All questions to: meshing, materials, boundary conditions and element properties
I'm interested in the deflection in thin plate caused by a force.
I first designed a beam 1000x100x25 and exported as a step file and meshed this with netgen.
this model compared with classical hand calculations is not deflecting enough.
a finer mesh gives more deflection however stil does not reach the deflection calculated classical.
as a second option i made a z88i file with dimensions 1000x100x25.
I can mesh this with element type 1. all the other ones give a crash just after pressing button "create mesh" and gives the error message "cannot read structure data"
with elemend type 1 i tried diffrent mesh sizing giving results all over the scale, some to much some to little deflection.
leaving me puzzled ..
what is the best practice for modelling this plate and any other plate in general?
I'm not Aurora support, but just another Aurora user try to help you. I'm very much a practical user.
I don't model / stress 'thin plates' directly,so sadly i can't offer you expert advice on that subject.
However, for Aurora in general i'm very happy When i compared 'classical' beam formula to results obtain from Aurora V2, once i examined and altered my LBC's and also changed the mesh in general and particularly refined the mesh at high stress points, the results were less than 0.2% difference from the theory - so that's perfection.
For myself, i'm very satisfied with results upto 5% from actual performance. it is most important to appreciate FEA type processes are based on a whole series / succession of approximations and assumptions all along the decision chain - we enter data exactly but really its only an approximation to the actual condition. Only the math computation is exact and to get good results out, you must enter good inputs.
It is really important to start with simple cases - as you have done already and understand / appreciate the subtle differences with different LBC's . As i'm sure you've noted, even in simple beam theory, there's an enormous deflection / stress difference between simply supported and constrained ends.
So the application of real world LBC's is truly critical for accurate real world results.
The mesh density is important and having the right density at critical areas/volumes is necessary for accurate results. The ability in V2 to refine locally the volume mesh, helps massively in this respect. Do not think that a trillion tetrahedron is the way to go as it will take way to long to compute. Coming quickly up to the 'convergence criteria' is whats required - a subject for good reading.
Prof. Rieg advises to always, without exception, check your results with other methods.
If you can wait, Prof. Rieg and the Aurora team ( probably more the team actually) is translating into English his recent 'FEA for Engineers' book - i don't know how long that will take to finish, they're currently working on it. If you can't wait, there are other good books easily available from the web but i'm really waiting on the Prof's book as all the examples are done with Aurora.
Read, experiment, alter, compare - its a necessary process.
Hope this in some way helps you. If it sounds too preachy - i apologize.
thank you for your respons.
Really it's not to peachy, don't worry.
I'm also very happy with the z88 auroro program and the nice help at the forum
You wrote down exactly my experience with tetrahedrons and classical beam theorie.
The diffrence between calculations in fem and by classical beam theory is very small.
the approache with terahedrons is very straight forward, and the results keep within a reasonable bandwidht.
but working with plate and classical beam seems to be very different, the deflection results are different sometimes 100%
depending on the methodes i use.
however i'm new into fem and i presume i do someting wrong.
i assume i need a diffrent element type.
Maybe this is the solution, but then z88 is not allowing me to select a diffrent element and crashes.
I need some help with that issue.
But basically I need to know if i'm working correct from a fem point of view.
It will be very helpfull also for other Aurora users to know how to work with shell/plates.
Thanks for your reply.
When you say Plates and Shells what thicknesses do you mean? Also, importantly what is the ratio of the thickness compared to the surface area?
Generally ( and if anybody else thinks differently please put me RIGHT gently), i attempt to put 2 layers of meshing between the 'thickness' of thin sections ( like in castings with deep ribs etc) and at this definition, combined with what i said previously about trying out alternative mesh sizing and local refining at high stress areas or sudden changes of thicknesses or other standard known 'stress raisers' to reach a convergence, then i would not expect anything like 100% variation from classical formula.
I trust Aurora and usually distrust myself first off. Experienced senior engineers can get it very wrong initially if not familiar with LBC's and over/under constrain meshes. 100% error would be very easy!
As far as i know, you may use 'good' tetrahedron quad to simulate any shape, be aware though, it may not be an efficient way to compute -again, if anybody thinks differently please put me right.
Frans - ideally could you post up your problem.
That way the Aurora guru's brains can be put to use. I want to learn more as well !
