Ug Nx Dau Mt10055 Workbook Design Applications Using Unigrap

DESIGN APPLICATIONS USING

UNIGRAPHICS

WORKBOOK

September 2002

MT10055 - Unigraphics NX

EDS Inc.

NIGRAPHICS

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Design Applications Using Unigraphics Workbook Publication History:

Version 15.0

February 1999

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Version 16.0

January 2000

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Version 17.0

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Version 18.0

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Unigraphics NX

September 2002

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Impeller Assembly - An approach in methodology

Design Applications Using

Unigraphics Workbook

-1

EDS

Impeller Assembly - An approach in methodology

The Impeller assembly is a conceptual design for a mechanism to translate

water flow into axile rotation. For this course, consider the design to be in

progress and know that it will not be totally completed in this class.

The design you will model may or may not be the correct approach. This in

itself mimics real life situations. As a design is reviewed by different disciplines,

it matures from the recommendations made by those disciplines. In this class,

what is more important is gaining an understanding of the methodology of using

a combination of Unigraphics functions to capture an aspect of the total design

intent.

Below is an illustration of the Impeller assembly you will model.

Impeller Assembly - An approach in methodology

Design Applications Using

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ÉÉÉ

Creating the Inner Moldline of the Bottom Housing

Design Applications Using

Unigraphics Workbook

1-1

EDS

Creating the Inner Moldline of the Bottom Housing

Section 1

The design intent for the bottom housing is that its size and shape be controlled

parametrically. This will be achieved by creating a sketch that defines the inner

moldline of the bottom housing. This same sketch will also be used later to

define the outside shape of the impeller.

Inner Moldline Sketch

inside_radius=15.000

p1=7.380

p2=33.000

p3=8.000

p4=1.000

p5=25.500

ÉÉÉ

Creating the Inner Moldline of the Bottom Housing

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Step 1 Using the seedpart file, dau_seedpart_in, create a new

(inch) part file called ***_housing_bottom.

Step 2 Create Generator geometry for the inside moldline.

Since one of the design requirements is that the size and shape be controlled

parametrically, the inside moldline will be sketched.

NOTE: Keep class layer standards in mind.

Create a sketch named, moldline, on the X-Z absolute

coordinate plane.

ÉÉÉ

Creating the Inner Moldline of the Bottom Housing

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1-3

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Sketch the curves as illustrated below and apply the required

constraints. Rename one of the constraints as shown below.

This is being done so that this constraint may be identified

easier, later in the course.

The inside moldline is made up of two lines and two arcs.

Curves that have a common end point should be constrained

tangent to each other.

The left endpoint of the lower left horizontal line is located

Point onto Curve relative to the vertical datum axis.

The two lines should have horizontal constraints.

R p2=33.000

p5=25.500

p4=7.380

p6=8.000

p7=1.000

Reference

Features

inside_radius=15.000

Name this

constraint as

shown

Step 3 Save the part and close.

ÉÉÉ

Creating the Inner Moldline of the Bottom Housing

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Creating the Bottom Housing

Design Applications Using

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2-1

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Creating the Bottom Housing

Section 2

In the previous section, an aspect of the design intent for the bottom housing

was captured by creating a sketch that controlled the size and shape of the

inner moldline. In this section of the activity you will continue to capture

additional design intent for the bottom housing. The additional aspects are:

The flange width is based on hole size

The number of holes are controlled parametrically

Bottom Housing

ÉÉÉ

Creating the Bottom Housing

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Step 1 Open ***_housing_bottom.

Step 2 Orient the WCS to the Absolute CSYS.

Step 3 Revolve the sketch geometry to create the housing body.

Create the body of revolution as illustrated below. The wall thickness is 0.5".

Remember, the sketch is defining the inside moldline.

Define the revolution by using the sketch datum axis that is parallel to the XC

axis.

Delta angle is 180

NOTE: Using a start angle of -90_ and an end angle of 90_ will

give the desired orientation as shown below.

ÉÉÉ

Creating the Bottom Housing

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Step 4 Create a variable expression.

In creating the flanges for this part, a couple of design issues need to be taken

into consideration.

