Convergence analysis for plate with a hole 1

[cspkumar]

Hi all,
I have a plate of 300*300 mm and a hole of 20 mm. I have applied a tensile pressure load of 200 MPa. I want to find the stress concentration factor. I have developed a quarter-symmetric model. I have used first-order plate elements. And this, is what I find when I do the convergence analysis.

No. of elements Stress Concentration factor
29 1.236666667
116 1.474666667
464 1.544666667
1856 2.188666667
7424 2.599333333
29696 3.733333333
118784 3.509333333

The SCF for a plate with a hole for the dimensions I have should be 2.81 (from Strength of Materials text book). But, I am unable to converge it to that value. What is happening here? Any sort of stress stiffenning?

Thanks
Kumar.

 

[FeaGuru]

It looks like it has not converged yet. Instead of just adding elements, refine the mesh locally (where the S.C.) is and see if it converges faster.

Second, are you sure you are applying the theory correctly? When using the S.C. are you subtracting out the hole diameter from the area when calculating the nominal stress? The nominal stress in this case is actually 200*300/280 MPa. After that you are doing something wrong, this should be a simple problem to get right.

 

[cspkumar]

I am perfectly sure that the theory is right and the nominal stress is absolutely right. But I have no clue why it isnt converging? The best reason I have is as the plate elements got smaller, they have become overly stiff.

 

[vineet1977]

Hi,

This is stress singualrity phenomena and not stress stiffening effect.
Just do stress singularity search and find threads related to this topic.

Vineet
vineet

 

[zuardy]

Yes, first of all, it is not clear how you refine your elements (automatically with h-elements?). If not, then i agree with FeaGuru suggestion : refine the mesh locally (where the S.C.) is and see if it converges faster. Because only the S.C region is of interrest.
Regarding stress stiffening effect, it could be the case, because thin walled elements will undergo this phenomenon. But what i probably don't understand, that you model your thin structure under pressure with plate elements, it should be modeled with shell elements, since the structure will have curvature under pressure load. Please see the theory about the difference between "plate" and "shell", any suggestion?

regards

 

[cspkumar]

I have refined my elements using h-method. As you can see from the data, each element has been split in the mid-side to obtain 4 elements. So, 29 elements in the first run has become 29*4=116 in the second run.

I have applied a uniform tensile load of 200 MPa on one edge of the plate. It is not a bending load. Hence, I think the use of plate element is justified. Any arguments and suggestions are most welcome.

 

[zuardy]

oic, you have applied "in plane" load to the elements, then the use of plate element is surely justified in this case. But it also means, that no stress stiffening effect will occure. To my know the stress stiffening takes effect only if the diplacement is normal to the stress direction, e.g. you have applied pressure normal to your plate structures (out of plane load), then the plate will have a curvature like diplacement. In this stage some portion of the load will go in plane direction (stiffening the plate), so that the displacement due to the other portion of the load (normal to the plate) will be smaller, and so the next step. You see, that this effect can be captured only with stepwise analysis or "non linear" analysis. Did you run non linear analysis?
Other aspect is that the stress after 6. step (elements = 29696), the stress is 3.733333333, whereby the theoretical stress should be 2.81, i.e. above the theoretical solution (the model is flexible then the reality). Normally FEM Model is stiffener then the reality/theory, so it should have small stress and the stress would increase with the inreasing of elements number. The step number 1 to 5 seems to be right, but 6. and 7. step is strange. I lose the theoretical explanation for those steps. May be you better do FeaGuru's suggestion and compare the solution to each other, Furthermore you have better control over the quality of the mesh.

regards

 

[prex]

You didn't clearly state that your tensile pressure load is 200 MPa as a mean value at the section passing through hole center: you would have to apply some 214 MPa at plate edge.
Apart from that, if I understand correctly your refinement procedure, in the last step you should have elements with a side of about 0.7 mm: this could be still a bit high to get a good approximation for the local stress. Moreover it is not clear how you account, in refining, for the hole curved edge: you could have locally elements with bad shapes.
What about trying a further step? However you should refine the mesh only around the hole, using there only nearly square elements in a polar, rather than cartesian, pattern. prex
motori@xcalcsREMOVE.com

http://www.xcalcs.com

Online tools for structural design

 

[elogesh]

Hai,
Have you applied right boundary conditions for your quarter symmertric model?

I feel stress singularity due to boundary conditions may be behind this phenomena.

