CAE results interpretation

About the development of the FEM module/workbench.

Moderator: bernd

taifun
Posts: 6
Joined: Thu Oct 14, 2021 11:00 am

CAE results interpretation

Post by taifun »

Hi!

I have made this structure (imported step) of S335JO and applied 1000kg force on it. I don't know what to check for and how to figure out if it holds.
Can you guys explain me how should I interpret the results?

EDIT: I forgot to mention that i am runing FreeCad on a Windows 10 machine.
Attachments
8.jpg
8.jpg (216.54 KiB) Viewed 4698 times
7.jpg
7.jpg (283.18 KiB) Viewed 4698 times
6.jpg
6.jpg (229.39 KiB) Viewed 4698 times
5.jpg
5.jpg (124.62 KiB) Viewed 4698 times
2.jpg
2.jpg (107.5 KiB) Viewed 4698 times
Last edited by taifun on Mon Oct 18, 2021 9:58 am, edited 1 time in total.
KAKM
Posts: 109
Joined: Tue May 04, 2021 12:17 am

Re: CAE results interpretation

Post by KAKM »

What you're asking isn't so much a FreeCAD question as an engineering question. There are a variety of different criteria that can be used to determine whether a structure fails (von Mises stress, max principal stress, and max displacement are three of them-there are more), and which ones you should use and how to tell if you've exceeded the allowable value is going to depend heavily on what precisely you've designed, its use conditions, the factor of safety you need, and a variety of other things. Additionally, you have to know how to tell whether what your FEA simulation has returned is valid–they sometimes produce junk if you aren't careful about your setup and meshing (garbage in, garbage out).

Basically, to properly answer your question, I would need to teach you pretty much the entirety of a junior level engineering class. If this is for a class project, go to your library and look for a textbook on advanced mechanics that includes failure criteria. If you want to really build this thing, I would strongly suggest finding a consulting engineer to run the analysis for you–1000kg is enough mass to do some serious damage if things fail.

Also, you said a 1000kg force–did you mean a 1000kg mass applied to the structure as a gravitational load, or a 1000N force? The resultant force will be different by about a factor of 10, which is going to have a pretty major effect on your analysis.
taifun
Posts: 6
Joined: Thu Oct 14, 2021 11:00 am

Re: CAE results interpretation

Post by taifun »

Hi! Thanks for the detailed replay.

This is not something i want to build, I only did this analysis to learn FEM and also ask for advice as i have never done this before. The force i ment to use is a static force of 1000kg which is aproximately 10000N if i'm correct. What i understand from the results is that the maximum displacement is 19.55mm (for the height of the structure 6000mm). I don't really understand the stress and i will look for a book to learn this stuff.

But for now what should i compare the stress to in order to know if the structure holds?
User avatar
bernd
Veteran
Posts: 12849
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland
Contact:

Re: CAE results interpretation

Post by bernd »

+1 to all what KAKM said.

As a start you could compare the von Mises stress with the yield stress of your material. If the stress in the structure is lower than the yield stress a big step is taken. But for further comparison the connections, the buckling and the deformation should get some love too.

cheers bernd

Interesting read in this regard ... You will lern a lot but for sure you will end up haveing even more questions as before if you carefully read this topic :mrgreen: https://forum.freecadweb.org/viewtopic.php?f=18&t=61036
User avatar
bernd
Veteran
Posts: 12849
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland
Contact:

Re: CAE results interpretation

Post by bernd »

moved to FEM ...
User avatar
NewJoker
Veteran
Posts: 3017
Joined: Sun Oct 11, 2020 7:49 pm

Re: CAE results interpretation

Post by NewJoker »

You should also do a mesh convergence study. This mesh looks quite coarse, refine it and check the maximum values of the results. If they differ significantly from the previous analysis, run again and repeat until the difference is small enough.

