2-d Cylindrical Roller Contact

Chapter 1: 2-D Cylindrical Roller Contact

1

2-D Cylindrical Roller Contact



Summary



Introduction



Solution Requirements



Analytical Solution



FEM Solutions



Modeling Tips



Pre- and Postprocess with SimXpert



Input File(s)

19 20 20

20

21 25

68

28

CHAPTER 1 19 2-D Cylindrical Roller Contact

Summary Title

Chapter 1: 2-D Cylindrical Roller Contact

Contact features

• • • • •

Geometry

2-D Plane strain (units: mm)

Advancing contact area Curved contact surfaces Deformable-deformable contact Friction Comparison of linear and parabolic elements • • • •

Material properties

F

Block height = 200 Block width = 200 Cylinder diameter =100 Thickness = 1

E cylinder = 210kN  mm 2

E block = 70kN  mm 2

 cylinder =  block = 0.3

Linear elastic material Analysis type

Quasi-static analysis

Boundary conditions

• Symmetric displacement constraints along vertical symmetry line. • Bottom surface of the foundation is fixed  u x = u y = 0  • Contact between cylinder and block

Applied loads

Vertical point load F = 35kN

Element type

2-D Plane strain • 8 -node parabolic elements • 4-node linear elements

Contact properties

Coefficient of friction  = 0.0

FE results

1. Plot of normal contact pressure against distance from center of contact 2. Plot of tangential stress against distance from center of contact 3. Plot of relative tangential slip against distance from center of contact 5000

and

 = 0.1

Contact Pressure N/mm 2 Analytical SOL 400 Contacting Surface

4000

SOL 400 Contacted Surface

3000 2000 1000 0

0

1

2

3

4

5

Distance (mm)

6

7

8

20 MD Demonstration Problems CHAPTER 1

Introduction A steel cylinder is pressed into an aluminum block. It is assumed that the material behavior for both materials is linear elastic. The cylinder is loaded by a point load with magnitude F = 35kN in the vertical direction. A 2-D approximation (plane strain) of this problem is assumed to be representative for the solution. An analytical solution for the frictionless case is known - (Ref: NAFEMS, 2006, Advanced Finite Element Contact Benchmarks, Benchmark 1 2D Cylinder Roller Contact).

Solution Requirements There are two solutions: one using a friction coefficient of 0.1 between the cylinder and block and one frictionless. • Length of contact zone • Normal pressure distribution as function of distance (x-coordinate) along the contact surface • Tangential stress distribution as function of distance along the contact surface These solutions demonstrate: • More elements near the contact zone • Which surface is treated as master (contacting) and slave (contacting) The analysis results are presented with linear and parabolic elements.

Analytical Solution An analytical solution for this contact problem can be obtained from the Hertzian contact formulae (Hertz, H., Über die Berührung fester elasticher Körper. J. Reine Angew. Mathm. 92, 156-171, 1881) for two cylinders (line contact). The maximum contact pressure is given by: p max =

F n E* -----------------2BR*

where F n is the applied normal force, E* the combined elasticity modulus, B the length of the cylinder and R* the combined radius. The contact width 2a is given by: a =

8F n R* ----------------BE*

Using the normalized coordinate  = x  a with x the Cartesian x-coordinate, the pressure distribution is given by: p = p max 1 –  2

The combined elasticity modulus is determined from the modulus of elasticity and Poisson’s ratio of the cylinder and block E cylinder , E block ,  cylinder , and  blo ck , as follows: 2E cylinder E block E* = -------------------------------------------------------------------------------------------------------------2 2 E block  1 –  cylinder  + E cylinder  1 –  block 

CHAPTER 1 21 2-D Cylindrical Roller Contact

The combined radius of curvature is evaluated from the radius of curvature of the cylinder and block R cylind er and R block , as follows: R cylinder R block R* = ------------------------------------------R cylinder + R block

For the target solution, the block is approximated with an infinitely large radius. The combined radius is then evaluated as: R* =

lim

R block  

R cylin der R block ------------------------------------------= R cylinder R cylinder + R block

Using the numerical parameters for the problems the following results are obtained: a = 6.21mm p max = 3585.37N  mm 2

Note that half the contact length is equal to 6.21 mm which corresponds to approximately 7.1 degrees of the ring. Hence, it is clear that, in order to simulate this problem correctly, a very fine mesh near the contact zone is needed.

