# FEA Master Class: Session 2 (Nonlinear Plasticity Effects on Wheel Rim) **URL:** \ **Category:** Using SimScale\ **Created:** [March 28, 2017, 8:26am UTC](https://www.simscale.com/forum/t/fea-master-class-session-2-nonlinear-plasticity-effects-on-wheel-rim/66191 "2017-03-28T08:26:46Z")\ **Posts on this page:** 20\ **Page:** 1
**Author:** ![anon5983385](https://www.simscale.com/forum/letter_avatar/anon5983385/32/6_22734026db12803ebb3e059622ac3534.png) [@anon5983385](https://www.simscale.com/forum/u/anon5983385)\ **Post date:** [March 28, 2017, 8:26am UTC](https://www.simscale.com/forum/t/fea-master-class-session-2-nonlinear-plasticity-effects-on-wheel-rim/66191/1 "2017-03-28T08:26:46Z")
> Tutorial Updated 2018-01 ## Recording * * * [![](https://www.simscale.com/forum/uploads/default/original/3X/c/8/c88db16b41322b575794d0267b4bf65d6253f3c0.jpeg "FEA Master Class: Nonlinear Material & Strength Theory") ](https://www.youtube.com/watch?v=9gZftcYU50Y) ## Introduction * * * The FEA Master Class: Session 2 underscores the significant impact that the material has on the outcome of the simulation. In this exercise, you will be enabled to utilize the SimScale Platform to setup a Finite Element Analysis (FEA) study to simulate the forces on a child’s bicycle wheel, if a sumo wrestler sits on it. The stress-strain curve describes the behavior of a material under loading. The primary aim of this analysis is to study the non-linear plasticity effects on a wheel rim and determine the role played by the material type on the physical significance of the result. ![](https://www.simscale.com/forum/uploads/default/original/2X/4/4db69e2274590c9a528c49c8f1d40b4316e9f555.png) Hence, our analysis is to be done post the yield strength point (non-linear region) of the wheel rim material, i.e., **Polypropylene**. ![](https://www.simscale.com/forum/uploads/default/original/2X/d/db98e434929c1fbe3a16fd83119a2d48437aa136.png) ## Import Project * * * Given below is the link to the initial point of the project: Handout Project: [Project Link](https://www.simscale.com/workbench/?publiclink=0d72271c-4f85-40e6-b427-b351a5d33dcd) Now that you have been provided with the Bike Wheel Geometry ( **wheelFEA** ), you can use it to set up a simulation that analyzes the effect of the material type on the results. ## Mesh Generation * * * Start up the **Mesh Creator** mode in the workflow. Select the **Meshes** in the Navigator and click on New to begin with the meshing procedure. ![image](https://www.simscale.com/forum/uploads/default/original/3X/8/a/8a763ba65467ae4e48bf094df99060361c50ba03.png) After assigning an appropriate **Name** to your mesh, select the **Base Geometry** as **wheelFEA**. ![image](https://www.simscale.com/forum/uploads/default/original/3X/1/4/14d3ec241c2b85f2d8db94ac8a8ecdf8ad44d079.png) Please a new **Operation** by clicking on **New**. ![image](https://www.simscale.com/forum/uploads/default/original/3X/f/7/f7eb0529c7d190a846e43933672cd0f516a0e8c9.png) A **Tet-dominant** mesh operation is used for this FEA study. The global mesh sizing may now be set as follows: ![image](https://www.simscale.com/forum/uploads/default/original/3X/0/5/05be19c874b5026eace92088e8bfc9a794cb878a.png) You may now proceed to make a mesh refinement by clicking on **New** in the **Mesh Refinements** tab below. With the intention of refining the surface, which is in contact with the ground, you can follow these steps: Set the Type as Local element size and the\*\* Element sizing\*\* as **Automatic**. The Mesh fineness should be **4-Fine**. To select the desired face, first, click on the **Pick Faces** tool displayed on the top of the viewer and then click on the face as shown below. Proceed by clicking **Save**. ![image](https://www.simscale.com/forum/uploads/default/original/3X/d/e/deed4f452f29e4c34c929573b113c672a9e66a4b.png) Essentially, the ground is an immovable rigid support on which we do not want to perform any calculations. Thus, we assign it the coarsest mesh possible. To make a new mesh refinement, right click on **Mesh Refinements** and select **Add mesh refinement**. ![image](https://www.simscale.com/forum/uploads/default/original/3X/6/9/6942e3b73e86294e1a3bb23562240640eb1b143c.png)   ![image](https://www.simscale.com/forum/uploads/default/original/3X/f/7/f71d543a6d3153515c0bab33df47c2f0e78206f5.png) To avoid numerical divergence in the solver, it is imperative that the contact