There’s an old grey-haired engineer in every office who talks about FEA models and “rubbish in equals rubbish out”. Today’s analysis software are very advanced and allow Structural Engineers to design truly complex buildings. This means that the quintessential “black box” of analysis is not only alive and well but potentially getting blacker, and larger every day. So how do you check if your ETABS analysis model is correct or not?
First lets take a look at the two quips which opened this article in the paragraph above… lets start with the old “black box” analogy…
In Structural Engineering terms, a “black box” is a colloquial expression for Structural modelling software (usually finite element based). The expression is usually also extended to cover the actual specific model generated within the given software. The term broadly expresses an Engineers uncertainty of the accuracy and methodology of the analysis being performed within the model. As a result, this then leads to un-certainty and lack of confidence in the final results which the model produces.
This then leads to the next quip.. “rubbish in equals rubbish out”…
“Rubbish in equals rubbish out” is a term often used by very smart engineers. The term is an indication of the acceptance of the black box phenomenon and if trust is to be placed in the black box, the controlling variables need to be confirmed as being correct (the inputs).
The rubbish in equals rubbish out adage is where we will begin this article…
(Do you enjoy using ETBAS? Would you like to learn more? Take a look at THIS article which explains a step-by-step process to modelling cracked shear wall behaviour in your ETABS model).
Assessing Inputs to Check if your ETABS Model is Correct.
If you are sanity checking your own analysis model or reviewing somebody else’s model, the best place to start in order to build confidence in the results is the inputs to the model.
There are a large number of inputs which go into a building model. It can be overwhelming and confusing where to start. You can use the following table to act as a check-list when performing QA on your next analysis model in ETABS. Note that this check list along with other pointers in this article are not just specific to ETABS but can be applied to any FEA modelling software for buildings you may be using…
|Element to be Checked in FEA Model (ETABS)
|Check geometry (column, wall and beam spacing, floor-to-floor heights, slab extents, member sizes etc.)
|Material Properties (concrete, steel, timber values for Young’s Modulus, density, strength grade etc.)
|Confirm wind loading inputs are correct (Depending on your country this may include, Terrain Category, Wind Speed, Exposure type/classification, Topography Factor and/or e1/e2 factors)
|Confirm seismic loading inputs are correct (Depending on your country this may include, Site soil class, probability factor, Hazard factor, performance factor and ductility factors as well as eccentricity allowances)
|Enveloped load combinations (if any are used)
|Member fixity settings (releases, springs, pints etc.)
|Cracking values in walls, beams and columns.
|Ensure correct design codes have been specified within software (if software is used to perform not just force check but member check also)
|Diaphragms are assigned and correct type is used
|Appropriate area properties are assigned for slabs (membrane vs shell etc.)
|If members/walls are manually meshed, do the mesh assumptions make sense, if auto mesh is used are the factors acceptable
|Check that frame elements node out and discontinuities do not exist (where they are not intended to exist)
|Is the mass source for seismic adequately defined
|If response spectrum analysis is used for seismic design, are the scaling factors acceptable and is the function properly defined
That is a pretty exhaustive list, there are a few other things you can check to see if your ETABS model is correct. However some things are easier checked after the analysis is performed (which we will touch on later).
Checks to Perform before Running the Analysis on your ETABS model.
The most obvious check to then perform in ETABS is provided by the software itself. ETABS has a built-in model auditing tool to check node tolerances and meshing. To locate this simply navigate to…
The following dialog box will appear…
Before running the check, you can set your desired tolerance and then select from a range of check boxes which are grouped into…
- Joint Checks
- Frame Checks
- Shell Checks
- Other Checks (Meshing, loading etc.)
In order to methodically go through your errors, its a really good idea to first run the model check with all the Joint Check boxes ticked and nothing else, then eliminate the errors. Then move to the Frame Checks and only tick those boxes and eliminate those errors and so on.
This approach allows you to eliminate each batch of errors in piecemeal. You may also find that eliminating errors in one group may prevent errors in other groups from popping up in the first place.
It is usually common to see a large quantity of errors if you are running the model check for the first time after you have set up your building in ETABS.
The next thing to check is that the load cases you want to run are activated. It can be a terrible waste of time to run a model which you are reviewing and waiting several minutes (or hours depending on how large the building is) only to find that the modal analysis hasn’t been completed!! To check which cases will be run navigate to….
Analyse>>>Set Load Cases to Run…
After you have made sure that the cases you want to run are properly activated, you are ready to run the analysis to check if your ETABS model is correct. But first one quick little clarification…
Running the Model in ETABS
Before you hit the “Run Analysis” button. You need to make sure that you are using the best solver for the job. To check the solver option for the analysis, you simply navigate to…
Analyse>>>Advanced SAPFire Options…
The following dialog box will then appear…
You will then see the following solver options…
The standard solver uses only one of your computers GPUs so it takes the longest time to run your model. However this solver gives the most comprehensive report on your buildings instabilities and errors (the errors which can not be picked up by the model check previously performed). For this reason, if you are running your model for the first time and want to check if your ETABS model is correct, or you have made significant updates to your model, you should use this solver. Once you are comfortable that your model is accurate and you have performed all the checks in this article you can then start to use the Advanced and Multi-threaded solvers for subsequent minor model updates.
The advanced solver is a middle ground between standard and multi-thread. It runs much faster than the standard solver because it splits the analysis problem into sections then allows each core of your computers GPU to solve the sections concurrently. It only gives minimal feedback on model instabilities so it is best used if you are reasonably comfortable with your model and you have only made moderate model updates since you last ran it and eliminated its errors.
