ME 6310 Assignments

All Home Work Problems are to be documented using the guidelines given in the 6310 syllabus.

Makeup Work: At least half credit will be deducted for unexcused late (one class meeting) homework.

You can find many useful material properties at www.matweb.com

HW #1 Assigned 1-16-19, Due 1-24-19

a. TUTORIAL ONLY: Work through the problems described in ME 6310 > ANSYS > ANSYS Examples Tutorials 2.A and 2.C. (Link1 still works in ANSYS but only from a txt file input.) Use any FEM software you like. Submit a print of your input text file and the deformed shape graphic.

b. TUTORIAL: Work the problem described in the University of Alberta Tutorial "Basic Tutorials > Two Dimensional Truss". You can solve this with menu picks as in the example or by using the text file provided under 'Command File Mode of Solution'. Submit a print of the deformed shape graphic. Again use any software you'd like. http://www.mece.ualberta.ca/Tutorials/ansys/index.html

In ANSYS Use PlotCtrls > Hard Copy > To Printer to get white background.

HW #2 Assigned 1-27-19, Due 1-31-19

a. ENGINEERING PROBLEM: By hand solve the two-element, 3 global node truss problem below.

Nodes 1 and 2 are connected by element e. Nodes 2 and 3 conected by element f.

1-------e--------2----------------------f-----------------3

If the symbolic representation of the element stiffness matrices is ke = [e -e; -e e] and kf = [f -f; -f f], draw a free body diagram of node 2 and use equilibrium and compatibility to derive the symbolic representation of the Global Stiffness matrix [K] in terms of the constants 'e' and 'f'.

Use steel as the material and let the trusses have a circular cross section. The applied load is P = 1000 times your weight.

The elements have a circular cross section. The length of element 'e' is equal to half the length of your arm; its diameter equal to half the width of your wrist. The length of element 'f' is equal to the length of your arm; its diameter is equal to the width of your wrist.

Problem A - The force P is applied to the right end (node 3) and the left end (node 1) is fixed.

Problem B - The force P is applied to node 2; nodes 1 and 3 are fixed.

Problem C - No force is applied. Nodes 1 and 3 are fixed. Node 2 is displaced an amount equal to the diameter of element 'f'. (For a specificied displacement boundary condition 'Q', set the boundary value to 'Q' instead of setting the boundary displacement to zero.)

In each case find and list the Global Displacements D1, D2, D3; the Global Loads R1, R2, R3; the force, stress and strain in element e and in element f.

Work in any units you choose but present your results in a TABLE in both MKS( meters, N, MPa) & IPS (inches, lbf, psi).

Solve these problems symbolically first giving your results in terms of A1, L1, A2, L2, E, etc. Substitute numerical vlaues for the parameters last.

Verify these results using FEM software.

HW #3 Assigned 2-1-19, Due 2-7-19

a. TUTORIALS Go through mae.uta.edu/~lawrence/ > ANSYS Examples > Tutorials 3.A, 3.B and 3.C. Submit a print of your input text file (if there is one) together with a graphic print (white background) of the final results of the exercise. Note that the stress plots are Element data plots, not Nodal data plots.

b. ENGINEERING PROBLEM A thin rectangular cross section (2.25 inch x 0.4 inch) steel cantilever beam is 15 inches long and has a load of 1000 lbf applied at the free end. The 2.25 inch dimension of the cross section is vetrical so that the bending stiffness is the larger of the two possibilities.

Find:

1. The end deflection and root bending stress using solid mechanics beam theory.

2. The total strain energy of bending and total strain energy of shear. Do this by integrating the expressions for Sigma-x and Tau-xy over the volume of the beam.

3. The end deflection and root bending stress using 2D plane stress elements. We will discuss the appropriate boundary conditions in class.

c. Repeat b. but the beam is only 5 inches long.

HW #4 Assigned 2-9-19, Due 2-14-19

Engineering problem. Document your work accordingly.