FEM Solutions A numerical solution has been obtained with MD Nastran’s solution sequence 400 (SOL 400) for the element mesh shown in Figure 1-1 using plane strain linear elements. The elements in the entire cylinder and entire block have been selected as contact bodies. Contact body IDs 5 and 6 are identified as a set of elements of the block and cylinder respectively as: BCBODY BSURF ...

5 5

2D 1

DEFORM 2

5 3

0 4

.1 5

6

7

6 6

2D 1242

DEFORM 1243

6 1244

0 1245

.1 1246

1247

1248

and BCBODY BSURF ...

Furthermore, the BCTABLE entries shown below identify that these bodies can touch each other: BCTABLE

BCTABLE

0 SLAVE

6 0 MASTERS 5 1 SLAVE 6 0 MASTERS 5

0. 0

1 0. 0

.1

0.

0

0.

0. 0

1 0. 0

.1

0.

0

0.

Thus, any deformable contact body is simply a collection of mutually exclusive elements and their associated nodes. The order of these bodies is important and is discussed later. For the simulations with friction, a bilinear Coulomb model is used (FTYPE = 6). The slave or contacting nodes are contained in the elements in the cylinder, whereas the master nodes or nodes or contacted segments are contained in the elements in the block.

22 MD Demonstration Problems CHAPTER 1

Steel Cylinder

Contact Body ID 6 Element IDs 1242 to 2641

Contact Body ID 5 Element IDs 1 to 1241

Aluminium Block Y Z

X

Figure 1-1

Element Mesh Applied in Target Solution with MD Nastran

Nonlinear plane strain elements are chosen by the PSHLN2 entry referring to the PLPLANE option as shown below. PLPLANE 1 PSHLN2 1 + C4

1 1 PLSTRN

1 L

+ +

Herein referred to as plane strain quad4 elements (PLSTRN QUAD4) or (PLSTRN QUAD8) for the linear and parabolic elements respectively listed in Table 1-1. All elements are 1 mm thick in the out-of-plane direction. Table 1-1

Applied Element Types in Numerical Solutions SOL 400

linear

PLSTRN QUAD4

parabolic

PLSTRN QUAD8

The material properties are isotropic and elastic with Young’s modulus and Poisson’s ratio defined as: $ Material Record : steel MAT1 1 210000. $ Material Record : aluminum MAT1 2 70000.

.3 .3

The nonlinear procedure used is: NLPARM

1

1

PFNT

Here the PFNT option is selected to update the stiffness matrix during every iteration using the full Newton-Raphson iteration strategy; the default convergence tolerance values (0.01) will be used. The convergence method and tolerances may be specified explicitly as shown here since they will be discussed later.

CHAPTER 1 23 2-D Cylindrical Roller Contact

Table 1-2

Nonlinear Control Parameters

1

2

3

NLPARM

1

1

+pb1

1.00E-02

1.00E-02

4

5

6

PFNT

7

8 UP

9

10 +pb1

1.00E-05

The obtained lengths of the contact zones are listed in Table 1-3. The exact length of the contact zone cannot be determined due to the discrete character of contact detection algorithms (nodes are detected to be in contact with an element edge for 2-D, element face for 3-D). It is clear, however, that the numerical solution is in good agreement with the analytical one. Table 1-3

Length of the Contact Zone and Pmax amin (mm)

aavg (mm)

amax (mm)

Error (%)

Pmax (N/mm2)

Error (%)

linear

5.99

6.33

6.67

2.6

3285

-8.38

parabolic

5.88

6.08

6.28

-1.5

3583

-0.05

The deformed structure plot (magnification factor 1.0) is shown in Figure 1-2. A plot of the Hertzian contact solution for the pressure along the contact surface is obtained with linear and parabolic elements as shown in Figure 1-3 and Figure 1-4.

amax amin Contacting Nodes

Contacted Nodes

Figure 1-2

Deformed Structure Plot at Maximum Load Level (magnification factor = 1)

24 MD Demonstration Problems CHAPTER 1

5000

Contact Pressure N/mm 2 Analytical SOL 400 Contacted Surface

4000

SOL 400 Contacting Surface

3000 2000 1000 0

0

1

2

3

4

5

6

7

8

Distance (mm)

Figure 1-3

5000

Comparison of Analytical and Numerical Solutions for Linear Elements without Friction