This is the fastest solver out of all the options. It also uses multiple cores to solve the analysis however it also utilises more of your machines RAM to further speed up the process. It gives almost no instability information. For this reason, it is best used if you are checking model iterations and “what if” scenarios for comparison when you need some quick answers. If you are making significant updates to your model or running it for the very first time, it is strongly advised to not use the multi-threaded solver.
Post Analysis Checks to Perform in ETABS to Ensure the Model is Correct
Now your model has been run. The first thing you need to do is check your error log for the analysis and locate any errors you still have and methodically go about eliminating them.
Checking for Floor Connectivity and Behaviour
A very effective check to run on your ETAB model after the analysis has been ran is to check your floors spanning behaviour. To do this, you must first isolate a single floor in the 3D view (note this check should be performed on all non-typical floors in your model). To isolate the floor you wish to check navigate as follows…
View>>>Set Building View Limits…
The following dialog box will appear…
You can isolate the view to one single floor by selecting the top story and bottom story to be the same level (as highlighted above).
Click OK then look at the 3D view of your isolated slab. Select “show deformed shape” in the tool bar to open the deflection dialog box.
It is best to choose a load case which will give the deflected response which is easiest to predict using engineering judgement. A good one to choose is the self-weight deflected shape (or the dead load).
Click OK then start the animation for the deflected shape. The start animation button should be at the bottom right of your screen…
The deflected animation tool for dead load on each of your floors is a great checking tool. While the animation is running you are looking for anything that looks funny or not quite right. Very large deflections in localised areas, beams disconnecting from columns/slabs etc. It is a good idea to rotate the model around a few times and look at the floor from different angles to see that everything is connected and behaving the way it should. Here is an example animation of an office floor showing the deflected shape animation…
Note that your deflected shape may look different depending on if you are using a membrane or a shell for your floor slab. For a further explanation on the differences between the two and what deflected shapes to expect, take a look at THIS article.
Checking your ETABS Model for Modal Response
Even if you are not interested in the modal response of your building (for whatever reason), drilling down on the modal results and deflected shape is a great way to check if your model is valid and tied together structurally.
The first thing to check is the fundamental period of your building (the period for Mode 1 of your model). For an in-depth look at vibration, oscillation of motion and modes, take a look at THIS article for further learning.
You can check the first mode period of your building by navigating to…
Then the following dialog box will appear…
In the dialogue box above, I have highlighted the tree location you need to navigate to in order to view the modal periods and frequencies for your analysis.
A table will then appear which gives the period for the buildings first 30 odd modes as shown above (I am only showing the first three here). The value for the fist mode is the one you are most interested in. To make sure that you are roughly within the limits of where you need to be you can perform the following check…
- Your first mode period should be roughly in the order of 0.08 to 0.15 multiplied by the number of storeys of your building.
This is a very rough guide, you are really trying to make sure you are in this vicinity (if you lie outside of this range a little its fine). For the example table provided above, it is a 24 storey building so the expected period should be…
( 0.08 to 0.15 ) x 24 Storey = 1.92 to 3.6 seconds
This means that the model is set up well and proportioned well. If the first mode was in the order of 20 seconds or more there would be serious concerns as there would if the period was 0.0001 seconds.
The next thing to check is the animated deflected shapes of the first three modes of your building. It is a similar process to when we looked at the single slab in isolation, however in this case you want the full building visible and you want to select Modes 1, 2 then 3 and check each.
Again you are looking for members or slabs flying around seemingly unattached to adjacent structural members. You are also looking to see your whole building move. If you can’t see your whole building move you most likely have a stray column or beam which is oscillating on its own which is not adequately restrained and needs your attention.
Next you need to make sure that your modal mass participation is above 90% to ensure you results will be meaningful and accurate, particularly for your frequencies and seismic analysis. To check this you need to navigate to…
Then the following dialog box will appear which we saw earlier…
This time however we are navigating to a different location in the table tree as I have highlighted above. This will then produce the next table for your model (the modal participating mass ratios)…
You then need to scroll to the bottom of the table, this will be dependant on how many modes you have ran. The last row of the “SumUX” and “SumUR” should be larger than 0.90, this will ensure adequate mass participation in your model. If you are not achieving this, you will need to re-run your model with more modes until you are hitting at least 0.90 (or 90%).
Verifying Base Reactions to Ensure that your ETABS Model is Correct
A great way to run another secondary check on your seismic/wind inputs is to verify the output reactions you are achieving in your model for each load case.
You should have a spread sheet handy to calculate both seismic/wind base shear and overturning moment reactions which you can use as a hand check verification. If you don’t have one which your organisation has supplied, you should work on your own and have it checked for accuracy before using on projects.
You should aim for +/-10 to 15% accuracy comparing your base shear and overturning moments between your spreadsheet check and the model output. If you are more than 15% off you should check your model inputs again.
You should also do a hand check on the vertical load reactions on a few vertical load bearing elements such as columns and shear walls. Again you want to be within +/-10 to 15% comparing your hand spot checks against the model results.
Once you have completed all of these checks your model should not be a black box anymore. You have successfully ran a check to see if your ETABS model is correct. You should now have a high level of confidence in the results the model is producing.
This doesn’t mean that your building won’t fall down though! We have merely checked your model for calculation, meshing an framing errors. You now need to ensure that your structural members are adequate for both strength and serviceability in accordance with the design codes of your region. You also need to ensure that your design satisfies the specific detailing requirements depending on the code you are using.
If you found this article useful and enjoy using ETABS as part of your day-to-day Structural Engineering life, you may also find these articles interesting: