First time on this site, so I hope I don't go to the wrong place to ask my question. I first take the temperature to know if I can afford to ask you for help on the subject below. If that's the case, I'd put more information of course.
Here's my problem: I want to simulate a load case on a metal structure, and I've never used the Generative structural analysis workbench before...
(For information, the structure in question is a two-level storage rack - with 4 storage spaces -, and each floor must be able to support 500kg) i.e. a total of 2 tons.
I've watched a lot of tutorials, and I don't think I made a mistake in the settings.
BUT.... I have a little trouble interpreting the results. In terms of displacements at the nodes, it seems correct, but concerning the Von Mises constraint, nothing is less certain... So I'm afraid I've oversized the structure... or the other way around.
I'm starting in RDM. Please be indulgent^^
I'm not asking for someone to do the work for me, I just want to get some advice about my results and tell me if I'm exceeding the elastic limits of my material, if the structure will undergo deformation, etc...
As said in my first message, I'm just starting out, and self-taught on Catia, I hope I'll be able to provide you with the necessary information.
The rack must be able to support a total weight of 2000kg (500kg per tray).
I'm putting the photo of the rack so you can better understand what it's all about.
The structure is made of steel. I saw that the yield strength for steel is between 255 and 355Mpa. If I have understood correctly, once this limit is exceeded, the material will undergo an irreversible deformation (I am starting from a long way ^^)
By wanting to lighten the structure, I have the impression that the displacement at the nodes has become more pronounced:
I get a translation at Max nodes of 0.644mm (is this acceptable? it seems to me bcp)
And the most critical Von Mises criterion is 2.39e07 Nm² (This is where I'm worried... it seems worrying to me, doesn't it?)
--> other question (sorry if my questions seem stupid): why does the value of the VM criterion increase the more you refine the mesh?
First remark, your case study seems to have several symmetry planes. You could study a quarter of the model by making simplification assumptions. which would allow you to save as much time on calculations;)
For the elastic limit of steel it depends on what you want to use, 235, 355 480 Mpa...
Past the elastic limit, you move into the plastic field = the deformations are permanent.
For your constraint value that increases with the mesh, it seems characteristic of a singularity. (related to an embedding or a sharp angle or a bad mesh) the more you refine your mesh, the more your constraint will tend towards infinity. But this constraint is not real since it corresponds to a modeling error. Sometimes it is impossible to do without this error to have a coherent model. We just have to learn to spot these singularities.
Indeed, there are planes of symmetry, I didn't have the reflex to simplify! Thank you
Regarding the constraint that increases with the mesh, I can't understand (well I understand what you explained to me, it was very clear) but... I made a model as simple as possible: a 50x50x2mm tube extruded to 100mm, and recessed at one of its ends)
I then applied a distributed force to the edge at the end of this tube, applying a more than small force to it: -1N
--> here again I find myself with a VM constraint that seems huge to me compared to this situation. I probably have a problem, right ? (1.11e04 Nm²) --> if I compare to the elastic limit of steel... It would mean that it deforms. How is this possible? I must have been wrong, because in this case, I don't think it's due to a singularity in the mesh, or a modeling error.
Ps: I know more or less the volume modeling under catia (surface it's another story ^^), I'm mostly new to RDM:)
As far as singularity is concerned, Catia is not a very good mesher by default, by which I mean that it risks creating distorted elements or very small in size compared to others, which can create local overstresses. But indeed these constraints are not "physical" and we can ignore them if they are not in a critical zone. or you have to rework the area to have a better quality mesh.
For the post-processing of stresses, your structure does not deform much and the elastic limit is not exceeded. If the yield strength of the material is 255 to 355 MPa, the calculated stress is 2.39e07N/m²=23.9MPa so it is well below the limit.
So much for me... I messed up in the units (I thought I was in N/mm²) and in fact no, I'm in N/m²
Which so, for my simple example (tube 50x50x2mm, length 100mm, force of 1N) --> my von mises constraint seems much more logical to me^^
So in the end, forgetting this unit problem, I get a maximum Von Mises constraint of 7.66e06 N/m² --> or if I'm not mistaken: 7.6Mpa
Based on the principle that the elastic stress of my material (steel) is between 255 and 355Mpa, can we say that there will be no deformation? And that the structure will not deform?
Without malice, before doing simulation, you should already master the basics of the RDM.
When you write: "I get a maximum Von Mises constraint of 7.66e06 N/m² --> or if I'm not mistaken: 7.6MPa. Based on the principle that the elastic stress of my material (steel) is between 255 and 355MPa, can we say that there will be no deformation? And that the structure will not deform?"
If there is stress, there is deformation. The question is whether or not this distortion (as small as it may be) poses a problem in relation to the application. In your case (storage rack), we can easily accept deformations created by a stress corresponding to 80% of the elastic limit. For a precision application (like a laser holder for Tokamak), a deformation of qq. tenths of a mm will be penalizing.
Given that it's the first time I'm sizing a metal structure, it would suit me enormously if you gave me your opinion so that I don't mess up too much.
I have taken note of all the advice you have given me. But I'm not sure of myself. You will find attached a folder containing my rack and the analysis.
Could a charitable soul tell me if the parameters I have set are good for me to exploit the results?
