The document discusses meshing techniques in finite element analysis (FEA), detailing the types of elements (1D, 2D, 3D) and their selection criteria based on geometry, analysis type, and project timelines. It emphasizes the importance of mesh quality, refinement in critical regions, and the criteria for element quality to avoid distortion and ensure accurate results. Additionally, the document covers practical considerations for effective meshing, including using symmetry, geometry checks, and balancing accuracy with computational limits.

1. UNIT II
Meshing Techniques
By
Dr. Dinesh Y. Dhande
Professor
Department of Mechanical Engineering
AISSMS College of Engineering, Pune

2. CONTENTS
Discretization of a Structure, 1D, 2D and 3D element Meshing, Element
selection criteria, Refining Mesh, Effect of mesh density in critical
region, Use of Symmetry.
Element Quality Criterion:-Jacobian, Aspect ratio, Warpage, Minimum
and Maximum angles, Average element size, Minimum Length,
skewness, Tetra Collapse etc., Higher Order Element vs Mesh
Refinement, Geometry Associate Mesh, Mesh quality, Bolted and
welded joints representation, Mesh independent test.

3. INTRODUCTION
• NEED OF MESHING:
• The basic concept of the FEA is based upon the calculations for only limited
number of points (or elements) and interpolation of the results for entire domain
(surface or volume).
• Any object in the space has infinite degree of freedom and its just impossible to
solve the problem.
• FEA reduces degree of freedom from infinite
to finite with the help of discretization (nodes
and elements) i.e. meshing.

4. TYPES OF ELEMENTS

5. DECIDING TYPE OF ELEMENT
• The type of the element is selected based on following criteria:
• Geometry size and Shape
• Type of analysis
• Time allotted for the project.
• Geometry Size and Shape:
• For the analysis, all three dimensions are required by the software. The
software cannot perform calculations unless and until geometry is defined
completely (via meshing i.e. nodes and elements)
• Geometry can be categorized as 1-d, 2-d and 3-d based upon the dominant
dimensions and type of element is selected accordingly.

6. 1-D:
• Shape of the 1-d element is line. When the element is created using two
nodes, the software understands only one out of three dimensions.
Remaining two dimensions i.e. c/s area must be defined as additional input
data and assign to respective elements.
• Practical Examples: Long shaft, rod, beam, column, spot weld, bolted joints,
pin joints, bearing modelling.

7. 2-D:
• 2-d meshing is carried out at the mid surface of the part. 2-d elements are
planer just like paper. By creating 2-d element, software understands 2 out of
three required dimensions. The third dimension i.e. thickness has to be
provided by user as an additional input data.
• The reason for carrying out 2-d meshing on mid surface is that the element
thickness specified by user is assigned half on element top and half on
bottom side. Hence, in order to represent the geometry appropriately, it is

8. Necessary to extract mid surface and then mesh on the mid surface.
• Practical Examples: All sheet metal parts, plastic components like
instrument panels.
• In general, 2-d meshing is used for parts having width/thickness ratio > 20.
• Limitations of mid surface & 2-d meshing:
• 2-d meshing would lead to higher approximation if used for variable part
thickness and for the surfaces which are not planner and have different
features on two sides.

9. • 3-d :
• It is used when all the three dimension are comparable.
• Practical Examples: Transmission Casing, Clutch Housing, engine block,
connecting rod, crank shaft etc.

10. • Based on type of analysis:
• Based on the type of analysis, the following types of elements are selected.
Type of Analysis Type of Element Preferred
Structural and Fatigue Quad, Hex are preferred over trias, tetras and pentas
Crash and Non-linear Priority to mesh flow lines and brick elements over
tetrahedron.
Mould flow analysis Triangular elements are preferred over quadrilateral
Dynamic Analysis When the geometry is broader case as per above
classification of 2-d and 3-d geometry, 2-d shell elements
are preferred over 3-d.

