LB01 - Ansys Basics - Axial Bar Example - Workbench Structural Static Ver. 2016 PDF

Preview

Summary

Create a model of a solid, circular steel axial bar with 2 in. diameter and 12 in. length with a concentrated axial tensile load of P = 10,000 lbf (lbf = pound force, not pound mass) at one end, and is fixed to a wall at the other end....

Description

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

Instructions. For each problem described below report your outcomes in writing to the best of your ability. Conceptual mistakes will be of much more importance compared to potential numerical/arithmetic errors. Show, display, argument and elaborate your analysis/design with a great deal of detail. Magic out-of-the-blue numbers not properly supported, justified or documented (e.g. missing diagrams, missing tables, missing numerical derivations) will be penalized. The more documentation the better will be graded. If needed, attach copies of screenshots, graphs, tables, handwritten scripts, handouts or any instrument employed to perform your assignment in order to fully document your work. Submission. Neat, systematic and methodical organization and presentation of the submitted laboratory report is key. Disorganized documents: (1) without proper sequencing, (2) without legible, clean and readable writing, and/or (3) marked with stains, scores, spots, etc., will also be penalized. The Laboratory Report must be delivered on time, no delays nor excuses nor misleads nor deceits of any kind will be accepted unless rightly justified and documented with dependable, trustworthy and official evidence. The delivery format will be digital copies submitted to the corresponding D2L-DropBox allocation before the deadline. Only in the extreme case scenario in which D2L-Dropbox was down and it was unattainable to upload the assignment, send the digital documents before the deadline to [email protected] and cc (carbon copy) to [email protected] emails (the latter is for attestation and verification of electronic submission purposes only) The ANSYS source file with extension .cdb must be submitted along with complementary documentation that support the model. Acceptable formats for submission are .txt, .docx, .jpg, .jpeg, .png, pdf. Note that submissions after the deadline time will not be graded. You are fully responsible for delivering uncorrupted, undebased, debaunched, undamaged and disinfected digital files. If the instructor points out, highlights or bespeaks corruption of submitted documents it will be considered as a late submission and will not be graded anymore. You must provide a clear, concise, and logical sequenced set of pages in ascending order within your submitted complementary single Pdf file (i.e. Page 1, Page 2, Page 3, ..., etc.) along with the source file with extension cdb , just as emulating a hardcopy submission. Insert photos/scans as legible and crisp as possible in that single pdf to be delivered; avoid unreadable shadows, glitters or brightness; employ high contrast and a readable but manageable resolution (avoid extremely big file sizes). Pdf files larger than 5MB per digital copy each one will be penalized. If your writing is in color, insert photos/scans in color, otherwise it will be interpreted as monochromatic. You may use the CamScanner app: iPhone: https://apps.apple.com/us/app/camscanner-pdf-scanner-app/id388627783; Android: https://play.google.com/store/apps/details?id=com.intsig.camscanner&hl=en_US&gl=US) to take photos of your work, build and mount your single PDF file. You may also use online resources such as https://smallpdf.com/edit-pdf or https://www.sejda.com/pdf-editor to edit your photos and/or documents, then build and mount your single Pdf file for delivery. Plagiarism, piracy, forgery or speculation of any kind will be strictly penalized as stated in the Syllabus File Duplication and Academic Dishonesty policies. Submissions will be benchmarked, audited and cross-compared against each other to identify any motive or inducement for plagiarism, sham, imitation, forgery or counterfeit. The instructor encourages the student to consult with him for any doubt, question, inquiry or intrigue around this handout description.

Task LB01-01. Create a model of a solid, circular steel axial bar with 2 in. diameter and 12 in. length with a concentrated axial tensile load of P = 10,000 lbf (lbf = pound force, not pound mass) at one end, and is fixed to a wall

Instructor: Dr. Antonio Velazquez

CIVT-3201K Civil Engineering Materials

1/46

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

at the other end (see figure below).

1. Open ANSYS Workbench. From the program menu list open the ANSYS folder and select Workbench. V iew the Project tab.

Instructor: Dr. Antonio Velazquez

CIVT-3201K Civil Engineering Materials

2/46

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

2. Set Units.

Instructor: Dr. Antonio Velazquez

CIVT-3201K Civil Engineering Materials

3/46

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

Set default units to US Customary to prevent modeling a bar 2 meters in diameter and 12 meters in length instead of a 2 in. diameter and 12 in. length. Click on Units from the Project menu bar. Switch to Display Values in Project Units insteadof as Defined.

3. Launch model. To perform a strength materials analysis add the correct building block from the ones enlisted in the Analysis Systems combo list (left-hand side [LHS] menu). ANSYS can perform advanced types of analyses, including thermal, dynamic, buckling, fluid interaction, etc. Setup Static Structural analysis (i.e., the bar will not move and will have static or pseudo-static unchanging forces applied. Drag the Static Structural object it into the Project Schematic window and drop it it off. This type of analysis will allow to determine the resulting displacements, stresses, strains, and internal forces on a material specimen caused by loads that are assumed to vary slowly (pseudo-static) with respect to time. This is exactly the same type of characterization for Strength of Materials when solving problems by hand using theoretical and/or approximate methods.

