Element Size v Stresses 5

[ellas1]

I am very rusty with FEA. To check the effects of the mesh size with the accuracy of the results, I analyzed two 1/2"x4"x10" simply supported plates loaded with 10 psi on the local Z axis. The first plate was meshed with 1"x1" elements and the second with 1/4"x1/4". The stresses on the 1/4"x1/4" element are double than the stresses on the 1"x1". Based on my hand calculations the bending stresses are close to the results of the 1"x1" mesh.Can anyone explain the differences?

Note: I always thought that smaller elements produce better or more accurate results.

Thank you

 

[corus]

A larger element size increases the model stiffness, and hence reduces the displacments and stresses. A finer mesh will be more accurate so the reason your results agree with the larger element size mesh is pure coincidence. Check both your model and hand calcs.

 

[kellnerp]

ellas1
Can you clarify how your boundary conditions are setup? Are all edges supported or just ends? If ends, the short or long ends?

What element type are you using?

As they say, a picture is worth a thousand words.

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

http://www.linkedin.com/in/engineeringtransport

Phenom IIx6 1100T = 8GB = FX1400 = XP64SP2 = SW2009SP3
"Node news is good news."

 

[ellas1]

Only the two long ends are supported (see attached). Picture a 1/2" deep, 4" wide and 10" long beam supported at the long ends (PIN-PIN). The load is applied as pressure on the local Z axis. I am using STAAD and "Quadrilateral" elements.

Thank you

 

[crisb]

Are the supports pinned i.e. fixed in xyz directions, or sliding at one end i.e. fixed at that end in only 2 directions? I would have thought you need one end pinned and the other end sliding. It may be helpful to post a picture of the deformed mesh and a stress plot. How do deflections compare with hand calcs?

 

[ellas1]

Yes the test plates are simply supported. Pinned on one end and slide on the other (see photo attached with all 4 plates).

Plate 1 (top) - 1" x 1" elements
Plate 2 (mid) - 1/4" x 1/4" elements
Plate 3 (mid) - Half 1"x1" elements and the other half 1/4"x1/4"
Plate 4 (bot) - Only the middle of the plate with 1/4"x1/4" elements and the remaining 1"x1"

The streses at the midspan of plates 1, 2 & 3 are approximately the same at around 3.0 ksi. The strsses at some of the elements at the midspan of the 4th plate are more than double at 7.47 ksi.

 

[crisb]

I don't think your small mesh is joined properly to the large mesh in pictures 3 and 4. Some of the nodes on the smaller mesh are not joined to anything, hence the high stresses at the corners where they are joined.
You need to have the same size subdivision on both meshes where they join.

 

[ellas1]

It makes sence. I guess RUSTY is a compliment.

Thanks CRISB and everyone else.

 

[kellnerp]

Or he needs to bond the mesh if STAAD allows that.

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

http://www.linkedin.com/in/engineeringtransport

Phenom IIx6 1100T = 8GB = FX1400 = XP64SP2 = SW2009SP3
"Node news is good news."

 

[Dasboot]

As mentioned by crisb the transition meshing is critical. Our FEA engineer gave us the attached results. VMmax = 3.02 ksi for 1/4 and 1/10 mesh. 2.97 ksi for 1" mesh.
Ellas can you post your hand calcs. to compare.

 

[Dasboot]

trying to attach plot.

 

[Dasboot]

trying again. Finally!

 

[JpPhysics]

Finer mesh = Better Results is absolutely false. If your mesh is too fine, you introduce an artificial stiffness into the equation resulting in poor or straight up wrong results.

Also, if you have any type of geometry change resulting in a stress concentration and you try to refine the mesh to get more accurate results, you will in fact acheive the opposite. Refining the mesh too much around a stress concentration causes the stress to approach infinity.
O = F/A, as A approaches 0, O approaches infinity.

If you have time in your analysis, you should run the analysis multiple times with different sized meshes. You are looking for a convergence of results. If the results stay fairly consistant between meshes, then you are good to go. If the resutls vary significantly, you need to take a closer look. Remember about the stress concentrations though, you have to go at least 3 to 5 elements away from the stress concentration to get an accurate reporting on the stress in the area.

Anyway, hope this helps.

 

[btrueblood]

"Finer mesh = Better Results is absolutely false."

!!!

"If your mesh is too fine, you introduce an artificial stiffness into the equation"

Never heard either of those before.

"O = F/A, as A approaches 0, O approaches infinity."

But if A is going to zero, won't F go closer to zero too?

"Remember about the stress concentrations though, you have to go at least 3 to 5 elements away from the stress concentration to get an accurate reporting on the stress in the area."

Unless the stress concentration is real...

 

[DanStro]

I have to agree with brtueblood. The way I understand how (typical) FEA software works is that the displacements are calculated. From those the strains are found and using the strains along with the material properties the stress is found. The area isn't playing into it, except for when the user wants the software to output something like contact area but that doesn't affect the accuracy of the results.

That being said I don't think that in EVERY case a finer mesh gets better results. I can't remember where I read it but I have a book that shows an example of a super fine mesh having some numerical instabilities that were not present in a coarser one. It may have been due to the element formulation just as much as the mesh density. But I think that in vast majority of cases as long as the element types are appropriate a finer mesh will give more accurate results.

Dan

Han primo incensus

 

[btrueblood]

I guess I could buy numerical instability (esp. if doing FEA on an 8-bit machine?), but not artificial stiffness. Numerical instability would tend to just give increasingly noisy results, or throw errors? Another possibility would be if the increasing mesh density was done poorly and resulted in grossly mis-shaped elements.

 

[JoshPlumSE]

How the elements behave with a very fine mesh depends on the element formulation. Most modern plate elements are pretty robust and can be sub-meshed very fine without experiencing the "Shear Locking" effects that old elements used to get. That may be what JpPhysics is referring to.

However, every element should have a point beyond which meshing further will not give better results. I'm not sure that I would call this "artificial stiffness". Rather, I prefer to think of it as meshing to a point where the plates are so think that the assumptions used in the derivation of that element are no longer valid.

 

[EngAddict]

No, shear locking will only be reduced by refining mesh density.

Numerical instability is due to the code being used, not the FE theory, but would be the only plausible reason IMO. If you could modelled steel with elements approaching the grain structure of steel would you not gradually approach an error less model?.. Now there are many variable in play that could could prove this untrue but theoretically many of the 'approximations' made by engineers to simplify a problem to a workable 'model' will be removed.

 

[JoshPlumSE]

In response to EngAddict:

Are you referring to 8 node solid element modeling or 4 node plate element modeling?. I cannot see using a plate element with a width equal to the "grain structure" of steel producing a reasonable result... at least not with the plate elements that I've seen used for most structural applications. Not sure what you're getting at there....

 

[EngAddict]

I was giving an example using solids, obviously you can't reproduce a 3D object with a 2D plate. However the point is the same, discretisation errors alone will be reduced for most real world applications.

What are you getting at.. you believe mesh refinement will lead to increased errors and unreliable stress results? An interesting view point..