First, when adding the flange, the length of the part should not increase.

Second, the allowance for hole size and edge distance determine flange

width.

For our design the hole diameter is 0.75 and the edge distance is 2D (2 x the

diameter). These circumstances provide a good opportunity to create an

expression for the hole size. This variable can then be referenced in other

features that rely on its value.

Create the following expression variable:

hole_dia=.75

Step 5 Create the first end flange.

Extrude and unite the solid edge illustrated below.

The extrusion should not change the length (along the XC

axis) of the solid body.

Use the following values:

Start Distance = 0

End Distance = .5

First Offset = 0

Second Offset = 1.25+3*hole_dia

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Creating the Bottom Housing

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NOTE: The polarity (+/-) of the second offset value will vary

depending on the direction of the offset vector.

Select this edge

Your part should now resemble the illustration below.

ÉÉÉ

Creating the Bottom Housing

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The parameter for the second offset was 1.25+3*hole_dia. The 1.25 value is an

allowance for the wall thickness of the revolved section, a 0.25 offset, and for a

0.5 fillet that will be applied later. The 3*hole_dia" is an allowance for the

edge distance and clearance for the bolt head up to the fillet. See the

illustration below.

2D for edge

distance

1D for bolt head to fillet

.25 offset + future .5 fillet

Wall thickness

1.25 value

Step 6 Create the second flange.

Extrude and unite the solid edge illustrated below. Use the

same values as before. Again, the extrusion should not

change the length of the solid body.

NOTE: The polarity (+/-) of the second offset value will vary

depending on the direction of the offset vector.

Select the inside edge

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Creating the Bottom Housing

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Your part should now resemble the illustration below.

NOTE: Remember to save your part periodically. If rain or solar

flares are in the forecast, save more often.

The illustration below points out the requirement for the top flanges. Notice

that the inside edge and outside edge run parallel to each other. Also notice

how the top flange is indented 0.25 from the end flanges.

Outside edge

Inside edge

Top View

Offset

.25

Step 7 Create the first top flange.

Extrude the solid edges illustrated below and unite.

ÉÉÉ

Creating the Bottom Housing

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NOTE: Remember, this is only 1/2 of the total housing. When

both halves are put together, a cross section normal to the

cylindrical axis should produce a round cross section. So, with the

WCS oriented to the Absolute Coordinate System, make sure the

extrude vector points in the -ZC direction.

Use the following values:

Start Distance = 0

End Distance = .5

First Offset = 0

Second Offset = 1+3*hole_dia

NOTE: The polarity (+/-) of the second offset value will vary

depending on the direction of the offset vector.

Select the four

edges that

define the

inside edge.

Your part should now resemble the illustration below.

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Creating the Bottom Housing

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Step 8 Mirror the top flange.

Mirror the top flange feature through the sketch datum

plane.

Your part should now resemble the illustration below.

Step 9 Create the bolt holes on the top flange.

The design requirements for this hole pattern are as follows:

0.75 diameter

Edge distance equals 2D

3 equally spaced holes of 15 degrees

In the next few actions you will create some reference features. The first

reference feature, a datum plane, will be used to locate the initial hole feature

on the flange. The next reference feature, a datum axis, will be used to define

the rotation axis of a circular array.

ÉÉÉ

Creating the Bottom Housing

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Choose Datum Plane.

Place the cursor over the edge shown below until the Quick

Pick cursor appears, then select the edge.

Select this

edges.

Choose the selection that defines an Edge.

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Choose Alternate Solution

until the datum plane is

oriented as shown below.

Choose OK.

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Creating the Bottom Housing

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Create a relative datum axis defined by the face illustrated

below.

Select this

cylindrical face.

Create a Simple Thru Hole by:

Defining the diameter with the hole_dia expression.

Select the placement face as shown below.

Select this

face here.

Locate the hole by positioning it Point onto Line relative to

the datum plane that intersects the placement face.

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Continue to position the hole by using Perpendicular from

the edge illustrated below. The distance should be defined by

2*hole_dia.

Select this edge.

Create a circular array of the hole feature as illustrated

below.