As they say, 'just my 2 cents worth!
edit: - just found this, makes for good reading: http://22.214.171.124/resource/pdf/486.pdf
and under the 'how to' chapter, there's no stopping 'selopez' with his yellow submarine shell meshing routine - makes my 2 mesh layer rule of thumb incorrect. I am so out of my depth here...
The problem is a square steal beam 1000x100x25mm supported on both ends and a force of 800N pushing on it in the middle bending it "easy way".
support 1 constraint on the edge in xyz, support 2 constraint on xy so it can move sideways(rolling support).
force is in the center as a basic force.
I will post more info tomorrow.
for some night reading
http://www.scribd.com/doc/34387710/Plat ... d-Pitfalls
indeed very interesting how the experts handle shells
About the best written, easy to read / comprehend, technical book i've ever come across. I NEED TO GET OUT MORE!
However the math is at too high level for me - I've been out of constant education for some time now
But the 'Message for the Chapter' is like a cold flannel on my brow - so smoothing/comforting and there the danger lies in thinking i understand it all now.
What i like particularly are the recommendations for post processor information.
The understanding, particularly for the major applied forces ( and not the summation of all forces) , as to the transference of forces / moments, into the supporting structure for a better appreciation of the structure design.
Thanks very much.
let me sum up your problem.
You are trying to simulate a steel beam of 1000x100x25 (mm^3) with two restraints at the ends of the beam and a line force pushing on the center of the beam.
You calculated manually a displacement of approx. 6,5 mm in the middle.
Did you check the results in the z88o*.txt-files? According to your screenshot (result fine mesh.JPG), Aurora calculated a max. displacement (Y-axis) of about 6 mm.
The next screenshots display the displacement in Z-axis. Did you change your geometry?
It would be very helpful if you could make your z88i*.txt-files available to us, so that we can confirm your results.
Z88Aurora Support Team
On the sized plate of steel 1000 L x 100 W x 25 D and using a force central of 800 N, the usual formula gives
max deflection of 0.6095mm.
Doing this hand calc is much faster than FEA and it give a simple indication( if the geometry was more complex) if the LBC's are correct and nothing silly has been forgotten.
Actually, i modeled only 1/2 the plate, so 500 L and for simplicity sake all end nodes were simply XYZ = 0 disp- this is a good approximation as really only the X direction is fixed and Y and Z should in theory be able to move as they surely do in practice albeit a very small amount.
Also, i refined the 'end' elements locally as this is the volume under max stress / constraint.
Input in aurora, 1 layer of elements in the .stl input file ( across 25 mm thickness) produced a mixed 1 to 2 element thickness after Netgen quad vol processing. Deflection was 0.602mm
2 layer of elements in the .stl input file etc. Deflection was 0.603mm
3 layer of elements in the .stl input file etc. Deflection was 0.606mm
3 layer of elements in the .stl input file etc. and not constraining all end element nodes in Y and Z. Deflection was 0.608mm
So, even the basic .stl input of basic 1 triangle in the thickness ( i used Netgen 5.0.0 surface mesh program)
has produced quite acceptable results and using 3 triangle thicknesses plus a little thought as to not over constraining nodes has produced a very accurate result compared to the hand calc.
Looking at your last post what input into Aurora are you using? Also, there is really no need for so many elements.
Frans. I think it's maybe a good time to look at the videos provided in the spider help and attempt
a few similar projects to more familiarize yourself. At this time, forget the Netgen meshing program and
just input basic/ simple shape .stl file directly from your cad system and check it with Aurora check .stl process. I say this i don't recognize the elements i see in your posts and im sure the amount of elements must takes ages to compute. Hint: even the 3 layer with refinement takes only 5 secs to compute using Pardiso on a basic machine. WARNING this solver stores its calcs in RAM and quickly uses it all up and may crash Aurora if it runs out of memory. Use it for only small / medium meshes! It's all in the theory manual.
ps - whoops, somehow the colours, red to blue are reversed the examples below. Sorry - that doesn't help!
The high accuracy
You understand correctly what i try to simulate.
But i want to simulate it with plate/shell elements.
The results with the fine mesh are good enough but they need an enormes amount of tetraeder elements.
So I try to mesh more intelligent with plate/shell elements because they better reflect the plate.
