Response Spectrum Analysis 1

[ericjacques]

It appears as though whenever I run a response spectrum analysis, SAP does not consider the effect of the mass of the structure. Does anyone know how to make SAP consider the effect of mass?

 

[stressed]

That sounds strange. By default, SAP considers the mass = selfweight of the structure (based on material and sections property) + additional joint or area mass that may have been assigned. Go to Define>Mass source for other options.

 

[Diquan]

In SAP2000 v11, go to define->mass source and check the 3rd option.

If the 1st one is checked to have to introduce the mass of the elements and any addiontal mass.

If the 2nd one is checked the program is going to calculate th mass from the lods you introduce.

And the 3rd the program is going to calculate it from the elements, loads and any aditional mass you introduce.

For the 2nd and 3rd option you have the tell the program the percentage of dead, live, wind, etc loads you introduce. For my country we use 100% of the dead load, 15% of the live load and 0% of the live roof load.

Also you can define the program to do that if the seismic code is build in the program.

Hope this will help, sorry for my english.

Diquan

 

[stressed]

"For the 2nd and 3rd option you have the tell the program the percentage of dead, live, wind, etc loads you introduce. For my country we use 100% of the dead load, 15% of the live load and 0% of the live roof load."

I agree with using this method for the 2nd option, but it would be incorrect to follow this procedure for the 3rd option. Using this method for the 3rd option would double count the selfweight in the mass model. The 3rd option is "from self and specified mass and loads". That means that by default, self weight is already included in the mass model. If you add DEAD load to that list, since DEAD load by default includes self weight, you will double count self weight in the mass model which could result in extreme errors.

The safest option usually is option #2, following a procedure similar to what Diquan suggests of DEAD (self weight + additional assignments), a reduced percentage of LIVE load, and any other load assignments which may have an effect on the mass model. For example, if you assigned heavy equipment or piping to another load case, it would probably be a good idea to have ETABS convert those loads into mass for your dynamic analysis.

On a related note, it's pretty straightforward to model the foundation as part of the 3D model using slab/shell type element with thickness equivalent to your basemat foundation in order to obtain a more accurate model for dynamic analysis. In reality, the foundation is not "rigid" and massless, and it's reasonable to account for this flexibility if you're running a dynamic analysis. If you decide to model the basemat foundation, you'll need to delete the restraints at the base of your columns and walls, model the basemat as a slab/shell type element, and mesh the basemat shell in order to connect the columns and walls to the foundation shell elements. Next, you will need to select the foundation shell elements, and Assign>Shell>area springs to assign soil springs in all 3 directions. If you have a .15 Kip-in subgrade modulus, you would assign .15 Kip-in area spring in the vertical 3 direction which is normal to the shell area, then assign area springs in the lateral directions (1 and 2 local direction) using a reduced spring stiffness, typically 1/2 to 2/3 the stiffness of the packed soil vertical spring. For example, if you assigned .15 Kip-in area spring in the vertical 3 direction based on subgrade modulus, you might assign .1 Kip-in area spring in the lateral 2 and 3 directions. Using the area spring, ETABS automatically determines joint spring values based on tributary area

If you have a pile supported structure, you would model the basemat foundation the same way, but you would not assign area springs for soil supports, but instead mesh your basemat not only at column and wall joint locations, but also at pile locations and assign joint restraints or joint springs at pile locations with K values calculated by hand based on pile properties, depth and soil properties along the length of the pile. If you wanted, you could even explicitly model the piles as column elements with springs for the soil, but that would probably be overkill for most situations. Make sure there is stiffness in at least the 3 translational directions on your foundation pile supports to avoid numerical instability problems. For pile supported foundations, I've seen rotational springs added too, typically 10% of the vertical pile stiffness

 

[stressed]

if you assigned .15 Kip-in area spring in the vertical 3 direction based on subgrade modulus, you might assign .1 Kip-in area spring in the lateral 2 and 3 directions

Oops, I made an error in the statement above. It should have said .1 Kip-in area spring in the lateral 1 and 2 directions, not 2 and 3. Local 3 is always normal to the area, which in the case of a slab or basemat means vertical