Contact Pressure N/mm 2 Analytical SOL 400 Contacting Surface

4000

SOL 400 Contacted Surface

3000 2000 1000 0

0

1

2

3

4

5

6

7

8

Distance (mm) Figure 1-4

Comparison of Analytical and Numerical Solutions for Parabolic Elements without Friction

The contact pressure plotted for the contacting nodes shows, even with this mesh density, an oscillating type of behavior. This is reduced for the parabolic elements. Generating the same plots along the contacted nodes produces a smoother curve. Numerical solutions have also been obtained with a friction coefficient of 0.1 (bilinear Coulomb). The contact normal and tangential stress along the contacting nodes are shown in Figure 1-5. All stresses show an oscillating type of behavior. This can be improved by refining the mesh in the contact zone.

CHAPTER 1 25 2-D Cylindrical Roller Contact

5000

Pressure Linear

Contact Stress N/mm 2

Pressure Parabolic

4000

Tangential Linear Tangential Parabolic

3000 2000 1000 0

0

1

2

3

4

5

6

7

8

Distance (mm) Figure 1-5

Normal and Tangential Stress Along Contact Surface

Modeling Tips About Convergence Although the nonlinearity of the force-displacement relation in this problem is quite mild, looking more closely at the convergence of this problem will be useful for subsequent problems in this manual, and worthy of mention here as a matter of introduction. Table 1-4 controls the number of iterations in the Newton-Raphson process illustrated below in Figure 1-6. Table 1-4

Convergence Output Error Factors

Load Step

No. Inc

IRT

Disp

Load

Work

1

1

1

1.00E+00

9.78E-01

9.78E-01

1

1

2

3.70E+00

8.83E-01

4.57E+00

1

1

3

2.80E+00

6.83E-01

3.98E+00

1

1

4

1.43E+00

3.81E-01

2.26E+00

1

1

5

4.96E-01

7.28E-02

8.84E-01

1

1

6

3.72E-04

1.51E-02

9.98E-04

1

1

7

6.00E-05

2.69E-05

8.69E-05

26 MD Demonstration Problems CHAPTER 1

Load Fy (N)

60000

Newton-Raphson Path

Fy , v

50000

2

Point C

40000 30000 Point D

20000

Applied Load = 17500

Point B

10000 Displacement v (mm) Point A

0.0

Figure 1-6

0.5

1.0

1.5

2.0

2.5

3.0

3.5

4.0

Newton - Raphson Path for Load-Displacement Curve

At the beginning of the analysis (Point A in Figure 1-6), the tangent modulus (slope of load-displacement curve) is used to project to the applied load to Point B, which does not satisfy the convergence criteria. Then equilibrium is reestablished at Point C, and a new slope is computed. The Newton-Raphson iterative procedure continues until the convergence tolerances are satisfied, Point D. The convergence criteria are based upon displacement, load or work either individually or in some combination. The Newton-Raphson iterative scheme is recommended for all SOL 400 analyses because the degree of nonlinearity is typically significant. For the parameters in Table 1-3, the output (Table 1-4) shows the following convergence characteristics. The percent sign helps to locate the line in the output file. In this case, the criteria used is both the displacement, U, and load, P - specified through the UP keyword for the convergence type on the NLPARM command - with a value of 0.01 for each. This means that both relative displacement and load measures (error factors) must be below 0.01 for convergence to be permitted. This can be seen in Figure 1-7. In this case, there is no checking on the work, even though it has a low tolerance. 1 Log(work)

0

Log(disp)

-1 -2

Log(epsp = epsu)

Log(load)

-3 -4 -5

Log(epsw)

Figure 1-7

Error Factors For Each Iteration

About the Order of Contact Bodies The nug_01aw.dat input file changes the order of the contact body detection, in which the coarser mesh (block) is the contacting surface. Although acceptable to the contact algorithm, the results are degraded since it is best to have

CHAPTER 1 27 2-D Cylindrical Roller Contact

the body with the most nodes as the contacting body. Run nug_01aw.dat to see the differences as shown in Figure 1-8.

