1 / 33

AE4131 ABAQUS Lecture Part III

AE4131 ABAQUS Lecture Part III. Patrick Roberts gt0398b@prism.gatech.edu x5-2773 Weber 201. Starting ABAQUS CAE. You can start ABAQUS CAE from the start menu or with a command line by typing abaqus cae

andrew
Télécharger la présentation

AE4131 ABAQUS Lecture Part III

An Image/Link below is provided (as is) to download presentation Download Policy: Content on the Website is provided to you AS IS for your information and personal use and may not be sold / licensed / shared on other websites without getting consent from its author. Content is provided to you AS IS for your information and personal use only. Download presentation by click this link. While downloading, if for some reason you are not able to download a presentation, the publisher may have deleted the file from their server. During download, if you can't get a presentation, the file might be deleted by the publisher.

E N D

Presentation Transcript

  1. AE4131ABAQUS LecturePart III Patrick Roberts gt0398b@prism.gatech.edu x5-2773 Weber 201

  2. Starting ABAQUS CAE You can start ABAQUS CAE from the start menu or with a command line by typing abaqus cae TIP: You should start ABAQUS CAE via command line from the directory you want your results files to end up.

  3. 3D problem • To continue learning about ABAQUS CAE we will work through building a 3D cantilevered beam that is subjected to a pressure load on the top of the beam of 0.5 MPa. • We want to view the stresses inside the beam near the root and we want to observe the motion of a point on the free end of the beam during loading. • The length of the beam is 200 mm, height is 20 mm, and width is 25 mm.

  4. Part Module • Create a new part as • 3-D • Type : Deformable • Basic feature: solid • Approximate size: 300 • Extrude: 25

  5. Your 3D part geometry

  6. Property Module • We will add the material of Steel and give it values of 209 × 103 MPa and Poisson's ratio of 0.3. • We will create a section called BeamSection and give it a category of solid, type Homogeneous. • We then assign this material to this section.

  7. Assembly Module • We will create one instance of this beam.

  8. Step Module • We will add a step after the system created Initial step called Load Step. • The procedure type is General and the type is Static. • For the output we want stresses, strains, displacements, forces/reaction. • We also want to select a point at the free end of the beam to observe the motion during loading.

  9. Step Module (cont.) To create a node set and monitor a particular degree of freedom: • Select Tools Set Create • Name the node set Monitor, and click Continue • Select a corner point at the free end of the beam.

  10. Step Module (cont.) 4. From the main menu bar, select Output DOF Monitor. 5. Toggle on Monitor a degree of freedom throughout the analysis (The node set Monitor that you just created is selected in the Point region text field. ) 6. Type 1 in the Degree of freedom text field, and click OK. Note the following key points: • Sets can be defined throughout the modeling process. • The progress of a job can be monitored through a particular degree of freedom.

  11. Step Module (cont.) • Go to: Output > HistoryOutputRequests > Manager > Edit • Domain: Set name: Monitor • Put a check by Displacement/Velocity/ Acceleration, Click OK.

  12. Load Module • We want to fully constrain (encastre) the left end of the beam. Fixed boundary conditions must be placed in the system created Initial step. We will call this boundary condition Fixed. • The pressure load must be added in the step we created earlier called Load Step. Call this load Pressure and it has a value of 0.5 and is applied to the top of the beam.

  13. Beam with BC’s and loading

  14. Mesh Module • First we need to decide on the Mesh controls. In this case we will use quadrilateral. • Next we choose element type. Under Family you will see 3D Stress highlighted. If we choose linear with reduced integration we will be using the following element. • C3D8R: An 8-node linear brick, reduced integration, hourglass control.

  15. Mesh Module (cont.) • We need to define how course/fine the mesh will be by the use of seeds. • The system will suggest a seed value. To make the mesh finer enter a smaller number. Larger numbers will make the mesh more course. • The system suggested 20 so we’ll choose 10.

  16. Mesh Module (cont.)

  17. Job Module • We will create a job called 3DBeam • Once this has been created just submit the job. • The analysis should only take a couple of minutes.

  18. Visualization Module • Once your analysis is complete we want to see the results. • If we look at Von Mises stress distribution we see

  19. Stress distribution

  20. Additional Results To see additional results choose Field Output and you can choose the type of output you would like to see. It will only show you what you initially choose in the Step Module. All of the results files are in the directory you started CAE in. For any errors, warning or other system data on how the analysis ran look at those files.

  21. Viewing stresses in a cross section One of the biggest benefits to finite element methods is the ability to see what is going on inside a structure when loaded. In our case we would like to see what the stresses are like in the elements closest to the root.

  22. Picking the elements for viewing In order to view the interior of a structure you must either • Pick the elements by element number in the Visualizationmodule • Partition off a section of the structure during assembly and place the elements in that section into an element set.

  23. Picking the elements for viewing In our case we will pick the actual elements. In the Visualization module choose Plot Undeformed Shape. In this dialog turn on Element numbering and make it a color you can easily see.

  24. Picking the elements for viewing To pick the elements at the root we need to rotate the structure.

  25. Picking the elements for viewing In this example we want elements 150 through 120. We call this a display group. In the menu bar click on Tools, DisplayGroup, Create. A pop up dialog will be shown You can enter the name of the display group and the elements you want to see.

  26. Picking the elements for viewing In this dialog choose • Item : Elements • Selected Method: Element Labels • Labels Field: Enter the element numbers • Click on the Replace button at the bottom

  27. Picking the elements for viewing

  28. Picking the elements for viewing Now you can reorient this section of the beam and pick the type of stresses you would like to see.

  29. Shear Stress ( ) at the root

  30. Observing the Displacements at the monitored node • Click on Result, History Output… • Click the Variables tab • Choose which degree of freedom you like. We will choose U1, then click the Plot button.

  31. Displacement in the transverse direction

  32. Exporting to external file You may want to export data to an external file to be used in another application like MATLAB. Here’s how.. • You must plot the data like you’ve just seen. • In CAE click on Report, XY… • In the File section of the dialog enter the path and file name and click OK. • You now have an ASCII file of this plotted data.

  33. Online tutorials ABAQUS CAE has three very good tutorials: • Simple 3D cantilever beam • Two hinges/ rigid pin assembly • Viewing and working with your output

More Related