PDF
Contact Analysis of a Rubber Boot Seal
Introduction
Rubber boot seals are used in several industrial applications to protect flexible joints from dirt, dust, humidity and other environmental agents, as well as to prevent leakage of lubricants. In, for example, the automotive industry they are used for joints on the drive shaft among other applications. Many of these joints can undergo large deformations, hence a rubber boot seal needs to be designed to accommodate severe deformation, including both rotation and elongation, without breaking. To accomplish this the seals are generally made from synthetic elastomers that can be exposed to significant stretching without rupturing.
In this example, the deformation of a so-called multiconvolution boot seal connected to a rigid pipe is studied. As the pipe rotates and the seal deforms, the flanges of the seal self-intersect and it also come into contact with the pipe. This causes significant deformation of the rubber.
Model Definition
Figure 1 shows the geometry of the boot seal and the connected pipe. The seal has five convolutions with decreasing radius to seal the pipe to its mating surface.
]
Figure 1: Model geometry.
The pipe is in the example assumed be rigid and a generic rubber material is used for the boot seal. The mechanical behavior of the rubber is described by a nearly incompressible Yeoh hyperelastic model which isochoric strain energy is given as
where the material constants used are c1 = 100 kPa, c2 = 6 kPa, and c3 = 0 Pa.
The study is divided in two steps. In the first step the seal is mounted on the pipe which has a slightly larger diameter compared to the seal. This will create a shrink fit connection that ensures a tight seal. In the second step, a rotation of 40 degrees around the y-axis is incrementally applied to the bottom of the pipe. Given that the deformation is only applied around a single axis, one symmetry plane is utilized such that only half of the seal is modeled. The bottom of the seal is fixed in both study steps.
Since the pipe and seal are created as two disconnected parts in an assembly, a contact condition is set up between the exterior of the pipe and the interior of the seal. The contact condition also includes Coulomb friction with a friction coefficient equal to 0.7, which is representative for metal to rubber contact. Moreover, as the pipe is rotated the deformation of the seal will be large enough to cause its flanges to self-intersect. To avoid any unphysical overlap of boundaries, self-contact conditions are also set up for both the interior and exterior boundaries. Friction is also considered for these interactions with a friction coefficient equal to 0.8, which is typical for rubber to rubber contact. The Nitsche method is used to implement all contact conditions in the model since it has better accuracy compared to, for example, the penalty method. This is especially important for problems where the contact surfaces undergo large deformations as the seal in this example.
Results and Discussion
Figure 2 shows the deformed shape of the seal at the end of the second step at a 40-degree rotation of the pipe. It can clearly be seen how the flanges at the compressed side of the seal are folded and in contact with themselves. The highest stress in the seal is on the opposite side where it is stretched. Even though there are significant stress concentrations visible, the magnitude is still well below the typical tensile strength of rubber.
Figure 2: Deformed shape and stress distribution.
The deformation at different rotations of the pipe is shown in Figure 3 and the surfaces in contact at the final step are highlighted in Figure 4. In the latter figure on can clearly see that contact occurs between both interior and exterior surface of the seal, but also between the seal and the pipe at different locations.
Figure 3: Deformed shape at increasing rotations of the pipe. Displacement are given in millimeters.
Figure 4: Parts of the surface of the seal in contact with another surface highlighted in red.
Notes About the COMSOL Implementation
Self-contact is in COMSOL Multiphysics modeled by selecting the same boundaries as source and destination in a Contact Pair. Here three contact pairs are used, one with an unsymmetric selection to set up contact between the pipe and the interior of the seal, and two with a symmetric selection to define self-contact between the interior and exterior surfaces of the seal.
When modeling self-contact of convoluted surfaces it is recommended to manually control the search distance of the Contact Pair. The automatic search distance is based on the size of the geometry and can lead to false detection of contact points on, for example, the backside of the surface at which considered the contact point is located. Here a much smaller search distance is used for the two contact pairs used for the self-contact. Apart from making the contact search more robust, using a smaller search distance will also improve the performance of the search algorithm.
Application Library path: Nonlinear_Structural_Materials_Module/Hyperelasticity/rubber_boot_seal
Modeling Instructions
From the File menu, choose New.
New
In the New window, click  Model Wizard.
Model Wizard
1
In the Model Wizard window, click  3D.
2
In the Select Physics tree, select Structural Mechanics > Solid Mechanics (solid).
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select General Studies > Stationary.
6
Click  Done.