And it would be good to perform the same analysis but with beam elements, this type of structure is a typical case for such approximation.
aerospaceweeb
Posts: 118
Joined: Fri Apr 09, 2021 3:26 am

Re: CAE results interpretation

Post by aerospaceweeb »

So, the way that you can learn what these results mean is to keep two things in mind.

The first, is what your simulation actually is, and the second, is what the philosophical concept of "failure" actually means.

1.) Your simulation uses only two values (not that the powerful FreeCAD material selector would let you know that without prior knowledge). It uses the Youngs Modulus, the "stiffness" of the material, and the Poissons Ratio, which you can think of as a number which quantifies how uh... "quickly" a stress can spread transversely through a material. This is what a linear static simulation does. It uses what is basically Hookes law, Force = Stiffness * Displacement, and solves for displacement by dividing force by stiffness. Now, you meshed this thing very coarsely, with solid elements. I believe this was a mistake. Solid elements produce less accurate results the more "skewed" the elements are. "Skew" here really should capture a bunch of complicated metrics such as "warpage" and "aspect ratio" but all you've gotta know is that the more "pointy looking" your element is, the less accurate its results will be (AND the slower the simulation solves!). This means that thin stuff is really bad to mesh with solid elements, as you need a TON of them in order to properly fill the volume without having poorly shaped elements. Now, because structural engineers are good at their jobs, they make an artform out of building strong stuff with a little material as possible. This means that efficient structures are disproportionately "thin walled" enough to be efficient against things like bending stresses, which reward "section height" at a cubic rate with regards to stiffness, whereas tensile/compressive stresses reward mere cross sectional area at a linear rate with regards to stiffness.

Back on topic, your simulation would run faster, and probably produce slightly more accurate deflections per degree of freedom if you used simpler elements like shells or bars or beam elements, but you're patient, and this isn't too important, so this should be fine for things like "deflections", but that's only assuming that you've modeled all of your boundary conditions and load applications correctly, which is absolutely not going to be true for the first 100 times you run your model, and even then you wouldn't know for certain until you did full scale structural testing. Off topic. Moving on.

2.) What "failure" means. Sometimes, a deflection limitation is needed. An example of this is a hammock. A hammock isn't a good hammock if it's so stretchy that your butt touche the ground when you sit in it. It's failed even though it's not "broken." Other times, deflection is a loss of stiffness or permanent deformation. This happens when the yield stress is exceeded, meaning plastic deformation has occured, which is not fully reversable. For many things such as aircraft, this is the case... but they need to not avoid yield, as that would make the airplanes too heavy to work, which is terrifying. Most of the time, people who don't do structural analysis for a living refer to "failure" as "tensile ultimate failure" with regards to the "equivalent von mises stress criteria." This is not perfect, as the von mises stress criteria is ONLY representative of a true tri-axial stress state in the linear elastic regime, and ultimate failure (for ductile materials) does not occur in the linear elastic regime. That doesn't matter too much, however, as it's almost always conservative to use a linear elastic analysis and perform load scaling and superposition to write margins of safety to both yield, and ultimate material allowables.

In order to figure out "if your structure holds", FEA originated stress analysis is typically extremely inadequate. Right now, you have no clue if you set it up correctly, and even if you did know you set it up correctly, you don't know how over or under conservative your assumptions are. The correct way to do any of this kind of analysis is to propogate forward, starting at the load, to the boundary conditions, part by part, doing net section stress analysis and joint analysis with hand calculations. This is typically extremely easy, if done correctly, and almost universally produces answers that are more useful and fast to get than a simulation which is detailed enough to capture things like the loads through bolted joints with many fasteners.

