It would be helpful to have a step type, or a sub step, that multiples the magnitude of forces from previously defined steps (with the same boundary condition).
For example
Step 1 - self weight
Step 2 - cargo
Step 3 - wind in x
Step 4 - wind in y
Combination
C1 = step1*1.35 + step2*1.5 + step3*1.25
C2 = step1*1.35 + step2*1.5 + step4*1.25
C3 = step1*1.35 + step3*1.5
C4 = step1*1.35 + step4*1.5
This would allow the user to define a distinct load on the structure, run it, review the effect of that load on the structure and perform a check. Then this load can be used multiple times with different magnitudes without the possibility of user error and the ability to alter the step once without having to alter multiple copies of the original load.
For a liner static analysis, I believe this can be done post in processing.
It would also be useful if a maximum von mises stress of all combinations could be produced.
Apart from supporting load cases (that might be a request for CalculiX too), it could be also implemented as an additional scale factor for loads/BCs that can be easily changed in each step. The 3DEXPERIENCE platform (Abaqus on cloud) has something like this in addition to magnitude:
This functionality is partly implemented in the code, but there is no GUI for it yet. The easiest way to implement it would be using Field Outputs defined by equations. But currently, this is also not possible since there is no way to define the time (step) of the field in the equation.
There are Envelope field output operations too (regarding the search for extreme or average values across all frames). It would have to be glued together (maybe also with Parameters) to form load case/combination feature, but let’s also keep in mind that load cases could be implemented on the solver side (*LOAD CASE keyword) for more efficient matrix operations in static perturbation steps.
combination result in commonly structural analysis programs like addition or envelopes by superimposed is appropriate for linear elastic case only. Nonlinear case needs to define in loads before solver running and generate results, it can be general solution with some disadvantages in longer computational times for large loads combo.
Yes, load cases and superpositions are normally applicable only to linear analyses. However, what’s interesting, Abaqus has (since the 2020 FD04 version) a similar feature for nonlinear analyses too. It’s the *MANIFEST keyword that can be used to automatically execute simulations with a common base state.
Could the initial load sets (ie self weight, cargo) be defined in "initial conditions” and then selected and multiplied in magnitude in “sets” this would require one run per combination instead of one run per load set. but would be a lot easier to check.
For context
the Eurocode (civil engineering code for building and bridges) requires each type of load (weight, wind, snow, traffic, thermal, seismic) to be calculated for a probability of not being exceeded 1 in 50 years, this is the leading variable load. When two or more variable loads can occur at the same time, a reduction is made to the accompanying loads, to represent a lower probability, so you need one load case for each variable load. Then a factor of safety is applied to all loads, however when an accompanying load results in a reduction in load in any part of the structure (favourable contribution), then it should be considered with a reduced factor of safety. This results in hundreds of potential load combinations from a relatively small number of initial loads. Many of these combinations can be excluded by inspection. but it takes time to work through the list, and the consequences of a mistake could be costly.
If a matrix of load combinations factors could be defined this would be very useful. If this function was restricted to linier static analysis then time could be saved by running the smaller number of initial conditions first and then combining the stresses after.
thank you for your hard work this is an excelent bit of software.
