# Step by Step Tutorial : Rubber Seal Sliding Analysis **URL:** \ **Category:** Solid Mechanics / FEA\ **Created:** [July 19, 2016, 2:30pm UTC](https://www.simscale.com/forum/t/step-by-step-tutorial-rubber-seal-sliding-analysis/33433 "2016-07-19T14:30:37Z")\ **Posts on this page:** 5\ **Page:** 1
**Author:** ![anon89049096](https://www.simscale.com/forum/letter_avatar/anon89049096/32/5_5575768a8748004e209b776fc1b2916d.png) [@anon89049096](https://www.simscale.com/forum/u/anon89049096)\ **Post date:** [July 19, 2016, 2:30pm UTC](https://www.simscale.com/forum/t/step-by-step-tutorial-rubber-seal-sliding-analysis/33433/1 "2016-07-19T14:30:37Z")
Our aim is to analyse the sliding of a rubber seal on a rigid body due to applied displacement. In this project rubber seal will be given a displacement of approximately 1 cm which slides on a rigid body. Only 1 degree sector of geometry is being considered due to circular symmetry. ## Step-by-Step Import the project by clicking the link below. (Crtl + Click to open in a new tab). [https://www.simscale.com/workbench?publiclink=e1502214-5500-42a1-8c82-12e3fc217bf2](https://www.simscale.com/workbench?publiclink=e1502214-5500-42a1-8c82-12e3fc217bf2) Once the project is imported, the workbench is automatically opened. Then follow the steps below for setting up the simulation. ### Meshing - In the **Mesh Creator** tab, click on the geometry **Seal\_geometry\_1Deg**. - Then, click on **New Mesh** button in the options panel. ![](https://www.simscale.com/forum/uploads/default/original/2X/2/2833e882fa2bc988c110b7f8650b6066fe988557.jpg) - Select **Tet-dominant** [1] for the mesh and use the following parameters [2] - **0.0006** and **0.0003** as maximum and minimum mesh edge length respectively, **First order** for the desired mesh order, **3-Moderate** fineness and **4** computing cores. - **Save** [3] the settings. ![](https://www.simscale.com/forum/uploads/default/original/2X/4/47924a15f00f5d8b22606c92fc137c30237de265.jpg) - To add a mesh refinement, click on **New** button in the bottom. This is done to locally refine small geometric features. In this geometry, some fillets are grouped into a topological set called **outer\_rounds** , which needs to be refined. ![](https://www.simscale.com/forum/uploads/default/original/2X/5/5195d1fd7151a5ddb36bda1d58fdf7c8ebb81db7.jpg) - Use the parameters given in the figure below for local refinement at the fillets. Select **face sets** in the ‘Topolgical Mapping’, click on the **outer\_rounds** and then **Save** the settings. ![](https://www.simscale.com/forum/uploads/default/original/2X/5/52cad30e63c0ffaac22971acc6a034917a255e5b.jpg) - Go back to **Operation 1** and then click on **Start** button to start the meshing operation. The meshing job will start in a few moments and all computation is done via cloud computing. ![](https://www.simscale.com/forum/uploads/default/original/2X/9/9748408d64fe3f0bd94ad0523bde2b9605f264e0.jpg) - The mesh operation takes about 1 min to complete and gives a **Finished** status in the lower left corner once it is over. The meshed geometry can be seen in the viewer. ![](https://www.simscale.com/forum/uploads/default/original/2X/d/d88467e5417aa790255e944b2ac225596042660a.jpg) ### Simulation Setup - For setting up the simulation, switch to the **Simulation Designer** tab [1] and select **New simulation** [2]. - A create new project window will pop-up. Give a suitable project name (optional) e.g. **Seal simulation** in this case and click **Create** [3]. ![](https://www.simscale.com/forum/uploads/default/original/2X/6/636b44be27670ab0d87e096fe686b5ec026b3e35.png) - Since our simulation involves physical contact, select the analysis type **Static analysis - advanced** under **Code\_Aster** ( **Solver Perspective** ), change Nonlinear analysis to **true** and click **Save**. ![](https://www.simscale.com/forum/uploads/default/original/2X/f/fb689e1a7c79277c6a91b1b23bea12e670600f47.png) - After saving, the simulation tree now looks as shown below. Here the tree entries in red must be