Learning Forum

[Jigar Patel]

How can the result of the current load step be transferred to the next load step of the linear static structural analysis?

Let's assume I run the simulation with 6 different load steps. Now I want to transfer the results of load step 1 to load step 2 and so on. In the end I want to get the combined results of all load steps (6 load steps) in single load steps (in the 7th load step).

I have tried a lot to do this, but I did not get the desired results.

Could someone please suggest a solution to the problem? Any kind of assistance is appreciated.

 

[Aniket Chavan]

If your loads are cumulative, that means if load1 which is applied in step 1 continues in load step 2 it is already combined in load step 2.

If you are removing load1 in step 2 and other subsequent steps or using multiple static structural systems, then you need to use solution combination.

https://ansyshelp.ansys.com/account/Secured?returnurl=/Views/Secured/corp/v195/wb_sim/ds_Solution_Combinations.html

 

-Aniket

Guidelines on the Student Community

How to access ANSYS help links

[Jigar Patel]

Thanks Aniket for your Reply.

 

I have combined the all the load steps as following using APDL script. Is this correct method? 

 

!                See Solving Units in the help system for more information.

!   Commands inserted into this file will be executed immediately after the ANSYS /POST1 command.

!   Active UNIT system in Workbench when this object was created:  Metric (mm, kg, N, s, mV, mA)
!   NOTE:  Any data that requires units (such as mass) is assumed to be in the consistent solver unit system.
!                See Solving Units in the help system for more information.

FINISH

/POST1

!*************************************************************************************************************
!Transformation of load steps into the load cases
!*************************************************************************************************************
! Total number of load steps in the ANSYS Simulation
NSTEPS = 6

! Do this for defining the load steps into load case files
*DO,i,1,NSTEPS,1
    LCDEF,i,i,1
*ENDDO

!*************************************************************************************************************
!Defination of all the load cases. Combined Load Cases = Torque load +  All the parasitic loads
!*************************************************************************************************************

! Zeroes the results portion of the database
LCZERO         

!*****************Addition of the individial load cases resulting in 'Combined Load Case'*********************

! Performance of Torque load case
LCOPER,ADD,1  

! Performance of Parasitic load cases
LCOPER,ADD,2            ! Performance of Converter Ballooning
LCOPER,ADD,3            ! Performance of Axial Load
LCOPER,ADD,4            ! Performance of Bending Load
LCOPER,ADD,5            ! Performance of Rotational Velocity Load
LCOPER,ADD,6            ! Performance of Thermo-mechanical load

!*************************************************************************************************************
!Combined Load Cases (7) = Torque load case (1) + All the parasitic load case (2 + 3 + 4 + 5 + 6)
!*************************************************************************************************************

! Appends results data from the database to the results file
! Combines all the above load cases result database as 7th (Combined Load) Load Case
RAPPND,7,7

! Creates a Combined load case by writing results to a load case file
LCWRITE,7,ALL_COMBINED_LOADS,L7