0
$\begingroup$

This is my first time performing an FEM analysis, and I'm using the Ansys Workbench and Mechanical software.

My situation is pretty straightforward--it's a straight beam that is fixed at one end and displaced at the other end in the transverse direction, causing a significant amount of bending. I have attached screenshots from the analysis software so you can see what I'm describing.
enter image description here enter image description here

Material
Thermoplastic Polyurethane (TPU): $S_y\approx60~\text{MPa}$, $E\approx2.4~\text{GPa}$, $\rho \approx 1210~\text{kg/m}^3$

Boundary conditions

  1. Fixed anchor on exterior surface of the base
  2. Displacement of 1.2 mm in the x-direction on an edge of the snap feature hook, fixed in y, and free in z

Mesh: Generated automatically, 18677 elements

Results
$\sigma_\text{max,global}\approx4.45\times10^8~\text{Pa}$
$\sigma_\text{max,fillet}\approx4.05\times10^8~\text{Pa}$
$\text{SF}_\text{fillet}\approx0.15~~~\therefore~~~\text{failed}$
enter image description here enter image description here

As you can see, the maximum stress in the part is extremely high and the part will supposedly yield far before it reaches the necessary deflection. I do not believe these resulting stress numbers are accurate from my experience with the TPU material (not much, but I can visualize its behavior in this scenario). I do not have the means to prototype the part right now, otherwise I would perform an experimental comparison.

I would like to ask for the opinions of this community about whether these stress numbers seem accurate for the given properties, geometry, and boundary conditions. If there is a problem, in the software or otherwise, I would appreciate any advice on how to fix it. Let me know if there is more info I can provide, thanks a lot!

$\endgroup$
5
  • $\begingroup$ The only way to determine if the stresses are accurate is to do a mesh convergence study. Refine the mesh, use quadratic elements, etc. and see whether you converge to a (relatively) steady solution. $\endgroup$ Aug 13 at 20:49
  • 2
    $\begingroup$ The mesh in your picture looks rather strange. Presumably the very small and distorted elements around the edges were an attempt to auto-mesh small fillet radii. It would be better to delete those from the geometry (or tell the software to ignore them) and make a FE model with "sharp edges and corners." Also the elements seem to have straight edges. Elements with mid-side notes and curved edges will give much better results around the large radii. $\endgroup$
    – alephzero
    Aug 14 at 3:25
  • $\begingroup$ @alephzero what are "mid-side notes"? Is it some quadratic of higher order element formulation? Btw I wanted to upvote the comment because it also look to me that the mesh is funny. However I double clicked it and then I couldn't upvote it again $\endgroup$
    – NMech
    Aug 14 at 8:56
  • 1
    $\begingroup$ @NMech I believe he is speaking of midside nodes. From what I understand, they increase the effectiveness of tetrahedral elements by placing a node at the midpoint of each edge of the element, thus reducing its rigidity (great for corners, etc.). $\endgroup$
    – Benjamin
    Aug 14 at 16:59
  • $\begingroup$ Ok nodes... Yes that makes sense... $\endgroup$
    – NMech
    Aug 14 at 17:00
3
$\begingroup$

First of all, whenever I see stresses so localised near the boundary, I always think that there is something wrong.


IMHO, the max stress at corner is an artifact, probably due to overconstraining the model. I.e. I expect you have fixed the entire face, and as a result there is an additional (non-real) component of the stress. There may be other factor assisting that (like poor quality/aspect ratio of the mesh locally etc).

In any case, what you could do to test that is, change from fixing the entire surface to the following three conditions:

  • fix the normal to the surface translation direction for the whole surface.
  • fix one corner for all translation directions
  • fix another corner to one of the inplane directions

That should provide adequate fixture to the model (I hope I am not forgetting a dof), and it will also let the model contract/expand due to the Poisson ratio. For the same mesh you should see more reasonable results.

Element size Fixed not overconstrained
Coarse 5 mm enter image description here stress 21.4 kPa enter image description here stress 24.8 kPa
Fine 2 mm enter image description here stress 23.3 kp MPa stress 26.7 kPa
Ultra Fine 1 mm enter image description here stress 28.48 kPa enter image description here stress 26.1 kPa

Notice for the "not overconstrained model" that for the Coarse mesh, the stress at the corner is less (due to averaging). As the mesh becomes more refined, the stress converge to their "real" value. This is not something that occurs in any of the other examples.


Additionally I expect that near the fillet area you also have a geometry/meshing artifact. I.e. the value does not correspond to real stresses.

You can test that by refining the mesh size more (smaller elements). Depending on the material model you are using you should see a further increase (I did not misspell) of the stress at the fillet.

By increasing the element size the problem should be mitigated around those edges.

Element size R = 1 R = 5
Coarse 5 mm enter image description here max stress 60.9 kPa enter image description here max stress 47.1 kPa
Fine 2 mm enter image description here max stress 69.7 kPa max stress 50.4 kPa
Ultra Fine 1 mm + max stress 82.6kPa enter image description here max stress 52.6 kPa
$\endgroup$
1
$\begingroup$

You have a small re-entrant fillet radius which creates a large stress concentration. In real life, either there will be a small region of plastic yielding, or a crack will start to form.

I don't have any experience with thermoplastics so I have no idea what would actually happen.

If you are comparing the FE model with a hand calculation using beam theory (or something similar) the hand calculations ignore the stress concentration.

Stress concentration around the fillet and feasible modification.enter image description here

Large fillet

enter image description here

$\endgroup$
3
  • $\begingroup$ I deleted @r13's picture showing "deformation magnified 2000x" because whatever it showed is just an artefact of the plotting process, and not useful from an engineering point of view. $\endgroup$
    – alephzero
    Aug 14 at 3:30
  • $\begingroup$ Sorry to piggyback on your posting which I consider has already adequately answered the OP's question but lack of visualization, one of the better tools for engineers especially the younger ones. But, it's your answer. $\endgroup$
    – r13
    Aug 14 at 11:46
  • $\begingroup$ Thank you for the visual, but what do you mean by "the hand calculations ignore the stress concentration"? I performed hand calculations to create the beam geometry, and I chose the current fillet radius to minimize stress concentration at that edge (any larger fillet should not reduce the SCF significantly). $\endgroup$
    – Benjamin
    Aug 14 at 16:14
0
$\begingroup$

I have not performed with FEM, but maybe is this effect from static rigid bodies:

when two rigid links are fixed and a force is applied in the middle, the reaction force in links tend to infinity. Since there is no perpendicular reaction, reaction on the linked part tend to increase in order to achieve static equations.

enter image description here

Maybe you need to increase the number of nodes, avoid floating edges with restrictions or use fixed points not the entery plane.

$\endgroup$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.