Global Definitions
Parameters 1
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
overlap
1[mm]
0.001 m
Shrink fit overlap
para1
0
0
Continuation parameter, step 1
para2
0
0
Continuation parameter, step 2
Geometry 1
The geometry sequence for the model is available in a file. If you want to create it from scratch yourself, you can follow the instructions in the Appendix — Geometry Modeling Instructions section. Otherwise, insert the geometry sequence as follows:
1
In the Geometry toolbar, click Insert Sequence and choose Insert Sequence.
2
Browse to the model’s Application Libraries folder and double-click the file rubber_boot_seal_geom_sequence.mph.
Cylinder 1 (cyl1)
The outer radius of the cylinder is larger than the inner radius in order to create a shrink fit.
1
In the Model Builder window, under Component 1 (comp1) > Geometry 1 click Cylinder 1 (cyl1).
2
In the Settings window for Cylinder, locate the Size and Shape section.
3
In the Radius text field, type (60)/2-3+overlap.
4
In the Geometry toolbar, click  Build All.
Definitions
Contact Surface, Outside
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type Contact Surface, Outside in the Label text field.
3
Locate the Input Entities section. From the Geometric entity level list, choose Boundary.
4
Select Boundaries 63, 66, 69, 75, 79, 83, 87, 91, and 95 only.
Contact Surface, Inside
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type Contact Surface, Inside in the Label text field.
3
Locate the Input Entities section. From the Geometric entity level list, choose Boundary.
4
Select Boundaries 70, 71, 73, 80, 81, 88, 89, 96, and 97 only.
Contact Pair 1 (p1)
1
In the Definitions toolbar, click  Pairs and choose Contact Pair.
2
Select Boundaries 116 and 124 only.
3
In the Settings window for Pair, locate the Destination Boundaries section.
4
Click to select the  Activate Selection toggle button.
5
Select Boundaries 41, 51, 53, 56, 70, 80, 88, and 96 only.
Contact Pair 2 (p2)
1
In the Definitions toolbar, click  Pairs and choose Contact Pair.
To model self-contact, select the same boundaries as source and destination.
2
In the Settings window for Pair, locate the Source Boundaries section.
3
From the Selection list, choose Contact Surface, Outside.
4
Locate the Destination Boundaries section. From the Selection list, choose Contact Surface, Outside.
5
Locate the Advanced section. From the Search distance list, choose Manual.
The automatic search distance is based on the size of the geometry. Use a smaller search distance to improve performance and also to avoid detecting false contact points due to the convoluted geometry of the seal.
6
In the Distance text field, type 1.
Contact Pair 3 (p3)
1
In the Definitions toolbar, click  Pairs and choose Contact Pair.
2
In the Settings window for Pair, locate the Source Boundaries section.
3
From the Selection list, choose Contact Surface, Inside.
4
Locate the Destination Boundaries section. From the Selection list, choose Contact Surface, Inside.
5
Locate the Advanced section. From the Search distance list, choose Manual.
6
In the Distance text field, type 1.
Solid Mechanics (solid)
Hyperelastic Material 1
1
In the Physics toolbar, click  Domains and choose Hyperelastic Material.
2
In the Settings window for Hyperelastic Material, locate the Domain Selection section.
3
From the Selection list, choose All domains.
4
Locate the Hyperelastic Material section. From the Material model list, choose Yeoh.
5
From the Volumetric strain energy list, choose Hartmann–Neff.
The pipe is assumed to be rigid.
Rigid Material 1
1
In the Physics toolbar, click  Domains and choose Rigid Material.
2
Select Domains 25 and 26 only.
Prescribed Displacement/Rotation 1
1
In the Physics toolbar, click  Attributes and choose Prescribed Displacement/Rotation.
Apply a rotation around the y-axis at the bottom of the pipe in the second study step using para2.
2
In the Settings window for Prescribed Displacement/Rotation, locate the Center of Rotation section.
3
From the list, choose Centroid of selected entities.
4
Locate the Prescribed Displacement at Center of Rotation section. Select the Prescribed in x direction checkbox.
5
Select the Prescribed in y direction checkbox.
6
Select the Prescribed in z direction checkbox.
7
Locate the Prescribed Rotation section. From the By list, choose Prescribed rotation.
8
Specify the Ω vector as
0
x
1
y
0
z
9
In the ϕ0 text field, type 40[deg]*para2.
Center of Rotation: Boundary 1
1
In the Model Builder window, click Center of Rotation: Boundary 1.