11. • Based on time allotted for the project:
• When time is not constraint, appropriate selection of elements, mesh flow lines
and good mesh quality is recommended. But sometimes, due to very tight
deadline, analyst is forced to submit the report at the earliest. For such situations
• Automatic or batch meshing tools could be used instead of time consuming
but structured and good quality providing methods.
• For 3-d meshing tetras preferred over hexas.
• If assembly of several components is involved then only critical parts are
meshed appropriately. Other parts either coarse meshed or represented
approximately via 1-d beams, springs, concentrated mass etc.

12. DECIDING ELEMENT LENGTH
• Based on previous experience if similar type of problem (successful correlation
with experimental results).
• Type of analysis: Linear static analysis could be easily carried out that too quite
fast with high number of nodes and elements, but crash, non-linear, CFD or
dynamic analysis consumes lot of time. Keeping control on number of nodes and
elements is necessary.
• Hardware Configuration and graphics card capacity of available computer.
Experienced CAE Engineer know limit of nodes that could be satisfactorily
handled with given configuration of the hardware.

13. PROCESS OF MESHING
• Spend sufficient time in studying the geometry. Observing geometry several
times and thinking from all the directions is strongly recommended. Mental
visualization of the steps or planning before starting the job is the first step to
achieve good meshing.
• Time Estimation: Time estimation is very relative and one can find lot of
difference in estimation by different engineers. Usually a less experienced
engineer will estimate more times as compared to the experienced one. If the
similar kind of jobs are given to the same Engineer again and again, the
meshing time will reduce drastically.
• Geometry Check: Usually the geometry is supplied with ‘*.igs’ format.

14. • Irrespective of software used and accuracy of the software claimed, ‘ geometry
cleanup’ is an integral part of the meshing activity. Before starting meshing
activity, the geometry should be carefully checked for free edges, scar lines,
duplicate surfaces, small fillets, small holes, intersection of parts (assembly of
components)
• Symmetry Check: (i) Complete Part Symmetry:
• In the above case, meshing of only quarter part and reflecting twice is advisable.

15. • Sub part symmetry, repetition of features and possibility of copy paste command.
• Meshing highlighted 22.5 portion and then reflection and rotation would lead to faster
meshing as well as structure of elements and nodes around critical areas (holes)

16. • Selection of type of elements: In real life one type of element is rarely used. It is
usually a combination of different types of elements, i.e. 1-d, 2-d, 3-d and others.
• In above figure, the handle of the bucket is modelled by beam (1-d) elements, bucket
body by shell (2-d) elements and connection between handle and bucket body through
RBE2 (rigid) elements.

17. • Type of Meshing :
• Geometry Based: Mesh is associated to the geometry. If geometry is modified mesh
will also get updated accordingly (automatically). Boundary conditions could be applied
on geometry like surface or edge.
• FE Based: Mesh is non-associative. Boundary conditions to be applied on elements
and nodes only.
• Joint Based:
• (a) Special instructions for bolted joints (specific construction around holes)
• (b) Spot and arc weld
• (c) Contact or gap elements & requirement of same pattern on 2 surfaces in contact.
• (d) Adhesive Joint

18. • Splitting the job:
• In case, if the time available is very less or if engineers in other group are free or sitting
idle, then the job can be splitted among several engineers by providing common mesh
or interfaces.

19. (a) Structured Meshing (b) Unstructured Meshing

20. Mesh adaptation: (a) Original hexahedral
mesh. (b) Refined mesh. (c) Coarsened mesh.

21. MESHING TECHNIQUES

22. • Batch Meshing/Mesh Advisor: Now a days, all softwares provide special programs for
automatic geometry cleanup and meshing with no or little interaction from user. User
has to specify all the parameters like minimum hole diameter, min. fillet radius, avg. and
min. element length, quality parameters etc. & software will run a program to produce
best possible mesh by fulfilling all or most of the specific instructions. Though these
programs are still in progress and its performance will improve over coming years.