Use an FEM program to solve for the maximum stress in an aluminum plate that is 800 mm x 400 mm and 2 mm thick. The plate has a 100 mm diameter hole (50 mm radius) in the center and is loaded on the 400 mm edge by tensile force of 12 kN. Convert the force into an equivalent negative pressure. Take advantage of symmetry and use elements with mid-side nodes. Material properties can be found at www.matweb.com

Compute the maximum stress in the direction of the loading as well as the displacement of the loaded edge. Compare the stress results obtained using a coarse mesh and a fine mesh. Compute only the 'No Average' stresses (in APDL). Also compare the result from the fine mesh to the result you can compute from solid mechanics using the theoretical stress concentration factor.

Tell me a specific aluminum to use so that the plate does not yield at the point of high stress. (Compare max von Mises stress with the material yield point strength Sy.)

HW #5 Assigned 2-20-19, Due 2-28-19 Engr Probs

a. Determine the matrix [B] and the matrix [E] for the three node Constant Strain Triangle element for the case of axisymmetric behavior.

b. Use calculus to find the integral of f(x) = 1 + x^3 over the interval -1 to +1. Also use Gauss quadrature to find an approximation to the same integral. Use 1, 2, and 3 Gauss points and comupte the error in your result when compared to the analytical solution.

I = approx {Sum Wi*f(xi)}; Wi = 2 and xi = 0 for one point; Wi = 1, xi = +/- 0.577... for two points, etc. See Cook page 209 and http://en.wikipedia.org/wiki/Gaussian_quadrature.

c. The stiffness matrix for a three node truss element is [k]= (AE/(6L))[14 -16 2; -16 32 -16; 2 -16 14]. See http://www.solid.iei.liu.se/Education/TMHL08/Lectures/Lecture__8.pdf.

Use Static Condensation to condense the node in the middle (assuming that no force is applied at the middle node), giving a 2 x 2 matrix. Compare this 2 x 2 stiffness matrix with the stiffness matrix for a two node element. (See FEAModelling.pdf slides 11-14)

d. Review the Verification Manual problems in ANSYS Help to get an idea of the large number of test problems available in commercial software. ( ANSYS > Help > ANSYS APDL > Verification Manual ... ). We'll use some of these later.

HW #6 Assigned 3-26-19, Due 4-2-19

a. A circular aluminum plate 0.25 inches thick and 25 inches in diameter is simply supported along its outer edge and loaded with a uniform pressure of 2 psi. Let E = 1e7 psi and nu = 0.3

Use an ANSYS APDL (or other FEM) Axisymmetric model to determine the location and values of the maximum displacement and bending stress in the plate. Compare your results with the theoretical solution for small deformations of thin plates. Thin plate theoretical solutions can be found at:

http://www.roymech.co.uk/Useful_Tables/Mechanics/Plates.html

While MKS units are referenced in the roymech equations, the expressions should be independent of the unit system; check to see.

b. Repeat problem a. using plate (shell) elements with either a quadrant, a half or full model of the plate. Use the 8-node shell element.

HW #7 Assigned 4-8-19, Due 4-16-19

Refer to Blackboard files 'Hardening Spring'.

a. Duplicate the results shown on slides 3,4,5. Instead of using a Newton method as shown, supply a series of horizontal displacements and compute the corresponding force P.

b. Also duplicate the results shown on slides 7-8 (Eignevalue buckling load estimate 135 N).

c. Duplicate the forced displacement results shown on slides 9-11. (Point of instability 92 N).

In b. and c. referenced figures a 6153 element tet solids model was used but in Cook beam elements are used. See Cook p. 655. You can use either.

a. Refer to the cantilever beam of HW# 3 b. but make the applied load P = 1.0 lbf. The load is applied in a direction parallel to the 2.0 inch cross section dimension. The theoretical end deflection for a rectangular cross section is given by the following equation:

d = d1 + d2 = PL^3/(3EI) + (6/5)(PL/(GA))

The first term is the bending deformation and the second is the deformation due to shear.

a.1 Use the theoretical equation to compute d1, d2, d, d1/d (in per cent), d2/d (in per cent) for L = 20 inches.

a.2 Repeat for L = 2.0 inches.

a.3 Use ANSYS APDL or equavilent FEM code to solve for the stress and deflection for these two cases (L = 20, L = 2). Use eight node plane stress elements (with thickness). Create a mesh with about 10 elements through the height of the beam. Distribute the end load equally to the nodes on the free end of the beam. Apply boundary conditions at the support so as not to restrict the Poisson contraction/expansion. Submit a plot of the deformed and undeformed mesh at the support and a plot of the unaveraged stress at the top and bottom of the beam at the support to show that no singularity at these points has been introduced by your boundary conditions.