2
Select Boundaries 117 and 122 only.
Contact (Pipe-Seal)
The Nitsche contact method is better at resolving the contact condition for large deformation problems.
1
In the Model Builder window, under Component 1 (comp1) > Solid Mechanics (solid) click Contact 1.
2
In the Settings window for Contact, locate the Contact Method section.
3
From the list, choose Nitsche.
Create the shrink fit at the top connection of the seal to the pipe by adding an offset to the destination surface that will be removed incrementally.
4
Click to expand the Contact Surface Offset and Adjustment section. In the doffset,s text field, type -overlap*(1-min(para1,1)).
5
In the Label text field, type Contact (Pipe-Seal).
Friction 1
1
In the Physics toolbar, click  Attributes and choose Friction.
2
In the Settings window for Friction, locate the Friction Parameters section.
3
In the μ text field, type 0.7.
Add a second Contact node for the self-contact of the rubber seal.
Contact (Seal-Seal)
1
In the Physics toolbar, click  Pairs and choose Contact.
2
In the Settings window for Contact, locate the Pair Selection section.
3
Click  Add.
4
In the Add dialog, in the Pairs list, choose Contact Pair 2 (p2) and Contact Pair 3 (p3).
5
Click OK.
6
In the Settings window for Contact, locate the Contact Method section.
7
From the list, choose Nitsche.
8
In the Label text field, type Contact (Seal-Seal).
Friction 1
1
In the Physics toolbar, click  Attributes and choose Friction.
2
In the Settings window for Friction, locate the Friction Parameters section.
3
In the μ text field, type 0.8.
Symmetry 1
1
In the Physics toolbar, click  Boundaries and choose Symmetry.
2
Select Boundaries 1, 3, 7, 12, 15, 20, 23, 28, 33, 36, 39, 45, and 103–114 only.
Fixed Constraint 1
1
In the Physics toolbar, click  Boundaries and choose Fixed Constraint.
2
Select Boundaries 9 and 100 only.
Roller 1
1
In the Physics toolbar, click  Boundaries and choose Roller.
2
Select Boundaries 11 and 99 only.
Add Material
1
In the Materials toolbar, click  Add Material to open the Add Material window.
2
Go to the Add Material window.
3
In the tree, select Built-in > Rubber.
4
Click the Add to Component button in the window toolbar.
5
In the Materials toolbar, click  Add Material to close the Add Material window.
Mesh 1
Mapped 1
1
In the Mesh toolbar, click  More Generators and choose Mapped.
2
Select Boundaries 1, 3, 7, 12, 15, 20, 23, 28, 33, 36, 39, 45, 126, 128, 132, 135, 138, 141, and 142 only.
Size 1
1
Right-click Mapped 1 and choose Size.
2
In the Settings window for Size, locate the Element Size section.
3
Click the Custom button.
4
Locate the Element Size Parameters section.
5
Select the Maximum element size checkbox. In the associated text field, type 5.
Distribution 1
1
In the Model Builder window, right-click Mapped 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
In the Number of elements text field, type 2.
4
Select Edges 6, 8, 16, 18, 26, 28, 34, 36, 44, 46, 51, 59, 62, and 246 only.
Distribution 2
1
Right-click Mapped 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
In the Number of elements text field, type 6.
4
Select Edges 20, 30, 38, and 53 only.
Mapped 2
1
In the Mesh toolbar, click  More Generators and choose Mapped.
2
Select Boundary 115 only.
Distribution 1
1
Right-click Mapped 2 and choose Distribution.
2
In the Settings window for Distribution, locate the Edge Selection section.
3
From the Selection list, choose All edges.
4
Locate the Distribution section. In the Number of elements text field, type 1.
Swept 1
1
In the Mesh toolbar, click  Swept.
2
In the Settings window for Swept, click to expand the Control Entities section.
3
From the Smooth across removed control entities list, choose Off.
Distribution 1
1
Right-click Swept 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
From the Distribution type list, choose Predefined.
4
In the Number of elements text field, type 16.
5
In the Element ratio text field, type 3.
Distribution 2
1
Right-click Distribution 1 and choose Duplicate.
2
Select Domains 13–24 and 36–40 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
Select the Reverse direction checkbox.
Distribution 3
1
In the Model Builder window, right-click Swept 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Domain Selection section.
3
Click  Clear Selection.
4
Select Domains 25 and 26 only.
5
Locate the Distribution section. In the Number of elements text field, type 25.
6
Click  Build All.
