Modelling of a perforated sheet metal.

[MarkCopland]

I would like to know what sort of boundary conditions do I need to place in a “unitary cell” (a symmetric model of a perforated sheet metal).

I would like to model the unitary cell as a shell, but I am not clear with the boundary conditions do I need to place on the symmetry edges.

The perforated sheet will support a pressure load.

Thanks for any answer.

 

[rb1957]

"The perforated sheet will support a pressure load." ... how ? (do you have a non-structural, non-perforated liner ?)

are you modelling just one side of a box, hoping to cover all of them ? ... different sides have different edge conditions and different loads.

 

[MarkCopland]

Thanks.
I am chemical engineer, and I am beginning to do some FEA.

basically: image a perforated sheet metal with a 6.35 mm hole with a triangular pich, with give you 40.3% open area.

I suppose that this is a classic symmetry boundary condition problem.

I want to evaluate the perforated sheet metal under pressure and I know that analysing a unitary cell will give me good results, but I am not clear what boundary condition do i need to place to simulate it on the unitary symmetry edges..(I am using shell elements).

If you got a large perforated sheet metal will be to computer demanding to simulate for example 1 m2 of sheet metal ( some like more than 30000 holes!.) and if I take a unitary cell how to take into account the simple supported or fixed condition on the outer border of this 1 m2 sheet metal.

or do I am missing something?.

 

[gwolf2]

Mark,

This analysis is more tricky than you think. The fact that there is symmetry in the small scale geometry does mean that there is symmetry in the loads/stresses. The shape of the plate as a whole (e.g. square, circular, etc) and the way in which the edges are supported (clamped, simply supported) governs the way in which you model it and the resulting stresses around individual holes.

If you had less holes I would suggest that you model a quarter of the whole plate (if it is square)with mirror symmetry boundary conditions, or a sector of the plate (if it is circular)with cyclic boundary conditions.Given that you have 30000 holes there is no way that you can use this method. In cases such as this I advise the following:

1) Make a small test model with an array of say 10 x 10 holes. Apply bending loads and membrane loads to the model. Compare the deflections to the same model but with no holes. Then come up with a reduced value of modulus E which you can apply to a plate without holes in order to get the same deflection with holes. You may need to use different values of E for bending and membrane.

2) Analyse the global structure with reduced E.If the sheet is very thin then nonlinear analysis may be necessary.

3) In areas of interest create a sub-model with real holes and apply deflections from the global model as boundary conditions.

If this all sounds a bit daunting then hire an FE specialist. There may be some short cuts depending upon what information you want from the model (detail stress, deflection, natural frequencies etc.)

gwolf.

 

[corus]

I believe in the ASME pressure vessel code they derive a value of a modified E for perforated tube sheets dependent upon the hole size and spacing. Perhaps that's a way of modelling the w-hole sheet (pardon the pun).

corus

 

[gwolf2]

Correction:

The fact that there is symmetry in the small scale geometry does NOT mean that there is symmetry in the loads/stresses

 

[rb1957]

am i missing something ... how can a perforated panel react pressure ? personally, i'd model the panel and use a Kt to adjust the panel stresses for the holes. if you do this, you'll need to be careful about the stress solution used in the FEM. linear stress equations assume small displacements, your model (a flat thin membrane under pressure) will probably show very large displacements ('cause the bending stiffness of the thin membrane is very low). in the real world, the flat membrane deflects enough to form a curved surface and reacts the pressure with in-plane tension stress (re hoop stress). what you might do is to run the full model (with simple non-perforated sheets) to determine the stress in the sheet under pressure, then run a "unitary cell" applying this stress (and not out-of-plane pressure).

 

[gwolf2]

w.r.t. rb1957

> how can a perforated panel react pressure ?
If there is a flow through the holes

> use a Kt to adjust the panel stresses for the holes
I doubt there is one for this configuration of loads and hole size/pattern.

> then run a "unitary cell" applying this stress (and not out-of-plane pressure).
In a sub-model of this type you must apply the pressure loads from the global model as well as the boundary conditions to get the correct result.

 

[rb1957]

i take it you've measured the pressure drop (across the perforated sheet)

there is a Kt solution for holes closely spaced with in-plane stresses (the effect of the pressure is to create in-plane loads, tension and bending)

you can run a global model to get the internal stresses in a coarse model of the structure. you can then apply these loads to a small detailed model. these would be effectively a load/reaction set of loads (i'd expect in your case bi-axial tension).

if you apply the pressure load to a "unitary cell" you won't get the right answer. because the structure works as a whole. the skins of your box react to the pressure load with in-plane tension (hoop stress) and (depending on how thick the sheets are) in-plane bending; a balloon (or an airplane fusleage) are examples of membranes (which don't have significant bending stiffness) and react the internal pressure with in-plane tension. Flat pressure buklheads (as in some planes) react the pressure principally by bending (their bending stiffness is large enough to prevent out-of-plane deflection of the bulkhead).

 

[GregLocock]

So, why not model a segment (a pie slice) accurately? The BCs along the edge of the cut are pretty straightforward if the loading and the structure are entirely symmetrical.

Cheers

Greg Locock

SIGlease see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[MarkCopland]

That is my point, if you got a 1 m2 panel with edges BC let said "simple supported" how I can I model a "small section" or even a unitary cell?... how this unitary cell will take into account the BC on the far away edges from the 1 m2 panel?.

I have a look at Peterson stress concentration factor, and there not a Kt tabulated for this case. (Which is really silly because it most be the more common application in sheet metal).