The Rotation Axis is to be defined by the datum axis shown

below.

Use the following values:

Number = 3

Angle = +/-15 (apply the right hand rule.)

Datum Axis

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Creating the Bottom Housing

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Step 10 Add a duplicate set of holes to the opposite flange.

In the model navigator, use the Drag and Drop functionality,

to reorder the

CIRCULAR_ARRAY

before the

MIRROR_SET

TIP

Place your cursor over the CIRCULAR_ARRAY feature, click MB1,

drag the circular array on top of the MIRROR_SET, and release

MB1.

Edit the

MIRROR_SET

to add both the INSTANCE and

CIRCULAR_ARRAY

features.

Step 11 Create the blends.

Create the blends as shown below.

.5 Radius

1.0 Radius

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Creating the Bottom Housing

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In the Edge Blend dialog box, toggle Add Tangent Edges to

ON.

Select one of the edges illustrated below.

All of the tangent edges are also selected.

Now select the other edge illustrated below.

Once again, the tangent edges are selected.

Select this edge.

Select

this edge.

Apply a 0.5 blend to the edges.

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Creating the Bottom Housing

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Select the four edges as illustrated below and apply a 0.1875

blend.

Select this edge

at the four different

locations.

Step 12 Move the Reference features to layer 62.

Step 13 Save the part and close.

ÉÉÉ

Creating the Bottom Housing

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ÉÉÉ

Creating the Assembly Part File

Design Applications Using

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3-1

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Creating the Assembly Part File

Section 3

In this section of the activity you will apply the Master Model concept by

creating an assembly part file that will be used to integrate the different parts of

the impeller assembly. You will then add the bottom housing to the assembly

part file, using the BottomĆUp modeling technique, making it the first

component part file of the assembly.

Step 1 Using the seedpart file, dau_seedpart_in, create an inch

part file called ***_impeller_assm.

Step 2 Add the ***_housing_bottom to the assembly part file

using the BODY reference set and original layers.

Step 3 Save the parts and close them.

ÉÉÉ

Creating the Assembly Part File

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ÉÉÉ

Creating the Upper Housing

Design Applications Using

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4-1

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Creating the Upper Housing

Section 4

The upper half of the housing is almost identical to the lower half except for the

inspection port located on top. The design intent dictates that if the bottom half

of the housing changes the top half will reflect those edits. The WAVE

Geometry Linker Mirror function will be used to capture this aspect of the

design intent. Also, the size of the inspection port is based on the overall size of

the housing. Because it is the sketch in the lower housing that controls size and

shape; interpart expressions will be used to to make the size of the inspection

port associative.

Upper Housing

ÉÉÉ

Creating the Upper Housing

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Step 1 Open the ***_impeller_assm part file.

Step 2 Create a new empty component part file named

***_housing_top.

Step 3 Use the Wave Geometry Linker to mirror the lower

housing into the ***_housing_top component part file.

Create a relative datum plane in the ***_housing_bottom

part file to mirror the housing through.

NOTE: Make sure you save the ***_housing_bottom after

creating the datum plane.

Mirror the housing.

NOTE: Make sure At Timestamp is toggled OFF before

performing the mirror.

ÉÉÉ

Creating the Upper Housing

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Step 4 Create the inspection port on the top housing.

Because the design intent for the housing is to be able to change in size and

shape, the inspection port must also be modeled to address these possible

changes. With that in mind the following design intent will be imposed on the

inspection port feature.

Length = 2/3 of the housing's largest interior radius perpendicular to the

revolution axis.

Width = 3/5 of the port's length.

Height = 4 inches above the outside cylindrical face.

Port is centered on the housing cylindrical axis.

Port is located 2 inches from cylindrical face edge (see illustration).

2.0

Make the ***_housing_top part the Displayed Part.

ÉÉÉ

Creating the Upper Housing

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Create the Relative Datum planes as shown below.

First, create this datum plane

tangent to the cylindrical face

and parallel to the flange

face.

Cylindrical face

Flange face

Second, create this datum

with a 4" offset relative to the

previous datum plane.