completed. ![](https://www.simscale.com/forum/uploads/default/original/2X/f/f2e7414dad1a18c339c15a5070b46a0e80e0d3e4.png) #### Domain selection - Click on **Domain** from the tree and select the mesh created from the previous task. Click on the **Save** button. The mesh will be automatically loaded in the viewer. - Furthermore, change render mode to **Surfaces** for a cleaner view. ![](https://www.simscale.com/forum/uploads/default/original/2X/9/99a3e026c7d0cda7c25549f0af20412b326cac7b.png) #### Create Topological Entity Sets - In this tutorial, we need 4 topology entity sets for specifying the boundary conditions and physical contacts. ![](https://www.simscale.com/forum/uploads/default/original/2X/f/f21f738b404df69ce314ec4b0f42d2311553b6c6.png) - Click on the tree entry **Topological Entity Sets**. ##### **Symmetry BC set:** - To create the first set, select the shown surface and click on the **New from selection** button to create a set named **Symmetry BC set**. ![](https://www.simscale.com/forum/uploads/default/original/2X/b/b50014f06c60dcaca1fd1faaa483b6669f0b2b1f.png) ##### **Rigid-seal contact:** - Follow the same step as above for creating the second topological set with a different set of faces as shown in the figure below. Here, we are making a set of faces from the rigid body which is in contact with the seal. For showing all the faces of this topological set, the seal body is hidden in the figure below. ![](https://www.simscale.com/forum/uploads/default/original/2X/b/bce7436f5d5ddc7ed860a01f3b5316567a1f5178.png) ##### **Seal displacement BC set:** - Follow the same step as above for creating the third topological set with a different set of faces as shown in the figure below. Here, we are making a set of faces from the seal body where displacement will be applied. ![](https://www.simscale.com/forum/uploads/default/original/2X/9/9f4a7006593766d831679f02e69b60147e67f7ae.png) ##### **Seal-rigid contact:** - Follow the same step as above for creating the fourth topological set as shown in the figure below. Here, we are making a set of faces from the seal body which is in contact with the rigid body. For showing all the faces of this topological set, the rigid body is hidden in the figure below. ![](https://www.simscale.com/forum/uploads/default/original/2X/5/5908c9038ae9368aa4e506ddff877c805618b79c.png) #### Select Solid Material - Now we will define material for our rigid body (Steel) and seal (Rubber). Select **Material** from the sub-tree and click **New**. - Click on **Import from material library** and select **Steel** and then **Save**. ![](https://www.simscale.com/forum/uploads/default/original/2X/f/f8f75cc8f9e6150ecf5293752e049ef944714f54.png) - Select **volumeOnGeoVolumes1** (rigid body) to add the volume to which steel is assigned and then **Save**. - You can highlight the selected volume by clicking on **Select assignment**. ![](https://www.simscale.com/forum/uploads/default/original/2X/d/dfe9aa49b80ac2705072dd4193179ae919dab33c.png) - Similarly add rubber material for the seal following same steps as above. ![](https://www.simscale.com/forum/uploads/default/original/2X/1/1081c6209bc2e5d01c5835827b0fbced422380ff.png) ![](https://www.simscale.com/forum/uploads/default/original/2X/5/581fad6d61cdc7ea8d855679413988c17b12752f.png) - Select **Hyperelastic** for ‘Material behaviour’ and in the ‘Hyperelastic model’ choose **Signorini**. Use the parameters given in the figure below. - Select **volumeOnGeoVolumes0** (seal) to add the volume to which rubber is assigned and then **Save**. - You can highlight the selected volume by clicking on **Select assignment**. ![](https://www.simscale.com/forum/uploads/default/original/2X/7/701470ce2d43e643f507bdb5f62a9c0abda81209.png) #### Physical Contacts In this section we will define the physical contact between the seal and the rigid body. We are using penalty method for modelling the contact. - Select **Physical Contacts** and then click on **New**. The Penalty method is available as default and don’t change any options