errors. Check the *.log file for clues to the errors. Example :
PROGRAM ABORTED : IEEE OVERFLOW
PROCEDURE TRACEBACK ...


Q12.12 : In running a ABAQUS analysis with the user subroutine option the output file written to in the user subroutine couldn't be found. What s wrong?

The specified file is created and then deleted with the run-time files. This can happen when the file-name used does not include the full path name.
Example : open(26, file='user.out',status=new)
Specify the full path name and then this file will not be deleted at the end of the ABAQUS run. To find out the full path name use the pwd (which represents "present working directory") command in the Unix system.
Example :    If typing "pwd" yields the following :
            /homes/courses/ugrad/05/abcnn/abaqus

Then append the file name to the directory as follows :

       open(26, file='/homes/courses/ugrad/05/abcnnc/abaqus/user.out',status=new)


Q12.13 : I have used the cylindrical co-ordinate system to specify the nodal position using *NODE with SYSTEM=C. Does it mean that the displacements printed at the end of the analysis will be in terms of the cylindrical co-ordinate system?

No. the displacements printed will still be in terms of the global axes. Use *NODE with SYSTEM=C is just for ease of specifying the position of nodes in a cylindrical co-ordinate system. It does not mean that the nodes belong to a different local co-ordinate system.

Q12.14 : What is the default option for printing stresses and strains in the printed output (*.dat) file?

In the absence of *EL PRINT keyword ABAQUS will not print any stresses or strains as no output is the default option.

Q12.15 : How do I get the bending moments written to the output data base (*.odb) and to the printed output (*.dat) file?

Include the following statemets to get the bending moments written to the output database :
*OUTPUT, FIELD
*ELEMENT OUTPUT, POSITION=INTEGRATION POINTS
SF

Include the following statemets to get the bending moments written to the printed output file :
*EL PRINT, POSITION=INTEGRATION POINTS, FREQ=1
SF
*EL PRINT, POSITION=NODES, FREQ=1
SF
*EL PRINT, POSITION=AVERAGED AT NODES, FREQ=1
SF
There will be 3 tables with the first giving the bending moments calculated at the integration points. Thes econd table at the nodes of the element and the final table with the bending moments averaged at the nodes.
This is illustrated in the example input file for shell elements
© Cambridge University Engineering Dept
Information provided by abaqus-support@eng
Last updated: 23 June 2009