nug-01aw.dat Steel Cylinder Contacted Nodes

Contacting Nodes

Aluminium Block

Figure 1-8

nug-01am.dat Steel Cylinder Contacting Nodes

Contacted Nodes

Aluminium Block

Deformed Mesh of Different Contact Body Ordering

28 MD Demonstration Problems CHAPTER 1

Pre- and Postprocess with SimXpert Units All data imported or created in MSC SimXpert is assumed to be in a single consistent system of units, as specified in the Unit Manager. It is important to specify the appropriate units prior to importing any unitless analysis files, such as an MD Nastran bulk data file, or creating materials, element properties, or loads. This is so that the MSC SimXpert user is assisted in being consistent with the use of numerical quantities that have units. The system of units is specified in a dialog accessed by selecting Tools: Units Manager. For the illustration below, the geometry is created, meshed with linear elements using frictionless contact, and finished by comparing results with the analytic solution. a. Tools b. Options c. Units Manager d. Basic Units

a

c d

b

CHAPTER 1 29 2-D Cylindrical Roller Contact

Create a Part for the Block Parts are the main components of a model and may be used to specify specific attributes (geometry, properties etc.). For example, here the part/block, is created (bottom right) that will be later used by picking the part from the model tree in the Model Browser (bottom left). We will find that in defining material properties picking parts from the model tree is easier than trying to pick a group of elements. Later the last part, cylinder, is created. a. Assemble b. Create Part c. block; click OK

a b

c

30 MD Demonstration Problems CHAPTER 1

Create the Block Geometry The geometry of the part/block, is created here and results in a simple rectangular shaped object. More geometry is added to this part in subsequent steps. a. Geometry b. Filler c. X, Y, Z Input enter 0,200,0; click OK X, Y, Z Input enter 30,200,0; click OK X, Y, Z Input enter 30,170,0; click OK X, Y, Z Input enter 0,170,0; click OK

p

( p

)

a b

c c

CHAPTER 1 31 2-D Cylindrical Roller Contact

Create a Curve to Define a Surface Edge Continuing to add geometry to the part/block, a curve (line) is created below the previous rectangle. This curve is used to generate a surface between the rectangle and line. a. Geometry b. Curve c. X, Y, Z Input enter 0,100,0; click OK X, Y, Z Input enter 100,100,0; click OK OK

a b

c c

32 MD Demonstration Problems CHAPTER 1

Create a Surface Between Two Curves Now the surface is generated between the curve on the bottom of the rectangle and the previously created curve. The part/block now contains two surfaces: a rectangle and quadrilateral. a. Geometry b. Filler c. enter 2 Curves; click OK

a b

c

CHAPTER 1 33 2-D Cylindrical Roller Contact

Create a Surface by Defining Its Vertices Another surface is added using one point and three vertices. a. Geometry b. Filler c. Enter 1 point, 3 vertices; click OK d. X, Y, Z Input enter 100,200,0; click OK

a b

c d

34 MD Demonstration Problems CHAPTER 1

Create a Surface by Sweeping a Curve The final surface added to the part/block, is created by sweeping the bottom horizontal curve downward for 100 mm. a. Geometry b. Sweep c. Vector, two point normal, pick Curve, Length of Sweep; click OK

a

b

c

CHAPTER 1 35 2-D Cylindrical Roller Contact

Stitch Surfaces Finally, all of the surfaces that comprise the part/block, are stitched together. Stitching surfaces creates congruent surfaces with aligned normals within a stitch tolerance. Unconnected or free edges are displayed in red whereas shared edges are displayed in green as shown below. a. Geometry b. Stitch c. 4 bodies; click OK

a

b

1 2 c

3

4

36 MD Demonstration Problems CHAPTER 1

Create a Part: Cylinder Now the cylinder part is created. a. Assemble b. Create Part c. Cylinder; click OK

• c. cylinder, OK

a

b

c

CHAPTER 1 37 2-D Cylindrical Roller Contact

Create an Arc The cylindrical surface is generated by an arc and a line. The arc is defined below. a. Geometry b. Arc c. Dir-Radius 0,250,0;0,250,-1 d. Arc.1, 40,0,180 VERTEX(indicated); click OK

a b

c

d

38 MD Demonstration Problems CHAPTER 1

Create a Curve Along a Line of Symmetry The cylindrical surface is generated by an arc and a line. The line is defined below. a. Geometry b. Curve c. 2 Vertices; click OK

a b

c

CHAPTER 1 39 2-D Cylindrical Roller Contact

Break Line and Arc into Two Curves for Two Surfaces Before generating a surface from these two curves, each curve (line and arc) is broken into two equal pieces respectively. This allows for generating two surfaces that ultimately generate different meshes. a. Geometry b. Edit Curve c. Split d. Parametric, 2 Curves; click OK

