Using Staad.pro to model dynamic loading problem

[nkclarke]

I'm unsuccessfully trying to analyse a frame that is subjected to dynamic fluid loading. I'll describe the structural problem, how I want to model it using STAAD and why I don't trust the output. I'd welcome any suggestions on how I can get it to work or if STAAD just isn't up to the job.

I have a space frame that is subjected to a force time history loading extracted from CFD analysis. More specifically, the horizontal beams at the top of my frame is subjected to the time history vertically upwards loading that is read in from a text file. Because the columns cannot be connected to the base slab (for reasons to prevent damage to the floor), they need to be connected into heavy concrete blocks (kentledge blocks) instead that have sufficient mass to limit uplift of the entire structure to perhaps 50mm off the ground.

I thought the problem would be relatively simple for STAAD. I wanted to create spring supports at each of the columns with a large stiffness that only allowed a few millimeters of downward vertical displacement (since the whole thing is sitting on a thick concrete slab) but in the upward direction I wanted to allow the structure to uplift as much as it needed to under the substantial upwards force time history (that is, the spring only acts in compression and not at all in tension).

My first problem is that STAAD does not appear to like it when I try to use compression only springs for a dynamic analysis and gives an error when I try to run it. I thought I might be able to work around it by using a normal spring but it's not very satisfactory. I don't get very good results since I did some hand calculations and STAAD seems to give a very high upwards displacement compared to my calcs (STAAD gave 400mm uplift compared with 20mm in my calcs). In addition, my colleague created the same model in Abaqus and his uplift agreed with the hand calcs.

Is it true that I can't use the compression only springs for a dynamic loading problem? Does anyone have any information or tips that might help me obtain more realistic uplift values? Why is STAAD giving me highly exaggerated uplift compared to all other methods?

I can provide additional information on my model if needed. Thanks for any help.

 

[JoshPlumSE]

I don't think you're going to be able to do this type of analysis with STAAD. If I remember correctly, STAAD's Time-History analysis is based entirely on modal super-position. If so, then I don't believe it will allow for any non-linear behavior (compression springs or such).

From what it sounds like you're looking for a true non-linear time history analysis. Best stick with SAP2000 for that. Though I imagine that Abaqus would work as well.

It does seem odd that using a linear spring would result in such a large discrepancy btw STAAD and Abaqus though. How many modes have you solved for in STAAD? What is the frequency of your input accelerations or forces? Generally, you want to capture modes with a frequency of about 4 times your input / load frequency. What is the time step of your integration? Generally, you want to have the time step be about 1/20th of the input / load frequency.

 

[WARose]

I’m not sure I understand your support condition......if these blocks have sufficient mass to hold the base down with any calculated reaction (which they should) than why model the base as compression only?

 

[nkclarke]

Thanks for the replies. JoshPlum, that's disappointing that I might not be able to do this type of analysis with STAAD since I've burned quite a few hours in the budget already building the model. That'll teach me to start off with a simple model to test out the features of unfamiliar software. Despite that, I'm still interested in finding out why Abaqus isn't giving me similar displacements when both models used linear springs. I'm still hopeful of finding a solution for that and thanks for taking an interest.
Perhaps my answers to your questions will go some way to finding out. Forgive me if I don't answer correctly; I'm not a dynamics expert but I'm trying to learn. I solved for a lot of modes - possibly 200. The first mode had at least 64% mass participation and the 3rd had about 36% in the vertical direction. The frequency of my force time history was every 0.1 seconds (is that what you meant?). I'm not entirely sure about what you meant by asking the time step of my integration. I'll take a guess and assume you're asking about the following STAAD input paratmeter
DEFINE TIME HISTORY DT 0.0013888
If that's not what you meant, could you please clarify and I'll provide an answer. If that is what you meant then it looks like my time step might be too low. Do you think that might be causing a problem?

WARose, The problem is that my blocks don't have sufficient mass to hold down the structure. I know that under the dynamic loading, the structure will uplift by as much as 20 to 50mm but this is what I want to know. I wanted to use compression only springs so I could make it stiff in the vertical downwards (compression) direction whilst making the spring stiffness weak in the upward (tension) direction.

 

[WARose]

If your blocks have insufficient mass to stop the uplift forces it will see from this dynamic force……it may be better to model them as mass attached to your structure (rather than as a support). In STAAD you would do this by applying a static force where the mass is attached.

Since you say this mass (at least as I understand you) would be in contact with the ground when the dynamic force has gone ½ cycle (i.e. in compression) and would be much harder to displace......you may have to do 2 models: one as I describe above (with those points modeled as mass attached) and a second one for the case where the blocks are being pressed upon (with the necessary checks for both).....in the second one the blocks would be modeled as a vertical spring (with equal stiffness in compression and tension).

By the way, frequency is typically expressed in cps (cycles per second) or Hz. Your DT value seems ok (I think it’s the default value).