here. ![](https://www.simscale.com/forum/uploads/default/original/2X/c/c293603dc261307be2108fd2fc927992cfd6fce1.png) - Change the ‘Name’ to **Seat with rigid contact** (optional) and give a very high value of ‘Penalty factor’ ( **1e13** ). - Here, we are not considering friction at the contact, therefore choose **Frictionless penalty contact** as ‘Type’. - Select **Rigid-seat contact** as a ‘Master entity’ and **Seal-rigid contact** as ‘Slave entity’ and then click **Save**. ![](https://www.simscale.com/forum/uploads/default/original/2X/9/9ef9d10128d31ee4bf7932eee4a93a7edd97c07c.png) #### Boundary Conditions In this section we will define the fixation of the rigid body, symmetry boundary conditions for seal along the circumferential direction for modelling axisymmetry and displacement of the seal body. - Let’s first define fixation. Select **Constraint** in the tree and click **New**. ![](https://www.simscale.com/forum/uploads/default/original/2X/a/a8b56a36b46223f9e021930c6aedf8f3f2920c8c.png) - Rename the Boundary condition to **Fixation** (optional). Choose the ‘Type’ **Fixed value**. Under **Topological Mapping** , change ‘Filter for entity types’ to **volumes** and select **volumeOnGeoVolumes1** (rigid body). Then click **Save**. ![](https://www.simscale.com/forum/uploads/default/original/2X/4/41988cb960e2d636a17970850a0e0c1d979f61f2.png) - For defining the symmetry boundary conditions, select **Constraint** in the tree and click **New**. ![](https://www.simscale.com/forum/uploads/default/original/2X/3/3b587919833123512109393458497e168ee39267.png) - Rename the Boundary condition to **Symmetry** (optional). Choose the ‘Type’ **Symmetry plane**. Under **Topological Mapping** , change ‘Filter for entity types’ to **face sets** and select **Symmetry BC set**. Then click ‘ **Save** ’. ![](https://www.simscale.com/forum/uploads/default/original/2X/a/afdf33808abf52b340c7d8556606264b863f9484.png) - For defining the seal displacement, select **Constraint** in the tree and click **New**. ![](https://www.simscale.com/forum/uploads/default/original/2X/2/288e1aa2b78d8e6d8668e86a5e74843721da5b4a.png) - Rename the Boundary condition to **Seal displacement** (optional). Choose the ‘Type’ **Fixed**. Choose **unconstrained** for x and y displacement and for the z displacement, specify it as a function by clicking on ‘function button’ and give **0.011\*t** in the ‘Formula’. - Under **Topological Mapping** , change ‘Filter for entity types’ to **face sets** and select **Seal displacement BC set**. Then click **Save**. ![](https://www.simscale.com/forum/uploads/default/original/2X/3/3da09bdbb5d63f5f6ae7b045bb10064a0131dc30.png) #### Simulation Control - Click on **Simulation control** and change ‘Initial time step length [s]’ to **0.05** under details of ‘Timestep definition’, ‘Number of computing cores’ to **4** , under details ‘Number of cores used for the computation’ to **4** and **Maximum runtime [s]** to **3600**. ![](https://www.simscale.com/forum/uploads/default/original/2X/c/c429a0ede44e98acfcc632d28ef790cb27c2e9e5.png) - Click on **Simulation runs** and create a new run. ![](https://www.simscale.com/forum/uploads/default/original/2X/4/42659e8575b0ec21122e7fca084db1da7820df5f.png) ![](https://www.simscale.com/forum/uploads/default/original/2X/5/5d5e3a0b23cb195f7e9cb1ac43d3555cb2981a61.png) - The new run will be created under **Simulation Runs**. Click **Start** to run the simulation. ![](https://www.simscale.com/forum/uploads/default/original/2X/f/f0bed25298747968be09f4e4546114356409829f.png) - The run takes approximately 4min. After the run is finished you can see the ‘Status’ as **Finshed** and the convergence plot can be seen by selecting **Convergence plots**. ![](https://www.simscale.com/forum/uploads/default/original/2X/4/4dd8d087fb2d6b727ab75cebbfe0adcf3471c780.png) ### Post-processing - Once the simulation is over, click on **Post-processor** tab to view the results and select **Solution fields**. ![](https://www.simscale.com/forum/uploads/default/original/2X/8/8f923487a3a8c4fb05ef542903592c34b69f4065.png) - In