For the L = 2 case see if you can detect the shear deformation at x = L/2 by listing and plotting the FEM solution for the horizontal displacement of the nodes at this cross section and showing that they are not linearly proportional to their distance from the neutral axis.

HW #8 Assigned , Due

a. Workbench Tuturial. Work through all steps of the Mavspace > WBtutorial-14-Ch4-STEP.pdf tutorial. Submit images of yours corresponding to slides 28, 33 and 50. You may have to increase or decrease the allowable error to achive results similar to slide 50.

b. Use stress stiffening methods to find the buckling load of a simply supported beam following the methods described in slides 6-10 of Mavspace > FEM Slides > 16_NonlinearProblems.pdf except use two beam elements over half the length of the beam. Compute and report the per cent error in your result when compared to solid mechanics theory.

HW #9 Assigned , Due

a. Read the material from Ventsel & Krauthammer, page 5-7, Mavspace > FEM Slides > 13_Plates.pdf. Review the material on Plate Theory > https://en.wikipedia.org/wiki/Kirchhoff%E2%80%93Love_plate_theory; Read the introductory paragraph and review the figures in this article but studying the equation deveopment etc. is not necessary.

b. Create an ANSYS APDL model for a 1.2 X 1.2 x 20 in. solid steel cantilever beam (use Create > Block). Use an eight node SOLID185 ELEMENT to create a 3 x 3 x 14 mesh and solve for the free end deflection if the end load is 200 lbf. Element Type > Add/Edit/Delete > Options > Element technology K2 > Full Integration (2 X 2 X 2) ). Compute the end deflection using this deafult options.

Change the Gauss quadrature to 1 point (Element technology K2 > Reduced Integration) and repeat. Compare the end deflection results to theory.

c. The steel plate shown in text Figure 15.5-2 (c) is 1m X 1m and 0.05m thick. Find the deflection at corner '2' using plate elements.

Repeat using solid elements and compare your solutions. Select suitable meshes in each case.

HW # Assigned , Due

a. Duplicate the linear elastic buckling results for the flag pole problem in WBTutorial14-Ch9.pdf pages 54-58. Compare your results with theoritical results from Solid Mechanics. The bar is 0.5 inches thick.

b. Duplicate the linear elastic buckling results for the barrel roof problem in WBTutorial14-Ch10.pdf pages 13-16.

c. Duplicate the instability snap-through buckling simulation results for the barrel roof problem in WBTutorial14-Ch10.pdf pages 17-21. Compare your results to those in Ref: Computers & Structures, Volume 12, Issue 5, November 1980, Pages 759-768, "Postbuckling behaviour of plates and shells using a mindlin shallow shell formulation", A. Pica, R.D. Wood, doi:10.1016/0045-7949(80)90178-9 .

d. Duplicate the results in Mavspace > ME6310 > FEM Slides > NonlinearProblems > ME 6310 - Newton Methods. Use MATLAB, Mathematica, Excel, etc.; whatever you're comfortable with. First plot p(x) vs over a range of x that includes the solution point where p = pf

e. Use a unit cube of isotropic elactic solid with applied stress Sx to show that the material is incompressible if Poisson's ratio is 0.5. The initial volume is 1.0; compute the volume after Sx is applied if Poisson's ratio is 0.5.

HW # Assigned , Due

a. Answer questions 2, 3, 4, 5 on old exam Exam 2 Spring 2015.

b. Resolve the units conflicts and solve the coupling example problem in 1. FEM Slides > Composites > 4. VPatel-Composites slides 25 & 27 for 30 deg.

