# Understanding Shell Elements and Thickness Assignment **URL:** \ **Category:** Uncategorized\ **Created:** [September 9, 2022, 3:19pm UTC](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252 "2022-09-09T15:19:04Z")\ **Posts on this page:** 20\ **Page:** 1
**Author:** ![mishal49](https://avatars.discourse-cdn.com/v4/letter/m/e9c0ed/32.png) [@mishal49](https://calculix.discourse.group/u/mishal49)\ **Post date:** [September 9, 2022, 3:19pm UTC](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252/1 "2022-09-09T15:19:05Z")
Hello, In an attempt to understand how shell elements work in CalculiX, I set up a shell beam and set different thicknesses namely, 0.1, 0.5, 1 and 2. All of them are subject to a CLOAD of 10N in the negative y direction at one end. ![image](https://global.discourse-cdn.com/free1/uploads/calculix/original/1X/b316215b5a2ca33f7643e44da03f7b45bfb9c1fc.png) I assumed that the thickness value would not impact the resulting displacements or stresses however, the values are very different and I do not think this is accurate. I have attached a link to my 0.5 thickness case for reference. Where exactly have I gone wrong in the case set up? How may I be able to fix this? [https://myunt-my.sharepoint.com/personal/mishalraza\_my\_unt\_edu/Documents/Attachments/shell\_0.5.zip](https://myunt-my.sharepoint.com/personal/mishalraza_my_unt_edu/Documents/Attachments/shell_0.5.zip) Would appreciate any help. ---
**Author:** ![dichtstoff](https://avatars.discourse-cdn.com/v4/letter/d/dec6dc/32.png) [@dichtstoff](https://calculix.discourse.group/u/dichtstoff)\ **Post date:** [September 9, 2022, 3:25pm UTC](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252/2 "2022-09-09T15:25:38Z")
> [@mishal49](#): > > “I assumed that the thickness value would not impact the resulting displacements or stresses however, the values are very different and I do not think this is accurate.” What about your handcalculation for displacement of your beam? ---
**Author:** ![Calc\_em](https://avatars.discourse-cdn.com/v4/letter/c/43a26b/32.png) [@Calc\_em](https://calculix.discourse.group/u/Calc_em)\ **Post date:** [September 9, 2022, 3:27pm UTC](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252/3 "2022-09-09T15:27:57Z")
> [@mishal49](#): > > All of them are subject to a CLOAD of 10N in the negative y direction at one end. Is it bending ? It’s hard to say based on the picture since the geometry seems to be misaligned with axes of global coordinate system (or maybe it’s just a matter of unfortunate view orientation). Anyway, why would you expect no difference when the thickness of the beam is changed ? Then its stiffness will also change and stresses depend on the cross-section dimensions as well. Analytical calculations should clarify this. > [@mishal49](#): > > [Sign in to your account](https://myunt-my.sharepoint.com/personal/mishalraza_my_unt_edu/Documents/Attachments/shell_0.5.zip) Please try sharing the file again, this link leads to login page. ---
**Author:** ![mishal49](https://avatars.discourse-cdn.com/v4/letter/m/e9c0ed/32.png) [@mishal49](https://calculix.discourse.group/u/mishal49)\ **Post date:** [September 9, 2022, 5:25pm UTC](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252/4 "2022-09-09T17:25:49Z")
a concentrated load of 10N is applied on the end with 50 nodes so the value for displacement is supposed to be for 500N right? I got the displacement as 4 but the simulation gives 1.48 when I use: Max Disp = PL/3EI ---
**Author:** ![dichtstoff](https://avatars.discourse-cdn.com/v4/letter/d/dec6dc/32.png) [@dichtstoff](https://calculix.discourse.group/u/dichtstoff)\ **Post date:** [September 9, 2022, 5:27pm UTC](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252/5 "2022-09-09T17:27:47Z")
you can check the result of your boudary with: \*NODE PRINT,NSET=Nsbound\_01,totals=only RF working with bending properties it is recommended to work with quadrangle or hexahedra elements ---
