3-D "brick" elements

[abusementpark]

I was told that the three-dimension brick elements exhibit higher stiffness than you will see in a physical test. Can anyone elaborate on this? Or refer me to a paper that has quantified how much of a difference it can make?

 

[EdR]

It is impossible to provide an answer to the question you pose as the results obtained using (any) elements are dependent on the modeling not on the specific element....

Good results can be obtained with linear elements, parabolic elements, and even higher order elements than parabolic depending on how the elements are used, etc. Of course the particular mesh used with each type of element will vary to achieve the same (or equivalent) results........

Ed.R.

 

[Stringmaker]

You have to be much more specific in your question. Certain brick elements can be much stiffer than actuality. For instance, fully integrated 8-node brick elements exhibit shear locking when subject to bending. On the other hand reduced integration 8-node brick elements exhibit low or no resistance to other deformation modes for certain loadings. 20-node brick elements can be flakey too. You don't need to take a course in finite elements but you should read the user documentation of the software you use and understand what flaws certain elements can be subject of. This varies from package to package.

 

[abusementpark]

The specific problem I am looking at is an I-beam modeled with the SOLID45 (8-node) element in ANSYS. It is a simply supported beam, with a concentrated load at a quarter point along the span. It is a shear-controlled beam. The ultimate load I am achieving is corresponding well with experimental results as well as the overall behaviour, but the model is exhibiting significantly more stiffness that the physical test.

 

[johnhors]

"It is a simply supported beam," - this infers that there are zero displacments at the supports in your model. In reality this never happens, the infinitely stiff support does not exist. Try a hand calculation to estimate the stiffness of the supporting structure and then support your model with springs to ground using your calculated values.

http://www.Roshaz.com

 

[crisb]

Try parabolic elements or a substantial increase in the number of linear elements. I would expect this to give a better deflection estimate.

 

[Cmfg]

By three-dimension brick elements I suppose you mean 8-node bricks. These elements cannot represent properly bending. Technically speaking, much of the potential energy is consumed by spurious modes. In addition, if the beam that you are modeling is very slender you could have a phenomenon called locking. To overcome all those problems you should use 8-node bricks with enhanced modes, 20-node bricks or 8-node bricks with hourglass control.

 

[corus]

For an I beam I'd consider using thin shell elements.

corus

 

[EngAddict]

I would also use shell elements for this. Either way I would never use first order elements for stress analysis only displacement.

I think if you compare tet elements to brink elements you may find that the tet elements are slightly stiffer based on the inherent nature of their geometry. However, this varies from program to program, and between elements also.

 

[kellnerp]

Any FEA text book will cover this. Lookup Cook and FEA on Amazon.

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[ajose]

This is a very interesting issue. The model give some differences with prototype.

Your question is not very clear, so my questions are going to be some general ones:

I have some question about the match of the boundaries conditions including loads.

The supports, area of supports or border conditions, Are they accuracy enough?. It is seem if you over look the same, but if you compare the relations of the contacts areas, the location of rotation point on the support area of model and prototype, are the same?.

Something just like this could be told of the load application point.

To void this kind of problmes i normally model part of the support before reach the infinite stiffness support. I did the same with the point of load application just to have the same concentration load.

This one is a silly question but, did you test on elastic behavior of the material for model and prototype?

Besides that what ther hand what kind of 8 element did you use?, there is a lot of them, could you be more specific.