order to see the deformed shape of the rubber seal, click on **Add Filter** and then **Warp by Vector**. ![](https://www.simscale.com/forum/uploads/default/original/2X/3/3afcf6d6ceeceefc0c6bbe444eb8717e4b836b21.png) - Give a suitable ‘Scale Factor’ for scaling the deformation (say **0.005** ). Click on tick mark to apply the changes. You will see both deformed and undeformed geometry. In order to hide the undeformed geometry, click on the ‘Eye button’ at the left of **Run 1**. ![](https://www.simscale.com/forum/uploads/default/original/2X/5/59c04b75f1d66426e3e440d7a10d2405b6533ec4.png) - The result you see in the viewer window is only a 1 deg sector of the whole circular symmetric body. Since the problem is circular symmetric, the stress and deformation result will be also symmetric. - Hence, the result of the complete body can obtained by revolving the result along the axis. This can be done by clicking on **Add Filter** and then **Transform**. ![](https://www.simscale.com/forum/uploads/default/original/2X/4/40f941b8fadbaab47723cade414dd05a07ddc818.png) - Since the axis of symmetry is z axis and the sector is of 1 deg, give the value **1** for the ‘Rotate’ under 3rd column. Click on the tick mark to reflect the changes. This operation will create a copy of the result moved by 1 deg. ![](https://www.simscale.com/forum/uploads/default/original/2X/a/ac7ce8ebe89a9fc74467e1e407dcd31947c37572.png) - Repeat the same step 24 times to visualise the result for a 25 deg sector. The figure below shows von Mises stress of the seal. ![](https://www.simscale.com/forum/uploads/default/original/2X/d/da6df36d03897cfc6902f16f8358d1384aa09629.png) - You can also view total non linear strain of the body by selecting **total\_non\_linear\_strain** for all the filters. ![](https://www.simscale.com/forum/uploads/default/original/2X/f/f49d6a25e06efdc49786b26227d219cafaeadf65.png) - This can be done more elegantly in Paraview. Following link provides details on postprocessing in Paraview. [https://www.simscale.com/docs/content/postprocessing/local-postprocessing.html#post-processing-via-3rd-party-solution](https://www.simscale.com/docs/content/postprocessing/local-postprocessing.html#post-processing-via-3rd-party-solution) ---
**Author:** ![anon18194957](https://www.simscale.com/forum/letter_avatar/anon18194957/32/5_5575768a8748004e209b776fc1b2916d.png) [@anon18194957](https://www.simscale.com/forum/u/anon18194957)\ **Post date:** [August 2, 2016, 5:46pm UTC](https://www.simscale.com/forum/t/step-by-step-tutorial-rubber-seal-sliding-analysis/33433/5 "2016-08-02T17:46:23Z")
Great tutorial @anon89049096, thanks for sharing! ---
**Author:** ![JKuyper](https://www.simscale.com/forum/letter_avatar/jkuyper/32/5_5575768a8748004e209b776fc1b2916d.png) [@JKuyper](https://www.simscale.com/forum/u/JKuyper)\ **Post date:** [February 27, 2017, 8:17pm UTC](https://www.simscale.com/forum/t/step-by-step-tutorial-rubber-seal-sliding-analysis/33433/6 "2017-02-27T20:17:10Z")
I just went through the Tutorial. I learned a lot - thanks! I would like to point out, though, that it seems the Meshing interface has changed since you wrote the tutorial. There is no longer “Tetrahedral with local refinement” - I used “Tet-dominant” There are some other changes on that screen as well. Again, I found this tutorial very helpful as I am learning SimScale. Thanks! ---
**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:** [February 27, 2017, 8:55pm UTC](https://www.simscale.com/forum/t/step-by-step-tutorial-rubber-seal-sliding-analysis/33433/7 "2017-02-27T20:55:54Z")
Hi @JKuyper, glad that you liked the tutorial! 🙂 Thanks for the hints! I will put that on my to-do list! Enjoy your stay here! Jousef ---
**Author:** ![gmohedat](https://www.simscale.com/forum/letter_avatar/gmohedat/32/5_5575768a8748004e209b776fc1b2916d.png) [@gmohedat](https://www.simscale.com/forum/u/gmohedat)\ **Post date:** [March 18, 2017, 7:56pm UTC](https://www.simscale.com/forum/t/step-by-step-tutorial-rubber-seal-sliding-analysis/33433/8 "2017-03-18T19:56:42Z")
thank you