24. MESHING IN CRITICAL AREAS
• Critical Areas are high stress locations. Dense meshing and structured mesh
(no trias/pentas) is recommended in these regions. Areas away from critical are
general areas. Geometry Simplification and coarse mesh in general areas are
recommended.
• How critical areas are identified?
• Referring to previous analysis report, one can get fair idea about probable
locations of high stresses.
• If the analysis is carried out first time, then the analysis is run with reasonable
element length and the results are observed. Red colour regions are critical and
need to be remeshed with lesser element length, in second run.

25. REFINING MESH
• To get better results the finite element mesh should be refined in the following
situations :
(a) To approximate curved boundary of the structure
(b) At the places of high stress gradients.
Such situations are shown in Fig. (a) and Fig. (b) shown below.
Fig. (a)

26. Fig. (b) Refinement of mesh near curved boundary

27. USE OF SYMMETRY
• Wherever there is symmetry in the problem it should be made use.
• By doing so lot of memory requirement is reduced or in other words we can use more
elements (refined mesh) for the same capacity of computer memory.
• When symmetry is to be used, it is to be noted that at right angles to the line of
symmetry displacement is zero.
• In the below example, biaxial symmetry of the problem is utilized and only quarter of
the plate is taken for the analysis.

28. USE OF SYMMETRY EXAMPLE

29. EFFECT OF MESH DENSITY IN CRITICAL
REGION
• Let us consider the following example of analysis of plate. In this example, we
will mesh the plate with Quad 4 element and we will vary the number of elements
on hole which is the critical area.

30. • Exact answer : 3 N/mm2

31. • Now, if this is the conclusion, then why not very fine mesh with maximum
possible nodes and elements is created? Why usually 12/16 elements around
holes in critical areas guideline is widely used?

32. • The reason is that the solution time is directly proportional to (dof)2. Also, large size
models are not easy to handle on the computer due to graphics card memory
limitations. A fine balance between level of accuracy and element size (dof) is needed
which could handled satisfactorily with available hardware configuration.
• The optimum element number is decided based on simple exercise as done in above
case.
• Results of different mesh configurations are compared with known analytical answers
and the one which gives logical accuracy with reasonable solution time is selected.
• Following thumb rule is followed for number of elements on holes in most of the CAE
industries:
Minimum no. of elements in critical region : 12
In general region : 06

34. ELEMENT QULAITY CHECK CRITERIA
Why Element Quality Check is required? :
• The shape of Elements in FE Analysis must be distorted from their Ideal shapes when
meshing the irregular or complex geometric shapes.
• Every element is designed to work properly within a certain range of shape distortion.
Exactly how much distortion and what type of distortion is allowed before an element
degenerates depends on factors such as element type, numerical procedures used in
the element design, and so forth.
• The Ideal shape of [2D Elements] a triangular element is an equilateral triangle and a
quadrilateral, it is a square.
• The Ideal shape of [3D Elements] a Tetrahedron element is a Regular or Isosceles
Tetrahedron and a Hexahedron, it is a Cube etc.
• If the actual shape that the element assumes after mapping onto model geometry

35. differs too much from the natural shape, the element becomes degenerated and
produces erroneous results.
"Result Quality α Element Quality"
• ​The major types of degeneration are Aspect Ratio, Skewness, Jacobian Ratio,
Warping Factor, Maximum Corner Angle, Orthogonal Quality, Parallel Deviation, Taper,
Curvature distortion and mid-size node position.
• Generally, large angles between edges (close to 180 degree) are more degenerating
than small angles (close to 0 degree).
• Each FE mesh should be run through an element quality check, and degenerated
elements should be eliminated.
• In order to get reasonably accurate results, it is always important to generate a
structured mesh with good quality parameters.
• If Elements are Degenerated they will become too stiff and underestimate the
deformations and its derivatives like strain & stress values become erroneous

36. • Degenerated Elements increase the inaccuracy of the finite element representation and
have a detrimental effect on convergence of Finite Element Solutions.
• Now a days most of the FE Simulation softwares are equipped with In-Built Quality
Check Options and Quality Based Mesh Generation Algorithms.
• Maintaining element quality is always a challenge for analyst during mesh convergence
studies. Though element size is minimized it is of no use if they are violating quality
requirements.
• The various quality check parameters are : Jacobian, Aspect ratio, Warpage, Minimum
and Maximum angles, Average element size, Minimum Length, skewness

