Introduction to computational Mechanics, TMHL63, ht 2, 2013
modified 2013-11-19
Laboratory Problem IIa
Below follows a description of Lab IIa, which
· Consists of three parts (Part 1, Part 2 & Part 3)
· Is to be evaluated/reported by peer student evaluation and reporting to the examiner
Laboratory problem IIa; Part 1
Simple 2-dimensional elastostatic FE-analysis,
or
What does the stress state look like at an elliptical hole in a uniaxially loaded thin plate?
Introduction
We will here, as a simple application of FEM for 2-dim. elastostatic problems, study the stress state at an elliptical hole in a uniaxially loaded thin plate.
There are a number of reasons why we have chosen this problem
· It is a geometrically simple problem, for which the FE-results can be compared with dittos based on handbook expressions
· You will have the opportunity to take advantage of the symmetry in the problem (good to practice), a procedure which often reduces the computational cost substantially
· You will get an insight in how stress concentrations appear at holes in loaded structures. More generally one may say that
Stress concentrations appear at all rapid geometry changes in loaded structures, which is an issue that has to be taken into consideration in the design work!
· It is an appropriate problem for studying so called “mapped meshing” technique, where the structure is split into 4-sided regions such that it can be meshed with nicely looking rectangular/4 sided elements whose sizes can be easily controlled (see the figure below).
Aim
The aim of the problem is first of all that you are to analyze a simple detail by FEM, and that you at the same time will get some ideas about the stress state at an elliptical hole, how symmetries may be utilized and how to work with a mapped mesh.
Task
As mentioned above, the task is to study a uniaxially loaded thin plate with an elliptical hole located symmetrically at its centre. More specifically, you are to analyze the stress concentration that appears at the hole, which is to be done both analytically (by a handbook formula, see below) and numerically (by FEM).
It is up to you to choose the dimensions of the plate (width D and thickness t) and the load P, see below, but the far field stress is to be 100 MPa. However, you are to make the plate long enough, such that the effect of the hole is negligible at its ends, and that you do not get plastic yielding at the hole. Concerning the geometry of the hole, we would like you to study three different cases, namely
I) D/2a=2, a/b=2 II) D/2a=4, a/b=1/2 III) D/2a=4, a/b=1
You are to use all symmetries in the problem, and study the smallest possible part of the plate with relevant boundary conditions. Concerning element type and meshing, you can for some case(s) let ANSYS handle that, while you for Case III are to use a mapped mesh. For the mapped mesh case, we would also like you to study how an increase in mesh density (more elements) will affect your FE-result in comparison to the handbook solution. Finally, we would like you to consider what the stress concentration analytically will be for a circular hole which is small compared to the plate size, and what happens with the stress state when the hole becomes more and more like a transverse crack.
Analytical expression
The stress concentration at the hole is given by the following analytical expression (from Roark’s formulas for stresses and strains, 6:th Edition,
page 735), valid for 1/2 ≤a/b≤ 10)
How to carry out the work
A suggestion for how to carry out the work can be found below (initially you work in the toolbox DesignModeler, and then change to the toolbox Mechanical)
· Sketch a rectangle with chosen dimensions (consider the symmetry when choosing dimensions)
· Create a 2D-body (in the Concept-menu in DesignModeler)
· Create a new sketch, where you do an ellipse with chosen radii
· Use the tool Extrude to ”cut out” the hole in the plate
· Mesh, apply forces and restraints, solve the problem and study the result (all in Mechanical)
What a ”free mesh” and a mapped mesh may look like is shown below, where we in the latter case obviously can avoid a dense mesh in regions where it is not necessary, i.e. in our application far from the hole!
In order to achieve a mapped mesh, you do as described below
· Start from the plate geometry (with the hole)
· ”freeze” it by using the command Freeze (in the Tools-menu in DesignModeler)
· Define lines in a new sketch, that in a wanted way split your plate
· Split the plate into two sub-bodies by using the option Slice Material in the Extrude-tool (this requires that the body, to be split, is frozen)
· Redo the above procedure (create a new line and split the body with it) as many times as needed
· The so obtained sub-bodies are then put together in a common part, by first marking them and then using the command Form New Part (in the Tools-menu)
· Now you switch toolbox to Mechanical, where you mesh your new part (consisting of a number of sub-bodies). By this you will get a mesh which is continuous across the sub-body boundaries.
· By choosing the command Mapped Face Meshing and apply it for the complete plate (under Mesh in the ”activity tree”), you may then choose to have 4-noded elements (quadrilaterals) everywhere.
· By the command Sizing (under Mesh) you may then change the element size for the complete plate or for parts of it
· Furthermore, by the same command (Sizing), you can also give a “bias” to the element distribution along some edge, i.e. to make the mesh density increase in areas where a lot happen
Reporting
The stress concentration factor is to be calculated both analytically and by FEM for the above 3 cases, where the input data (dimensions and loading) is to be chosen such that the far field stress is 100 MPa.
For a description of the reporting, see the end of this document.
Laboratory Problem IIa; Part 2
Limitations of different element types, or
Can I always trust my results?
Introduction
It is of course a fact that one must always check the relevancy of the obtained FE-results. Errors can for instance be introduced via mistakes in the geometry creation (dimensions etc) or via mistakes in the specification of material data. Furthermore, an insufficiently locked structure (it can rotate and/or translate as a rigid body) may automatically be given a locking somewhere by the program (this can be checked by checking that the reaction forces are in equilibrium). Finally, it is in fact the case, as you will see, that the FE-formulation itself can work improperly for certain situations.
Here you are to study how different element types behave in a simple application, more precisely a cantilever beam subjected to a load applied at its free end. As you will see, some element formulations work not as well as others. By this we can draw the conclusion that
It is important to know that each element type has its limitations, i.e. there are situations for which it does not work well!