**Author:** ![mishal49](https://avatars.discourse-cdn.com/v4/letter/m/e9c0ed/32.png) [@mishal49](https://calculix.discourse.group/u/mishal49)\ **Post date:** [September 9, 2022, 5:29pm UTC](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252/6 "2022-09-09T17:29:56Z")
It is not bending. Just a bad view. ![image](https://global.discourse-cdn.com/free1/uploads/calculix/original/1X/71e5b639c7e6498fbcf0fc2dbb22cf4c14b837d8.png) Is this better? How do you suggest I upload? I am unable to upload a zip folder. I expect no difference because I thought the purpose of assigning a thickness to a shell was just to create a virtual volume that Calculix can use to solve. ---
**Author:** ![mishal49](https://avatars.discourse-cdn.com/v4/letter/m/e9c0ed/32.png) [@mishal49](https://calculix.discourse.group/u/mishal49)\ **Post date:** [September 9, 2022, 5:31pm UTC](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252/7 "2022-09-09T17:31:31Z")
This is my current .inp file: \*INCLUDE, INPUT=all.msh \*INCLUDE, INPUT=fix.nam \*INCLUDE, INPUT=load.nam \*MATERIAL, Name=EL \*ELASTIC 4000000, 0.3 \*DENSITY 3000 \*SHELL SECTION, Elset=Eall, Material=EL, OFFSET=0.5 0.1 \*STEP, INC=1000000 \*DYNAMIC, ALPHA=0.0, DIRECT 1.E-2, 5.0 \*BOUNDARY Nfix, 1,3,0 \*CLOAD Nload, 2, -10.0 \*NODE FILE U \*EL FILE S, E \*END STEP ---
**Author:** ![Calc\_em](https://avatars.discourse-cdn.com/v4/letter/c/43a26b/32.png) [@Calc\_em](https://calculix.discourse.group/u/Calc_em)\ **Post date:** [September 9, 2022, 5:47pm UTC](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252/8 "2022-09-09T17:47:16Z")
> [@mishal49](#): > > How do you suggest I upload? I am unable to upload a zip folder. You can use hosting services like Google Drive, Dropbox or even WeTransfer. Just make sure that everyone can download the files after clicking the link. > [@mishal49](#): > > I expect no difference because I thought the purpose of assigning a thickness to a shell was just to create a virtual volume that Calculix can use to solve. Shell elements represent thin solids and their thickness is important for calculations. Just like the cross-section shape and dimensions in the case of beam elements. ---
**Author:** ![mishal49](https://avatars.discourse-cdn.com/v4/letter/m/e9c0ed/32.png) [@mishal49](https://calculix.discourse.group/u/mishal49)\ **Post date:** [September 9, 2022, 5:47pm UTC](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252/9 "2022-09-09T17:47:23Z")
I tried this @dichtstoff How should I share the output file? ---
**Author:** ![dichtstoff](https://avatars.discourse-cdn.com/v4/letter/d/dec6dc/32.png) [@dichtstoff](https://calculix.discourse.group/u/dichtstoff)\ **Post date:** [September 9, 2022, 5:48pm UTC](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252/10 "2022-09-09T17:48:43Z")
maybe these can work: \*INCLUDE, INPUT=all.msh \*INCLUDE, INPUT=fix.nam \*INCLUDE, INPUT=load.nam \*MATERIAL, Name=EL \*ELASTIC 4000000, 0.3 \*DENSITY 3000 \*SHELL SECTION, Elset=Eall, Material=EL 0.1 \*STEP \*STATIC \*BOUNDARY Nfix, 1,6,0 \*CLOAD Nload, 2, -10.0 \*NODE PRINT,NSET=Nfix,totals=only RF \*NODE FILE U \*EL FILE , OUTPUT=2D S, E \*END STEP if you double thickness, displacement should be half and please check the definition of a beam with dimension ---
**Author:** ![mishal49](https://avatars.discourse-cdn.com/v4/letter/m/e9c0ed/32.png) [@mishal49](https://calculix.discourse.group/u/mishal49)\ **Post date:** [September 9, 2022, 5:49pm UTC](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252/11 "2022-09-09T17:49:29Z")
> **[shell\_0.5.zip](https://drive.google.com/file/d/13pxoa5y9jED88VuZlMgKSKvWWWtgWgO0/view?usp=sharing)** > > Google Drive file. Is this working? ---
**Author:** ![Calc\_em](https://avatars.discourse-cdn.com/v4/letter/c/43a26b/32.png) [@Calc\_em](https://calculix.discourse.group/u/Calc_em)\ **Post date:** [September 9, 2022, 6:45pm UTC](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252/12 "2022-09-09T18:45:20Z")
> [@mishal49](#): > > Is this working? Yes, I downloaded the files. The structure is clearly subjected to bending. Each node on the loaded edge receives 10 N and there are 50 nodes on that edge so the total load should be 500 N. What unit system are you using ? Are dimensions given in meters ? Why are you using dynamic step ? According to analytical calculations assuming linear statics, the maximum values should be y=4 and σ=120000. Try solving this with solid elements. ---