Third, create this

datum plane thru

the cylindrical axis

of the cylindrical

face at an angle of

to the

previously created

datum plane.

ÉÉÉ

Creating the Upper Housing

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Step 5 Create a sketch named, port, on layer 21, based on the

datum planes shown below.

Sketch plane,

normal should

point up.

Vertical

reference,

direction

should point in

the -XC.

Step 6 Create the sketch geometry and apply dimensional

constraints as illustrated below.

(Your expression names may vary from those illustrated below.)

Datum Plane

P5 is going

to the

endpoint of

this edge.

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Creating the Upper Housing

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Step 7 Create interpart expressions to control the length of the

port.

The design intent is that the length of the port is 2/3 (.66) of the housing's

largest interior radius as shown below. This step will capture that design

requirement.

First you must identify which expression controls the interior radius.

Review the MOLDLINE sketch in the ***_housing_bottom

part file. Identify the expression that controls the interior

radius (inside_radius=15.000) as illustrated below.

Interior

radius

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Creating the Upper Housing

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Review the PORT sketch in the ***_housing_top part file.

Identify the expression that controls the length of the port as

illustrated below.

Length

constraint

Create an interĆpart expression that links the port length to

the lower housings interior radius and then factor the 2/3

constant into the expression. The expression should look

similar to the following: (where xxx are your initials)

p2=xxx_housing_bottom::inside_radius*.66

The sketch will define the inside shape and size of the port. Next, you will

create associative offset curves to define the exterior shape and size of the port.

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Step 8 Create a set of curves that are an associative offset to the

sketch curves as shown below.

Sketch Curves

Associative Offset Curves

Step 9 Extrude the associative offset curves to the exterior

housing face, with a 5

draft, and unite.

Step 10 Extrude the sketch to the interior face of the housing with

of draft in the opposite direction and subtract it.

Step 11 Create the blends as shown below.

First, apply a 0.5

blend to the

interior corners.

Third, apply

a 0.5 blend

around the

base.

Second, apply a

1.0 blend to the

exterior corners.

ÉÉÉ

Creating the Upper Housing

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Step 12 In the ***_impeller_assm part file, replace the reference

set for all the component parts to BODY.

Step 13 Save the assembly and all of the component part files.

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Creating the Upper Housing

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ÉÉÉ

Creating the Impeller Ć Part 1, Defining Body & Blade

Design Applications Using

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5-1

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Creating the Impeller Ć Part 1, Defining Body & Blade

Section 5

The design intent in this section of the impeller creation is:

To allow the number of blades to changed.

To parametrically control the shape of the blade.

Impeller

ÉÉÉ

Creating the Impeller Ć Part 1, Defining Body & Blade

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Step 1 In the impeller assembly, create a new empty component

part file named ***_impeller.

Step 2 Change the workpart to ***_impeller.

Step 3 Create the main body of the impeller.

Create the cone to the specifications and orientation as

shown below. The WCS is shown in the absolute coordinate

orientation and location of 0,0,0.

Step 4 Define the blade generator geometry.

The definition of the blade cross section is supplied by an outside vendor. The

blade definition is provided through a CGM file. In the following steps, you will

import the CGM file, add it to a sketch, and then, constrain the sketch to

capture the design intent.

Choose File"Import"CGM.

Select the dau_blade_cross_section.cgm file from the parts

directory. The geometry should be placed on layer 41 and the

WCS should be oriented to the Absolute Coordinate System.

ÉÉÉ

Creating the Impeller Ć Part 1, Defining Body & Blade

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Notice, as illustrated below, that the quality of the geometry is a little less than

desirable. The repair of the geometry will take place after it has been added to

a sketch.

Step 5 Create the relative datum plane and two relative datum

axes as shown below.

These reference features will be used to create the sketch, that the imported

geometry will be added to.

Through

face axis.

Through

axis of face.

Through this

planar face

and datum

plane.

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Creating the Impeller Ć Part 1, Defining Body & Blade

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Step 6 Create a sketch called BLADE. The sketch plane will be

defined by the datum plane, the sketch normal should

point in the +ZC direction, and the horizontal reference

will be defined by the datum axis that is parallel to the

conical face axis.