Regards,
elogesh

 

[cspkumar]

The tensile load applied on the plate's edge is 200 MPa. The nominal stress in the plate should be 214 MPa. Why should I apply a load of 214 MPa. I am sorry, I could not understand this point.

I have applied the right boundary conditions, since the results of the quarter-symmetric model matched with the full scale model.

I will go ahead and refine only the area around the hole and try to get a converging solution. Any more suggestions and tips are highly welcome.

Thanks
Kumar.

 

[prex]

The stress concentration factor is normally given based onto the average stress in the weak section (passing through the hole). So to compare with theoretical results for scf you need to divide the local stress by that average value: to avoid calculating the average value in the model, simply increase the pressure at the edge by the ratio w/(w-d).
Now you are a little bit closer to your goal, but still a difference exists.
If you want more help may you describe how are your boundary conditions applied? prex
motori@xcalcsREMOVE.com

http://www.xcalcs.com

Online tools for structural design

 

I got factor of 2.837 using 1359 nodes and 1255 elements (max stress divided by the average stress in the weak section).
So the solution should converge way before 100000 elements.

Maybe in your model, when splitting the elements, the boundary conditions were constantly applied only to the original corner nodes, not the the new ones (additional stress peaks)??

 

Hai Denzil Dexter,

Can you elaborate about the model and the boundary conditions used for the analysis?

Whether it is full model or quarter sysmmetry model?
Regards,
amar

 

[cspkumar]

The B.C's I applied for this quarter-symmetric model: Uy=0 on the bottom edge, Ux=0 on the left edge. The tensile load was applied on the right edge. Well, I think this is not a problem at all as the results of my full scale model matched with this quarter-symmetric model.

Denzil, could you tell me what was your maximum stress and the nominal stress and the way you modelled.

y
|
|
* * *
* *
* *
* *
* *
* * *--->x

Thanks
Kumar.

 

Hi there,

I modelled a quarter of the plate (150x150 mm, R10mm quarter hole at the corner) using MSC/Patran automatic paver mesh. Element size along the hole edge was 0.5 mm and 6 mm at the distance from the hole.

Boundary conditions were: SymmetryX (1,5,6) along left edge, SymmetryY (2,4,6) along lower edge, and Z (3) at every node.

Upper edge of the model was subjected to constant pressure=1. Thus, the average stress in the weak section is 150mm/140mm*1MPa = 1.0714 MPa.

Maximum stress from FE analysis was 3.04 MPa i.e. peak factor 2.837.

Regars Denzil

 

[idly123]

its a plane stress case, try using plane stress elements.. 4 node billinear element with 2 inplane dofs. i belive it should converge faster. u dont need these many elements as u have used.
reason for avaoidance of plate elements in the present problem is that...even if u use a plate element at lower refinement u should be intrested in getting stresses from higher order derivatives and at higher refinements u should be intrested in getting stresses from lower order derivatives....the end result being for the present problem its better if u go in for a plane stress element so that u reach a constant strain state earlier and that your results converge faster and not llike as we see in ur solution.

Refer to paper by barlow on stress extraction and refinement
may be i shall let u now the journal and vol in next post

hope it helps
regds
rAJ Raj

 

[prost]

Looks like a classic case of fixing a node that wants
to move. Call Node 1 the location of the highest
stress. From Kumar's drawing, that should be the
top of the hole, on the x=0 axis. If one fixed
the y displacement to be zero at Node 1, that
would not allow Node 1 to move down (Poisson
effect) when you pulled to the right. Does
the model deform as expected? What do the stress
contours look like? Refinement seems to be
the key answer, nevertheless a sparse mesh
does not explain why the stresses keep going up.
A bad boundary condition like a point constraint
does explain why the stresses keep going up.

 

[prost]

Kumar:
Here's what I did, using plane stress quads in p-version code StressCheck, took about 10 minutes to build mesh and get result. Solution converges quickly as there are no singularities. Kt=3.038 based on far field, 2.835 based
on net section stress. Only 1344 D.O.F. needed for less than 1% error. Same numbers for plane strain of course.

Now fix the node at the top of the hole in y-direction.
=================================
| DOF | Max. Sx
================================
| 27 | 1.964885E+000
| 95 | 2.526961E+000
| 203 | 2.793709E+000
| 351 | 3.009912E+000
| 539 | 3.115877E+000
| 767 | 3.250458E+000
| 1035 | 3.200530E+000
| 1343 | 3.320644E+000
==================================

Ugly, isn't it?
s