**Author:** ![mishal49](https://avatars.discourse-cdn.com/v4/letter/m/e9c0ed/32.png) [@mishal49](https://calculix.discourse.group/u/mishal49)\ **Post date:** [September 9, 2022, 7:16pm UTC](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252/13 "2022-09-09T19:16:20Z")
Thank you for checking. I ran this case with solid elements too but the results were different. > **[solid\_0.5.zip](https://drive.google.com/file/d/19a7pmCo4_lMbAWoJPqvzzsx2_C6wF8DI/view?usp=sharing)** > > Google Drive file. ---
**Author:** ![dichtstoff](https://avatars.discourse-cdn.com/v4/letter/d/dec6dc/32.png) [@dichtstoff](https://calculix.discourse.group/u/dichtstoff)\ **Post date:** [September 9, 2022, 7:18pm UTC](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252/14 "2022-09-09T19:18:14Z")
\*NODE, NSET=Nall 1,0.000000000000e+00,0.000000000000e+00,0.000000000000e+00 2,1.500000000000e+01,0.000000000000e+00,0.000000000000e+00 3,1.500000000000e+01,1.500000000000e+01,0.000000000000e+00 4,0.000000000000e+00,1.500000000000e+01,0.000000000000e+00 5,1.500000000000e+01,3.000000000000e+01,0.000000000000e+00 6,0.000000000000e+00,3.000000000000e+01,0.000000000000e+00 7,1.500000000000e+01,4.500000000000e+01,0.000000000000e+00 8,0.000000000000e+00,4.500000000000e+01,0.000000000000e+00 9,1.500000000000e+01,6.000000000000e+01,0.000000000000e+00 10,0.000000000000e+00,6.000000000000e+01,0.000000000000e+00 11,1.500000000000e+01,7.500000000000e+01,0.000000000000e+00 12,0.000000000000e+00,7.500000000000e+01,0.000000000000e+00 13,1.500000000000e+01,9.000000000000e+01,0.000000000000e+00 14,0.000000000000e+00,9.000000000000e+01,0.000000000000e+00 15,1.500000000000e+01,1.050000000000e+02,0.000000000000e+00 16,0.000000000000e+00,1.050000000000e+02,0.000000000000e+00 17,1.500000000000e+01,1.200000000000e+02,0.000000000000e+00 18,0.000000000000e+00,1.200000000000e+02,0.000000000000e+00 19,3.000000000000e+01,0.000000000000e+00,0.000000000000e+00 20,3.000000000000e+01,1.500000000000e+01,0.000000000000e+00 21,3.000000000000e+01,3.000000000000e+01,0.000000000000e+00 22,3.000000000000e+01,4.500000000000e+01,0.000000000000e+00 23,3.000000000000e+01,6.000000000000e+01,0.000000000000e+00 24,3.000000000000e+01,7.500000000000e+01,0.000000000000e+00 25,3.000000000000e+01,9.000000000000e+01,0.000000000000e+00 26,3.000000000000e+01,1.050000000000e+02,0.000000000000e+00 27,3.000000000000e+01,1.200000000000e+02,0.000000000000e+00 \*ELEMENT, TYPE=S4, ELSET=Eall 1, 1, 2, 3, 4 2, 4, 3, 5, 6 3, 6, 5, 7, 8 4, 8, 7, 9, 10 5, 10, 9, 11, 12 6, 12, 11, 13, 14 7, 14, 13, 15, 16 8, 16, 15, 17, 18 9, 2, 19, 20, 3 10, 3, 20, 21, 5 11, 5, 21, 22, 7 12, 7, 22, 23, 9 13, 9, 23, 24, 11 14, 11, 24, 25, 13 15, 13, 25, 26, 15 16, 15, 26, 27, 17 \*MATERIAL,NAME=Steel \*ELASTIC 200000,0.3 \*SHELL SECTION,ELSET=Eall,MATERIAL=Steel 1 \*STEP \*STATIC \*BOUNDARY 1,1,6,0 2,1,6,0 19,1,6,0 \*CLOAD 17,1,10000 \*NODE FILE, OUTPUT=2D U, \*EL FILE S, \*END STEP these simple inp file works perfect. very simple: dimension 120x30x1 E=200000 F=10000 f=Fxl^3x12 / 3 / E / t / h^3 = 12.80 CCX = 13.2 ---
**Author:** ![mishal49](https://avatars.discourse-cdn.com/v4/letter/m/e9c0ed/32.png) [@mishal49](https://calculix.discourse.group/u/mishal49)\ **Post date:** [September 9, 2022, 7:19pm UTC](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252/15 "2022-09-09T19:19:15Z")
Sorry, I just saw this. Will try this now ---
