ABAQUS/CAE Workshops

Transcription

1 ABAQUS/CAE Workshops University of Birmingham ABAQUS Training 27 th / 28 th October 2009 Workshop 1a: Create 3D Part Type: abaqus cae at the command prompt or select abaqus V6.9-1 from the start menu. Select: create model database or select file new. Select: Part (from top menu) Create, name Part, i.e. beam_3d Select: 3D Deformable Solid Extrusion, approx size = 300, click Continue. Within Sketcher: Create rectangle (e.g. 50mm x 20mm), using either the connected line or the rectangle icon option*. Add dimension (click icon*) select line, press return. Edit dimension (icon), if necessary, select Done. Give a depth of 300mm, click ok. * Tip: move your mouse over an icon to reveal its function! You should now have a grey Part! Save your model: File Save. Part manipulation: Select: View Toolbars Views. Also, you can rotate and translate and auto-fit a Part using icons from the icon top menu. Modify 3D Part Select: Feature Edit (from top menu), click on your Part (should turn red), select Edit Sketch. In sketcher, select Edit Dimension icon, select your dimension and modify, select Done. Use: Feature Edit to return your Part to the original dimensions. Rename Model to Beam_3D. Use: Model Rename. Save your Model. Workshop 1b: Createnew Models with diferent sections: Select Model Create, give name = Cylinder Create Part = Circle Create a solid cylinder in Sketcher, diameter = 25mm, Length = 500mm 1

2 Select Model Create, give name = Hexagon Create Part = Hexagon Create a solid Hexagon 250mm long with 10mm equal sides using the connected line option in Sketcher. Tip: use dimensions to modify side length. Workshop 2: Creating and Applying Properties Select: Property from the Module drop down menu. Select: Material (from top menu) Create, give name, i.e. Steel Select: Mechanical Elasticity Elastic Young s Modulus = , Poisons ratio = 0.3, click ok. Select: Section (from top menu) Create, give name, i.e. Beam. Select: Solid Homogeneous, click continue, click ok. Select: A sign Section, click on Part, click done, (Section = beam ), click ok. Part should now turn green! Workshop 3: Creating an Assembly Select: A sembly from the Module drop down menu. Select: Instance Create, select Part, toggle Independent, click ok. You should now have a blue asembled Instance. Create and position another Instance Select: A sembly from the Module drop down menu. Select: Instance Create, selectpart, toggle Independent and tick auto-ofset, click ok. Select: Instance Translate, select Instance in viewport, click ok. Select a start point pick any point on the instance. Select an end point pick any point on the instance, click ok. Try different positions/methods! Delete second Instance. N.B. If you want to delete an Instance, select Feature Delete. 2

3 Workshop 4: Defining Steps and Applying Loads & Boundary Conditions Create Step Select: Step from the Module drop down menu. Select: Step Create, give name, i.e. First, select: Static, General, click Continue. Write brief description in box, Time period = 1, Nlgeom = off, click ok. Create Load Select: Load from the Module drop down menu. Select: Load Create, give name, i.e., vert_load, Step = first Category = Mechanical Type = Concentrated force, click Continue. Select the two top face corner points (use shift key and hold), click Done. Insert numeric values in boxes as: CF1: = 0, CF2: = -200, CF3: = 0, click ok. Create BC s Select: BC Create, give name: encastre, Step = first Category = Mechanical Type = Symmetry/Antisymmetry/Encastre, click Continue. Rotate Instance and select the back face, click Done. Toggle: ENCASTRE, click ok. Workshop 5a: Meshing Select: Mesh from the Module drop down menu. Model should now be green! Select: Seed Instance, approximate size = 20, click ok, click done. Seeding ok? Select: Seed Instance, approximate size = 5, click ok, click done. Select: Mesh Instance, click Yes. You should now have a nice uniform mesh. Select: Mesh Verify, click on Instance, click Done, Select Highlight. How many elements are there? Points for Author: Rework some workshops including lug and partitioning etc. Repeat through Workshops: 2-5 but using Models; Circle and Hexagon. Workshop 5b: Partitioning Additional Workshop: Lug Analysis 3