Finite element analysis may be of massive assistance in doing these kinds of analyses. The typical way that finite element analysis is used in the world of structural analysis is universally as a "loads" model before it is as a "stress" model. This is fairly obvious, if you recall that the finite element method basically is just hooks law, but on continua rather than mathematical, lower dimensional "springs." The best way you could get this information is to take section cuts at all of your cross sections, pull the three forces and three moment components about the centroid (or neutral axis) and size the section using the interaction appropriate for the section and load in question. Bending Stress + Axial Stress + Shear Stress < Allowable Stress is almost always guaranteed to be a conservative interaction equation, but more sophisticated ones such as quadrature and von mises stress are common. Less common, is using the correct interaction equations which compensate for the fact that there's more to a material than the tensile yield strength.If you had, say, a foam structure, which was kind of strong against tension but weak against shear, then you wouldn't be able to use anything resembling von mises stress, as von mises stress just tries to turn everything into an equivalent "tensile stress"... which obviously doesn't work if tensile stress wasn't your concern anyways.

To learn more about this, I reccomend you not trust material properties in some random database (even if it's in FreeCAD!) and learn FEM with values you hunt for in a proper materials database like Mil-Handbook-5J. I also reccomend this relatively wonderful youtube video https://youtu.be/xkbQnBAOFEg, but it skips out heavily on the simplicities of practical stress analysis. A youtube channel called StructureFree is absolutely wonderful for some more of these nuances, https://www.youtube.com/playlist?list=P ... 99E4258070

Is there a specific kind of structure you'd like to learn more about analyzing? If it's ground structures like this that you're interested in, I highly reccomend picking up a copy of Bloodget: Design of Welded Structures. It's easily one of my favorite books to use for FAR more than just weld analysis. I do aircraft structures myself, and I'd be happy to answer any questions you've got about any of this jazz.

EDIT_01: If you're looking for books, I HIGHLY reccomend Finite Element Procedures by Bathe, if you want a single book with E V E R Y T H I N G in it (it's frighteningly dense) or any of the books by Cook, I like Finite Element Modeling for Stress Analysis by Cook. If you want a slightly better one for theoretical foundation that isn't as monsterous as Bathe, Taylor's "The Finite Element Method" is quite good as well. For nonlinear work, Belytchko's Nonlinear Finite Elements is the staple book, in my experience. Calculix'es developers would have far better opinions than mine on that topic, though.
cad1234
Posts: 331
Joined: Fri Dec 28, 2018 11:11 am

Re: CAE results interpretation

Post by cad1234 »

aerospaceweeb wrote: Mon Oct 18, 2021 2:55 am
Great Post! Many thanks!
taifun
Posts: 6
Joined: Thu Oct 14, 2021 11:00 am

Re: CAE results interpretation

Post by taifun »

Thx everyone for all the help, i will try to take a look at all the resources you shared (it might take some years).

In the meantime i made a few more analysis with finner meshes but i got some error from the solver. Here are my results and the console output with the error i encountered. In the attachment you can see the new load. With the new load the maximum stress is found at the fixed constraint.

The first line of the console output made me try another material and i got the same error.

Code: Select all

12:32:40  References: empty in MaterialSolid, MaterialSolid
12:32:40  References: Face in ConstraintFixed, ConstraintFixed
12:32:40  References: Face in ConstraintForce, ConstraintForce
12:32:40  Check prerequisites.
12:32:40  Check prerequisites.
12:32:40  References: empty in MaterialSolid, MaterialSolid
12:32:40  Start writing CalculiX input file
12:32:40  Write ccx input file to: C:\Users\ADMINI~1\AppData\Local\Temp\fcfem_9bzgldlk\FEMMeshNetgen.inp
12:32:40  ConstraintFixed:
12:32:40      Type: Fem::ConstraintFixed, Name: ConstraintFixed
12:32:40      ReferenceShape ... Type: Face, Object name: Solid, Object label: Defeatured051, Element name: Face26
12:32:40      ReferenceShape ... Type: Face, Object name: Solid, Object label: Defeatured051, Element name: Face59
12:32:40      ReferenceShape ... Type: Face, Object name: Solid, Object label: Defeatured051, Element name: Face13
12:32:40      ReferenceShape ... Type: Face, Object name: Solid, Object label: Defeatured051, Element name: Face8
12:32:40  ConstraintForce:
12:32:40      Type: Fem::ConstraintForce, Name: ConstraintForce
12:32:40      ReferenceShape ... Type: Face, Object name: Solid, Object label: Defeatured051, Element name: Face139
12:32:40  Writing time CalculiX input file: 13.28 seconds 