37. • Aspect Ratio:
• The ratio between maximum and minimum characteristic dimension of an element
is known as the Aspect Ratio.
• Large aspect ratios increase the inaccuracy of the finite element representation
and have a detrimental effect on convergence of Finite Element Solutions.
• An aspect ratio of 1 is ideal but cannot always be maintained. In general the
aspect ratios are maintained in between 1 to 5 at critical areas in a domain where
derivatives of field variable are significant.
• Along with solution accuracy the poor element shapes will often cause
convergence problems in nonlinear analyses.
• Aspect ratio is one of the other mesh quality parameters like Skewness, Warping,
Parallel deviation, Maximum corner angle, Jacobian and Orthogonal Quality.

39. • Skewness:
• Skewness is the Angular Measure of Element quality with respect to the
Angles of Ideal Element Types.
• It is one of the Primary Qualities Measures of FE Mesh. Skewness
determines how close to ideal (i.e., equilateral or equi-angular) a face or
cell is.
• Its ideal value is ‘0’ and accepted value is < 45

40. • Skewness for triangular elements= 90  – minimum angle between the lines from each node to
the opposing mid side and between the two adjacent mid sides at each node of the element.
• Skewness for quadrilateral element = 90  – minimum angle between two lines joining opposite
mid-sides of the element ()

41. Minimum Element Length:
• Very important check for crash analysis ( time step calculations). It is also applied in general to
check minimum length feature captured and presence of any zero length element.

42. Warp Angle:
• Ideally all the nodes of quadrilateral element should lie on the same plane but at curvatures and
complicated geometry profiles it is not possible. "Measure of out of planeness of a Quadrilateral
is Warping Factor or Warping Angle".
• Warp angle is defined as the angle between the normal to two planes formed by slitting the quad
element along diagonals.
• Maximum angle out of the two possibilities is reported as warp angle.
• Warp angle is not applicable for triangular elements.
• Its ideal value is 0 and acceptable values is < 10

44. Jacobian Ratio:
• Jacobian (also called Jacobian Ratio) is a measure of the deviation of a given element from
an ideally shaped element.
• The jacobian value ranges from -1.0 to 1.0, where 1.0 represents a perfectly shaped element.
• It is a scale factor arising because of transformation of coordinate system.
• The ideal shape for an element depends on the element type. The check is performed by
mapping an ideal element in parametric coordinates onto the actual element defined in global
coordinates. For example, the coordinates of the corners of an ideal quad element in parametric
coordinates are (-1,-1), (1,-1), (1,1), and (-1,1).

45. • The determinant of the jacobian relates the local stretching of the parametric space required to
fit it onto global coordinate space. The figure below illustrates an real QUAD4 element,
frequently found in a mesh, and the ideal QUAD4 element.

46. Included Angles:
• Skewness is based on overall shape of element and it does not take into account
individual angles of quadrilateral or triangular element.
• Included or interior angle check is applied for individual angles.
• For Quadrilateral Elements : Ideal Value = 90 ( Acceptable = 45 <  <135
• For Triangular Elements : Ideal Value = 60 ( Acceptable = 20 <  <120)
• For Taper : Ideal Value = 0 ( Acceptable < 0.5)

48. Tetra Collapse:
• Ideal shape for tetrahedron element is equilateral tetrahedron (all equilateral
triangular faces).
• When auto-generating a mesh in a complex or invalid geometry. A tetra element,
which seems as thin as a planar element, will be often generated. This type of the
element is called as a collapsed tetra, and this option enable to check for such a
collapsed element.