4 Type: abaqus cae at the command prompt or select abaqus from the start menu. Select: create model database or select file, new. Select: Part create, name part: lug_3d Select: 3D, deformable, solid, extrusion, approx. size = 200, click ok. Create profile (as shown in Fig.1), using the connected line option and the semi-circle option. Add dimensions, modify dimensions, if necessary, select done. Give depth of 50mm, click ok. You should now have a grey Part - Lug! Save your model 50mm 20mm Swept meshing technique = yellow Figure 1. 3D Lug. Partition Lug in the Mesh module until Lug turns completely green. Workshop 6: Analysis & Results 4

5 Revert back to Model: Beam_3D. Select: Job from the Module drop down menu. Select: Job from the title bar and click Create. Give name: first, select: Continue. Give a brief description of your model, toggle ful analysis, click ok. In the Job Managers box, click ok. Select Monitor for viewing progres. After the job has finished, click on Results. Select: Plot Contours, on deformed shape. Select: Results Field Output select: S33 Select: Results Field Output select: U2. Select: Results Field Output select: Mises Select: Animate Time History. Select: Animate Time History. Go back to Job Module and select Dismis. Go back to Step Module. Change number of increments to 10. Resubmit job and view animation. Go back to Step Module and open Step Manager. Edit Step and toggle Nlgeom to on. Resubmit job and view results. Revert to Model: Circle Change the diameter to 20mm Change the vertical load position to halfway along its length. Change the boundary conditions both ends and fix points in all three directions, i.e. a three point bend. Revert to Model: Hexagon Repeat load and BC s as for Circle Model. Analyse and view results for both Models: Circle and Hexagon. Producing and Saving Tiff files: File Print Save as select Tiff format, give filename. Plotting Select: Tools Path Create give name toggle node list. Part Instance = Beam_3D select nodes (pick add before ), click ok. Select: Tools XY Data create select Path, click continue. Select: Path (name), click plot. Workshop 7: Create Pin 5

6 Revert back to Model: Beam_3D Create a new Part named: Pin. The Pin dimensions are 7.5mm diameter and 75mm long. Create the Pin, and Partition the pin into four quadrants, as learnt in the previous Workshop. Create a Section for the Pin and Assign Steel properties. Workshop 8: Contact Analysis By this stage you should now have two Parts: Beam_3D Pin Create a 7.5mm diameter hole in the beam (as shown in Figure 2). Select: Shape Cut, select top surface and top edge on right side. Create and dimension hole in Sketcher, and click done when finished. Select: through al, click ok. Go to Assembly Module. The next stage is to bring both the beam and pin together in the Assembly Module. Create an Instance of the Pin. Translate and rotate the Pin Instance so that the pin is vertical in the hole and levelled with the bottom face of the beam (as shown in Figure 3.) Select: Tools Surface Create,give name hole, click continue. Pick the internal surfaces of the hole, click done. Select: Tools Surface Create, give name pin, click continue. Pick the external surfaces of the pin, click done. Go to Step Module Create Step Select: Step create, name horiz_force, description time period =10 toggle Nlgeom On, click ok. Go to Interaction Module Select: Interaction Property Create, give name, select: Contact, Select: Mechanical Tangential behaviour, select friction Penalty, give value 0.4, click ok. 6

7 Part Grey Colour 25mm Figure 2. 3D Beam with 7.5mm diameter hole. Figure 3. 3D Beam and Pin. 7

8 Select: Interaction Create, give name, step = horizontal force, type = surface to surface, click continue. Select: external surfaces of pin for master surface, select surface for slave and select hole surfaces. Select: Contact in Edit interaction box, click ok. Go to Load module. Create horizontal load and apply to top geometric point, give value of 500 in dir. 3. Go to Mesh Module Mesh both Parts: Beam and Pin. Go to Job Module Create Job and submit. Bring in results when finished. Used by Tyler Yang (27/28/10/09) Produced by Stephen Blair (22/23/10/07) 8