what's the differences between BEAM and BAR element

[lihouxin065]

FIG 1 BAR elementFIG 2 BEAM elementFIG 3 BAR element or BEAM element ?FIG 4 BAR element or BEAM element ?FIG 5 cross section of FIG4 ,shear center and the neutral axis does not coincide

[John_Holtz · Accepted solution]

Hi @lihouxin065

If the website from which you got the images does not describe the differences between a beam and bar element, then this website is a good source: http://www.stressebook.com/beam-and-bar-elements/

Here is some of the information from that page.

Similarities between BEAM and BAR elements: What is common?

• Both are 1D elements or line elements
• Element orientation definition methods are the same
• Both elements follow the classical beam theory, meaning plane section remain plane
• Both elements are capable of including shear deflection using shear area coefficients (more important for short stubby beams or bars)
• Both elements are capable of including nonstructural mass per unit length effects
• Both elements have 4 data and stress recovery points on the cross section
• Both elements are capable of up to 10 data points along the element length

Between the beam and bar elements, the beam element is capable of doing more as listed below:

• Beam elements can have tapered sections, meaning one end can be smaller/larger/wider/narrower/thinner/thicker than the other, but the shape cannot be totally different.
• Beam elements are capable of accounting for large deflections and differential stiffness due to large deflections
• Beam elements can have three different offsets. One for shear center, one for the neutral axis and one for the nonstructural mass axis. Whereas bar elements have only one axis, all three are the same neutral axis.
• For a bar element the grid points are located at the section centroidal neutral axis. For beam elements they are always at the shear center axis and the neutral axis is offset from the shear center axis. See figure 2 for more information.
• BAR elements are best for doubly symmetrical sections with load applied along centroidal planes, as they are not capable of accounting for bending or twisting or warping of the sections due to axial or transverse loads. This is only possible with BEAM elements.

The answer to Fig 4 is neither. Because the "beam" is short, it should be modeled as a solid.

Let us know if you have any other questions.

[lihouxin065]

thanks for your reply,

it is a column with eccentric axial load in fig4,

column with eccentric axial load

Which element type is properly in Nstran inCAD?

[John_Holtz · Accepted solution]

Hi @lihouxin065

The new figure is completely different from the original Figure 4 . If you have any doubts, use a beam element. It probably takes 2 seconds longer than using a bar element, so there is not much difference. (Actually, I have not done any tests to compare the run times, but I would not expect it to be that much different.)

From an education point of view, the difference for an eccentric loaded column comes down to these two items:

• What type of analysis are you performing? Linear uses small displacement theory, nonlinear can use large displacement theory. Beam elements are capable of accounting for large deflections and differential stiffness due to large deflections.
• Is the cross-section symmetric about two planes? Is the load in the plane of symmetry? BAR elements are best for doubly symmetrical sections with load applied along centroidal planes, as they are not capable of accounting for bending or twisting or warping of the sections due to axial or transverse loads.

[lihouxin065]

thanks

[Anonymous]

Good morning to all,

at first sorry for my bad english.

I'm attending this post, because I'm having some trouble about the correct definition of a Bar or Beam elements.

If I understand well , John Holtz is saying that both elements act with 6 d.o.f. at each node, with only a second level difference in behavior. And I just tested that solving an easy simply supported beam, bar and beam give the same result, using large displacements approach.

So, my question is: how to have a ROD (3 d.o.f. per node) element in Nastran InCAD?

Thanks

[Roelof.Feijen]

Hi @Anonymous ,

Rod's are part of the Connectors. They can be defined between 2 points (sketch points, work points).