49. HIGHER ORDER ELEMENTS VS REFINED
MESH
• Accuracy of calculation increases if higher order elements are used. Accuracy can also be
increased by using more number of elements.
• Limitation on use of number of elements comes from the total degrees of freedom the
computer can handle. The limitation may be due to cost of computation time also. Hence
to use higher order elements we have to use less number of such elements.
• The question arises whether to use less number of higher order elements or more number
of lower order elements for the same total degree of freedom.
• There are some studies in this matter keeping degree of accuracy per unit cost as the
selection criteria. However the cost of calculation is coming down so much that such
studies are not relevant today.
• Accuracy alone should be selection criteria which may be carried out initially on the
simplified problem and based on it element may be selection for detailed study.

50. • Associative mesh is very rarely used in practice by CAE teams. But this option is
provided by many of the CAE softwares for first hand calculations by design/CAD
engineers for initial guess/rough idea.
• For getting quick results, automatic meshing is carried out by picking surfaces or
volume of the geometry, simple boundary conditions are applied and solution is
obtained.
• Generated mesh is associative with geometry.
• Advantages:
• Mesh changes with change in geometry
• Boundary condition could be applied on geometry (edges, surfaces involved
instead of nodes and elements) which is more user friendly.
GEOMETRY ASSOCIATIVE MESH

52. MESH QUALITY
• Element Free edges
• Duplicate Element
• Duplicate node
• Shell Normal
• Geometry deviation
• Delete free/temporary nodes
• Renumber nodes/elements, properties before export operation
• Observe type, family and number of elements (element summary for complete
model)
• Check Mass (actual mass vs FEA mass)
• Free-free run or dummy liner static analysis.
• Request your colleague to check the model.

53. • Element Free Edges:
• Any quad element has 4 free edges.
• In this two elements connected, middle edge is shared and no more free. For a
real life FEA model, free edges should
match with geometry outer/free edges.
Additional free edges is an indication of
unconnected nodes.

54. • Duplicate Element:
• Mistakes during operations like reflect, translate etc. result in duplicate elements.
• These extra duplicate elements do not cause any error during the analysis but
increases stiffness of the model and result in lesser displacement and stress.
• For example, in case of a simple plate subjected to tensile load, consider that
due to some meshing operation, all the elements are duplicated and analysis is
carried out as it is, then it will show half the stress and displacement.
• Duplicate Node:
• Operations like copy, translate, orient, reflect etc. result in duplicate nodes at
common edges.

55. • Geometry Deviation:
• After completion of meshing geometry as well as mesh should be viewed
together (mesh line option OFF).
• Mesh Should not deviate from the geometry.
• Delete Free/Temporary nodes:
• Free nodes if not deleted result in rigid body motion.
• When auto singularity option is turned on, software via spring element of very
small stiffness connect free nodes with parent structure, resulting in warning
message during analysis.
• Mesh Should not deviate from the geometry.
• Renumber nodes, elements, properties etc before export operation:
• Frequent import/export operation could lead to very big numeric figure for nodes
and element labels.

56. • Some softwares refuse to read the file if node/elements label numbers are
greater than specific limit.
• This could be avoided by renumbering nodes, elements etc.
• Observe type, family and number of elements (element summary for
complete model):
• Mesh should be checked carefully prior to export operation as well as after
importing it in the external solver for element type, family, numbers etc.
• Some times, due to translator problem or if properties are not defined properly
of for non supportive elements, either elements are not exported at all or family
is changed (like membrane elements converted to thin shell).
• Plot, trance lines, element free edges, free faces if any should be deleted.
• Check Mass:
• When prototype/physical model of the component is available, FEA model mass

57. • should be compared with actual one.
• Difference means missing or additional components or improper material or
physical properties.
• Free-free run or dummy linear static analysis:
• Before delivering the final mesh to the client, free-free run should be performed.
• 6-rigid mode indicate all parts in the assembly are properly connected to each
other.
• In case of single component meshing job, linear static analysis with dummy
boundary conditions should be carried out.
• Request your colleague to check the model:
• Due to continuous working on same project, our mind take some of the things for
granted and there is a possibility of missing some important points. It is a good
practice to get it cross checked via colleague prior to the final delivery.