Instructor: Dr. Antonio Velazquez

CIVT-3201K Civil Engineering Materials

4/46

LB01 - ANSYS - Axial Bar

Instructor: Dr. Antonio Velazquez

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

CIVT-3201K Civil Engineering Materials

5/46

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

Give the deployment a new descriptive name. Double click on the default name of the block below and chang it to My Axial Bar.

This process defines a specific system block made up of several components called cells. These cells define the sequential steps needed to perform the specific type of analysis. Work through the cells in descending order from top to bottom defining corresponding inputs and parameters. To interact with the cells, you will typically do one of the following: Double-click: Double-click an object to initiate the default action, which may later help you increaseyour speed. Right- click: Right-click to display a context menu applicable to the current state of the selected object. 4. Save model. Before going any further, save current ANSYS workspace and virtual model by selecting File -> Save As from the toolbar. Assign a folder and be sure to save your work from time to time in case anything bad happens. Note that ANSYS does not have an Undo button so having previous saved versions can be useful in helping avoid frustration.

Instructor: Dr. Antonio Velazquez

CIVT-3201K Civil Engineering Materials

6/46

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

5. Create model. Define the Engineering Data and Geometry before accessing the Model cell group, and so on and so forth for the subsequent Setup, Solution and Results cell groups that are to be open in a cascade modality. Define: (a) the material used (steel), (b) the geometry of the bar (length and cross-sectional shape and dimensions), (c) the loading (force magnitude and direction) (d) the boundary conditions (the type and location of support), (e) the type of mesh element and the coarseness of the mesh used to analyze the system (resolution). A coarser mesh provide less accurate results than a more refined mesh, but the coarser mesh will provide quicker results as a tradeoff. (f) the type of static analysis. 5.1. Engineering data. Define the type of material, along with its mechanical properties. The deformation pattern response will depend on the material definitions. To view the default Steel material properties, right-click on the Engineering Data cell and select Edit

Instructor: Dr. Antonio Velazquez

CIVT-3201K Civil Engineering Materials

7/46

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

Set the material properties to reflect a standard A992 Steel material. The primary material property to be defined is the Modulus of Elasticity (Young Modulus) E = 29,000,000 psi [lb/in2] and Poisson s Ratio = 0.3. These two parameters are key to properly define the stress-strain relationship. Define the steel yield strength y = 50,000 psi [lb/in2] (50 ksi) and the steel ultimate strength u = 65,000 psi [lb/in2] (65 ksi). Note that these values are different from the default values provided by ANSYS, so change them accordingly. The A992 steel density A992 = 0.2836 lbm/in3 (lbm = pound mass) is the same as the default ANSYS steel material and is employed when the self-weight of the bar is part of the loading. To change each value, click on each of the cells in the lower left pane and then enter the desired quantity in the corresponding box at the upper right pane.

Instructor: Dr. Antonio Velazquez

CIVT-3201K Civil Engineering Materials

8/46

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

Save your work by pressing the Save button. To return to the Project tab either close the A2: Engineering Data tab or click on the grayed-out Project tab to the left.

5.2 Geometry. Right click on the Geometry cell in the System menu and select New Geometry. This will open the DesignModeler graphical user interface in a new window. This may take a little while depending on the capabilities of the computer.

Instructor: Dr. Antonio Velazquez

CIVT-3201K Civil Engineering Materials

9/46

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

Notice that the LHS menu now presents a Tree Outline. The Tree Outline matches the logical sequence of the geometrical model construction steps. You can right-click on a sub-branch object to open a context menu that relates to that object. You can rename objects prior to and following the solution process.

Instructor: Dr. Antonio Velazquez

CIVT-3201K Civil Engineering Materials

10/46

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

Using the DesignModeler draw the axial bar components using basic CAD drawing tools, then extrude a corresponding 2D cross-section into a 3D element. To do this, follow these steps: Change the Units from the default [meters] to [inch] using the toolbar Units. Notice how by default, the unitson the window scale (lower-right corner) are shown in meters instead of inches.

Click on the YZ Plane leaf which is located in the Tree Outline on the LHS in order to have that yz plane available to draw on with 2D shapes. This will make the X axis the axial (longitudinal) direction axis. Change the selection from the Modeling tab showing the Tree Outline to the Sketching tab that allows drawing. At this point you should see a set of Draw options listed in the LHS menu. The rest of the options included in the Sketching tab are hidden under the Modify, Dimension, Constraints, and Settings items.

Instructor: Dr. Antonio Velazquez

CIVT-3201K Civil Engineering Materials

11/46

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

Using the Draw options draw the bar circular cross-section. Click on the Circle draw command in the LHS Draw menu.

Using the mouse, hover over the axis origin and click to draw a circle shape. Drag themouse outward to create a circle in the XY plane. You do not need to worry at this point about the correct diameter dimension.