a b

c

d

40 MD Demonstration Problems CHAPTER 1

Create Surfaces from Curves Two surfaces (composing half of the cylinder) are generated from the curves previously constructed and are stitched together. a. Geometry b. Filler c. 2 Curves, click OK (repeat for other 2 curves d. Stitch, 2 surfaces; click OK

a b

c

d

CHAPTER 1 41 2-D Cylindrical Roller Contact

Create Mesh Seeds With the parts completed, each curve of each surface is seeded prior to meshing. Here the curves that comprise the surface of the lower portion of the cylinder are seeded with element sizes that include uniform and biased seeds. a. Meshing b. Seed: Arrows on curves indicate direction for nonuniform mesh seed c. Curve (seed as indicated in the 3 curves); click OK

a

b

c

42 MD Demonstration Problems CHAPTER 1

Create Mesh With the curves of this surface seeded, a quadrilateral dominate mesh is created by using the surface mesher. a. Meshing b. Surface c. Pick Surface, Mesh type and Method (indicated) d. Element Size 1 e. Quad Dominant f. OK yp

(

a b

c d

e

f

)

CHAPTER 1 43 2-D Cylindrical Roller Contact

Create Mesh The top cylindrical surface is meshed with a quadrilateral dominate mesh and the cylindrical part meshing is complete. a. Meshing b. Surface c. Pick Surface d. Element Size 2.5 e. Quad Dominant f. OK

a b

c

d

e

f

44 MD Demonstration Problems CHAPTER 1

Create Mesh The block part consists of four surfaces that are now to be meshed with the smallest rectangular surface being mesh with uniform elements with the indicated size using a quadrilateral dominate mapped mesher. a. Meshing b. Surface c. Pick Surface d. Element Size 1.5 e. Quad Dominant f. OK

a b

c

d

e

f

CHAPTER 1 45 2-D Cylindrical Roller Contact

Create Mesh Seeds The upper quadrilateral surface curves are seeded appropriately, and the surface is meshed. A similar exercise is done for the lower quadrilateral surface (not shown). a. Meshing b. Seed: Arrows on Curves indicate direction for nonuniform mesh seed c. Surface OK

a b

c b

b

46 MD Demonstration Problems CHAPTER 1

Create Mesh Finally, the lower rectangular surface of the block is meshed using the mapped mesher with uniform element sizes. a. Meshing b. Surface c. Pick Surface d. Element Size 5 e. Quad Dominant f. OK g. Pick Surface h. Element Size 5 i. Quad Dominant j. OK

a b

c

d

e

g

h

f

i

j

CHAPTER 1 47 2-D Cylindrical Roller Contact

Enforce Consistent Normals Although the surfaces of the cylinder and block parts were stitched together, the surface mesher may create elements with inconsistent outward normals. This is the case here, and elements need to be fixed such that their outward normals all point in one direction (+z). This is done by showing the element normals, then fixing the normals using a reference element to set the normal direction. Continue this process until all normals are consistent; namely, they all point in the same direction. a. Quality b. Fix Elements c. Normals d. Show (Fix) Normals, click OK

a

b c

d d

48 MD Demonstration Problems CHAPTER 1

Define Material Data Materials are defined by naming the material (steel and Al, respectively) while entering the properties. The problem statement required that the cylinder be made of steel and the block made of aluminum (Al). Since the basic units selected have derived units of pressure (stress or modulus) as N   mm  2 , Young’s modulus for the steel is entered as 210x10 3 and 70x10 3 for aluminum. Poisson’s ratio is dimensionless and entered as 0.3 for both materials. a. Materials and Properties b. Isotropic c. steel, (properties); click OK d. Al, (properties as shown); click OK