58. • Shell Normal:
• Consider following example:
• For 2-d meshing analysis, the mid surface is extracted and analysis is carried out on mid-surface
mesh.
• Shell normal helps us to view top and bottom side stresses.
• Every element has elemental (or local) coordinate system.
• Shell normal is direction of element normal (common practice is to represent normal via Z axis,
assuming element is oriented in XY plane.
• For viewing stress, commercial post processors provide options like top/bottom or Z1/Z2 indicating
positive and negative directions of the shell normal.

59. • The top or bottom is not decided by how the FEA model is oriented but on the +Z direction of the
elements.
• Top side (or Z1 direction) : Along the direction of the arrows as shown in above figure
• Bottom side ( or Z2 direction) : -Z axis.
• If shells are not aligned properly, there is no error in process point of view. But at the time of post
processing, the software does not understand, tension or compression. What is understands is shell
normal orientation.
• Let us consider that in below example, the shell normal orientation is in opposite direction.
• While viewing the results on bottom side (Z2 direction), all the elements except the reverse shell
normal orientation will show tensile stress (+) and odd one will shoe compressive (-) stresses as
shown in below figure.

60. • The beginner will interpret that there is something wrong in boundary conditions whereas experienced
engineer knows that this is due to inconsistent shell normal.
• FEA softwares provide special command for consistent shell normal. (all shell normal aligned in one
direction)
• Following table lists the mesh quality check summary when a model is received from vendor or
colleague.

62. BOLTED AND WELDED JOINTS REPRESENTATIONS
• In real life problems, most of the failures are due to stress concertation points or at
bolted /welded joints which is mainly because of fatigue. In common practice, many
of this are subjected to static loads and hence we cannot observe failure in such
cases. If the same joints are subjected to cyclic loading, they will fail early as
compared to static case.
• Some important points remembered in case of welded joints:
Static strength of weld >> static strength of parent material
Fatigue strength of weld <<< Fatigue strength of parent material
• There are no universal standard guidelines for modelling bolted or welded joints.
Simulation engineer has freedom to use his skill and perception to model such
joints.

63. MODELLING SPOT WELDED JOINT
• Spot welding is possible only for sheet metal parts. (thickness ≤ 2 mm)
• Classical Approach:
• Welding is neglected and two parts are assumed as single entity.
• This approach results in high stiffness and transfer of forces and moment at much
more contact area than actual one.
• This leads to safer results i.e. less stress and displacement than the actual one and is
not recommended.
• Beam Element:
• The spot weld is modelled using beam element at the locations as specified in
drawing.

64. • Beam Element diameter = Actual spot diameter
• Beam element should be exactly perpendicular to surfaces (matching mesh pattern on
two surfaces).
• Rigid Elements : Everything is same as beam element except rigid element is used
except beam.
• Coupled degree of freedom/RBE2 elements: Some organisations prefer coupled
dof/RBE2/RBE3 elements with specific dofs transferred to dependant nodes.

65. • Spring Elements:
• Spring elements with specific translational and rotational stiffness are used to represent
spot weld.
• ACM (Area Contact Method using brick elements):
• This is one of the popular method. Software automatically generates brick elements
with RBE2/RBE3 connections at the connector locations defined by user. The spot
diameter, thickness of joining surface and location of spot weld needs to be defined.
• Beam, rigid element or ACM are commonly accepted methods across the globe and are
recommended.

66. MODELLING ARC WELDED JOINT
• Shell Element:
• Weld is represented by shell elements.
• Weld element thickness = weld (throat thickness)

67. • Rigid Elements:
• Arc welding is represented by rigid elements, connected in the area of welding.