between the rim and the tyre has an identical mesh refinement. This is the intent of our **Contact Refinement**. Add new mesh refinement following the procedure described previously. Set the values as shown in the column (Figure 11). On the top right of the viewer, you will be able to see a Show/Hide box. Hide **solid\_0** and **solid\_2** by clicking on the Eye Icon next to them. The hidden items will be rendered transparent and the shown ones will still be colored. Now, you can easily select the three faces of the tyre as shown in the image below. ![image](https://www.simscale.com/forum/uploads/default/original/3X/d/9/d9c18999f9d7e9ff0726937aef07d1b31b69c16b.png) Subsequently, hide\*\* solid\_0\*\* and **solid\_1** and show **solid\_2**. The three faces of the rim which are in contact with the tyre should be selected. Use the same mesh refinement specifications as earlier. ![image](https://www.simscale.com/forum/uploads/default/original/3X/6/a/6a262962c4125a27014afdf983e9d34f4717b89b.png) Click **Save** after the global meshing and 3 local refinements have been setup. Open the Operation 1 tab and Start the mesh operation. ![image](https://www.simscale.com/forum/uploads/default/original/3X/0/b/0bce3b6592c8456c88d0b1b415e33bbf72c9891f.png) The meshing can be tracked from the progress bar shown below. ![image](https://www.simscale.com/forum/uploads/default/original/3X/6/4/648631e0b46103fa1bb6490cfa5da92e0e533d0d.png) The mesh may now be visualized in the viewer. ![image](https://www.simscale.com/forum/uploads/default/original/3X/b/2/b28cd98781cd15762434930f2afc2c22514efa67.png) _Kindly note: Confirm your mesh specifications with the ones shown in the image below before starting the Mesh Operation_ ## Simulation Setup * * * Select the **Simulation Designer** tab in the workflow and click on **New** to create a new simulation setup. ![image](https://www.simscale.com/forum/uploads/default/original/3X/0/b/0bb0c0ac5ed5dbb85f6aca2caafea4f48981b039.png) You will see an array of simulation types you can choose from. In our case, we choose the Static simulation under the category- **Solid Mechanics** ![image](https://www.simscale.com/forum/uploads/default/original/3X/6/7/670f1e9ef4ad95d6a02145c326e6dbf08a5ab3bc.png) Please assign an appropriate name to your simulation and set the **Nonlinear analysis** to\*\* true\*\*. This is because we want to study the non-linear plasticity effects on the wheel. ![image](https://www.simscale.com/forum/uploads/default/original/3X/1/2/127fb734edffb64ced6905b74abbe28a0be06af5.png) Select **Domain** from the **Navigator**. You will be able to see the mesh that you have created. Select the desired mesh on which the simulation is to be performed. ![image](https://www.simscale.com/forum/uploads/default/original/3X/5/9/590a8b91358131c743357323eceacf90f4171f3a.png) The mesh will be displayed on the viewer as shown in the figure below. Click Save to continue to the simulation set up. ### Contact Defnition Let us move on to assigning the contacts. Select Contacts in the Navigator and create a New contact ![image](https://www.simscale.com/forum/uploads/default/original/3X/b/9/b9edd5427df30841ac1d28a38d5eb5b2251b5f2d.png) Change the render mode to **surfaces** to proceed with the simulation setup. ![image](https://www.simscale.com/forum/uploads/default/original/3X/0/7/0712ad99b9f73bfca3c73e721d959cb9a7c2fbf4.png) Generally, it is considered to be a best practice to select the more rigid material as the **Master Entity**. In our case, that would be the rim. Select the faces of the rim that are in contact with the tyre. Moreover, change the **Type of Contact** to **Bonded Contact** and the **Tolerance** to \*\* 0.001\*\*. ![image](https://www.simscale.com/forum/uploads/default/original/3X/e/8/e891339687fc915f20cf7942c5f7cdd0fc928c44.png) Similarly, assign the surfaces on the tyre that are in contact with the rim as \*\* Slave Entity\*\*. ![image](https://www.simscale.com/forum/uploads/default/original/3X/7/d/7d868db6c3abb65370b90f1fd9abaa3641c45354.png) Since we intend to perform a static analysis, we assume that the contact between the tyre and the ground is set as a frictionless physical contact. Select the **Physical Contacts** option in the **Navigator** and create a **New** physical contact. ![image](https://www.simscale.com/forum/uploads/default/original/3X/8/d/8d8976f64d333b8cd453957caf3379cd0cf72afc.png) Select the Type as **Frictionless Penalty Contact** and increase the **Penalty coefficient** to **10000000000000** (10e+13). As you already know, the more rigid body should be assigned as the master entity. As we’re dealing with the contact between the tyre and the ground, the _ground_ would be the Master Entity. _Kindly Note: Make sure that you use to the face selection tool to select only the surface of the ground which is in contact with the tyre and not the entire volume._ ![image](https://www.simscale.com/forum/uploads/default/original/3X/d/f/df4c0210ba3aa7f6625af7d3f5c01b8b67463bd0.png) Likewise, assign the surface of the tyre that is in contact with the ground as the **Slave Entity**. ![image](https://www.simscale.com/forum/uploads/default/original/3X/3/1/31e5073e19ce568a3f67c3e0f4c22d28ec021b21.png) ### Material Selection Choose the **Materials** option in the **Navigator** and click on **New** ![image](https://www.simscale.com/forum/uploads/default/original/3X/e/b/eb32295173778410c63c06b4e18ff43d096ecde6.png) We need to assign the material Polypropylene to the wheel rim. To do this, click\*\* Import from material library\*\* select **PP-Polypropylene** from the list of Materials displayed in the library. ![image](https://www.simscale.com/forum/uploads/default/original/3X/a/5/a519ff5deaee2eb8bba530b67ea09847b126a94b.png)   ![image](https://www.simscale.com/forum/uploads/default/original/3X/7/6/76a99814c0039254c434a490715da64c5c4aab20.png) Since we intend to study the plasticity effects in the rim, the **Material behavior** should be set to **Plastic**. Please note that this would be our first varying parameter for the next simulation. Set the **Young’s modulus** to **1200000000** (1.2 GPa). Next, upload the required **.csv** file to the platform. This file contains the stress and strain data which defines the plastic behavior of the material. The prepared **.csv** file can be obtained from [here](https://drive.google.com/drive/folders/0B61zWr9oT-EQNXNCc2x1bDl2NUU). The steps are illustrated in the images shown below: ![image](https://www.simscale.com/forum/uploads/default/original/3X/a/3/a34714c4716c20ab98d9b47f52c753b90621ac4b.jpg)   ![image](https://www.simscale.com/forum/uploads/default/original/3X/b/9/b91dd08d67d10d08faf66f30f8f966750307cd36.png)   ![image](https://www.simscale.com/forum/uploads/default/original/3X/8/5/850c741c46dd22955dcc4f76f0bc4fe315e059f6.png)   This material is now mapped to the rim by selecting it in the viewer using **Pick Volumes**. To add a new material, right click on\*\* Materials\*\* in the **Navigator** and click on **Add Solid material**. ![image](https://www.simscale.com/forum/uploads/default/original/3X/6/0/601228b7a98eae37ac10b6f77473fab19a7313cf.png) You may now import the material **Rubber** from the **Material Library** by clicking on **Import from material library** and selecting **Rubber**. ![image](https://www.simscale.com/forum/uploads/default/original/3X/1/4/1485dfbe910c0951291cd0c219bc05057067b011.png) Set the material behavior to **Hyperelastic** , which is a more accurate representation of the physical behavior of rubber under loading. The Hyper-elastic model is set to **Mooney-Rivlin**. Please note that this would be our second varying parameter for the next simulation. This material is assigned to the tyre by selecting it from the viewer using **Pick Volumes**. ![image](https://www.simscale.com/forum/uploads/default/original/3X/f/b/fbe88a00023e93d508abec2f950ccc971b09971d.png) Now, we move on to assigning a material to the ground. As shown earlier, import new material from the library and choose **Concrete**. ![image](https://www.simscale.com/forum/uploads/default/original/3X/0/e/0e9fa254b2ab8068a46bf1802f58b45adf7a88bd.png) Assign the material to the ground by selecting it from the viewer and using \*\* Pick Volumes\*\*. ![image](https://www.simscale.com/forum/uploads/default/original/3X/a/7/a7518eca8cfb12c468124ef47432ec7b82f7e062.png) ### Assigning Constraints and Loads Here is an overview of the constraints and loads on the Wheel: ![image](https://www.simscale.com/forum/uploads/default/original/3X/8/e/8e5538677e9c5e4518338c7efbfcd9a63f0c1b5a.jpg) Let us proceed to add constraint boundary conditions. Select **Constraints** in the **Navigator** and click on **New**. ![image](https://www.simscale.com/forum/uploads/default/original/3X/a/8/a899cda2f58461e638a50b281be3669a834a6924.png) Now, we model the ground as per requirement. Set the type to\*\* Fixed Support\*\*, pick the **Ground volume** and click **Save**. ![image](https://www.simscale.com/forum/uploads/default/original/3X/2/f/2f595bfae21ed408705711aeeaac9e99199373ea.png) To add a new constraint, right click on **Constraints** in the **Navigator** and select **Add Constraints bound**. You could also click on **Constraints** and then **New** to add another constraint. ![image](https://www.simscale.com/forum/uploads/default/original/3X/b/e/be381b37ac765cba6172a90a4616c78b2d24f3de.png) Please follow the settings shown in the screenshots below to model the required boundary conditions. 1. The **Symmetry** in the **XZ Plane** : ![image](https://www.simscale.com/forum/uploads/default/original/3X/7/6/7642853a45e60b1b34e62b06a46626add90fe788.png) 1. The **Symmetry** in the **YZ Plane** : ![image](https://www.simscale.com/forum/uploads/default/original/3X/6/6/66ec8f5e606ac0446d8627edc249fa10d7fa05dc.png) 1. The orthotropic **Elastic support** : ![image](https://www.simscale.com/forum/uploads/default/original/3X/3/0/30adde33fb7795c22122b18d99b7fb2465a8d14d.png) 1. **Shaft Constraint** : The influence of the shaft and bearing on the wheel are modeled with the Shaft constraint ![image](https://www.simscale.com/forum/uploads/default/original/3X/3/5/35425b88dfdbab4bbde46540a6d776c6b1beaf1f.png) To create a new load, select **Loads** in **Navigator** and click on **New**. ![image](https://www.simscale.com/forum/uploads/default/original/3X/1/0/10bfadd8088613b5eede6843989fd49d463fb5c7.png) The load on the wheel is modeled with the **Cycle + Sumo Wrestler** constraint Click on f(x) in the fz [N] option to select a time-variant force. Add the formula, -505\*t, which governs the magnitude and direction of the force. Select the two internal faces which are in contact with the shaft. ![image](https://www.simscale.com/forum/uploads/default/original/3X/e/9/e93ddd9eddbef4632abaec0ff8bdac759271d9a0.png) ### Numerics Subsequently, navigate to **Numerics** and select the solver **MUMPS**. Set the parameter **Stop if singular** to **false**. This is done for the solver to prevent divergence in the initial iterations. ![image](https://www.simscale.com/forum/uploads/default/original/3X/b/1/b1f5a5d11bbd149cb81816d571f91d2eb828f0b6.png) ### Simulation Control Select **Simulation Control** in the **Navigator** and change the settings to those shown in the image below: ![image](https://www.simscale.com/forum/uploads/default/original/3X/c/9/c9617d13333991afab48589762836a67f9166448.png) ### Result Control For an effective analysis of the results, it is imperative to monitor the solution fields with **Result Control Items**. This can be done as follows: ![image](https://www.simscale.com/forum/uploads/default/original/3X/1/5/157090d369f2fda191cb9dd1871c702a9cf9ddb7.png) After assigning an appropriate name, set the **Type** to **minimum and maximum**. Select **Stress** , **von Mises Stress** and **von Mises** as the subsequent settings. Pick the **wheel rim volume** to assign it this **Result Control Item**. ![image](https://www.simscale.com/forum/uploads/default/original/3X/d/a/da4e8a703281de3551ed5ca5aa2ee5f60168b27d.png) To add a new Result Control Item, right click on **Volume Calculation** in the **Navigator** and select **Add Volume Calculation**. ![image](https://www.simscale.com/forum/uploads/default/original/3X/5/c/5cbef160c95dc0222be9fefc145599b6938a9dc1.png) As done earlier, assign an appropriate name and follow the settings as shown in the figure below. ![image](https://www.simscale.com/forum/uploads/default/original/3X/a/0/a00b6b8f032bc06a9be47acf2a7f4ef4430d4c3f.png) ### Initiating the Simulation You’re all set to start the simulation. Create a new run by selecting **Simulation Runs** in the **Navigator** and clicking on **New**. Now, you may **Start** the run. ![image](https://www.simscale.com/forum/uploads/default/original/3X/8/e/8ea2f115c1d36cfc29917d7d53039e8c89b4fbea.png) ![image](https://www.simscale.com/forum/uploads/default/original/3X/e/8/e860116a968559a7823bd2e3c4a789b2818ad0eb.png) _Kindly note: You may receive the following warning when creating a simulation run:_ “Warning: Displacement and force boundary conditions on the following entities. faceGroupOnGeoFaces\_31, faceGroupOnGeoFaces\_26” You may ignore this warning and proceed to the simulation by clicking **OK**. You may **Name** the run as you like and **Start** the simulation. The simulation progress can be tracked in the bottom left of the viewer. ![image](https://www.simscale.com/forum/uploads/default/original/3X/3/7/37f1365570bf3093feaedf8a814f43d54194f40a.png) Post the simulation run, you will be able to see this plot and the total time taken for convergence. In case you wonder why it is taking so long, you may note that the simulation takes approximately an hour to converge. This is due to the mesh refinement. ## 2nd Simulation set up * * * To duplicate your simulation setup, go to your first simulation in the **Navigator** , right click on it, and select **Duplicate**. ![image](https://www.simscale.com/forum/uploads/default/original/3X/2/d/2dc8d0bc233d5b082cf3e1a3966b84ccf33b9f89.png) After assigning an appropriate name to your simulation, click **Save**. ![image](https://www.simscale.com/forum/uploads/default/original/3X/3/6/36afb673c5d057ec03915a071c57d7fd92cf09d2.png) Again, change the rendering mode to **surfaces** for better visualization. ![image](https://www.simscale.com/forum/uploads/default/original/3X/f/f/ffe8490633b80319bd138be75d40addac2cdb2cb.png) The 2nd simulation is similar to the 1st simulation except in a few regards. In this simulation, all the materials are treated as **Linear elastic**. You can follow the changes shown in the image shown below to set up your second simulation. Under **Materials** , change the **Material behavior** of **PP-Polypropylene** to **Linear elastic**. Also, make sure the **Young’s modulus** is set correctly. ![image](https://www.simscale.com/forum/uploads/default/original/3X/2/4/2458660b3b61b552540b534345767a660c70bc88.png) Next, change the **Material behavior** of **Rubber** to **linear elastic**. ![image](https://www.simscale.com/forum/uploads/default/original/3X/5/c/5c1f52e83b47afec073a4299e2b5d1635f8882c0.png) Maintain the behavior of **Concrete** as set in the previous simulation (linear elastic). ![image](https://www.simscale.com/forum/uploads/default/original/3X/b/2/b202b5d176cfe096f5741e3472be6c3fcd7bebee.png) Create **New** Simulation, name it, and **Start**. ![image](https://www.simscale.com/forum/uploads/default/original/3X/e/8/e886e55cc6e390a608a759fbd5c42f5ffada78a6.png)   ![image](https://www.simscale.com/forum/uploads/default/original/3X/b/7/b70ad346ba5f8f957e33b007e069196f4ff34038.png) The simulation progress can be tracked as shown in the figure below. ![image](https://www.simscale.com/forum/uploads/default/original/3X/8/1/811fda6f45a405af34117219af0f789376ac5d3b.png) After completion of the simulation, the following plot will be displayed onto your screen: ![image](https://www.simscale.com/forum/uploads/default/original/3X/4/b/4b6e5dbea6c3fed6ae51a90cedde474c4abbac68.png) ## Post-Processing * * * To begin with, open the **Post-Processor** in the workflow. You may now see the result in the viewer, by clicking on **Run 1** (or whatever name you had assigned to it) and the selecting **Solution Fields**. In order to identify the regions undergoing high strain, the displacement may be visualized. Also, it would be a good idea to rescale the custom data range to the values shown in the image below. ![image](https://www.simscale.com/forum/uploads/default/original/3X/d/e/de372938dadd582a6d9cdcfb3de8cb5572a6f391.jpg) Now, add a filter ( **Warp by Vector** ). This will enable you to better visualize the displacement of the wheel under loading. It may be added as follows: ![image](https://www.simscale.com/forum/uploads/default/original/3X/8/4/84290c3d17c94768cc43f8d465bda7e8f6f5a81a.jpg) Click **Apply** to activate the filter. The image below shows the rendered image after the filter is applied. ![image](https://www.simscale.com/forum/uploads/default/original/3X/c/7/c72bb6e916111f7453c907229f1c9d4484a204d9.jpg) Once the filter has been applied, you may reduce the **Opacity of Run from 1 to 0.5**. This will give a clearer representation of the displacement occurring. Change the **Field** to **Solid color** and click **Apply**. ![image](https://www.simscale.com/forum/uploads/default/original/3X/0/4/04b8eeba4ca4ac571d7a7f113b5abc51f9a82ecd.jpg) Next, we can obtain the stress contours by switching back to **WarpByVector1** and the field to **von Mises stress [point-data]**. Moreover, adjust the scale to the one shown in the image below. ![image](https://www.simscale.com/forum/uploads/default/original/3X/a/4/a4e50d359a48ecb5b01e9b9c92460b0a064e00eb.jpg) To