• d. Al, (properties), OK

a

b

c

d

CHAPTER 1 49 2-D Cylindrical Roller Contact

Define Material Data The properties defined are now applied to the parts accordingly along with the planar element properties. Parts and materials are selected from the Model tree (not shown). a. Materials and Properties b. Plane c. Plane Property (cylinder and block); click OK

c. Plane Property (cylinder and block), OK a

b

c

50 MD Demonstration Problems CHAPTER 1

Contact Data for Cylinder Since the cylinder will come into contact with the block, contact data needs to be specified. A contact body consists of a set of elements and their associated nodes that are mutually exclusive from other elements. While we know that only a small number of elements in the cylinder and block will ultimately come into contact, there is no need to specify this information; the contact algorithm completely determines where and when contact happens. Hence, our choice is simple. We will create two contact bodies, consisting of all elements in the two parts we have defined: the cylinder and block. Although one might be tempted to only pick those elements suspected of coming into contact, it is best (and less time consuming) to just pick all the elements in the part as done here. a. Loads and Boundary Conditions (LBC) b. Deformable Body c. Select cylinder; click OK

• b. Deformable Body • c. Select cylinder, OK

a b

c

CHAPTER 1 51 2-D Cylindrical Roller Contact

Contact Data for Block Similar to the cylinder contact body, all elements in the block are selected to be in the next deformable contact body. a. Loads and Boundary Conditions (LBC) b. Deformable Body c. Select block; click OK

a b

• Define a deformable contact body for the block

c

52 MD Demonstration Problems CHAPTER 1

Define Contact Tables Although a contact table is not necessary for this particular problem (see BCONTACT = ALLBODY in the QRG), one is used here for illustration. Here, the contact table indicates that all contact bodies touch each other, including themselves. In general, contact tables describe how contact is to take place between contact bodies (touching, glue, none) and may change during the analysis by selecting different contact tables. A contact table allows one to define the coefficient of friction between the two touching bodies and its nonzero value overrides any previous value. a. Loads and Boundary Conditions (LBC) b. Table c. BCTABLE_INIT; click OK

• c. BCTABLE_INIT

a

b

c

CHAPTER 1 53 2-D Cylindrical Roller Contact

Define Constraints The horizontal component of displacement for all nodes on the symmetry plane is fixed to be zero by selecting the associated curves. a. Loads and Boundary Conditions (LBC) b. General c. Symmetry (Tx = 0 only) d. 5 Curves; click OK

y

y(

y)

• d. 5 Curves, OK

a

b

c

d

54 MD Demonstration Problems CHAPTER 1

Define Constraints The horizontal and vertical displacement components of all nodes on the bottom of the block are fixed by selecting the associated curve. a. Loads and Boundary Conditions (LBC) b. General c. Bottom (Tx, Ty = 0 only) d. 1 Curve; click OK

c. Bottom (Tx, Ty

0 only)

• d. 1 Curve, OK

a

b

c

d

CHAPTER 1 55 2-D Cylindrical Roller Contact

Define Point Load The load of 35 kN is applied to the top node in the downward direction. However, since only half of the material is being modeled because of the plane of symmetry, a load of 17.5 = 35/2 kN is applied to this “half” of the model. a. Loads and Boundary Conditions (LBC) b. Force c. 1 Node d. 17500, (direction); click OK

• d. 17500, (direction), OK

a

b

c d

56 MD Demonstration Problems CHAPTER 1

Create Nastran SOL 400 Job with Default Layout An analysis job is set up using a general nonlinear analysis type (SOL 400) and the name of the solver input file is specified. a. Right click File Set Create new Nastran job b. Job Name c. General Nonlinear Analysis (SOL 400) d. Name input file; click OK

p

a b

c d

CHAPTER 1 57 2-D Cylindrical Roller Contact

Create Nastran SOL 400 Job with Default Layout The global loadcase is created and the initial contact table is selected. a. Right click Load Cases b. Create Global Loadcase OK c. Under Global Loadcase, Right click Loads/Boundary Conditions d. Select Contact Table BCTABLE_INIT; click OK

a

c b

d

58 MD Demonstration Problems CHAPTER 1

Select Contact Table BCTABLE_INIT for Loadcase DefaultLoadCase The default loadcase is created using the same contact table. a. Right click Loads/Boundaries under DefaultLoadCase b. Select Contact Table c. Select Contact Table BCTABLE_INIT d. Click OK

c

d

a

b

CHAPTER 1 59 2-D Cylindrical Roller Contact

Define Large Disp. and Contact in SOL 400 Nonlinear Parameters Here, we are specifying some nonlinear parameters that allow forces to follow in a large displacement analysis and set the bias factor used in contact detection. a. Double click Solver Control b. Select Solution 400 Nonlinear Parameters c. Large Disp and Follower Force, Apply d. Contact Control Parameters e. Bias = 0.90 f. click Apply g. click Close

