CosmosWorks Results Accurate? 4

[PLCKing]

I'm doing a FEA model of stresses in a plate. The plate ASTM A36 steel and dimensions are 140" x 250" x 0.25" thick. The plate is restrained along all 4 0.25" edges. The bottom side has stiffeners that are 0.125" thick and also A36 material and are spaced every 16". The stiffeners are "L" shaped with the bottom of the "L" welded to the bototm of the plate. The long part of the "L" is 9" long and the short part (welded part) is 2" long. The stiffeners are 140" long and run the whole length of the plate. The bottom of the plate is exposed to a 30psig pressure distributed evenly accross the plate.

I'm using cosmosworks to do the analysis with a sold mesh (2" x 0.1"). The results I get is that the von mises stresses in the web of the stiffener are approx. 300 ksi and the max von mises stress at the edges of the plate is approx 450 ksi. These stresses are way over the materials 36 ksi.

What I'm having trouble with is how accurate the results are. I think the result stresses are way to high, but I'm having a hard time proving that they are wrong. Any advice on error checking the analysis would be greately appreciated.

PLC.

 

[GBor]

Thank you for a very good description of the problem, but I think you've chosen the wrong element type for the results to be accurate...bricks are overly stiff for everything except, perhaps, the 2" leg of the "L". Also, with a solid mesh of 2"x0.1", it seems as though you would typically have only 2 elements through the thickness of the plate (maybe 3 if you hand meshed) and 1 through the thickness of the stiffeners (possibly 2).

Sounds like ship structure...pretty certain it can handle 30 psi.

Garland E. Borowski, PE
Borowski Engineering & Analytical Services, Inc.
Lower Alabama SolidWorks Users Group
Magnitude The Finite Element Analysis Magazine for the Engineering Community

 

[vonlueke]

PLCKing: The aspect (length-to-thickness) ratio of your elements is too large, which is an inherent problem with trying to use solid elements to mesh thin plates. Shell elements, on the other hand, are ideally suited for meshing thin plates.

You can perhaps perform a reality check on your fea results by hand calculating the stress on a 16-inch-wide strip across the 140 inch width of your plate. We can expect the stress on this strip to be, say, 15% (?) too high, because it neglects the stiffness contributed by the y direction of the plate. The moment of inertia of the strip is Iy = 26.55 in^4, with an extreme fiber distance c = 8.146 inch. Treating the strip as simply supported gives a midspan von Mises stress of sigma = 2488 MPa. Dividing sigma by 1.15 to account for the expected error gives sigma/1.15 = 2163 MPa (313.7 ksi). If the ends of the strip (and stiffeners) are instead clamped, the strip midspan stress divided by 1.15 would then be sigma/1.15 = 721 MPa.

 

[PLCKing]

Thanks for the replys guys I appreciate your help with this. The problem I was having with using shell elements is that I'm modeling it as an assembly and in an assembly you need to select reference faces and then give it some thickness. When I do this, for some reason the analysis fails. I need to play around with it a bit more to get the shell mesh working. Any advice on how to use the reference surface shel mesh in an assembly?

Vonlueke, thanks for the hand calculation. The edges of the plate and the stiffeners on the side are all fully restrained as to simulate them being welded. So from your calculation the stresses should be about 104 ksi(722 MPa). Since the material has a yield strength of 36 ksi then it would fail, so my results seem to be off by a factor of 3.

 

[JStephen]

If you refer to Roark's Formulas For Stress and Strain, one of the load cases will be a rectangular plate with all edges fixed. Take one panel of your plate and check it using that equation. I wouldn't expect results to be identical, but they should be reasonable.

A couple of other concerns. When deflections in a plate exceed about half the plate thickness, tension stresses in the plate become important- it can be supported in a catenary fashion regardless of bending effects. Your modeling may or may not handle this correctly, but it is something be aware of.

Also, with beam sections with thin webs, web buckling can control the design. Check the web and flange buckling effects from AISC or other steel codes.

You mention 1/8" A36 stiffeners. I'm not sure A36 is actually made in that thickness, although it should have little effect on your results.