graphically represent the variation of von Mises Stress with time, click on **Volume calculation** and then **vonMises stress** under **VonMisesStress\_Rim**. The maximum **Von Mises Stress** can be seen by hovering over the topmost point of the plot. ![image](https://www.simscale.com/forum/uploads/default/original/3X/a/f/afe3ba23db952ae1eb08d4968128b319989db943.png) Similarly, the von Mises Stress for the tyre can be plotted by clicking on **vonMises stress** under the **VonMisesStress\_Tyre** option. ![image](https://www.simscale.com/forum/uploads/default/original/3X/3/d/3d7bafe740f51d58f4448ab831e59e413ea53546.png) The maximum loads acting on the tyre and the rim can be analyzed with the help of respective von Mises Stress Plots. _Kindly Note: The maximum range is scaled down to 18 MPa, which is the yield strength of Polypropylene. This enables us to accurately visualize the regions undergoing plastic deformation._ ---
**Author:** ![anon5983385](https://www.simscale.com/forum/letter_avatar/anon5983385/32/6_22734026db12803ebb3e059622ac3534.png) [@anon5983385](https://www.simscale.com/forum/u/anon5983385)\ **Post date:** [March 28, 2017, 8:26am UTC](https://www.simscale.com/forum/t/fea-master-class-session-2-nonlinear-plasticity-effects-on-wheel-rim/66191/2 "2017-03-28T08:26:49Z")
---
**Author:** ![anon5983385](https://www.simscale.com/forum/letter_avatar/anon5983385/32/6_22734026db12803ebb3e059622ac3534.png) [@anon5983385](https://www.simscale.com/forum/u/anon5983385)\ **Post date:** [March 28, 2017, 12:49pm UTC](https://www.simscale.com/forum/t/fea-master-class-session-2-nonlinear-plasticity-effects-on-wheel-rim/66191/3 "2017-03-28T12:49:04Z")
---
**Author:** ![divtyagi](https://www.simscale.com/forum/letter_avatar/divtyagi/32/6_22734026db12803ebb3e059622ac3534.png) [@divtyagi](https://www.simscale.com/forum/u/divtyagi)\ **Post date:** [March 29, 2017, 8:12pm UTC](https://www.simscale.com/forum/t/fea-master-class-session-2-nonlinear-plasticity-effects-on-wheel-rim/66191/4 "2017-03-29T20:12:22Z")
Hello, I am Divyansh Tyagi. I wanted to discuss on the “shaft constraint”. As of now, I am using fixed value constraint in the bearing housing part as it will prevent the wheel movement in XZ-plane. And again the same constraint on the flat face of the rim as it will constraint the rim movement in Y-direction (probably by the use of a nut). Can any other better constraint be used for this purpose? ---
**Author:** ![ahmedhussain18](https://www.simscale.com/forum/user_avatar/www.simscale.com/ahmedhussain18/32/140_2.png) [@ahmedhussain18](https://www.simscale.com/forum/u/ahmedhussain18)\ **Post date:** [March 29, 2017, 10:08pm UTC](https://www.simscale.com/forum/t/fea-master-class-session-2-nonlinear-plasticity-effects-on-wheel-rim/66191/5 "2017-03-29T22:08:20Z")
Hi @divtyagi! These constraints are already well defined. A small correction: > [@divtyagi](#): > > constraint on the flat face of the rim as it will constraint the rim movement in Y-direction (probably by the use of a nut). The constraint along y-direction on flat rim and tire face is not due to nut. This constraint is used to retain the symmetry along y-axis. Same is done on the orthogonal side along x-axis. Due to the symmetry, only 1/4th of the model is considered. I hope this helps. In case of any question/s, feel free to ask. Best, Ahmed ---
**Author:** ![divtyagi](https://www.simscale.com/forum/letter_avatar/divtyagi/32/6_22734026db12803ebb3e059622ac3534.png) [@divtyagi](https://www.simscale.com/forum/u/divtyagi)\ **Post date:** [March 29, 2017, 11:11pm UTC](https://www.simscale.com/forum/t/fea-master-class-session-2-nonlinear-plasticity-effects-on-wheel-rim/66191/6 "2017-03-29T23:11:51Z")
Hello @ahmedhussain18 Thank you for replying. Yes, I understand that only 1/4th of the model is being used. Actually by flat face I meant the face as shown in the below picture. ![](https://www.simscale.com/forum/uploads/default/original/2X/d/d707029c56420b96f94d1962d69b1f3993ed7731.JPG) I would request you to share the details of the “Shaft Constraint” as it is not given in the above material. Regards. ---