12:32:40  Writing CalculiX input file completed.
12:32:40  Run CalculiX ...
12:32:40  CalculiX failed with exit code 255
12:32:40  --------start of stderr-------
12:32:40  --------end of stderr---------
12:32:40  --------start of stdout-------
12:32:40  
************************************************************

CalculiX Version 2.17, Copyright(C) 1998-2020 Guido Dhondt
CalculiX comes with ABSOLUTELY NO WARRANTY. This is free
software, and you are welcome to redistribute it under
certain conditions, see gpl.htm

************************************************************

You are using an executable made on Thu Jul 23 21:43:50 CEST 2020

  The numbers below are estimated upper bounds

  number of:

   nodes:       497405
   elements:       442409
   one-dimensional elements:            0
   two-dimensional elements:            0
   integration points per element:            4
   degrees of freedom per node:            3
   layers per element:            1

   distributed facial loads:            0
   distributed volumetric loads:            0
   concentrated loads:        16416
   single point constraints:          852
   multiple point constraints:            1
   terms in all multiple point constraints:            1
   tie constraints:            0
   dependent nodes tied by cyclic constraints:            0
   dependent nodes in pre-tension constraints:            0

   sets:            5
   terms in all sets:      1695948

   materials:            1
   constants per material and temperature:            2
   temperature points per material:            1
   plastic data points per material:            0

   orientations:            0
   amplitudes:            2
   data points in all amplitudes:            2
   print requests:            1
   transformations:            0
   property cards:            0


 STEP            1

 Static analysis was selected

12:32:40  
--------end of stdout---------
12:32:40  --------start problems---------
12:32:40  
--------end problems---------
12:32:40  CalculiX finished with error 255.
Attachments
10.JPG
10.JPG (42.11 KiB) Viewed 4148 times
11.JPG
11.JPG (53.08 KiB) Viewed 4148 times
User avatar
NewJoker
Veteran
Posts: 3017
Joined: Sun Oct 11, 2020 7:49 pm

Re: CAE results interpretation

Post by NewJoker »

aerospaceweeb wrote: Mon Oct 18, 2021 2:55 am EDIT_01: If you're looking for books, I HIGHLY reccomend Finite Element Procedures by Bathe, if you want a single book with E V E R Y T H I N G in it (it's frighteningly dense) or any of the books by Cook, I like Finite Element Modeling for Stress Analysis by Cook. If you want a slightly better one for theoretical foundation that isn't as monsterous as Bathe, Taylor's "The Finite Element Method" is quite good as well. For nonlinear work, Belytchko's Nonlinear Finite Elements is the staple book, in my experience. Calculix'es developers would have far better opinions than mine on that topic, though.
I've used many books about FEA but my favorite ones when it comes to theory are those written by Bathe ("Finite Element Procedures") and Cook ("Concepts and Applications of Finite Element Analysis", I don't know the other one you've mentioned). I would recommend Crisfield ("Non-linear Finite Element Analysis of Solids and Structures") if you want to study nonlinearities and Wriggers ("Computational Contact Mechanics") in case you want to focus on contact modeling.

Personally, I don't like "The Finite Element Method" trilogy written by Zienkiewicz and my colleagues share this point of view. Those books are hard to read and discuss rather exotic topics.

There are also two books about practical aspects of FEA worth recommending: "Building Better Products with Finite Element Analysis" by Adams and "Practical Finite Element Analysis for Mechanical Engineers" by Madier. The first one is a bit old (written in late 90s) but still relevant. The other one was written last year and is a very good start.
Post Reply