I have had similar requirements for Section VIII Div 2 FEA, It's one of the things that drove me to learn the Simulation API which would be the most efficient (and maybe only) way to accomplish this. It does require familiarity with Visual Basic (VBA) and object oriented programming methods
I have some sample code ir you want to go this route.
Thanks. I am definitely interested. I could also use this for the strain based elasto plastic local failure criteria checks. We're you able to create your own stress plots?
Awesome! Thanks for the heads up. This is great news. I have not installed 2015 , but I will now. Much appreciated.
Thanks for the responses.
It's great they added that tri-ax plot. It seems every time I hit a wall with SW Sim they expand features so I don't have to go to a different package .
The API gives you access to all the plot settings programmatically but does not create plot types outside of the built-in types. What I have done is write results to an Excel sheet and charted results. In particular if you're doing pressure vessel work the API gives access to all the linearized stress components according to ASME VIII Div 2. Here's an excerpt of code:
Set CWObject = swApp.GetAddInObject("SldWorks.Simulation")
Set COSMOSWORKS = CWObject.COSMOSWORKS
Set ActDoc = COSMOSWORKS.ActiveDoc()
Set StudyMngr = ActDoc.StudyManager()
Set cwResults = Study.results
linearizedStress = cwResults.GetLinearizedStressValues(swsStressComponentVON, 10.423, 6.111, -22.409, 147, 6.4537, -22.409, 10, 0, errCode)
It's not very well documented in SIm API help so it takes some trial and error to get it right. Then Excel API methods would be used to write to a spreadsheet.
In the asme code for strain based local damage failure. The code instructs to compare the total equivalent plastic strain (from non linear analysis) to the limiting strain for each point in the structure.
1. In solidworks we can list tabular results for total equivalent strain or plastic strain. I am not clear which strain should be compared to the calculated limiting strain for each point.
2. I can only list tabular results for element values of strain and not nodal values. Is there a means to list nodal strain results. Is it necessary per the code?
This area of the code is not clear. I have rarely gone to the plastic approach but of course each case is different. Stress linearization seems to be a good middle ground if you're dealing with local stress risers.
Hope that helps.
Atillo. Im with you. Linear fea takes less time and computing resourses to run but more post processing. Non linear fea is a more pass/fail criteria, but takes longer to solve and is more technical. I am learning and think I am ready to take the next step using the nonlinear approach. I have studied the asme section viii div 2 code, the asme example problem manual, and have worked with my reseller on questions regarding settings and stress strain curve inputs versus the code requirements.
I have an answer on the strain requirements. It appears the code requires the plastic strain (Not total elastic + plastic strain) to be compared to the limiting strain. By total strain, I belive the code implies plastic strain + forming strain. This confused me.
I have not found any formal clarification as to whether the strain should be nodal or elemental. However, if the mesh is sufficiently converged (5% or less is our criteria) then the elemental and nodal values should be close in magnitude. Simulation non linear fea only outputs elemental strain values (based on my experience - unless I am missing something ).