Previous my model took 0,5 hour to calculate, but after a few changes this has increased to several days...
Any suggestions on how to reduce the calculations time?
Solved! Go to Solution.
Nonlinear seismic why should not be used
1. Stiffness matrix for modal analysis is taken from the last calculated case
before modal case so some tension members "are not working" in this case and
this state will be fixed for next modal case(s)
2. Modes should (may) activate \ deactivate some different tension bars depending
on direction they are acting but this effect can not be considered due to point 1
3. Even if we calculate model after combining results for most tension bars it may
appear that results are "not existing" because combining "not existing" results
and some value results gives "not existing" finally
4. Spectral/seismic analyse is based on assumption of harmonic vibrations which
is not true for nonlinear model. In such case you should use time history instead.
One have to convert time - acceleration data into time - displacement data and
finally apply them to the supports of your structure (to model movement of the ground).
More complete explanations related to above points:
Existence of tension-only members (or any other nonlinear objects like cables, uplift supports, etc) results in non-linear behaviour of the structure and in such case the precise approach to seismic analysis is using non-linear time history analysis. It is possible in Robot but:
1/ it is necessary to input time history of ground motion
2/ non-linear time history is the type of analysis requiring significant hardware resources and requiring quite a long time
Another possibility (applicable in some cases) is using standard modal and seismic analysis (response spectra) which is a linear dynamic analysis (with constant stiffness) – in such case model is linearized. Such approach is not recommended for users without significant experience in seismic design and it can be used for rather regular structures with regular arrangement of tension-only bracings.
Generally when model contains nonlinear objects (including tension-only members) and dynamic modal analysis is defined in it this modal analysis is performed for the stiffness of model resulting from the static load case directly preceding the modal load case.
So for instance if this static load case results on all tension-only bracings not working then modal (and seismic) analysis will be performed without influence of these bracings.
If the preceding static load case results in all tension-only bracings working then modal (and seismic) analysis will be performed with influence of all bracings. And so on – generally depending on static loads applied in preceding load case the vibration frequencies and other results of modal and seismic analysis performed for the same model can be completely different.
Of course it is not corresponding to the real behaviour of the structure.
But in case of for instance regular model with X bracings it is possible to define a preceding static load case with some notional horizontal load resulting in half of bracings working (one arm of each X bracing) so the stiffness of these bracings will be used in modal and seismic analysis. In real structure the active bracings are changing during vibrations – in the structure like this or one half or another half of bracings is active. In linearized model this change cannot be done but in case of X bracing it may be assumed that this simplification results in local change limited to each X bracing field.
In case of using such simplified approach it is also important to remember about combinations – combinations of static load cases in nonlinear models are iterated individually – superposition principle is not used for them. In case of linearization performed for seismic load cases the results for them are combined with static loads using superposition principle – as linear combinations.
Are you really sure that this model should be calculated as nonlinear model ?
This makes lots of difference in calculation time.
I used Multithreaded solver on this model -> calculation time = 15min
I also used multi-threaded solver, but in case nr 7 it calculates 32000 iterations... and this takes a lot of time..
What did you change to get it to run in just 15min?
I fact I have moved only node 4929 onto 77490.
But I looked closer to your model (coming from Revit) and I found some inaccurcies in it.
Walls 178 180 1414 1416 1893to1896 1320 1323 1325 1326 1889to1892 1899 1900 are not connected to each other:
Walls \ slabs \ beams may not be not connected to each other:
I have corrected some of them.
File : https://www.filemail.com/dl.aspx?id=LMBIERHYYDZWRG