When it’s all said and done you may want to verify with hand calcs (as Josh suggested).

 

[WARose]

By the way, for the uplift case, you say you have concrete blocks attached to the frame that have insufficient mass to take care of the uplift force……..just a question here: there are other supports right? The reason I ask is: if these concrete blocks are the only means of support and their mass is less than the (applied) unbalanced force……that’s an unstable structure. You don’t let that happen on static loading and it shouldn’t be anywhere near happening for dynamic loading. (It think the last equipment foundation I did, I had a factor of safety of about 60 in the vertical direction for that.)

Without seeing a picture of the whole system…..this is something that just jumped in my mind.

 

[JoshPlumSE]

I'm not all that familiar with STAAD. Back when I used it (late 1990's), it was not capable of doing a time-history analysis.... So, my knowledge is more related to generalized Time-History analysis.

It sounds like your "DEFINE TIME HISTORY DT 0.0013888" refers to a integration time step of 0.0013888 seconds. You said the approximate natural period of your input loading is 0.1 seconds. By my estimate you'd then want to have a maximum integration time step of about 0.005 seconds (1/20 the period of the input loading).

One other thing to look at is what your input Mass units are. Does STAAD allow you to input the weight of your structure and automatically convert to mass, or does it force you to define it in mass units? I've seen many models where the user has accidentally defined their mass as if it were in kips without dividing by the acceleration of gravity... which gives them a total mass of 32.2 or 386.4 times their actual mass (depending on whether their units are feet or inches). The biggest clue is usually when the natural periods of your structure come out much higher than you expect. If you made that mistake, it could easily cause the large discrepancy in the deflections between STAAD and Abaqus.

Whenever I'm investigating odd dynamic analysis results, I always check to see that the natural period is approximately equal to:
T = 2*pi*sqrt(M/K) = 2*pi*sqrt(W/(K*g))

If it's not, then I know that I've done something wrong in the model.

 

[WARose]

STAAD lets you input the weight without converting to mass. (It will make that conversion itself when it creates the mass matrix.) You just have to specify your input units.

usally, I've gotten DT by: (1/F[cps]) X 8 (8 points on a full cycle)

A lot of times that's given me too small of a time step and STAAD will default to s larger one (the 0.0013888).

 

[WARose]

Pardon me, above for DT I messed up the formula. It should be (1/F[cps]) / 8

 

[nkclarke]

Thanks again for your continued contributions guys; it's really helpful. I thought I'd give a little more background and clarification into what I'm trying to achieve with my model. Here's what I've got;
There is large tank filled with liquid inside an enclosure with a RC wall around it. If the tank catastrophically fails then there's going to be a big wave heading towards the bund wall. The structure I'm trying to analyse is a space frame that's going to be constructed around the inside perimeter of the existing (inadequate) bund wall. The part of the frame against the wall will have steel plates attached to it to prevent the liquid from going over the top. There's also a horizontal "roof" at the top about 6m long where the purpose is also to prevent the liquid going over the top. I can't fix the columns of the space frame to the existing floor so I have to rely on mass to limit uplift to a reasonable height. It's an accidental loadcase so I'm not overly bothered if there's some uplift. The whole structure can jump into the air a little bit if it wants to, then fall back down again. I can't get sufficient mass through the selfweight of the steel structure alone, so I want to give it additional mass by pouring a layer of concrete at the bottom. The dynamic loading phase lasts about 1 second and reaches a peak upwards load of about 800kN which is distributed over the members that comprise the "roof" (there's horizontal loading too but let's keep things simple). I wanted to use a spring where it was stiff in the compression direction but weak in the tension direction but that doesn't seem possible for STAAD due to the reasons that Josh mentioned previously. If I apply a linear spring then my dilemma is how stiff to make it. If I make it stiff to avoid excessive compression since it's resting on a concrete floor then under the upward loading the upwards deflection will be unrealistic. If I make it weak then it's going to compress a lot under its own weight. I have applied the concrete load to the bottom of the concrete as joint loads which I understand will get converted to mass.

I'm not really sure how I'd calculate the natural frequency of the overall structure either. Should I do some sort of pushover analysis to find the stiffness?

I hope the above has given you a little more insight into my goal and perhaps will prompt you to think of alternative ways of using STAAD.Pro to helping me how much the structure will realistically uplift. Thanks again for all your good ideas so far.

 

[WARose]

I was under the impression this was more of a sinusoidal type force application.....but apparently it’s more of a ramp loading. I think STAAD can do that type of loading but I’ve always found it more convenient to put a Dynamic Load Factor (DLF) on the equivalent static load (i.e. create a quasi static load) and analyze it statically.

The maximum DLF is 2…..but typically it is a great deal less (it just depends on the duration to period ratio).

STAAD has a command to calculate the natural frequency of a structure……you just have to look in the help manual (you can click on the on-line manual to see some examples). In post-processing, you can get the period and frequency per mode.