Time History Analysis Results - Member forces

Results like nodal displacements, support reactions, beam end forces are all correct in a time history analysis. However you need to remember that like the other items in a time history analysis, beam end forces are also individual maximums and may not be occurring at the same instant of time. Since intermediate section forces are derived based on the beam end forces, so it does not make sense to derive these based on quantities that do not coexist. Similar logic applies for derived stresses too. The note explains the same.

Hello Sye,

Thank you for your quick reply.

Another quick question if it is possible: the problem is that I am combining the Time History loads with the Static loads in a LOAD COMBINATION. In this case the result for the combination may be not the maximum, e.g. say that the static displacement result in Z direction for a certain node is +20mm, and for the dynamic load the displacement ranges between (-15mm and +10mm). The software will pick the highest magnitude for the dynamic load, i.e. -15mm; therefore, the combined result will be (+20)+(-15) = (+5mm). This is wrong because the most severe case would have been (+20)+(+10) = (+30mm). Is this interpretation right? How do I overcome this?

I) One idea might be to crate 2 combinations 1. static + dynamic, and 2. static - dynamic, and take the maximum results (deflections and forces) for each member out of the 2 cases. Is this right?

II) A second idea is to get first the displacements for the dynamic load only. There is an option where you can get the displacements (only displacements not forces) for the dynamic load in every time step. I guess for the time steps the results are realistic, not the maximums (maybe this has to do with the length of the time step, the smaller the better it is), can you confirm? Then after getting the results from static I can assess the best combination for the static and dynamic displacement.

Do you have any other suggestion and what would your comments be for my proposed methods?

Thank you a lot for your time.

Best Regards,

Skerdi

Hello Sye,

Thank you for your quick reply.

Another quick question if it is possible: the problem is that I am combining the Time History loads with the Static loads in a LOAD COMBINATION. In this case the result for the combination may be not the maximum, e.g. say that the static displacement result in Z direction for a certain node is +20mm, and for the dynamic load the displacement ranges between (-15mm and +10mm). The software will pick the highest magnitude for the dynamic load, i.e. -15mm; therefore, the combined result will be (+20)+(-15) = (+5mm). This is wrong because the most severe case would have been (+20)+(+10) = (+30mm). Is this interpretation right? How do I overcome this?

I) One idea might be to crate 2 combinations 1. static + dynamic, and 2. static - dynamic, and take the maximum results (deflections and forces) for each member out of the 2 cases. Is this right?

II) A second idea is to get first the displacements for the dynamic load only. There is an option where you can get the displacements (only displacements not forces) for the dynamic load in every time step. I guess for the time steps the results are realistic, not the maximums (maybe this has to do with the length of the time step, the smaller the better it is), can you confirm? Then after getting the results from static I can assess the best combination for the static and dynamic displacement.

Do you have any other suggestion and what would your comments be for my proposed methods?

Thank you a lot for your time.

Best Regards,

Skerdi

Yes, as you mentioned in point 1, one should use 2 combinations to capture the worst effect.

Regarding your point 2, first of all I would like to mention that it is possible to capture not only displacements but also member forces and support reactions at each instant of time. You can choose the SAVE option when defining the time history definition and that would save the member forces and reactions in a separate file by the name “model_name.frc” within the same folder where the model is. You can always browse that file to find out forces at any instant and as you said, these are not maximums but real time data. You can assess the worst effect. However this would be quite a task for a reasonably sized model and so personally, I would prefer to go with option 1.

Thanks a lot Sye, You were very helpful indeed.

Kind Regards,

Skerdi

Thanks. Good to know it helped.

Hello Sye,

As I was discussing with my manager we came up with some follow up questions, which are given below together with our scope:

For our analysis results from static cases and time history cases must be combined in order to check member deflections, end rotations and member stresses.

Combinations have been created with static + time history and static – time history numbers because the results are sensitive to the signs. This has been discussed previously.

The .tim and .frc files have been checked and it appears that the node 1 and node 2 values for the time history case for a particular beam and force or moment are the highest values from all the time-steps rather than the corresponding node 1 and node 2 values for one say most onerous time-step. It is not clear, but appears that either the highest +ve from node 1 and highest –ve values from node 2 have somehow been selected in order to give the highest member results. Please confirm if this is the case and if these combinations (static + time history and static – time history)are suitable to check the member stresses or if it is necessary to add the static results to each of the time-step values and check which case is most onerous. The question is if the software can be relied upon to always give the highest member stresses using these combinations.

For deflections/rotations, it is assumed that the .tim file output must be used because this is the only way of checking actual relative movements (for example in checking end rotations). The static results could be added to each time-step displacement in Excel and then rotations checked by hand. Please confirm.


I would appreciate if you could give an answer to these queries ASAP.

Many thanks for your time.

Kind Regards,

Andi

The forces that you get in the frc file at each instant of time, are the corresponding values at the start/end nodes of the member at that instant. The individual maximum value out of all time instants is reported for each node in the post processing table in STAAD.Pro. For determining this maximum value, all +ve and all –ve values in the frc file, for that node, are considered and the one which is highest in magnitude ( positive or negative ) is reported in the postprocessing table. The member force values reported at the nodes in the postprocessing table are therefore not corresponding values but individual maximums. In other words, what you get in the postprocessing mode at the start or end nodes is the highest magnitude of response ( positive or negative ). That is why, when you do a static + time history and a static – time history, you are covered for the worst case scenario.

As long as you are interested in the member start/end forces or reactions, you are fine with what STAAD is reporting in the tables or output. All you need to do is create two combinations ( static+/- time history). On the other hand, if you would like to get results at intermediate sections then you would need to get the values at the ends at each instant from the frc file and then find out the intermediate section forces manually. Subsequently you will need to add the static effect to it.

Same logic applies for the .tim file as well. As long as you are trying to find out max nodal displacements, you will get it directly from the post processing tables. If you would like to get relative displacements/rotations between the start and end node then you would have to know the corresponding values at the nodes at each instant and would need to refer to the .tim file.