Dear Masoud

In the Visualization module, select "Options" tab then "Contour..." which will open Contour Plot Options window, then go to the Limit tab and enable "Show Location" checkmark. By this, you will be able to see the maximum or minimum of a field output.As you know, by this, you will only see the Max/Min values in the specified frames and not for all increments. 

If you are willing to have the max stress for all increments, you may use "VUSDFLD" subroutine if you are implementing the expilicit scheme. By this subroutine, you will be able to write down the max value for stress in every increment with the corresponding element number (integration point) into the log file.   

Dear Mr.Hajializadeh

thank you for answering

my model step is dynamic implicit

I think it must be an easier way than using subroutine to solve this issue

I look forward, but I don't find anything until now

You can do this with python scripting. I think the scripting user guide has an example on how to find the max. value of a variable.

Python scripting in Abaqus is a bit hard to learn due to the very complex data structures used, but it is well worth the effort.

Alternatively, if what you are doing can be done with a few mouseclicks in Abaqus, use the macro manager to record a macro; you can then edit the macro-file and call it directly from Abaqus.

Hello,

To report field outputs such as stress field S[S11, S22, S33, S12, S13, S23] at the end of an analysis step Step_Name use the following script:

from odbAccess import *

odb = openOdb('Job_Name.odb')

lastFrame = odb.steps['Step_Name'].frames[-1]

Stress=lastFrame.fieldOutputs['S']

fieldValues=Stress.values

fileS = open('S_out','w')

for v in fieldValues:

fileS.write('%10.2e\t%10.2e\t%10.2e\t%10.2e\t%10.2e\t%10.2e\n' % (v.data[0], v.data[1], v.data[2], v.data[3], v.data[4], v.data[5]))

fileS.close()

This script will report stress components in a file called S_out.

You can also report any kind of output variables from fieldOutputs.

Dear Mr.Baeker

Thank you for your answer and help

I follow up it

Regards,,,

Dear Mr.Bakir

Thank you for your answer, but the problem is how to obtain the max value for the model without evaluating the stress for all elements, because the elements are numerous and cause the calculation too heavy.

Regards,,,

To find maximum values, just add a few lines of python code to Ahmads script, roughly like (did not check, but should work)

maxStress=0

  for v in fieldValues:

  if (v.data[0] > maxStress):

    maxStress = v.data[0]

This will find the max value in v.data[0]

(probably there is a python function that can directly find he max entry in an array as well...)

hi masoud

to find the max values as Martin said you should write some code

you could try

a=( )

for v in fieldValues:

  a+=((v.data[0]),)

print 'maxStress= ' , max(a)

Hi guys. This is the answer I think:

from abaqus import *

from abaqusConstants import *

from caeModules import *

from driverUtils import executeOnCaeStartup

from odbAccess import *

f1=openOdb('Job-test.odb')

f2=f1.steps['Step-1'].frames[1]

f2.fieldOutputs['S'].getScalarField(componentLabel='S11')

field=f2.fieldOutputs['S'].getScalarField(componentLabel='S11')

max([ (g.data,g.elementLabel,g.integrationPoint) for g in field.values ])

Source:

https://stackoverflow.com/questions/42783385/max-stress-node

Hi guys.this code finds the max and min stress of all increments and gives the max and min stress increment number and the element label in a file.

odb = openOdb(' Job-1.odb')

lenframes=len(odb.steps['Step-1'].frames)

a=0

b=100000000

maxl=0

minl=0

inc=0

incmax=0

incmin=0

max=open('result','w')

for j in range(0,lenframes):

f1=odb.steps['Step-2'].frames[j].fieldOutputs['S'].values

for i in f1:

if(i.data[0]>=a):

a=i.data[0]

maxl=i.elementLabel

incmax=j

if(i.data[0]