**Author:** ![mishal49](https://avatars.discourse-cdn.com/v4/letter/m/e9c0ed/32.png) [@mishal49](https://calculix.discourse.group/u/mishal49)\ **Post date:** [September 9, 2022, 8:03pm UTC](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252/16 "2022-09-09T20:03:17Z")
@dichtstoff, I tried this with 0.5 thickness and I got 3.59 as displacement which is close to theoretical value of 4! However, is this considered normal? Isn’t the error quite big? Also, I ran the same case for a solid section but got a displacement value of 6.81. Is this because I now have more nodes in the load NSET? How may I set this up so that I could get the same results as a shell? ---
**Author:** ![mishal49](https://avatars.discourse-cdn.com/v4/letter/m/e9c0ed/32.png) [@mishal49](https://calculix.discourse.group/u/mishal49)\ **Post date:** [September 9, 2022, 8:05pm UTC](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252/17 "2022-09-09T20:05:27Z")
Units are SI. is this stress value, σ=120000, the SXX? ---
**Author:** ![dichtstoff](https://avatars.discourse-cdn.com/v4/letter/d/dec6dc/32.png) [@dichtstoff](https://calculix.discourse.group/u/dichtstoff)\ **Post date:** [September 9, 2022, 8:40pm UTC](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252/18 "2022-09-09T20:40:25Z")
triangle elements are a bit stiffeners than hex or quad elements you have your load in one node, and not over the hole length, beam is defined with a less hight and more length, you have opposite you can use 2-elements or you can calc. with selfweight i guess it is possible to get the same result with shell elements ---
**Author:** ![mishal49](https://avatars.discourse-cdn.com/v4/letter/m/e9c0ed/32.png) [@mishal49](https://calculix.discourse.group/u/mishal49)\ **Post date:** [September 11, 2022, 6:01pm UTC](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252/19 "2022-09-11T18:01:06Z")
Okay @dichtstoff. So, if I get this correctly, I should change the elements I use for the solid right? to get closer results. Also, what do you mean about the beam? Do you think I could have better dimensions? Like a longer beam? Right now it is 10 units long and 1 x 0.5 cross section. Also, do you think I could use a DLOAD on the node set to get similar results? I tried generating a distributed file with CGX using the following command: “send load abq pres 10.0” however, the .dlo file generated is always empty and I am not sure why. ---
**Author:** ![dichtstoff](https://avatars.discourse-cdn.com/v4/letter/d/dec6dc/32.png) [@dichtstoff](https://calculix.discourse.group/u/dichtstoff)\ **Post date:** [September 11, 2022, 6:25pm UTC](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252/20 "2022-09-11T18:25:20Z")
> [@mishal49](#): > > So, if I get this correctly, I should change the elements I use for the solid right? to get closer results. yes, if you work with bending properties, you should use not triangle elements: for all elements, shell, solid or 2-D plane elements: (and from my experience, it makes in no different in ccx, if you use second order elements, for triangle elements, but you have to test it) you will find more information if you look for it like these: > **[Why is a Triangular Element Stiffer?](https://enterfea.com/why-is-a-triangular-element-stiffer/)** > > You have most likely heard that triangular elements are stiffer. But why exactly is that? I will explain the whole thing without using complex math! > **[Linear tetrahedral elements for solid mechanics. Don’t do it!](https://ckadapa.wordpress.com/2019/11/16/linear-tetrahedral-elements-for-solid-mechanics-dont-do-it/)** > > Linear tetrahedral elements (triangular elements in 2D) are the popular elements in the finite element community. Because of the ease of mesh generation, many FEA users use them without paying much… ![image](https://global.discourse-cdn.com/free1/uploads/calculix/original/2X/c/c96ea05977478b76e5b4d731e9a27034e261c3d4.png) ![image](https://global.discourse-cdn.com/free1/uploads/calculix/original/2X/b/b804c281bfe1e18b47c421ce40993efee73d3b86.png) > **[Ihr persönlicher Freigabelink | GMX Cloud](https://c.gmx.net/@324820432001700943/jGzoLNMlTeiEgSLHVpoEzw)** > > Mit diesem Link erhalten Sie Zugriff auf die mit Ihnen geteilten Daten. [Next page](https://calculix.discourse.group/t/understanding-shell-elements-and-thickness-assignment/1252.md?page=2)