 

[cbrn]

Hi,
PLCKing, depending on which version of CosmosWorks you are using, there may be an issue on the calculation of the stiffness made by the program: in CW 2004, I had a hard time with the same identical loadcase as yours but a circular plate. It calculated a global stiffness more than 4 times the one given by B.Barp/C.Freimann (Elastizitaetsgleichungen kreisformiger Platten). I believe this severe error has been fixed in successive releases, but you can check the behaviour of the program as suggested by JStephen.
Be also aware of local numerical effects such as "edge effect" or "corner effect": in general, I agree with the suggestions already given.

Regards

 

[brep]

This should be run as a nonlinear analysis (geometric nonlinearity - the out of plane bending will result in the membrane stresses stiffening up the structure)

 

[PLCKing]

I'm using solidworks office premium 2007, so I'm hoping the bugs are worked out. I am running it as a non-linear analysis. For some reason I can't get the shell mesh using surfaces to work properly when being analyzed. I select the plate face and give it a thickness, then I select each of the stiffeners and give them a thickness, but when the model gets analyzed, it fails because of "failed restraint" I get several messages like that dring the post processing.

I also re-ran the model with a fine mesh 0.75" x 0.0375" and the results came out very close to as before. I need to figure out how to use the surface shell mesh.

PLC

 

[rb1957]

i re-did the hand calc above and got the same answer (M = 1.2E6in.lbs, stress = 360ksi), so i reckon the problem is in the structure ...

however, a problem with flat bulkheads resisting pressure is that a small deflection allows them to react the pressure with membrane endload. in this case, the s.s. beam would deflect only about 3" so the effect is small (could be confirmed by a non-linear run)

whilst a agree with the previous comments about your choice of element, the results look reasonable

 

[PLCKing]

I appreciate all the replies, you guys have given me excellent information to go on with. I have a couple more questions.

This analysis I’m modeling is for a UL142 specification tank. The UL certification test requires for the tank to be pressurized to 175 kPa and held for 2 minutes. During operation of the tank will never see this high of a pressure and the tank will be pressure relieved at 30 kPa. I’m wondering, how long would the plate or the webbing of the stiffeners hold at stresses 25% above the materials Ultimate Tensile Strength before it would crack or rupture? For example if the materials UTS is 58 ksi, the analysis shows von misses stresses in the stiffener webbing or top plate of 90 ksi when a pressure of 175 kPa is applied to the top plate. I understand that surpassing a materials UTS is where failure will occur, but is this failure instant? Or is it gradual for a ductile material like steel?

PLC

 

[rb1957]

by my calcs 30psi = 101.325/14.7*30 = 207kPa, but maybe we're rounding things ... 175kPa, 30psi the results are much the same ... i'd be very surprised if your structure holds together for 2 minutes ! particularly if we're rightin predicting a stress 3 times ultimate, but then 36ksi is pretty low for a steel.

i suspect your steel is pretty ductile, and that your loading rate will be slow, so the failure should be reasonably plastic and slow, as i think we're talking about a tension failure of the tip of the stiffener.

for my 2cents, i think you need to reduce the pitch of the stiffeners, and replace the L-stiffeners with Z-stiffeners (ie add a flange to the standing leg).

 

[GBor]

How large an area does this excessive stress cover? If it is in a small portion of the stiffener, a non-linear analysis may show the stress redistribution such that you don't see quite that high of a peak stress and you may not see ultimate at all. Loading would be slow, I would think, so a non-linear static (disregarding inertial effects) would do. It may just require that you tie the stiffeners in a little differently.

Also, it appears that the stress is at the edge of the plate near the boundary conditions. This may be causing some analytical stresses that don't really exist. You may try balancing your forces and using minimal boundary conditions. JohnHors and I wrote an article on this in last month's

http://www.feamag.com,

but you have to be a member to read the entire article, and since I'm the editor-in-chief, I'm kinda' selling something, for which this forum isn't intended, so there's my "sales pitch".

 

[PLCKing]

Yes,you're right rb1957, 30 psig is 207 kPa, I was putting in 5 psig as a safety factor.

Yes, the tip of the stiffener will let go first as that tha's the highest stress concentration, but that part will be welded to the side of the tank, so a strong weld will be important there. But I was also curious about the webbing or vertical part of the "L" stiffener because the model shows high stresses in them.

