how can I evaluate the maximum value of a parameter in visualisation module?
,,,
Hi everyone
I have an issue with evaluating the maximum value of a parameter (for example stress or displacement) in visualization module in ABAQUS.
My model has numerous elements and a dynamic step with too many increments.
So, I can't evaluate stress for every element per every increment and then calculate the maximum stress for each increment. because it's so difficult.
Regards,,,
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
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]
Omid Habibi Hi Omid, thanks for sharing the code. Could you please guide me on how to apply it as subroutine? Also please let me know what to change if I also need to have strain values in the report. Thanks in advance.
Hi Farzam. For obtaining strain values, I think you need to replace S with (LE, PE) in the fieldOuput part .
- Badges
- Science topic