b

c a

d

e

f g

60 MD Demonstration Problems CHAPTER 1

Define Nonlinear Static Parameters Finishing the selection of nonlinear parameters, we select the stiffness update method along with convergence criteria. a. Loadcase Control b. Subcase Nonlinear Static Parameters c. Pure Full Newton, 1, 50 d. Check Displacement error, enter 1.0e-2 e. Check Force Error, enter 1.0e-2 f. Check Vector Component Method

b c

d a

e

f

CHAPTER 1 61 2-D Cylindrical Roller Contact

Request Output In order to visualize results, nodal and elemental output requests are made. a. Output Request b. Nodal Output Requests c. Create Constraint Force output Request; click OK d. Elemental Output e. Create “Nonlinear” Stress Output,; click OK

d a b c

e

62 MD Demonstration Problems CHAPTER 1

Run Analysis The preprocessing is now complete and the job is submitted. Upon successful completion of the job, the results are attached and visualized. a. Right click job, cylinder_roller_contact, under Simulations b. Run.

a

b

CHAPTER 1 63 2-D Cylindrical Roller Contact

Results The results are attached. a. Attach Results b. Select *_xdb file

a b Select *.xdb file

64 MD Demonstration Problems CHAPTER 1

Results - Fringe Plot A fringe plot of the Y-component of the Cauchy stress tensor is plotted below. a. Results b. Fringe c. Cauchy Stress d. Y Component e. Update

• b. Fringe • c. Cauchy Stress • d. Y Component • e. Update

a

b

e

c d

CHAPTER 1 65 2-D Cylindrical Roller Contact

Results - Chart Data Since the contact area is very small, it is useful to plot the Y component of Cauchy stress along the X component of the nodal positions, which is done by constructing the chart below. a. Results b. Chart c. Stress, Y Comp., Nodes d. Advanced Picking Tool e. From Curve f. Select Curve g. X Global h. Add Curves a. Results

• b. Chart • c. Stress, Y Comp., Nodes • d. Advanced Picking Tool • e. From Curve • f. Select Curve • g. X Global • h. Add Curves

b a d

h

c g

e

f

66 MD Demonstration Problems CHAPTER 1

Chart Data - Exporting Chart to Excel Ultimately, we wish to compare the data contained in the chart above with the analytical solution. The results in the chart can be extracted to the clipboard by selecting the Table under XY Chart Properties; then right click the table, Select All, and then copy. Once in the clipboard, the data can be pasted into Excel to be used in further comparisons. a. XY Chart Properties, Check Table b. Mouse on Table, Select All, Copy c. Paste into Excel

a

c

b

CHAPTER 1 67 2-D Cylindrical Roller Contact

Chart Data - Exporting Chart to Excel The chart data in the clipboard one pasted into Excel is then compared to the analytical solution. a. Plot with Analytical Solution in Excel

Chart Data - Exporting Chart to Excel • a. Plot with Analytical Solution in Excel a

68 MD Demonstration Problems CHAPTER 1

Input File(s) Snippets from the first four Nastran input files listed below are used to illustrate the simulation throughout various sections of this chapter except the section, Pre- and Postprocess with SimXpert. This later section illustrates the simulation using the SimXpert workspace environment, instead of the Nastran input file(s). While both illustrations ultimately lead to the same solution, viewing the simulation from these two different viewpoints facilitates a better understanding of how to perform the simulation. For example, nug_01am.dat, uses contact body IDs 5 and 6 as the set of elements for the block and cylinder, respectively; whereas the input file, ch01.bdf, (derived from the SimXpert workspace’s database, ch01.SimXpert) uses contact body IDs 1 and 2 as the set of elements for the block and cylinder, respectively. It is important to understand that while the contact bodies in these two input files are different (they use different IDs with a different set of elements), they yield the same solution since the loads, boundary conditions, and material properties are the same. File

Description

nug_01am.dat

Linear Elements Without Friction

nug_01aw.dat

Same as above but contact bodies are in wrong order

nug_01bm.dat

Linear Elements With Friction

nug_01cm.dat

Parabolic Elements Without Friction

nug_01dm.dat

Parabolic Elements With Friction

ch01.SimXpert

SimXpert Model

ch01.bdf

Nastran input model (Linear Elements Without Friction)