I first tried with rather big element 1 blocks which give a to big deflection of 14mm.
But after trying smell element 1 blocks this gives an even bigger deflection of 68mm.
I want to try a element 22 but need some help to get a fem-model.
i can no find the z88i*.txt file
uploading txt files is not allowed, can i send you an e-mail?
I made an big error, i wrote 800N but i simulated 800kg.....
that explains the big difference.
a smaller error the simulations are done with a beam 1020x100x25 but still i miss 0.5mm deflection compared with my hand calculation.
uploading txt files is not allowed, can i send you an e-mail?
I calculated the displacement manually (2D beam theory):
With L=1000mm, B=100mm, H=25mm, F=800N, E=206GPa and point of load application at center, the resulting displacement is 0.621 mm (small differences occur when using 210GPa or rounding at intermediate steps).
So TAH1712's calculation is fine and represents the displacement which is due.
When using 800kg instead of 800N, the result changes to 6,09mm.
@frans: Your results in "result fine mesh.JPG" (6,01 mm) are not so bad regarding the differences between simulation and 2D beam theory and use of different input values. If you still want to use plate/shell elements and experience problems, you can supply us with your input files so we can check them. (E-Mail at "email@example.com")
Well, I do not believe there is a rule that shell elements best describe thin plates behavior.
Given reasonable results can be obtained with 1 element layer in the thickness along with selective refinement being easy if necessary, and the tremendous pardiso solver speed ( < 1sec for the basic example above) surely alot of FEM ing can be done easily without using shell elements. Just my thoughts...if i'm fundamentally wrong..
please please, can someone put me right.
At 800kg or 400kg if modeling only 1/2 the beam ( hint: 1/2 processing compute time), then the deflection i make to be 5.96 mm.
frans, you can always send me a message via this forum.
Take a look at this video - its background FEMAP advice about node matching when modelling with shells.http://www.youtube.com/watch?feature=pl ... fcTrswuozQ
In your conversation I find a good opportunity for check the E24 plates obtained from IGES or STEP files. As you can see at the images I apply a rather coarse mesh (triangle sides = 35 mm). The part is constrained at both lower 100 mm edges. In X, Y, Z at the right one, and only in Z at the other. Concerning the load, I guess that we're talking about a "Line Load" where the 8000 N are distributed among the nodes according the FEA rules, and not about an "Uniformly Distributed Force" where each selected node is charged with the 8000 N. Material: Structural Steel from Aurora's library. With these BLC's, the output for the maximal deflection is of 5.68 mm. For me, and for what I expect from FEA, this output is close enough to that of the canonical calculation.
I'd like to know your opinions about all these. If you're interested, I can email you the z88i1.text file (and needed instructions) of this case, for you to make your own tests. Not yet shared with you the method for produce E24 plates from common CAD files, because I've still some doubts that I hope to resolve when I receive the comments from the AURORA team.
- tabla 01.jpeg (73.44 KiB) 9860 mal betrachtet
- tabla 02.jpeg (52.02 KiB) 9860 mal betrachtet
Yes, that looks a great new way in inputing ( making) E24 shells from ordinary .igs or.stp. I hope it really pans out for you and the procedure is adopted. A fantastic and important contribution to Aurora!
But, to the point here, a question re your last post above.
If using steel of E = 210 000 N/mm2 then deflection = 6.095mm
If using steel of E = 206 000 N/mm2 then deflection = 6.214mm
What i'm interested in, can you re-run your procedure to approach closer to theoretical deflection as above, or, is there some accuracy trade-off vs procedural facility / ability?
My results from frans original info resulted ( best result using 3 element height in thickness) in .608mm deflection for 400 N , so for 4000 N, without a re-run, the deflection will be 6.08mm (<0.3 % from theoretical).
I'm particularly 'nuts' about precision as i'm a Opto-Mechanical instrument designer having to design structures to hold optics sometimes with distortion allowances of 1/10 fringe ( 1/20 wavelength) or
approx 0.025 microns over 150mm. Theory is important to put it mildly and practice just as precise.
Anyway, precision is always a problem for me - even in decisions where accuracy /precision isn't or shouldn't be an issue - so in this case, i ask out of interest.
Cheers and regards.
ps. are you using the pardiso solver? If too many nodes it will fail, but it's amazingly fast!