Study 1
Step 1: Stationary
1
In the Model Builder window, under Study 1 click Step 1: Stationary.
2
In the Settings window for Stationary, click to expand the Results While Solving section.
3
Select the Plot checkbox.
4
From the Update at list, choose Steps taken by solver.
Incrementally remove the contact surface offset so that the shrink fit is created in the first study step using para1.
5
Click to expand the Study Extensions section. Select the Auxiliary sweep checkbox.
6
Click  Add.
7
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
para1 (Continuation parameter, step 1)
0 1
 
Add a second study step where the pipe is rotated using para2 while para1 is kept constant.
Step 2: Stationary 2
1
In the Study toolbar, click  Stationary.
2
In the Settings window for Stationary, locate the Results While Solving section.
3
Select the Plot checkbox.
4
From the Update at list, choose Steps taken by solver.
5
Locate the Study Extensions section. Select the Auxiliary sweep checkbox.
6
Click  Add.
7
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
para1 (Continuation parameter, step 1)
1
 
8
Click  Add.
9
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
para2 (Continuation parameter, step 2)
range(0,0.1,1)
 
10
From the Sweep type list, choose All combinations.
The robustness and performance of the solution can be improved by making some modifications to the default solver.
Solution 1 (sol1)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 1 (sol1) node.
3
In the Model Builder window, expand the Study 1 > Solver Configurations > Solution 1 (sol1) > Dependent Variables 1 node, then click Auxiliary Pressure (comp1.solid.hmm1.pw).
4
In the Settings window for Field, locate the Scaling section.
5
In the Scale text field, type 1e5.
6
In the Model Builder window, expand the Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 1 node, then click Parametric 1.
7
In the Settings window for Parametric, click to expand the Continuation section.
8
Select the Tuning of step size checkbox.
9
In the Maximum step size text field, type 0.5.
10
In the Model Builder window, under Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 1 click Fully Coupled 1.
11
In the Settings window for Fully Coupled, click to expand the Method and Termination section.
12
From the Nonlinear method list, choose Constant (Newton).
13
In the Maximum number of iterations text field, type 8.
14
In the Model Builder window, expand the Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 2 node.
15
In the Model Builder window, expand the Study 1 > Solver Configurations > Solution 1 (sol1) > Dependent Variables 2 node, then click Auxiliary Pressure (comp1.solid.hmm1.pw).
16
In the Settings window for Field, locate the Scaling section.
17
In the Scale text field, type 1e5.
18
In the Model Builder window, under Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 2 click Parametric 1.
19
In the Settings window for Parametric, locate the Continuation section.
20
Select the Tuning of step size checkbox.
21
In the Initial step size text field, type 0.005.
22
In the Maximum step size text field, type 0.025.
23
In the Model Builder window, under Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 2 click Fully Coupled 1.
24
In the Settings window for Fully Coupled, locate the Method and Termination section.
25
From the Nonlinear method list, choose Constant (Newton).
26
In the Maximum number of iterations text field, type 8.
27
In the Study toolbar, click  Compute.
Results
Stress (solid)
Click the  Go to Default View button in the Graphics toolbar.
Volume 1
1
In the Model Builder window, expand the Stress (solid) node, then click Volume 1.
2
In the Settings window for Volume, locate the Expression section.
3
From the Unit list, choose MPa.
4
In the Stress (solid) toolbar, click  Plot.
Plot the deformed boot seal at different solution parameters.
Mirror 3D 1
1
In the Results toolbar, click  More Datasets and choose Mirror 3D.
2
In the Settings window for Mirror 3D, locate the Plane Data section.
3
From the Plane list, choose ZX-planes.
Displacement
1
In the Results toolbar, click  3D Plot Group.
2
In the Settings window for 3D Plot Group, type Displacement in the Label text field.
3
Click to expand the Title section. From the Title type list, choose None.
4
Locate the Plot Settings section. Clear the Plot dataset edges checkbox.
5
Click to expand the Plot Array section. From the Array type list, choose Square.
6
From the Array plane list, choose xz.
Surface 1
1
Right-click Displacement and choose Surface.
2
In the Settings window for Surface, locate the Coloring and Style section.
3
From the Color table list, choose SpectrumLight.
4
Locate the Data section. From the Dataset list, choose Mirror 3D 1.
Deformation 1
1
Right-click Surface 1 and choose Deformation.
2
In the Settings window for Deformation, locate the Scale section.
3
Select the Scale factor checkbox. In the associated text field, type 1.