For the size of the mesh I put 15mm
Arrow: 2mm (but I admit that I did it a bit randomly)
Distributed forces on the upper floors: I chose to apply them on the outer edges, because for me it is the simulation of the most critical load case
Distributed forces on the lower floors: I applied it to the support surfaces (i.e. on the 2 x 3 tubes)
Recessed at the level of the 4 plates
I get:
Von Mises max: 6.55e07 Nm²
Max knot displacement: 0.58mm
What worries me is that even if I double my applied forces (going from 5,000N to 10,000N, i.e. 4T in total, the yield strength is still not exceeded... yet my rack is not a tank either... It's strange, isn't it?)
Is that why I come to you:)
Another question: I saw that all the parts had to be assembled to the main body to be able to simulate the load case. So in my part I put everything together with a Boolean operation. Is this enough to simulate welds? Is this the right solution?
I hesitated before registering on this site, precisely so as not to end up with silly questions to ask. But I don't regret it, I'm learning as I go along. I don't take your comment badly, far from it, all your answers are constructive for me.
I did indeed express myself badly, I rather wanted to say "irreversible deformation", if it is said of course... the kind of distortion that is not acceptable.
It's true that for my application, I can accept a certain distortion because, as you said, I'm not in a precision application, where I understand that this is very important.
Indeed it seems oversized. But I have several remarks on things that you can't know as a beginner in Rdm and on Catia GSA:
1) Your structure is made of thin tubes and the lengths of the members are long in relation to their cross-section, so you have to use 2D shell elements or 1D elements. Your tetrahedral elements are very large here and therefore very crushed and I wouldn't trust too much of the values that come out of them. The skin would then have to be extracted from each bar and then shifted to make a neutral fiber. These new skins would then be meshed in quadrangles and adorned with a thickness (that of sheet metal). This means that everything must be disassembled first. This is the lightest method, otherwise, you have to start from a product to consider each main part body.
2) For a tubular structure, the most important thing is the resistance to buckling. I added a case of buckling on your model and the good news is that it goes well for the first modes, so no worries but you should check with a shell mesh.
3) For the question of weld resistance: Catia allows you to model welds (by spot, by bead,...). This locally manufactures small networks of rigid knot-to-node rigids at the place of the weld but it is, as in other computing softwares, out of the question to post-process at this level because even if the software gives you a fair value, which is debatable, physically the material (metalurgy) has nothing to do with what it is 1 cm away. In your case, I would redo the calculation with shells and surface glues (between the shell meshes) where the tubes overlap (by making pairs of welded contacts) and if the stress is low enough with respect to the Re, I wouldn't ask myself any questions. If not, I would add a gusset.
4) Do you have to lift the loaded assembly with a forklift?
5) Is it the most restrictive load? Not only in absolute terms but in distribution. Position of the centre of gravity in relation to the supports (stability).
PS: In your archive (*.rar), don't put the calculation results. It's very quick to recalculate from the analysis and the share and it takes less time to download.
I'm in R21 so I can't give you the model with modifications.
Sorry to be my killjoy but BEFORE doing finite element calculations you have to LEARN the RDM.
When I see units of constraints in "Nm²" and sentences like "7.66e06 N/m² --> or if I'm not mistaken: 7.6Mpa" I'm really very very scared.
Finite element analysis tools should only be used by people who are really familiar with RDM, otherwise it is really too risky. Just because the template is green or red doesn't mean your design is good.
Seeing the errors and approximations in what you write, it's clear that you have no notion of RDM (or it's really too far away).
And if you don't know the basics, you won't ask yourself the right basic questions in finite element calculus : how is my part fixed and how are the loads applied. The best modeling in the world with unrealistic loading and fixing assumptions will get you out of the wrong results. The abuse of the recessed for example quickly leads to models that are too light (if you consider your 4 recessed legs you greatly limit the deformations / stresses of your model and the possible risks of buckling).
In conclusion, doing calculations by finite elements cannot be improvised but it can be learned (and if possible not alone in your corner but with a real course module). A simple 3-day training at your dealer is not enough: he teaches you how to use the software, not how to do RDM.
For my part, I would have an opinion almost contrary to Froussel even if in a way he is right when he says that it is very risky to predict a physical behavior from a software, especially if you don't know much about it (physics and software).
Here, Fany is taking the right approach. That of confiding in us through this forum precisely to avoid messing up. Telling him to give up because he is ignorant is discouraging and unconstructive.
Having taken the time to look at his model, I see two things:
1) Fany has gone far (beyond his skills) and we can congratulate him for his courage. 2) Even if the mesh is unsuitable and the boundary conditions are debatable (which can be improved), its structure seems to be oversized with very low stresses (yes around 20MPa).
So, what you say is right in absolute terms, but in the case of Fany's structure, we are not in the mood to try to optimize cost or mass by taking a risk on the hold.
Finally, let's remember that not so long ago (and it is still true in many cases) metal objects were created without a "digital crystal ball" with certainly an oversizing but without disaster either. Conversely, some structures have required large human and digital resources and are not able to stand.
So, Fany, if you don't have any constraints on the mass or the price, I think that launching the thing as it is is is not stupid. You'll be careful when charging the first time. I would also like to remind you that the embedding of the welded parts must be done in the art of boilermaking (consult the people of the trade). If necessary, add gussets.