**Author:** ![ahmedhussain18](https://www.simscale.com/forum/user_avatar/www.simscale.com/ahmedhussain18/32/140_2.png) [@ahmedhussain18](https://www.simscale.com/forum/u/ahmedhussain18)\ **Post date:** [March 30, 2017, 7:44am UTC](https://www.simscale.com/forum/t/fea-master-class-session-2-nonlinear-plasticity-effects-on-wheel-rim/66191/7 "2017-03-30T07:44:56Z")
Hi @divtyagi! Ah! sorry I got you wrong there! I think you can try but this constraint will not make a huge difference here as tire is already constrained in y direction on the other side which is not that far away. Seeing the results also show that the displacement of nodes on this face along y-axis is quite negligible. Please see the below image for reference: ![](https://www.simscale.com/forum/uploads/default/original/2X/a/a603cf6b24b06bd89a838433e629bac0400569cd.png) Best, Ahmed ---
**Author:** ![divtyagi](https://www.simscale.com/forum/letter_avatar/divtyagi/32/6_22734026db12803ebb3e059622ac3534.png) [@divtyagi](https://www.simscale.com/forum/u/divtyagi)\ **Post date:** [March 30, 2017, 1:14pm UTC](https://www.simscale.com/forum/t/fea-master-class-session-2-nonlinear-plasticity-effects-on-wheel-rim/66191/8 "2017-03-30T13:14:06Z")
Hi @ahmedhussain18 ! Thank you for the reply. I got it what you are trying to say. My question is: How should I model the “Shaft Constraint”? As it is mentioned in the guide that the influence of the shaft and bearing on the wheel is modeled with this constraint. But the details of it aren’t provided. Kindly provide the details of this constraint. I guess it’s a necessary input cause my solver is failing to generate results if I try running simulation without it. Regards. ---
**Author:** ![anon5983385](https://www.simscale.com/forum/letter_avatar/anon5983385/32/6_22734026db12803ebb3e059622ac3534.png) [@anon5983385](https://www.simscale.com/forum/u/anon5983385)\ **Post date:** [March 31, 2017, 10:19am UTC](https://www.simscale.com/forum/t/fea-master-class-session-2-nonlinear-plasticity-effects-on-wheel-rim/66191/9 "2017-03-31T10:19:17Z")
Hi @divtyagi! Got it! I saw your point here. The image for the shaft constraint is missing. I will add it in a while. Best, Krishna ---
**Author:** ![anon5983385](https://www.simscale.com/forum/letter_avatar/anon5983385/32/6_22734026db12803ebb3e059622ac3534.png) [@anon5983385](https://www.simscale.com/forum/u/anon5983385)\ **Post date:** [March 31, 2017, 11:53am UTC](https://www.simscale.com/forum/t/fea-master-class-session-2-nonlinear-plasticity-effects-on-wheel-rim/66191/10 "2017-03-31T11:53:38Z")
Hi @divtyagi, The tutorial has now been updated with the picture for shaft constraint. Best, Krishna ---
**Author:** ![divtyagi](https://www.simscale.com/forum/letter_avatar/divtyagi/32/6_22734026db12803ebb3e059622ac3534.png) [@divtyagi](https://www.simscale.com/forum/u/divtyagi)\ **Post date:** [March 31, 2017, 12:49pm UTC](https://www.simscale.com/forum/t/fea-master-class-session-2-nonlinear-plasticity-effects-on-wheel-rim/66191/11 "2017-03-31T12:49:32Z")
Hi @anon5983385, I think there is a mistake cause the “Elastic Support constraint” photo has been repeated twice instead of the “Shaft Constraint” photo. Kindly check. Regards. Divyansh ---
**Author:** ![anon5983385](https://www.simscale.com/forum/letter_avatar/anon5983385/32/6_22734026db12803ebb3e059622ac3534.png) [@anon5983385](https://www.simscale.com/forum/u/anon5983385)\ **Post date:** [March 31, 2017, 1:30pm UTC](https://www.simscale.com/forum/t/fea-master-class-session-2-nonlinear-plasticity-effects-on-wheel-rim/66191/12 "2017-03-31T13:30:55Z")
Yes, you are right. It has been updated now. PS: I definitely need to get some more coffee 😄 Best, Krishna ---
**Author:** ![jousefm](https://www.simscale.com/forum/user_avatar/www.simscale.com/jousefm/32/34908_2.png) [@jousefm](https://www.simscale.com/forum/u/jousefm)\ **Post date:** [April 1, 2017, 5:34pm UTC](https://www.simscale.com/forum/t/fea-master-class-session-2-nonlinear-plasticity-effects-on-wheel-rim/66191/14 "2017-04-01T17:34:38Z")
Dear participants of the FEA Master Class, here you can find the printable PDF version of the Workshop. ### **[PDF Version of the Master Class](https://drive.google.com/open?id=0B6TV-M2capMJYWE2NlR4Smh1RGc)** Feel free to add your comments or send me a private message if you have any problems or wishes for future workshops. Happy SimScaling! ---
**Author:** ![aravindbaskar](https://www.simscale.com/forum/user_avatar/www.simscale.com/aravindbaskar/32/15856_2.png) [@aravindbaskar](https://www.simscale.com/forum/u/aravindbaskar)\ **Post date:** [January 3, 2018, 8:19am UTC](https://www.simscale.com/forum/t/fea-master-class-session-2-nonlinear-plasticity-effects-on-wheel-rim/66191/15 "2018-01-03T08:19:32Z")
Singularity error pops up in the simulation run, I have used the exact setup as in the tutorial. Could anyone tell me if there is some error? Here’s the link - [SimScale](https://www.simscale.com/projects/aravindbaskar/wheelfea_handout_1/) ---