Solution Array 1
1
In the Model Builder window, right-click Surface 1 and choose Solution Array.
2
In the Settings window for Solution Array, locate the Data section.
3
From the Parameter selection (para2) list, choose From list.
4
In the Parameter values (para2) list, choose 0, 0.2, 0.4, 0.6, 0.8, and 1.
5
Locate the Plot Array section. From the Array shape list, choose Square.
6
In the Displacement toolbar, click  Plot.
Contact Area
1
In the Results toolbar, click  3D Plot Group.
Create a plot highlighting boundaries that are in contact.
2
In the Settings window for 3D Plot Group, type Contact Area in the Label text field.
3
Locate the Title section. From the Title type list, choose None.
4
Locate the Plot Settings section. From the Frame list, choose Spatial  (x, y, z).
Surface 1
1
Right-click Contact Area and choose Surface.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type if(elemgpmax(8,solid.incontact),1,NaN).
4
Locate the Coloring and Style section. From the Coloring list, choose Uniform.
Deformation 1
1
Right-click Surface 1 and choose Deformation.
2
In the Settings window for Deformation, locate the Scale section.
3
Select the Scale factor checkbox. In the associated text field, type 1.
Selection 1
1
In the Model Builder window, right-click Surface 1 and choose Selection.
2
In the Settings window for Selection, locate the Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domains 1–24 only.
Surface 2
1
In the Model Builder window, right-click Contact Area and choose Surface.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type 1.
4
Locate the Coloring and Style section. From the Coloring list, choose Uniform.
5
From the Color list, choose Gray.
Deformation 1
1
Right-click Surface 2 and choose Deformation.
2
In the Settings window for Deformation, locate the Scale section.
3
Select the Scale factor checkbox. In the associated text field, type 1.
Transparency 1
1
In the Model Builder window, right-click Surface 2 and choose Transparency.
2
In the Settings window for Transparency, locate the Transparency section.
3
Find the Transparency subsection. In the Transparency text field, type 0.8.
4
Find the Fresnel transmittance subsection. In the Fresnel transmittance text field, type 0.2.
5
In the Contact Area toolbar, click  Plot.
Appendix — Geometry Modeling Instructions
From the File menu, choose New.
New
In the New window, click  Model Wizard.
Model Wizard
1
In the Model Wizard window, click  3D.
2
Click  Done.
Geometry 1
1
In the Model Builder window, under Component 1 (comp1) click Geometry 1.
2
In the Settings window for Geometry, locate the Units section.
3
From the Length unit list, choose mm.
Work Plane 1 (wp1)
1
In the Geometry toolbar, click  Work Plane.
2
In the Settings window for Work Plane, locate the Plane Definition section.
3
From the Plane list, choose yz-plane.
Work Plane 1 (wp1) > Plane Geometry
In the Model Builder window, click Plane Geometry.
Work Plane 1 (wp1) > Polygon 1 (pol1)
1
In the Work Plane toolbar, click  Polygon.
2
In the Settings window for Polygon, locate the Object Type section.
3
From the Type list, choose Open curve.
4
Locate the Coordinates section. In the table, enter the following settings:
xw (mm)
yw (mm)
100
20
100
0
Work Plane 1 (wp1) > Quadratic Bézier 1 (qb1)
1
In the Work Plane toolbar, click  More Primitives and choose Quadratic Bézier.
2
In the Settings window for Quadratic Bézier, locate the Control Points section.
3
In row 1, set xw to 100.
4
In row 1, set yw to 20.
5
In row 2, set xw to 110.
6
In row 2, set yw to 35.
7
In row 3, set xw to 110.
8
In row 3, set yw to 45.
Work Plane 1 (wp1) > Quadratic Bézier 2 (qb2)
1
In the Work Plane toolbar, click  More Primitives and choose Quadratic Bézier.
2
In the Settings window for Quadratic Bézier, locate the Control Points section.
3
In row 1, set xw to 110.
4
In row 1, set yw to 45.
5
In row 2, set xw to 110.
6
In row 2, set yw to 52.
7
In row 3, set xw to 90.
8
In row 3, set yw to 55.
Work Plane 1 (wp1) > Circular Arc 1 (ca1)
1
In the Work Plane toolbar, click  More Primitives and choose Circular Arc.
2
In the Settings window for Circular Arc, locate the Properties section.
3
From the Specify list, choose Endpoints and start angle.
4
Locate the Starting Point section. In the xw text field, type 90.
5
In the yw text field, type 55.
6
Locate the Endpoint section. In the xw text field, type 90.
7
In the yw text field, type 58.
8
Locate the Angles section. In the Start angle text field, type -55.
9
Select the Clockwise checkbox.
Work Plane 1 (wp1) > Quadratic Bézier 3 (qb3)
1
In the Work Plane toolbar, click  More Primitives and choose Quadratic Bézier.
2
In the Settings window for Quadratic Bézier, locate the Control Points section.
3
In row 1, set xw to 90.
4
In row 1, set yw to 58.
5
In row 2, set xw to 110.
6
In row 2, set yw to 65.
7
In row 3, set xw to 110.
8
In row 3, set yw to 73.
Work Plane 1 (wp1) > Quadratic Bézier 4 (qb4)
1
In the Work Plane toolbar, click  More Primitives and choose Quadratic Bézier.
2
In the Settings window for Quadratic Bézier, locate the Control Points section.
3
In row 1, set xw to 110.
4
In row 1, set yw to 73.
5
In row 2, set xw to 110.
6
In row 2, set yw to 80.
7
In row 3, set xw to 76.
8
In row 3, set yw to 85.
Work Plane 1 (wp1) > Circular Arc 2 (ca2)
1
In the Work Plane toolbar, click  More Primitives and choose Circular Arc.
2
In the Settings window for Circular Arc, locate the Properties section.
3
From the Specify list, choose Endpoints and start angle.
4
Locate the Starting Point section. In the xw text field, type 76.
5
In the yw text field, type 85.
6
Locate the Endpoint section. In the xw text field, type 76.
7
In the yw text field, type 88.
8
Locate the Angles section. In the Start angle text field, type -55.
9
Select the Clockwise checkbox.
Work Plane 1 (wp1) > Copy 1 (copy1)
1
In the Work Plane toolbar, click  Transforms and choose Copy.
2
Select the objects ca2, qb3, and qb4 only.
3
In the Settings window for Copy, locate the Displacement section.
4
In the xw text field, type -14 -28.
5
In the yw text field, type 30 60.
Work Plane 1 (wp1) > Quadratic Bézier 5 (qb5)
1
In the Work Plane toolbar, click  More Primitives and choose Quadratic Bézier.
2
In the Settings window for Quadratic Bézier, locate the Control Points section.
3
In row 1, set xw to 48.
4
In row 1, set yw to 148.
5
In row 2, set xw to 58.
6
In row 2, set yw to 150.
7
In row 3, set xw to 58.
8
In row 3, set yw to 164.
Work Plane 1 (wp1) > Quadratic Bézier 6 (qb6)
1
In the Work Plane toolbar, click  More Primitives and choose Quadratic Bézier.
2
In the Settings window for Quadratic Bézier, locate the Control Points section.
3
In row 1, set xw to 58.
4
In row 1, set yw to 164.
5
In row 2, set xw to 58.
6
In row 2, set yw to 174.
7
In row 3, set xw to 48.
8
In row 3, set yw to 174.
Work Plane 1 (wp1) > Quadratic Bézier 7 (qb7)
1
In the Work Plane toolbar, click  More Primitives and choose Quadratic Bézier.
2
In the Settings window for Quadratic Bézier, locate the Control Points section.
3
In row 1, set xw to 48.
4
In row 1, set yw to 174.
5
In row 2, set xw to 30.
6
In row 2, set yw to 174.
7
In row 3, set xw to 30.
8
In row 3, set yw to 195.
Work Plane 1 (wp1) > Polygon 2 (pol2)
1
In the Work Plane toolbar, click  Polygon.
2
In the Settings window for Polygon, locate the Object Type section.
3
From the Type list, choose Open curve.
4
Locate the Coordinates section. In the table, enter the following settings:
xw (mm)
yw (mm)
30
195
30
225
Work Plane 1 (wp1) > Union 1 (uni1)
1
In the Work Plane toolbar, click  Booleans and Partitions and choose Union.
2
Click in the Graphics window and then press Ctrl+A to select all objects.
Work Plane 1 (wp1) > Thicken 1 (thi1)
1
In the Work Plane toolbar, click  Conversions and choose Thicken.
2
Select the object uni1 only.
3
In the Settings window for Thicken, locate the Options section.
4
From the Offset list, choose Asymmetric.
5
In the Upside thickness text field, type 3.
Work Plane 1 (wp1) > Fillet 1 (fil1)
1
In the Work Plane toolbar, click  Fillet.
2
On the object thi1, select Points 21, 28, 36, and 37 only.
3
In the Settings window for Fillet, locate the Radius section.
4
In the Radius text field, type 1.
Work Plane 1 (wp1) > Fillet 2 (fil2)
1
In the Work Plane toolbar, click  Fillet.
2
On the object fil1, select Points 5, 6, 9, 10, 13–20, 25–28, and 37 only.
3
In the Settings window for Fillet, locate the Radius section.
4
In the Radius text field, type 1.5.
Work Plane 1 (wp1) > Rectangle 1 (r1)
1
In the Work Plane toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 5.
4
In the Height text field, type 5.
5
Locate the Position section. In the xw text field, type 27.
6
In the yw text field, type 220.
Work Plane 1 (wp1) > Plane Geometry
Partition the domain to facilitate better control of the mesh.
Work Plane 1 (wp1) > Line Segment 1 (ls1)
1
In the Work Plane toolbar, click  More Primitives and choose Line Segment.
2
On the object fil2, select Point 50 only.
3
In the Settings window for Line Segment, locate the Endpoint section.
4
Click to select the  Activate Selection toggle button for End vertex.
5
On the object fil2, select Point 53 only.
6
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 2 (ls2)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 1 (ls1) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 51 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 54 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 3 (ls3)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 2 (ls2) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 58 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 61 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 4 (ls4)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 3 (ls3) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 57 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 60 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 5 (ls5)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 4 (ls4) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 44 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 42 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 6 (ls6)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 5 (ls5) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 40 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 38 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 7 (ls7)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 6 (ls6) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 39 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 37 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 8 (ls8)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 7 (ls7) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 41 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 43 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 9 (ls9)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 8 (ls8) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 56 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 62 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 10 (ls10)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 9 (ls9) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 55 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 59 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 11 (ls11)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 10 (ls10) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 32 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 30 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 12 (ls12)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 11 (ls11) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 28 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 26 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 13 (ls13)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 12 (ls12) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 27 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 25 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 14 (ls14)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 13 (ls13) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 29 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 31 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 15 (ls15)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 14 (ls14) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 46 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 48 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 16 (ls16)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 15 (ls15) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 45 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 47 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 17 (ls17)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 16 (ls16) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 24 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 22 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 18 (ls18)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 17 (ls17) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 20 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 18 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 19 (ls19)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 18 (ls18) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 19 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 17 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 20 (ls20)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 19 (ls19) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 21 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 23 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 21 (ls21)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 20 (ls20) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 34 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 36 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 22 (ls22)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 21 (ls21) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 33 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 35 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 23 (ls23)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 22 (ls22) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 14 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 11 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 24 (ls24)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 23 (ls23) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 10 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 6 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 25 (ls25)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 24 (ls24) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 7 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 5 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 26 (ls26)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 25 (ls25) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 13 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 12 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 27 (ls27)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 26 (ls26) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 15 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 16 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 28 (ls28)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 27 (ls27) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 8 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 9 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 29 (ls29)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Line Segment 28 (ls28) and choose Duplicate.
2
In the Settings window for Line Segment, locate the Starting Point section.
3
Click to select the  Activate Selection toggle button for Start vertex.
4
On the object fil2, select Point 1 only.
5
Locate the Endpoint section. Click to select the  Activate Selection toggle button for End vertex.
6
On the object fil2, select Point 3 only.
7
Click  Build Selected.
Work Plane 1 (wp1) > Line Segment 1 (ls1), Work Plane 1 (wp1) > Line Segment 10 (ls10), Work Plane 1 (wp1) > Line Segment 11 (ls11), Work Plane 1 (wp1) > Line Segment 12 (ls12), Work Plane 1 (wp1) > Line Segment 13 (ls13), Work Plane 1 (wp1) > Line Segment 14 (ls14), Work Plane 1 (wp1) > Line Segment 15 (ls15), Work Plane 1 (wp1) > Line Segment 16 (ls16), Work Plane 1 (wp1) > Line Segment 17 (ls17), Work Plane 1 (wp1) > Line Segment 18 (ls18), Work Plane 1 (wp1) > Line Segment 19 (ls19), Work Plane 1 (wp1) > Line Segment 2 (ls2), Work Plane 1 (wp1) > Line Segment 20 (ls20), Work Plane 1 (wp1) > Line Segment 21 (ls21), Work Plane 1 (wp1) > Line Segment 22 (ls22), Work Plane 1 (wp1) > Line Segment 23 (ls23), Work Plane 1 (wp1) > Line Segment 24 (ls24), Work Plane 1 (wp1) > Line Segment 25 (ls25), Work Plane 1 (wp1) > Line Segment 26 (ls26), Work Plane 1 (wp1) > Line Segment 27 (ls27), Work Plane 1 (wp1) > Line Segment 28 (ls28), Work Plane 1 (wp1) > Line Segment 29 (ls29), Work Plane 1 (wp1) > Line Segment 3 (ls3), Work Plane 1 (wp1) > Line Segment 4 (ls4), Work Plane 1 (wp1) > Line Segment 5 (ls5), Work Plane 1 (wp1) > Line Segment 6 (ls6), Work Plane 1 (wp1) > Line Segment 7 (ls7), Work Plane 1 (wp1) > Line Segment 8 (ls8), Work Plane 1 (wp1) > Line Segment 9 (ls9)
1
In the Model Builder window, under Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry, Ctrl-click to select Line Segment 1 (ls1), Line Segment 2 (ls2), Line Segment 3 (ls3), Line Segment 4 (ls4), Line Segment 5 (ls5), Line Segment 6 (ls6), Line Segment 7 (ls7), Line Segment 8 (ls8), Line Segment 9 (ls9), Line Segment 10 (ls10), Line Segment 11 (ls11), Line Segment 12 (ls12), Line Segment 13 (ls13), Line Segment 14 (ls14), Line Segment 15 (ls15), Line Segment 16 (ls16), Line Segment 17 (ls17), Line Segment 18 (ls18), Line Segment 19 (ls19), Line Segment 20 (ls20), Line Segment 21 (ls21), Line Segment 22 (ls22), Line Segment 23 (ls23), Line Segment 24 (ls24), Line Segment 25 (ls25), Line Segment 26 (ls26), Line Segment 27 (ls27), Line Segment 28 (ls28), and Line Segment 29 (ls29).
2
Right-click and choose Group.
Partition Objects
In the Settings window for Group, type Partition Objects in the Label text field.
Revolve 1 (rev1)
1
In the Model Builder window, under Component 1 (comp1) > Geometry 1 right-click Work Plane 1 (wp1) and choose Revolve.
2
In the Settings window for Revolve, locate the Revolution Angles section.
3
Click the Angles button.
4
In the Start angle text field, type -90.
5
In the End angle text field, type 90.
Partition Objects 1 (par1)
1
In the Geometry toolbar, click  Booleans and Partitions and choose Partition Objects.
2
Select the object rev1 only.
3
In the Settings window for Partition Objects, locate the Partition Objects section.
4
From the Partition with list, choose Work plane.
Cylinder 1 (cyl1)
1
In the Geometry toolbar, click  Cylinder.
2
In the Settings window for Cylinder, locate the Size and Shape section.
3
In the Radius text field, type (60)/2-3.
4
In the Height text field, type 275.
5
Locate the Position section. In the z text field, type -10.
6
Click to expand the Layers section. In the table, enter the following settings:
Layer name
Thickness (mm)
Layer 1
3
Delete Entities 1 (del1)
1
In the Model Builder window, right-click Geometry 1 and choose Delete Entities.
2
In the Settings window for Delete Entities, locate the Entities or Objects to Delete section.
3
From the Geometric entity level list, choose Domain.
4
On the object cyl1, select Domains 1, 3, and 4 only.
Form Union (fin)
1
In the Model Builder window, under Component 1 (comp1) > Geometry 1 click Form Union (fin).
2
In the Settings window for Form Union/Assembly, locate the Form Union/Assembly section.
3
From the Action list, choose Form an assembly.
4
Clear the Create pairs checkbox.
Ignore Faces 1 (igf1)
1
In the Geometry toolbar, click  Virtual Operations and choose Ignore Faces.
2
On the object fin, select Boundaries 12, 15, 25, 38, 44, 47, 62, 68, 71, 81, 84, 101, 104, 162, 165, 182, 185, 201, 204, 210, 225, 228, 234, 244, 251, and 255 only.
Mesh Control Faces 1 (mcf1)
1
In the Geometry toolbar, click  Virtual Operations and choose Mesh Control Faces.
2
On the object igf1, select Boundaries 4, 9, 23, 35, 51, 73, 74, 85, 90, 109, 132, 144, 153, and 154 only.
3
In the Settings window for Mesh Control Faces, click  Build Selected.