68. • Spots are stronger in shear (than the normal load). Most of spot weld failures are
caused by tension/compression or normal stress.
• Just by changing spot weld orientation (changing nature of stress to shear) could also
avoid the failures.
• For very thin sheet metal parts, (below 0.8mm thickness), spot welding should be
preferred over arc welding. Arc welding burns the parent metal itself and causes
weakness in the vicinity of the joint.
PRACTICAL CONSIDERATIONS FOR WELDED JOINTS

69. • Following types of analyses are carried out when weld properties are unknown : Static
analysis, Dynamic analysis and fatigue analysis.
• Some organisations carry out transient thermal analysis (special material properties
assigned to weld) first to find out residual stresses due to high temperature and
subsequent cooling and then transfer it for structural analysis. This is very time
consuming and requires lot of computational efforts.
• Instead, fatigue analysis after performing static or dynamic is much more simpler,
faster and reliable.

70. MODELLING BOLTED JOINTS
• For modelling bolt joint:
• Minimum two layers around the bolt hole (1.5 to 2.0 times core diameter) representing
washer/bolt head are recommended.
• 12 to 16 elements on circular hole.
• Usually the aim is to analyse parent structure and not bolts.
• Special techniques for bolt simulation are based on representation of bolts by
equivalent stiffness modelling via 1-d or RBE2, RBE3 elements. Commonly used
methods are discussed below:
• Beam Elements :
• Centre of the bolt is connected to inner and outer layers via beam elements of
diameter equal to ‘d’ and 2 times ‘d’ (d = core diameter) as follows.

72. • Rigid Elements:
• Method 1 : Everything is same as beam method except RBE2 or RBE3 (one to
multiple nodes) for washer area connections (both inner as well as outer layers) while
bolt shank portion represented via beam elements (beam dia equal to core dia)
• Method 2: RBE2 and RBE 3 elements are created as shown in below figure, shank
modelled using beam element.

73. • In some of the organisations, it is a standard practice to neglect stress at outer layer
elements (washer area and one more layer surrounding beam/rigid connection) due to
high stresses observed at beam/rigid and shell/solid connections. In this case, two
more circular layers around the washer layer are recommended. Results are viewed
by neglecting elements in washer area and connected elements.
• Modelling of bolt threads:
• Shank portion of the beam (blue element) is split into
multiple beam elements, (very small dia. = 0.1 to 1 mm)
or rigid elements (RBE2 spider, green elements) connected
to shell layers at an angle = thread helix angle.

74. • How to apply preloads:
(1) Special commands in commercial software : Most of the commercial softwares
have special commands for applying bolt torque either by directly specifying the
torque or otherwise equivalent axial force produced due to torque.
(2) Temperature method: To achieve the axial compression beam element
(representing shank) is subjected to thermal loading (negative temperature).
Negative temperature causes compression of the beam.
(3) Direct Force application: Bolt clamping force is directly applied on washer area.
(4) FEA is not recommended for designing standard components like Nuts, Bolts,
Gears etc.
• In some of the organisations, bolts are simulated via 3-d elements ( as per actual
geometry i.e. threads etc.) and then analysis is carried out by defining contact between
threads of mating parts and bolt head and resting surface etc.)

75. FEA CONVERGENCE AND MESH
INDEPENDENCE TEST
Why?
• Numerical software packages solve problems using a series of discrete points.
Each point, or node, adds degrees of freedom (DOF) to the system. So the more
DOFs in the model the better it will capture the structural behavior.
• Each DOF adds complexity and increases solve time. The engineer needs to
balance the complexity of the model with solve time.
• Too few DOFs and the response could be incorrect.
• Too many DOFs and the model could take days to run.
• So how does an engineer develop an accurate but efficient FEA model? :By
assessing convergence and demonstrating mesh independence.

76. • It doesn’t take much for a finite element analysis to produce results. But, for results
to be accurate, we must demonstrate that results converge to a solution and are
independent of mesh size. To begin, let’s define a few key terms:
• Convergence: Mesh convergence determines how many elements are required in
a model to ensure that the results of an analysis are not affected by changing the
size of the mesh. System response (stress, deformation) will converge to a
repeatable solution with decreasing element size.
• Mesh Independence: Following convergence, additional mesh refinement does
not affect results. At this point the model and its results are independent of the
mesh.
• A mesh convergence study verifies that the FEA model has converged to a
solution. It also provides a justification for Mesh Independence and additional
refinement is unnecessary.