A) Is that am I wrong to try to model a unitary cell?
B) How repetitive symmetry can help me? And if it yes, how do I do?

Yes, the panel need to support a pressure drop due to a fluid, so bending in the panel is my concern.

 

[rb1957]

my copy of petersen has fig123 and 124 for a regular array of holes.

i don't think a "unitary cell" will correctly reflect the complete structure.

i think you need to model the global structure; you could reduce the thickness to account for the holes (thk*(1-d/w)), where w is the spacing of the holes. this'll give you the stresses in the nominal sheet, add in the Kt factor and that'll be your answer; or model a "unitary cell".

do you anticipate a fatigue question (cyclic pressure loading) ? or are you concerned about the static stress peak at the edge of the holes ?

 

[GregLocock]

Well, if it is all symmetrical then there will be no rotation about the straight edges of the pie slice, but there is perpendicular to that in the plane of the material, so the boundary condition is something like 0,1,0,1,0,0 off the top of my head (0 is free, 1 is fixed) in that coordinate system, Z being out of the plane.

But it just needs a bit of noodling on the back of an envelope.

I actually agree with rb, modifying E is the way to go, ie treat it like a composite, for most practical purposes, unless you really are worried about stress raisers at the perforations, for which you could just model a patch in great detail using displacement constraints at the boundary derived from the first model.

Cheers

Greg Locock

SIGlease see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[MarkCopland]

Hello, rb1957

If you are referring to chapter 4 (Peterson’s 2th edition), all cases for holes and holes arrays are for in-plane forces (meaning that the forces for a x, y coordinate system are apply in that plane only), and because the case I am talking about is an of out-plane (pressure force applied normal to the sheet metal), those Kt doesn’t work.

Can some body explain me why a unitary cell can not work..

 

[napoleonm]

Hello every body.

I believe this is a typical FEA study case, and the interpretation of boundary conditions are critical even if it seen to be a simple problem.

I agree with gwolf2, you can find some information about strength calculation for perforated sheet metal on:

http://www.iperf.org/strength.html,

here you will find useful information about strength calculation, this information is based in the same criteria as gwolf2 said, they introduce an “equivalent elastic module”, “equivalent Poisson ratio” and an “equivalent strength “, all these value are being calculated from re-estimation of the elastic material properties based on “experimental?? deflection”, ( I introduce ?, because I am not sure about this point, but it seen to be the real path).

ASME as well introduce in section Vlll div 1, the concept of “Ligaments” (which is an hole array in pressurized elements).

I would say that if you want to model a section taking into account the far away edge condition, you can model a section using repetitive symmetry on the line were you will cut your model, but the best simulation will be only model a section let said 20 holes x 20 holes and place the edge condition you need, that can give you an approximation of your problem.

 

[rb1957]

mark,
the out-of-plane pressure produces in-plane forces (and moments) ... that's what's going to drive your stress concentration.

the unit cell doesn't work for the simple reason of the question you're asking ... what boundary conditions to apply. consider is the cell in the middle of the panel loaded the same as the one on the edge ? the answer is it depends ! if the sheet is acting like a flat plate in bending, then the two location are loaded very differently (sort of like a beam). if the sheet is acting like a membrane, then they are very similar. how do you know ? run a global model with an equivalent panel thickness, get the global behaviour, then model a unit cell. if you're smart the global model would be set up so you can easily determine a boundary (say 1 element) for which you can extract the free body forces (yes, if you insist you can model the out-of-plane pressure and it'll be reacted by shear at the boundary). now the boundary restraint question goes away ('cause you're applying a balanced set of loads and reactions).

btw, how much pressure do you get across your perforated sheet ?

 

[MarkCopland]

My panel will be all the time in the elastic region, so a lineal analysis is enough for me (just to make every thing more simple), I am not going to pass my material yield point.

The stress on the hole edges and the stress on the edges boundary conditions are the ones I am looking for.

thanks napoleonm..the info you send me is really useful.

so rb1957, a unit cell is ok just for in-plane loads only?.
that mean I need to model the panel for a pressure load (which produce bending only)?, it interesting your point of view.

 

[rb1957]

no ... a linear model probably won't produce good numbers, it'll most likely predict unreasonable out-of-plane deflections, and so unreliable results. i expect that your (correct) out-of-plane deflection will be something like 2*the sheet thickness which voids the "small displacement" assumption in linear FEA and because the sheet adopts a curved shape the load paths change and the sheet develops in-plane hoop stresses to react the out-of-plane pressure.

and no, the unit cell isn't good only for in-plane loads; but IMHO in your case the in-plane loads are the most significant ones ... how much force does the in-plane pressure create over your unit cell ?

 

[napoleonm]

Well, If your pressure load produce a deflection less than half of the thickness, a lineal assumption is Ok.

and as mark said:"My panel will be all the time in the elastic region", so a lineal analysis will be valid.

if you got the option of large deformation in your software, will be usseful to tunr it on, because if your load produce a deflection nearly half of the thickness, is probably that this load will have a diferent behaviur allowing large deformation, run both cases and apply your engineeing knwolege.

 

[rb1957]

true enough ... assuming the pressure drop is low (as you'd expect with a perforated sheet) but for a 1m2 panel it'll need to be really low to get a deflection of only 1/2 the thickness.

still the approach should be (IMHO) a global model follwed by a detailled model. and the detail model is supported just to remove the 6 rigid body dofs and loaded with a balanced set of internal loads from the global model.