difference between Elemental and element nodal?

[Walterke]

Can anyone tell me what can cause a big difference in results between elemental and element nodal stresses? (von mises)

I'm calculating a point load on a sheet to be used as the floor of a work platform. The tolerated stresses are 50N/mm² (aluminum+safety factor). With elemental stresses the maximum stress is 38, but with element nodal, the maximum stresses go over 100.

I've tried making the mesh both smaller and bigger, but neither seem to help.

Any ideas?

NX 7.5
Teamcenter 8

 

[BlasMolero]

Hello!,
Elemental stresses are computed at the center of the element, and nodal stress is the average of all the elements that contribute to that node, take a look here:

http://www.iberisa.com/soporte/femap/tensiones_nodales.htm

In general, you must take in cosnideration both values: nodal & elemental stress, the real life will be between them.

In order to make the finite element results to be reasonable you must pay attention to the way you prescribe loads & boundary conditions: if you apply a point load in a node, the stress at that node is infinite, then this is not a correct procedure. Please note real life is complex, then your model should reflect this, loads are applied in a region, not in a point, then better apply pressure loads instead nodal forces.

The same to say with constraints: in real life nobody cosntraint an isolated point, but a region, etc..

Also the quality of mesh will affect the quality of results as well: is you mesh with triangle or tetraedral elements with a highly distorted mesh you will have high stresses values, the high values are artificial, not real, the reason is the bad quality mesh. Instead, I suggest to mesh with CQUAD4 or CHEXA elements, you will realize of the difference ...

In summary: compare results, use a mesh with reasonbale quality & elements size, check how you apply loads & constraints, make real assumptions, if not the FEA results will be nothing.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[Walterke]

Thanks a lot for the info. The problem is that our norm EN280 describes the following:
"The mass of each person is assumed to act as a point load on the work platform"

So, in that way, I am obliged to use a point force.
I've considered creating a circular region and applying the force there, but the difference in resulting stresses between, for example, a circle with diameter 50mm and one with diameter 100mm is rather big, and I'm not really sure if I'm allowed to do this.

The only 3D meshes I can chose from are Ctetra10 and Ctetra4. Since the construction is built up out of tubes and sheets, I find it easier to work with 3D elements rather then with 2D. Should I change this?

NX 7.5
Teamcenter 8

 

[BlasMolero]

Dear Walterke,
The combination of Point load + CTETRA elements is a bomb, you will have high nodal stresses for sure: you are mixing a detailed 3-D solid mesh + global point load, and this is not correct. To understand better: point load are valid for CBAR/CBEAM 1-D elements global models, no problem to prescribe loads or moments in a node of the beam, but if you mesh with CTETRA solid elements this is a detailed mesh, and then your loads & BCs should be in consonance of this meshing approach, you should prescribe loads as pressures.

In the mesh side, if you look for accurate stress results, CHEXA 8-node 3-D solid elements & Shell CQUAD4 4-nodes 2-D elements should be your choice, any other option should pay a price in the accuracy.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[johnhors]

Dare I say it, but your "norm EN280" was either written by people with little or no understanding of FEA or more likely it is not in fact a guide on how to build and run your FEA. Does it just describe the contribution from the mass of persons in a free body diagram?

As Blas pointed out, applying point loading to a model built of continuum elements is unacceptable. If you are interested in stresses at the point of application of the load then you will have to make the model as realistic as possible, using pressure loading (varying over the floor?).

DO NOT USE 4 node tetrahedral elements! However a fine mesh of well conditioned 10 node tetra should be accepatable.

http://www.Roshaz.com

quality, cost effective FEA solutions

 

[Walterke]

The EN280 is the European standard and I'm not sure if it was created with FEA in mind.

As said before, the mass of each person(=80kg) has to be considered as "point" loads. The mass of equipment can be regarded as an evenly distributed load.

I'm currently trying to figure out how to properly apply a chexa to my part. I'll let you know how that went.

How do you define "well conditioned" regarding the 10 node tetra mesh?

The floor would consist out of a 2,5x0,8m² alu sheet with 2,5mm thickness, supported by several 2mm thick steel sheets and/or tubes (still trying to figure out which will be better/lighter/stronger)

NX 7.5
Teamcenter 8

 

[Walterke]

So I changed the mesh to a CHEXA(8) and now the difference between my elememtal and my element-nodal stresses is even bigger (factor 10).
I guess applying point-loads really is a no-go here...

Is there any standard way to apply the force of a human being standing on a plate?

NX 7.5
Teamcenter 8

 

[Walterke]

Bumping with further actions:

I applied a the force on a 300x160mm² rectangle which gave a decent result.
I also calculated it manually using roark's formulas for stress and strain, and got about the same results.

Would you consider the area I used a good reference (it's about the size of 2 shoes)

NX 7.5
Teamcenter 8

 

[ZeroExperience]

Good job on the verification.

 

[trainguy]

If someone named ZeroExperience tells you you've done a good job, have you really done a good job?

tg