77. MESH CONVERGENCE EXAMPLE
• Let’s consider convergence of a finite element model of a steel beam.
• Convergence studies varies the sizing and configuration of the FEA mesh.
• Our example is a rectangular beam so we can vary mesh parameters in three
directions. We can vary by element size or number of divisions. For our example we
will use “number of divisions” with equal spacing. Our mesh will vary the number of
elements along:
• Beam Width
• Beam Depth
• Beam Span
• Using an iterative method, we increase the number of elements along each side
and solve. We record the complexity of the model vs. response. For us, complexity
is the number of elements and subsequent degree of freedom. Our response of

78. • interest is the maximum vertical deflection. Varying the number of elements along
each edge, we can develop a table of mesh size vs deflection and solve time:
• We can then plot maximum vertical deflection vs. the number of elements in the
model. At a point, the response of the system converges to a solution. Refinement
of the mesh (the addition of more elements) has little to no effect on the solution.
• When this occurs we have a converged solution.

79. • We also can plot solve time and vertical deflection vs. the number of elements. The
addition of elements increases solve time. At a point, more elements increases solve
time with no refinement in solution. Refinement past this point is an inefficient
application of FEA.

80. • The results of an FEA model must be independent of mesh size. A convergence
study ensures the FEA model captures the systems behavior, while reducing solve
time.

81. When modeling a problem using a finite element program, it is very important to check
whether the solution has converged. The word convergence is used because the output
from the finite element program is converging on a single correct solution. In order to
check the convergence, more than one solution to the same problem are required. If the
solution is dramatically different from the original solution, then solution of the problem is
not converged. However, if the solution does not change much (less than a few percent
difference) then solution of the problem is considered converged.
Currently, two types method are used to demonstrate the numerical convergence of the
solution :
1). h – method 2). p – method
The h- and p- versions of the finite element method are different ways of adding degrees of
freedom (dof) to the model (Figure 1).
P and H MESH REFINEMET METHOD

82. h-method –> The h-method improves results by using a finer mesh of the same type of element.
This method refers to decreasing the characteristic length (h) of elements, dividing each existing
element into two or more elements without changing the type of elements used.
p-method –> The p-method improves results by using the same mesh but increasing the
displacement field accuracy in each element. This method refers to increasing the degree of the
highest complete polynomial (p) within an element without changing the number of elements used.
The difference between the two methods lies in how these elements are treated. The h-method
uses many simple elements, whereas the p-method uses few complex elements.

83. H-Method
More accurate information is obtained by increasing the number of elements. The name for the h-
method is borrowed from mathematics. The variable h is used to specify the step size in numeric
integration. If a part is modeled with a very coarse mesh, then the stress distribution across the part will
be very inaccurate. In order to increase the accuracy of the solution, more elements must be added.
This means creating a finer mesh. As an initial run, a course mesh is used to model the problem. A
solution is obtained. To check this solution, a finer mesh is created. The mesh must always be changed
if a more accurate solution is desired. The problem is run again to obtain a second solution. If there is a
large difference between the two solutions, then the mesh must be made even finer and then solve the
solution again. This process is repeated until the solution is not changing much from run to run.

84. P-Method
The p in p-method stands for polynomial. Large elements and complex shape functions are used in p-method problems.
In order to increase the accuracy of the solution, the complexity of the shape function must be increased. Increasing
the polynomial order increases the complexity of the shape function. The mesh does not need to be changed when
using the p-method.
As an initial run, the solution might be solved using a first order polynomial shape function. A solution is obtained. To
check the solution the problem will be solved again using a more complicated shape function. For the second run, the
solution may be solved using a third order polynomial shape function. A second solution is obtained. The output from
the two runs is compared.
If there is a large difference between the two solutions, then the solution should be run using a third order polynomial
shape function. This process is repeated until the solution is not changing much from run to run.