Goal
Even if we in the course do not have time to go any deeper into element type limitations, you are to see that they do exist! Specific details can be found in the FE literature.
Task
As was mentioned previously, the task is here to study a cantilever beam subjected to a transversal load at its free end.
You are to analyze the deflection of its free end, analytically as well as by different (membrane) element types. More specifically, you are to analyze a beam of length α , height 5 cm and width 2 cm (it will clearly be slender enough for the beam theory to work well). Furthermore, you are to use 10 rectangular elements in your analysis. For that/those cases where you obtain a poor result (a too small deflection), you are to refine your mesh and study how the results converge towards the correct solution.
The length α is
1.01m for group 1
1.02m 2
…
1.11m 11
etc
Furthermore, let Young’s modulus be equal to E=2E11 Pa and the applied force P=1E3 N
Element types to test
(Choose 3D-analysis in the Project Menu, but model your beam as a 2D-body with the “surface from sketch”-tool!)
a) The 4-noded element that is standard/default in ANSYS in a 2-dimensional analysis (a higher order element).
b) The 4-noded membrane element PLANE42. This element type must be requested by the user by adding a small command file in the MECHANICAL-part of ANSYS, and more specifically under “Geometry”, see below.
By the command file you overwrite the default choice of element type in Workbench. The rows you are to add look like
ET,1,PLANE42,,1,3
R,1,0.02
MP,EX,1,2E11
MP,NUXY,1,0.3
What you do here, is to say that you would like to use the element type PLANE42, of thickness 0.02, with the Young’s modulus 2E11, and with the Poisson’s ratio 0.3. Further details can be found via the ANSYS-help menu. It is to be noted that you here actually use the 4-noded bilinear iso-parametric QUAD4-element that we have studied on Lecture 7 and Teaching Class 6.
Reporting
For a description of the reporting, see the end of this document.
Laboratory Problem IIa; Part 3
A closer look at isoparametry and
numerical integration
Introduction
As the third part of this laboratory work you are to take a closer look at numerical integration for element stiffness calculations. From the lectures and teaching classes we know that we use Gauss-quadrature for this purpose, and that a minimum integration order is needed in order to obtain the correct result. The task is here to write a MATLAB-program that calculates the element stiffness matrix for the 4-noded bi-linear iso-parametric QUAD4-element that we studied on Lecture 7 and Teaching Class 6. The program is to be written in a general fashion, in that it from provided input data (nodal coordinates, Young’s modulus, Poisson’s ratio and thickness) calculates the element stiffness matrix!
Task
As was mentioned previously, the task is here to write a MATLAB-program for calculation of the element stiffness matrix for a QUAD4-element, where 4-point integration is to be used (c.f. Teaching Class 6).
Reporting
The MATLAB-program should be checked with a program which can be reached via the course home page. When successfully checked, you will get a code which is to be written on the peer student assessment form.
For a description of the reporting, see the end of this document.
Reporting
The evaluation/reporting of this lab work is to be carried out by both peer student evaluation and reporting to the teacher. More precisely
· The laboratory work is to be carried out in groups of 2 persons (possibly one group with 3 persons)
· Each lab group is to carry out the tasks for Part 1, Part 2 and Part 3 presented above.
· Each lab group evaluates the work of 1 other lab group for the lab tasks listed below (Group A evaluates Group B, Group B evaluates Group C, Group C evaluates Group D, etc, i.e. two groups are not to evaluate each other’s work). Thus, each group shall be evaluated 1 time, and are to evaluate 1 time- no more and no less! In the evaluation, you are to step by step carefully check that
o for Part 1:
the same stress concentration factor is found analytically and by FEM for the three different hole-geometries. Observe! Each group make a separate model for each of the cases (in the same ANSYS project) and save them as a basis for your evaluations. The mapped mesh shall be of the type shown in the Figure above (with “nicely” looking elements). The analytical expression is probably most easily handled by MATLAB.
o for Part 2:
the same deflection of the free end of the beam is found both analytically (by using the elemental case for a cantilever beam) and by ANSYS (with standard higher order elements), and that an approximate result is found by ANSYS using a sufficiently fine mesh of QUAD4-elements.
o For Part 3
no peer student assessment for Part 3.
· The peer student evaluation is to be reported on the form/sheet which is found below, which is to be handed in BOTH electronically (by e-mail to Kjell S) and in printed form (in the bookshelf in the corridor of Solid Mechanics) no later than 18:00, Friday, December 13, 2013.
In addition to the form discussed above, this, and exactly this (no more and no less) is to be handed in
o Part 1: A stress plot from ANSYS (with elements shown) for a mapped mesh for Case III, where the maximum normal stress in load direction can be seen (only electronically)
o Part 2: A deflection plot from ANSYS where the value for the lateral deflection of the beam is seen for the case of “sufficiently” many QUAD4-elements and where the element mesh is seen (only electronically).
o Part 3: The MATLAB-program file (only electronically), directly runnable as a .m-file, prepared with the input data you used to get the code number. It shall be given the name labIIagroupXX.m, where XX is your group number!
Note that the peer student evaluation aims at giving you an experience in critical evaluation of another groups simulation work, and is to be done carefully! Furthermore, it is the responsibility of both groups that the reported results are correct. An erroneous “report” of bad quality, may have a negative effect on the final grade (for both groups)!
If a group’s work is not approved at the first peer student assessment, then appropriate modifications of the work are to be undertaken, and another assessment (with the same groups) to be done. If the work is not approved the second time, the two groups are to contact the examiner!
If the groups do not agree, they are to contact the examiner!