Please find enclosed model with ekill option used. I'm wondering why the plastic strains appear in results since only elastic material is used. Thank You for Your effort.
I am guessing that you duplicated the analysis system in Workbench to create the three systems. When duplicating B to create C, you would/may have deleted the plasticity material data in the engineering data cell (C2). When you have done this it appears to have cause an error in the material data stored in Mechanical, where it has not updated the material properties, but mechanical thinks all the data is up to date. To remedy this I actually created a new structural steel, from engineering data sources, and when I refreshed the material data, both structural steel definitions correctly showed no reference to Bilinear Kinematic Hardening.
1st image showing the reference to Bilinear Kinematic Hardening
2nd image showing the original structural steel definition without the reference to Bilinear Kinematic Hardening
3rd image showing the new structural steel definition without the reference to Bilinear Kinematic Hardening
I am unable to solve to confirm, but I believe this should solve your problem. That being said, there is still a weird part of the script that creates an ETABLE result based on equivalent plastic strain. Not sure how this will function if there is no plastic strain in the results. You may intend for this to be EPEL?
Just to be clear, you may not have to redefine the material definitions when copying analysis systems. There is no way to know how this occured without knowing the steps that lead to this. I frequently copy/duplicate analysis systems and have never encountered this issue with materials. I have however encountered issues where mechanical and workbench are out of sync with regard to what information they think is up to date, usually associated with geometry updates. This happens time to time, and as with all things FEA, the user should be vigilant as to what is going into the solver.
If plastic strains are calculated, then non-linear material properties are defined. You should check Engineering Data to ensure that only elastic properties are defined.
The image below is the material in this model.
However, there is a Command Object in the model that has the following code:
!total number of steps for solve, strain is checked only after each step
!Find out the final solution time set in Analysis Settings
!After the solve, go post process strain
!Limited to Named Selection "killelem"
!Create component (Named Selection) of elements that are above failure strain
!A restart opens the ANSYS restart database (*.rdb) which is written after the first
!solve command. Therefore, all the stuff above does not exist in the rdb.
!Write out the components to a file so they can be read in for the restart solve
!Write out the parameters to a file so they can be read in for the restart solve
!Restart... wipes out all of our post processing data that we just obtained
!Read in the parameters
!Read in all components and kill the elements
*GET, exists, COMP, MYELEM%j%, TYPE
The Command Object will not trigger a plastic solution, but it appears that there might be a restart. Is that true? If so, were plastic material properties defined in the original analysis? You could place a Command Object in the tree and just before the solve issue MPLIST,ALL an TBLIST,ALL to check the material properties just before the solve.
Ok, I will do that, but where does it list these properties?
If it is in solution output then probably it is this part of listing:
I found no more info about material in solution info.
This in fact suggest that it is material from the second block of this project, but why is it so, since only geometry is passed through to third project block?
It is not my project. I downloaded it from another place in this forum to be able to use ekill command in my project. I've already done it correctly, but it is just my curiousity if there is an error in software or if something else is wrong in the model. This is just to know the program better and omit its bugs. Anyway, thank You for Your effort. At least now we know that we have to define materials from scratch while duplicating Workbench systems. And Your in-depth analysis is very precious to me.
Responding to Your question: using ekill command without nonlinear behaviour of steel in my opinion makes no sense, therefore in my project i left eppl and defined bilinear hardening, just as it is in the faulty example :)
Thanks again and cheers from Poland!
Thanks for your insights on this model and the related APDL code. For some background information on Damian's question, I posted a discussion in May 2018 (link below) that @damkow began using and asked the question this discussion opens with.
The APDL code was written for me by a Support Engineer at SimuTech Group, a Premier ANSYS Partner company in the US. He had been using a version of this code for years and gave me permission to share it on this forum. So to answer your question, I believe the EPPL is intentional.
The correct usage of this demonstration model is to have the Bilinear plasticity in system C. Unfortunately, when the old Student Community website was converted to this new Forum website, the model attached to the original discussion (link above) was deleted. The archive file was eventually recovered after several members requested it and I attached that archive in a later post in that thread.
I forget the version of ANSYS I originally used with this model, but one thing I have seen when opening old ANSYS files in newer versions of ANSYS is some error appears, though very rarely. For example, I have seen the units get changed and a model in mm shows up in m.
That is a great bit of context @peteroznewman, specifically because this is material database related. You mention that moving a project between versions in Ansys can cause errors although rarely. But there are actually some very consistent errors that the user can test for themselves. For example in the 2020R1 update, Mechanical gained the ability to create cross sections within mechanical and assign them. Any beam model prior to 2020R1 required a remesh if that system/model was being used in an assembly. Something about the change to Cross Sections changed how (or what) data was used in the assembly process. There was a similar issue when Mechanical introduced material assignments, and then later, the updated GUI with the material properties overlay/window. I have a feeling this error is related to this update as the original model was in version 19.2, which is post material assignment (within mechanical) feature, but prior to the updated GUI.
Ansys customers with active commercial software licenses can access the
customer portal and submit support questions. You will need your active account number to register.