**Author:** ![jousefm](https://www.simscale.com/forum/user_avatar/www.simscale.com/jousefm/32/34908_2.png) [@jousefm](https://www.simscale.com/forum/u/jousefm)\ **Post date:** [January 3, 2018, 9:08am UTC](https://www.simscale.com/forum/t/fea-master-class-session-2-nonlinear-plasticity-effects-on-wheel-rim/66191/16 "2018-01-03T09:08:33Z")
Hi @aravindbaskar! I can see that every run that you submitted finished with 100% and no errors occurred. Can you tell me which project you are speaking about? The name of the simulation would also be good to know to directly find the culprit 😉 Cheers! Jousef ---
**Author:** ![aravindbaskar](https://www.simscale.com/forum/user_avatar/www.simscale.com/aravindbaskar/32/15856_2.png) [@aravindbaskar](https://www.simscale.com/forum/u/aravindbaskar)\ **Post date:** [January 3, 2018, 9:25am UTC](https://www.simscale.com/forum/t/fea-master-class-session-2-nonlinear-plasticity-effects-on-wheel-rim/66191/17 "2018-01-03T09:25:35Z")
The project name is non linear analysis of wheel 😃 ---
**Author:** ![jousefm](https://www.simscale.com/forum/user_avatar/www.simscale.com/jousefm/32/34908_2.png) [@jousefm](https://www.simscale.com/forum/u/jousefm)\ **Post date:** [January 5, 2018, 12:13pm UTC](https://www.simscale.com/forum/t/fea-master-class-session-2-nonlinear-plasticity-effects-on-wheel-rim/66191/18 "2018-01-05T12:13:28Z")
Please pardon the delayed response @aravindbaskar! I have shared my project with you. You will see that I simply changed the **two symmetry** boundary conditions to **fixed value** boundary conditions with two unconstrained directions respectively. Tell me if you want to know anything else and if you are happy with the results! Happy SimScaling! Jousef ---
**Author:** ![aravindbaskar](https://www.simscale.com/forum/user_avatar/www.simscale.com/aravindbaskar/32/15856_2.png) [@aravindbaskar](https://www.simscale.com/forum/u/aravindbaskar)\ **Post date:** [January 8, 2018, 3:40am UTC](https://www.simscale.com/forum/t/fea-master-class-session-2-nonlinear-plasticity-effects-on-wheel-rim/66191/19 "2018-01-08T03:40:40Z")
@jousefm Thanks, it worked, but I would like to know the need to use fixed value instead of symmetry. From the help text, it says only for face that are orthogonal w.r.t to global coordinates axis, we need to use fixed value condition. ---
**Author:** ![jousefm](https://www.simscale.com/forum/user_avatar/www.simscale.com/jousefm/32/34908_2.png) [@jousefm](https://www.simscale.com/forum/u/jousefm)\ **Post date:** [January 8, 2018, 2:00pm UTC](https://www.simscale.com/forum/t/fea-master-class-session-2-nonlinear-plasticity-effects-on-wheel-rim/66191/20 "2018-01-08T14:00:48Z")
Hi @aravindbaskar and sorry for the delayed reponse - university started today 😉 That is a very interesting question indeed! @rszoeke gave a good answer on that topic: “Generally you should try to replace a symmetry constraint with the equivalent **fixed value** constraint whenever possible. The reason is that a symmetry constraint always creates a linear relation between the DOFs of the nodes involved: \vec n \cdot \vec u = 0, where \vec n is the element normal and \vec u the displacement vector. If now any DOF that is not **exactly** (and in numerical analysis usually nothing is exact) normal to the symmetry plane is constrained by another boundary condition or contact, the DOF will be over-constrained. By using a fixed value constraint and defining the mentioned DOF as **unconstrained** you won’t have a problem. Obviously this technique will not work if the symmetry plane is not orthogonal to any of the coordinate axes.” (**[Related post](https://www.simscale.com/forum/t/pin-the-problem-with-contacts/37071/6)**) Hope that clears things up a bit! All the best! Jousef ---
**Author:** ![aravindbaskar](https://www.simscale.com/forum/user_avatar/www.simscale.com/aravindbaskar/32/15856_2.png) [@aravindbaskar](https://www.simscale.com/forum/u/aravindbaskar)\ **Post date:** [January 10, 2018, 10:27am UTC](https://www.simscale.com/forum/t/fea-master-class-session-2-nonlinear-plasticity-effects-on-wheel-rim/66191/21 "2018-01-10T10:27:17Z")
Thanks @jousefm