Once the circle is drawn input now the correct the diameter dimension by changing to the

Instructor: Dr. Antonio Velazquez

CIVT-3201K Civil Engineering Materials

12/46

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

Dimensions menu from the Draw menu on the LHS and clicking on the Diameter option.

Click anywhere on your circle to define the D1 parameter location. When you do this an arrow defining the diameter will appear on your sketch with the label D1. In the text box that appears on the LHS, type 2 inside the D1 box and hit Enter to define the circle s actual diameter of 2 inches. Note that the circle dimension changes in the sketch to reflect this new value.

Use the zoom ribbon tool to modify the view scale of the drawing.

Instructor: Dr. Antonio Velazquez

CIVT-3201K Civil Engineering Materials

13/46

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

Now select the function Extrude from the top tool bar. You will see a wireframe extrusion of the 2D cross- section into 3D in the x-axis direction inside the Sketch.

Instructor: Dr. Antonio Velazquez

CIVT-3201K Civil Engineering Materials

14/46

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

Change the FD1 value in LHS menu that appears showing the details of the Extrude1 to 12 inches. Click then on the G eom et ry property enlisted above, then Apply. This will create a solid circular bar with this exact extrusion length.

Now as a final to create the 3D bar element click on the Generate option on the toolbar above

Instructor: Dr. Antonio Velazquez

CIVT-3201K Civil Engineering Materials

15/46

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

(it has the lightning bolt next to it). You should now have a 3D cylindrical bar. Use the zoom features again to adjust the scale view.

Note that you will find that you have been thrown out of the Sketching tab and back into the Modeling tab. This is fine. Rename some of the sketches and parts of the model. Click on the + signs in the LHS tree menu to expand each option.

Right-click on each label and rename the Sketch1 as CircularBarCrossSection and the extruded body part created as AxialBar. For simple models this is not perhaps very useful; but with more complex models it helps with searching to find a specific object. Don t forget to save your work!

Instructor: Dr. Antonio Velazquez

CIVT-3201K Civil Engineering Materials

16/46

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

Go back to the Workbench graphical user interface. You should now see a green checkmark next to the Geometry cell.

Instructor: Dr. Antonio Velazquez

CIVT-3201K Civil Engineering Materials

17/46

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

Right-click on the Model cell and select Edit to work with. A new instance will open that is tagged with a red ball and giant M icon that stands for Mechanical. This Mechanical interface allow to work on the meshing of the axial bar. A mesh is needed to run a Finite Element Analysis (FEA). Finite element analysis (FEA) is a computerized method for predicting how a product reacts to real-world forces, vibration, heat, fluid flow, and other physical effects. Finite element analysis shows whether a product will break, wear out, or work the way it was designed. A Finite Element is a small mechanistic element that simulates a material particle or group of particles. Hundreds or thousands of these particles will conform the material under study. The mesh is a type of jacket or envelope that contains thos hundreds/thousands of little mechanistic particles to simulate the actual material.

Instructor: Dr. Antonio Velazquez

CIVT-3201K Civil Engineering Materials

18/46

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

Refer to the Tree Outline from the Mechanical graphical user interface. You should see a Mesh leaf. Right-click on Mesh then select Generate Mesh.

Instructor: Dr. Antonio Velazquez

CIVT-3201K Civil Engineering Materials

19/46

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

For now we will use the default mesh configuration. A different output model is obtained when changing the type of finie element (bar element, triangular element, trapezoidal element) or the size of the finite elements employed to characterize the material. Once the mesh is generated it will appear on the 3D bar as shown above. Explore the different properties of the mesh adopted in the Details of Mesh combo list. The default ANSYS element type is officially a 3D quadratic tetrahedron (solid) element.

Note*: If you want to rotate the axial bar in space use any of the view/zoom buttons in the toolbar.

Instructor: Dr. Antonio Velazquez

CIVT-3201K Civil Engineering Materials

20/46

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

Under the Sizing Menu Item on the LHS change the Sizing -> Relevance Center from Coarse (rude, rough) to Medium (mid polished, mid neat) mesh resolution. Right-click on the Mesh leaf and click Update to verify that the mesh generated become more refined (more purified, more gracious), i.e., more finite elements are implemented. Typically, the Medium mesh give better results (more accuracy) than the Coarse mesh, although it may take more time to do so. Try assigning a Fine mesh and see the outcome.

Instructor: Dr. Antonio Velazquez

CIVT-3201K Civil Engineering Materials

21/46

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

Leave the model with the Medium mesh. Save your work! Go back to the ANSYS Workbench and verify a green check mark next to the Model cell.

Instructor: Dr. Antonio Velazquez

CIVT-3201K Civil Engineering Materials

22/46

LB01 - ANSYS - Axial Bar

Fall 2021

Deadline: Monday, September 20th, 2021, 10:00A.M.

Go back to the Mechanical window view. You can visually identify model parts based on a property of that part. For example, if an assembly is made of parts of d...