×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Element Size v Stresses
5

Element Size v Stresses

Element Size v Stresses

(OP)
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  

RE: Element Size v Stresses

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.  

RE: Element Size v Stresses

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
www.engtran.com  www.niswug.org
www.linkedin.com/in/engineeringtransport
Phenom IIx6 1100T = 8GB = FX1400 = XP64SP2 = SW2009SP3
"Node news is good news."

RE: Element Size v Stresses

(OP)
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         

RE: Element Size v Stresses

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?

RE: Element Size v Stresses

(OP)
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.

     
          

RE: Element Size v Stresses

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.

RE: Element Size v Stresses

(OP)
It makes sence. I guess RUSTY is a compliment.

Thanks CRISB and everyone else.   

RE: Element Size v Stresses

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.

RE: Element Size v Stresses

trying to attach plot.

RE: Element Size v Stresses

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.

RE: Element Size v Stresses

"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...

RE: Element Size v Stresses

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

RE: Element Size v Stresses

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.   

RE: Element Size v Stresses

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.  

RE: Element Size v Stresses

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.

RE: Element Size v Stresses

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....  
 

RE: Element Size v Stresses

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..

RE: Element Size v Stresses

EngAddict -

I was limiting my discussion to plate elements only since that was the nature of the OP's question.  With most plate elements there is a thickness to least width ratio beyond which the element formulation begins to degrade and results do not improve with further sub-meshing.  In fact, the results are supposed to degrade.  

RE: Element Size v Stresses

Thanks for the clarification.

I don't have any references that support this, perhaps you could list some for my own understanding?

All my testing on plates elements show the stress converging then not increasing any discernible amount, but not degrading..

These stresses at my convergence point match very accurately the hand calculations too.

Therefore I can only conclude that the mesh should be refined until the stress converges, regardless of whether using solid elements or plate elements. Any further refinement will not compromise the results but will only waste computational time.

Maybe the observation of stress degradation is limited to a particular plate element type with a few select codes? Perhaps now outdated with newer code revisions?..

RE: Element Size v Stresses

when modelling spot welds in a plate model using beam elements node to node connected a fine mesh can lead to stiffnesses that are too low due to local bending deformation.

Also if you are talking about a 20mm thick plate you wouldn't use a 1mm mesh size.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources