# Cantilever beam with load at one end **URL:** \ **Category:** General Questions\ **Created:** [November 12, 2023, 4:46pm UTC](https://prepomax.discourse.group/t/cantilever-beam-with-load-at-one-end/1241 "2023-11-12T16:46:03Z")\ **Posts on this page:** 16\ **Page:** 1
**Author:** ![CrisBab](https://avatars.discourse-cdn.com/v4/letter/c/22d042/32.png) [@CrisBab](https://prepomax.discourse.group/u/CrisBab)\ **Post date:** [November 12, 2023, 4:46pm UTC](https://prepomax.discourse.group/t/cantilever-beam-with-load-at-one-end/1241/1 "2023-11-12T16:46:04Z")
Hello, I’m testing a simple 3d cantilever model. The analytical results are max displacement 22.57um and max VM stress 10.7MPa. With PrePoMax I tried different mesh refinements obtaining the results below. The u\_max value is quite stable but a bit higher, the VM stress value increases as the mesh size decreases. I tried also with GetDP and I got the same instability of the max stress. How can I get more stable values? Mesh elm size u\_max VM\_max 10mm 22.69 10.36 2mm 22.74 13.68 1.5mm 22.75 15.21 1mm 22.76 17.41 0.75mm 22.76 19.21 Thanks ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/d/d2f7765fdf85b21b16f712aeaeeaa051538f8a5b.png) ---
**Author:** ![FEAnalyst](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/feanalyst/32/688_2.png) [@FEAnalyst](https://prepomax.discourse.group/u/FEAnalyst)\ **Post date:** [November 12, 2023, 5:14pm UTC](https://prepomax.discourse.group/t/cantilever-beam-with-load-at-one-end/1241/2 "2023-11-12T17:14:05Z")
That’s how stress concentrations work in FEA. You should run mesh convergence studies until the maximum stress doesn’t increase significantly anymore. Unless you encounter a stress singularity where the stress doesn’t stop increasing. Fixed constraint doesn’t accurately represent the real-life problem. There are several articles on this topic but those can be particularly interesting in this case: > **[FEA Meshing](https://www.valuedes.co.uk/meshing.html)** > > Tutorial on how meshing affects FEA Analysis results. Example of a beam in bending and comparing tetrahedral, brick, shell and beam elements. > **[Stress singularities, stress concentrations and mesh convergence](http://www.acin.net/2015/06/02/stress-singularities-stress-concentrations-and-mesh-convergence/)** > > 1. Introduction > The FEM (Finite Element Method) is a way of obtaining a of finding a solution to a physical problem. It relies on discretizing a continuum domain into finite elements. The accuracy of the solution greatly depends on the number of... > **[Mesh convergence with examples](https://enterfea.com/mesh-convergence/)** > > You don't know how to choose the correct mesh size? The best approach is to perform a mesh convergence check! > **[Stress singularity - an honest discussion](https://enterfea.com/stress-singularity-an-honest-discussion/)** > > Stress singularity in FEA is just one of those pesky problems you need to deal with! Learn why you get this error, and how to deal with it effectively! ---
**Author:** ![ANYS](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/anys/32/7737_2.png) [@ANYS](https://prepomax.discourse.group/u/ANYS)\ **Post date:** [November 12, 2023, 9:04pm UTC](https://prepomax.discourse.group/t/cantilever-beam-with-load-at-one-end/1241/3 "2023-11-12T21:04:37Z")
When comparing with analytical solutions do not forget many times Poisson Ratio effect is not taken into consideration on those formulas. Looking at your Stress distribution, you are probably considering Poisson and the fixed support is inducing peak stresses as Calc\_em explained. If you want to compare with the closed form look for BC that deliver stress profiles like this, with a well-defined neutral fiber down to the base and nearly non discontinuity with the sides. > **[FEA Meshing](https://www.valuedes.co.uk/meshing.html)** > > Tutorial on how meshing affects FEA Analysis results. Example of a beam in bending and comparing tetrahedral, brick, shell and beam elements. ![imagen](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/f/fd239013db2b07a5943e128c7e33cae958cc72bb.jpeg) ---
**Author:** ![CrisBab](https://avatars.discourse-cdn.com/v4/letter/c/22d042/32.png) [@CrisBab](https://prepomax.discourse.group/u/CrisBab)\ **Post date:** [November 12, 2023, 10:08pm UTC](https://prepomax.discourse.group/t/cantilever-beam-with-load-at-one-end/1241/4 "2023-11-12T22:08:09Z")
Thank you very much for your references. @ANYS, do you mean periodic boundary conditions on sides? ---
**Author:** ![FEAnalyst](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/feanalyst/32/688_2.png) [@FEAnalyst](https://prepomax.discourse.group/u/FEAnalyst)\ **Post date:** [November 12, 2023, 11:32pm UTC](https://prepomax.discourse.group/t/cantilever-beam-with-load-at-one-end/1241/5 "2023-11-12T23:32:53Z")
There are no actual periodic BCs in PrePoMax (and defining them in CalculiX input file is possible but not easy) but you don’t need such advanced BCs. You can just use symmetry in the form of translation being blocked in the normal direction. ---
**Author:** ![fatigue.pro](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/fatigue.pro/32/1786_2.png) [@fatigue.pro](https://prepomax.discourse.group/u/fatigue.pro)\ **Post date:** [November 14, 2023, 7:42am UTC](https://prepomax.discourse.group/t/cantilever-beam-with-load-at-one-end/1241/6 "2023-11-14T07:42:02Z")
> [@CrisBab](#): > > I’m testing a simple 3d cantilever model. With suitable models, anlalytic results can also be recalculated in FEM. I therefore used the “SAE keyhole benchmark” and recalculated it with Calculix in FreeCAD. And then the stress results also come closer as the mesh becomes finer. [https://fatigue.pro/2023/02/freecad-fem-results-in-fatlab#SAEkeyhole](https://fatigue.pro/2023/02/freecad-fem-results-in-fatlab#SAEkeyhole) > In FreeCAD we get a maximum stress in X direction of 34.1 MPa and a maximum P1 stress of 34.3 MPa. And that is very close to the estimated analytical results of 33.6 MPa. ![](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/8/8830fadc49ba71a8818bac0b4968df860a544c0b.png) ---
**Author:** ![ANYS](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/anys/32/7737_2.png) [@ANYS](https://prepomax.discourse.group/u/ANYS)\ **Post date:** [November 14, 2023, 10:17am UTC](https://prepomax.discourse.group/t/cantilever-beam-with-load-at-one-end/1241/7 "2023-11-14T10:17:20Z")
Hi, Fatigue.pro, That is an excellent validation example to work with. I used it recently to get a better understanding of ccx + the new stress linearization tool in Mecway. Agreement was excellent. ![imagen](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/e/e8065c60954c079c03fc9906cad2664ef96eaf01.png) ---
**Author:** ![CrisBab](https://avatars.discourse-cdn.com/v4/letter/c/22d042/32.png) [@CrisBab](https://prepomax.discourse.group/u/CrisBab)\ **Post date:** [November 19, 2023, 2:04pm UTC](https://prepomax.discourse.group/t/cantilever-beam-with-load-at-one-end/1241/8 "2023-11-19T14:04:25Z")
Do you mean symmetry on the clamped surface? u\_x = 0? or uz=0 on the beam sides? In this case, It would be a plane strain condition that is not correct I think. ![image](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/5/5e61c7eaa326719a5103bae796202e8272bf63d5.jpeg) Thanks ---
**Author:** ![ANYS](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/anys/32/7737_2.png) [@ANYS](https://prepomax.discourse.group/u/ANYS)\ **Post date:** [November 19, 2023, 3:17pm UTC](https://prepomax.discourse.group/t/cantilever-beam-with-load-at-one-end/1241/9 "2023-11-19T15:17:27Z")
x y and z constrains. Slab should be able to freely slide in the yz supporting plane so Poisson has minimum effect on that area. Poisson should be zero as you want to compare with the ideal analitycal solution. ![imagen](https://global.discourse-cdn.com/free1/uploads/prepomax/original/2X/b/bcf28a7044bafe64b5ce9bfbf25cd3edc17557b4.jpeg) ---
**Author:** ![CrisBab](https://avatars.discourse-cdn.com/v4/letter/c/22d042/32.png) [@CrisBab](https://prepomax.discourse.group/u/CrisBab)\ **Post date:** [November 19, 2023, 4:06pm UTC](https://prepomax.discourse.group/t/cantilever-beam-with-load-at-one-end/1241/10 "2023-11-19T16:06:20Z")
Hi, your solution works if the mesh is structured and the edges coincide with the position you need. For tetra mesh, I have to draw additional support lines and nodes, right? Can you suggest any reference books that deal with basic/advanced structural problems to check with FEA? Thanks ---
**Author:** ![Matej](https://avatars.discourse-cdn.com/v4/letter/m/a698b9/32.png) [@Matej](https://prepomax.discourse.group/u/Matej)\ **Post date:** [November 19, 2023, 6:23pm UTC](https://prepomax.discourse.group/t/cantilever-beam-with-load-at-one-end/1241/11 "2023-11-19T18:23:53Z")
Singular stresses can occur on different occasions. Mainly on fixed (rigid) supports, sharp internal corners, and under concentrated forces. The reason for their appearance is idealization in the modeling approach. For fixed supports, the alternative is a spring support. You can use fixed support to evaluate displacements and then replace the fixed support with soft spring support to evaluate stresses. Of course, this approach is limited to linear analysis. ---
**Author:** ![ANYS](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/anys/32/7737_2.png) [@ANYS](https://prepomax.discourse.group/u/ANYS)\ **Post date:** [November 20, 2023, 8:33am UTC](https://prepomax.discourse.group/t/cantilever-beam-with-load-at-one-end/1241/12 "2023-11-20T08:33:01Z")
NAFEMS Finite Element Benchmarks is the right way to go. Different FE software’s rely on them to test their solvers. That means you can go to those software webpages to find them and avoid paying for the Nafems original. Google this “esrd Benchmarks-Guide-Standard-NAFEMS” or “NX Nastran 11 Verification Manual” for example. They are based on Nafems. DNV Standards are excellent too. Clear, well explained and typically have some examples to test your understanding at the end. In fact, using their examples as validation is part of DNV’s methodology. “calibration of analysis methodology” That makes all your work of validation a training but also a tool to “calibrate” your skills, methodology, solver performance,…. Abaqus itself has a lot of examples. Google “Abaqus Verification Manual” [https://classes.engineering.wustl.edu/2009/spring/mase5513/abaqus/docs/v6.6/books/ver/default.htm](https://classes.engineering.wustl.edu/2009/spring/mase5513/abaqus/docs/v6.6/books/ver/default.htm) It has the advantage that you can download the inp to see how they finally do it. From my point of view the problems are not so well stated and can be difficult to set up your model in exactly the same way. Also because Abaqus has additional features and elements . Don’t get obsessed with accuracy. If you get below 3%-4% agreement move on to the next. At the beginning it can be very frustrating. You need time and can be very tricky to go down below 1% on those validations. ---
**Author:** ![FEAnalyst](https://yyz2.discourse-cdn.com/free1/user_avatar/prepomax.discourse.group/feanalyst/32/688_2.png) [@FEAnalyst](https://prepomax.discourse.group/u/FEAnalyst)\ **Post date:** [November 20, 2023, 9:14am UTC](https://prepomax.discourse.group/t/cantilever-beam-with-load-at-one-end/1241/13 "2023-11-20T09:14:45Z")
> [@ANYS](#): > > Google “Abaqus Verification Manual” Abaqus has Benchmarks Manual and Example Problems Manual too, they can be better than Verification Manual which is focused on simple tests (often single-element tests) to verify various analysis features like material models and element types. And here’s a newer version of the Abaqus documentation (more recent ones require DS account): [http://130.149.89.49:2080/v2016/index.html](http://130.149.89.49:2080/v2016/index.html) I would also recommend those examples: [https://www.simscale.com/docs/validation-cases](https://www.simscale.com/docs/validation-cases) and Code\_Aster validation cases on which several examples from that website are based. ---
**Author:** ![lastairbender](https://avatars.discourse-cdn.com/v4/letter/l/9d8465/32.png) [@lastairbender](https://prepomax.discourse.group/u/lastairbender)\ **Post date:** [December 30, 2024, 6:19am UTC](https://prepomax.discourse.group/t/cantilever-beam-with-load-at-one-end/1241/14 "2024-12-30T06:19:18Z")
if you have your pmx file can you share this? ---
**Author:** ![andrea.starnini](https://avatars.discourse-cdn.com/v4/letter/a/46a35a/32.png) [@andrea.starnini](https://prepomax.discourse.group/u/andrea.starnini)\ **Post date:** [December 31, 2024, 7:42am UTC](https://prepomax.discourse.group/t/cantilever-beam-with-load-at-one-end/1241/15 "2024-12-31T07:42:52Z")
More than 10 years ago I made some comaprison with theory and NAFEMS benchmark on linear elastic field. If could be useful I attach the document [CCX Linear.zip](https://prepomax.discourse.group/uploads/short-url/dgXxtfQ5Z4Lp2KIBRUJQQIAQ3Uz.zip) (1.4 MB) ---
**Author:** ![lastairbender](https://avatars.discourse-cdn.com/v4/letter/l/9d8465/32.png) [@lastairbender](https://prepomax.discourse.group/u/lastairbender)\ **Post date:** [January 20, 2025, 10:44am UTC](https://prepomax.discourse.group/t/cantilever-beam-with-load-at-one-end/1241/16 "2025-01-20T10:44:01Z")
Thank you so much for your help!