Lumped mass model

[Sajjad2164]

I would like to get information about the equivalent or stick mass model (lumped mass model). I would like to know what this method is based on. I want to represent a big pressure vessel and its surrounding structures as beam-column elements and investigate the structure's response to seismic excitation.

 

[SWComposites]

Presumably it assumes the masses are more important to the response than the structural flexibility.

Frankly I have no idea how a pressure vessel could be represented as a beam-column; doesn’t seem to make sense.

 

[ThomasH]

I don't quite understand your question.

A lumped mass model usually means a simplified mass matrix and that can be used for any element type. You should be able to get a reasonable description with Google.

Regarding the analysis of a pressure vessel with a surrounding structure. The surrounding structure is probably possible to analyze with beam/columns, depending on the geometry. I have not worked a lot with pressure vessels but for the "non-pressure" vessels I have checked beam/columns would not have worked, due to the geometry.

 

[JoshPlumSE]

That's a bit of a weird question. Maybe you haven't fully explained yourself very well. But, I'll give it a shot:

a) Generally, a lumped mass model is exactly what it sounds like, the mass of an element is lumped into the nodes that define it.
b) Practically speaking this means that you might need to sub-mesh the model if you want to get mode shapes or dynamic response along the width of the original element.
c) Also, you have to check with your FEM package, but my impression is that most program will lump the mass into ONLY translational mass and do NOT include mass moment of inertia. That just means that the ROTATIONAL modes and response at those node wouldn't be directly captured. If that response is desired, the solution is the same as item (b).... meaning that you'd have to sub-mesh the model to encourage these modal shapes / response.
d) Finally, if you have lumped mass associated at nodes that restrained rigidly (i.e. support points) then this mass will essentially be lost and it will not be possible to capture it's response.

 

[Sajjad2164]

Thank you all!
Let me explain what I mean by a lumped mass model of the pressure vessel and its surrounding structures. Please look at the attached article; you will notice that the structures are equivalent, with some beam-column elements and several mass points. I want to learn how these mass points should be placed to represent the nearest behavior of the structure. How should the beam sections be defined?

 

[centondollar]

Just use a FE solver of your choice with shell elements and either consistent mass matrix or a diagonal (also called lumped) mass matrix and solve the response with e.g., implicit time integration. A pressure vessel is typically not of such dimensions that it can be estimated to be a collection of beams, and most paying clients could be expected to reject technical reports founded on such models.

Is this an academic exercise?

 

[GregLocock]

Back in the day we were wavefront limited in FEA and wasted an enormous number of engineer years trying to replace shells with beam/mass equivalents.

OK, thanks for the link, yes that looks feasible, as they have approximated each cylindrical tower as a series of beams and point masses. You'll need at least 3 points per half wavelength of each mode, and you'll need the section properties of each part of each tower to derive its mass and equivalent beam.

However it is an awful lot of error prone work compared with knocking up a shell model.

On my quick read of the paper they don't explain why they bothered with the lumped mass model, although 'just to see if it works' is a valid reason in itself.

Cheers

Greg Locock


New here? Try reading these, they might help FAQ731-376

http://eng-tips.com/market.cfm?

 

[Sajjad2164]

Thanks!
The best answer to why this method is used is that if you use even shell elements, you will encounter a huge model, which is time-consuming and computationally heavy to be solved with even workstation units. This is a solution to solve the problem with ordinary computers.

 

[centondollar]

A linear dynamic analysis should not be too computationally heavy for a modern workstation. The model size can be reduced by selective mesh refinement, and if you don't include plasticity, the mesh need not necessarily by very refined to obtain results useful for design or capacity checks of existing structures.

 

[ThomasH]

According to the paper the model has ~400 000 modes, it's large but I don't think it is unmanageable. And from what I can after a quick reading, the solution is linear. If it was non-linear the solution and involved plasticity, that could take time. It also debends on how many iterations the analysis requires. Is it one analysis to check the structure ore several to also modify.

Keep in mind that the article is nearly 10 years old, and some of the references is another 10 years.

But as a research subject for a paper I think the question is valid.

 

[gnc89]

Hi Sajjad,

One of the ways to arrive at the simplified model with mass points and beams is to use super elements (Matrix50 element type in ANSYS). You start with a 3-D model and divide it in few sections and define a master node at start and end of these sections i.e. two nodes per section. Then create a super element (with two nodes - master nodes defined previously) for each section which essentially reduces the section to masss (mass point) and stiffness matrix (your beam section). Do this for each section and use these super elements to define your 1-D model.

If you are wondering why not use 3-D model directly the reason is not because the model isn't solvable due to sheer size of model but due to number of load cases for which it needs to be solved. The seismic (earthquake) analysis is probabilistic in nature and the number of load cases ranges from anywhere between 50 to 200. On top of that, one is in interested in complete time history of response where the total time ranges from 20-50 seconds depending on the norms used for analysis. Hence it is worth to get the dynamic response in 1-D model and use output of force from dynamic analysis as input to stress analysis which is done on 3-D model.

 

[rb1957]

I see this method as being fraught with potential "finger" problems. Ok, you may have a super complex model, clearly looking for detail results.

This method is probably not very accurate, maybe conservative, but not what you want to "hang your hat on". I might use this to iterate the design, and then run the final analysis through the full model. Instead of this, I'd be more tempted to simplify the detail model for something to cycle through quickly, and then the full model for the final run.

"Hoffen wir mal, dass alles gut geht !"
General Paulus, Nov 1942, outside Stalingrad after the launch of Operation Uranus.