HW # Assigned , Due

Refer to Mavspace folder AEME probelms 4-12-16.pdf

a. Prob 1.a.

b. Prob 1.b.

c. Prob 2.a.

d. Prob 2.b.

c. OMIT THIS PROBLEM Work the stiffening problem described in Nonlinear Probs B Slides 11 & 12. Use the incremental load method to find the displacement at a final load of P = 10, that is, let deltaP = P/N, calculate deltaU, update k(u), repeat. See slide 9.

d. Use hand calculations to verfiy the Mavspace Orthotropic Materials stress strain calculations pages 11-13.

a. Use the methods of Mavspace file VPatel-Composites.pdf and 8-Node Shell elements (Shell281) to solve the problem described in ANSYS Verification Manual Problem VM82 (ANSYS Help > ANSYS Documentation > Verification Manuals > Mechanical APDL Verification Manual > Verification Test Case Descriptions > VM82) Document your solution appropriately.

e. Use a unit cube of isotropic elactic solid with applied stress Sx to show that the material is incompressible if Poisson's ratio is 0.5.

HW # Assigned 4-, Due 4-

Consider a column fixed at one end free at the other and loaded by a compressive force F at the free end. The column is made of steel and is 0.5 x 1.5 x 25 inches. (See Mavspace ME6310 > FEM Slides > NonlinearProblems WBtutorial-14-Ch 9.pdf page 39.)

a. Solve this problem by hand using elementary solid mechanics column buckling theory to find the load that causes elastic buckling about the neutral axis with smaller area moment of inertia.

b. Solve this by hand using the stress stiffening matrix methods described in Mavspace ME6310 > FEM Slides > 16-NonlinearProblems.pdf pages 4-10 and Mavspace ME6310 > FEM Slides > Nonlinear Problems A.pdf page 5. Use one beam element.

c. Repeat b with two beam elements.

d. Solve using WB following the tutorial from WBtutorial-14-ch 9.pdf. Compare the results of parts

HW #8 Assigned , Due

a. Use ANSYS Workbench to find the buckling load for the column described in HW#7. See Mavspace ME6310 > FEM Slides > Nonlinear Problems A.pdf or Mavspace ME6310 > FEM Slides > WBtutorialCh9.pdf page 39-43. Use 8 node bricks, then use 20 node bricks.

b. Repeat 7b. but use Two beam elements.

c. Summarize your results of HW #7 & #8 in a table showing the Value from the Theoretical Solution, the Value by method 7a., per cent error, the Value by method 7b., per cent error, the Value by method 8a., per cent error.

HW # Assigned , Due at 4:30pm in Room 204 WH

a. Duplicate the results in Mavspace > ME6310 > FEM Slides > NonlinearProblems > ME 6310 - Newton Methods. Use MATLAB, Mathematica, Excel, etc.; whatever you're comfortable with. First plot p(x) vs over a range of x that includes the solution point where p = pf

b. Solve the problem described in Mavspace > ME6310 > FEM Slides > NonlinearProblems > Nonlinear Problems B, Slide 5.

c. Alberta Tutorial described on slides 23-34.

d. Problem on pages 38-48; use Workbench.

e. Work the stiffening problem described in Nonlinear Probs B Slides 11 & 12. See also Slide 60.

f. Problem described on slides 49-59. Beams have square cross section 8 mm x 8 mm. E = 200 GPa.

g. Work through the first (beam) tutorial described in Mavspace > ME6310 > FEM Slides > NonlinearProblems > WBTutorial Chaper 10. Submit results similar to those in slides 10 & 13.

HW # Assigned , Due

a. Work through transient structural tutorial Beam Transient Response B. Submit results similar those on Slides 13, 20, 21.

b. Work through Mavspace > ME6310 > WBtutorialCh7 > Tutorials 7A and 7C. Submit Figures from Slides 12, 40, 43, 45, 46, 47.

HW # Assigned , Due

a. Work through the Transient 2D Conduction tutorial described in https://confluence.cornell.edu/display/SIMULATION/ANSYS+Learning+Modules

Submit the heat flux plot at about 1 min into the video and the plot and table of temperature along line 1-2 at about 1.75 min into the video.