By Z-stiffeners do you mean C-stiffeners? or is there an advantage of having the web of the stiffener on an angle?

 

[rb1957]

Z is a way to show an L with a cap ... it doesn't mean a inclined web.

i'd've thought that your over-stress covered an extensive area, and in a real problem.

the welds are close to the neutral axis of the section and should be checked by flexural shear, but probably aren't a problem (but then i'm not a weld-man)

 

[PLCKing]

The excessive stress covers most of the stiffeners "web" and also the top plate. I was trying to get an idea of how much I need to "beef up" the design so it would pass the 175 kPa test. Do I need to get the stressed below 58 ksi (A36's UTS) or do I need to get below the yield stress of 36 ksi, or would 75 ksi hold for the 2 minutes.

I should look into using other steels like tempered or quenched as they would have a higher strength. The nice thing about A36 is that it's relatively low cost.

 

[GBor]

For the entire length? Or just at the end? Can you post a graphic of the results so we can take a look? Also, are you using some kind of smoothed results, or unsmoothed?

Generally, going this high dictates a non-linear analysis to see how it will hold. Does the test allow some local yielding? Or are you required to stay in the elastic region? If you are required to stay elastic and the stress is not localized, it's time to consider a little design work. If you are allowed some plastic deformation, a non-linear analysis may show that you don't peak as high as you think.

I used to work in the shipbuilding industry where A36 is prolific...that's why the low cost. You may also want to check HY80 and HY100. They are much more expensive, but may be worth it for your application. I'm sure there are many other options (A286, perhaps some high-strength aluminums, etc.).

 

[JStephen]

You should be able to find higher strength materials without going to quench-and-temper. A lot of the structural available is 50 ksi yield, and 50ksi strip/coil should be available as well. Keep in mind that if elastic buckling limits strength, you won't gain a whole lot from the higher strength material.

 

[PLCKing]

GBor, the stresses in the web of the stiffener are at max in the middle of the stiffener and then go approx. a 1/3 of the length each way from the middle. I'm not sure how I can post a pic, but if I figure it out I'll put it up. For the UL142 testing, I believe that you can go above the materials yield strength. The structure just needs to hold together for the test. (This is the way I understand the UL spec from the way it's written, but I could be wrong)

I have a pretty good handle on the analysis. The trick with using shell elements on selected surfaces is the forces and restrains need to be applied to the mesh face and mesh edges. Also contact faces need to be determined in assemblies.

I did some "playing" around with the model and compared results between using a solid mesh and using a shell mesh. What I found is that when I use a shell mesh, the difference in results between a fine mesh & a coarse mesh is approx. 15%, but if using a solid mesh, the difference in results between a fine and coarse mesh can be about 50%. Comparing a fine shell mesh and a fine solid mesh, the results were within 1% of each other.

One thing that surprised me is that I would of expected the anlysis (meshing & calculations) using a shell mesh to be faster then a solid mesh, but because of the defined contact surfaces it seems to take as long or even longer. When defining contacts, is it better to use Node to Node, or Node to surface, or surface to surface? Now I'm trying to figure out if it's better to have a fine mesh with a coarse tollerance or a coarse mesh with a fine tollerace. Any suggestions?

I'd like to thank you guys again for you help. I've learned lots and got some excellent advice. I realize that the design has to change which I'm currently working on.

PKing

 

[EdDanzer]

I think using a thicker flat bar in place of the “L” shape will provide more stiffness with the same weight. It may help to taper the bars so they are taller in the middle to spread the stress over a larger area. Another option is to use a “T” shape stiffener to make the cross section look like an “I” beam.

 

[rb1957]

a stress peak ant the ends means that you've got a fixed end boundary condition ... you need to check your strcuture to ensure you can transfer these moments to the rest of the structure. remember, if this is a box, then the adjacent sides are also loading these corners.

I assume that the tip of the stiffeners is in compression ... compression strength is usually limited to fcy (=fty) ... make sure of your crippling allowables. A flange width/thickness of < 8 is good.

it simple enough to play with geometry (stiffener shape, stiffener pitch) with an excel spreadsheet (consider a single stiffener pitch) to get an idea of what's needed to get the structure to work, then the FE to fill in the details.

i'm surprised you've got a contact issue ... but you know your structure !