Step 7 Add the imported geometry to the sketch.

Step 8 Assign geometric and dimensional constraints to the

sketch.

Apply a tangency constraint to four pairs of curves shown

below.

Pair 1

Pair 4

Pair 3

Pair 2

Apply a coincident constraint to the 4 pairs of endpoints as

shown below.

Pair 1

Pair 2

Pair 4, Select the two endpoints

Pair 3

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Creating the Impeller Ć Part 1, Defining Body & Blade

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Create the dimensional constraints as illustrated below.

This is a dimensional

constraint between

the R 1.5 arc center

and the horizontal

datum axis.

Step 9 Extrude the blade geometry.

Extrude the sketch 12 inches in the +ZC direction and unite

it to the cone feature.

Step 10 Create interpart expressions to control the length of the

extrusion.

To allow for a clearance amount to be trimmed later, the extrusion distance

must always equal the largest interior radius of the housing. This will be

accomplished by using an interĆpart expression.

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Creating the Impeller Ć Part 1, Defining Body & Blade

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Review the MOLDLINE sketch in the ***_housing_bottom

part file. Identify the expression that controls the interior

radius as illustrated below.

Interior

radius

Identify the expression that controls the length of the blade

extrusion.

Create an interĆpart expression, that links the blade

extrusion length expression, to the lower housing's interior

radius as shown above.

Step 11 Create a Circular Array of 6 equally spaced blades

around a datum axis.

Step 12 Save the assembly and all component parts; close all

parts.

ÉÉÉ

Creating the Impeller Ć Part 2, Trimming the Blades

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Creating the Impeller Ć Part 2, Trimming the Blades

Section 6

The design intent in this section of the impeller creation is:

The end of the blade conforms to the interior shape of the housing with a

0.125 clearance between the end of the blade and the housing.

Impeller

ÉÉÉ

Creating the Impeller Ć Part 2, Trimming the Blades

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Step 1 Open the ***_impeller_assm part file.

Step 2 Review the assembly part file.

Notice how the blades pierce the housing walls.

Step 3 Create an associative sheet solid.

This step will guide you through creating an associative sheet solid that will be

used to trim the blades to the inside profile of the housing.

The first step in creating the sheet solid is to use the WAVE Geometry Linker

to create a link between the housing profile and the impeller.

In the assembly part file we need to see the housing sketch geometry. One way

to do this is to create a reference set of the sketch geometry and replace the

body reference set with the sketch reference set.

Create a reference set called sketch" in the

***_housing_bottom part file and add the sketch to it.

In the assembly part file, replace the ***_housing_bottom's

BODY reference set with the SKETCH reference set that

was just created.

NOTE: If you do not see the sketch geometry make sure layer 21

(or the layer the sketch is on) is selectable. Remember, the lower

housing component part was added to the assembly using the

Original Layers option.

Use the Wave Geometry Linker to link the sketch to the

***_impeller component part file.

Set the modeling preferences Body Type to Sheet.

In the ***_impeller part file, revolve the linked sketch

geometry about the datum axis 360

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Creating the Impeller Ć Part 2, Trimming the Blades

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Step 4 Use Offset Faces to edit the sheet body to provide the

0.125 clearance needed between the impeller and housing.

The sheet solid that was created is the exact shape as that of the inner moldline.

If the blades were trimmed to this sheet solid in the present configuration,

there would be no clearance. In this step you will use the Offset Face function

to offset the entire feature a distance of 0.125. The offset face function is

parametric so, if the size or shape of the parent geometry changes, the sheet

solid will update to maintain the 0.125 clearance.

Step 5 Trim the impeller solid body to sheet solid.

Step 6 Create the hole features as illustrated below.

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Creating the Impeller Ć Part 2, Trimming the Blades

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Step 7 Create the keyway.

Create the datum plane as illustrated below.

Create this datum

plane thru the cylindrical

axis 90

to the first

datum plane.

Create a Rectangular Pocket on the XC-YC (if the wcs is in

the absolute orientation) datum plane; the normal should

point up. Identify the horizontal axis with the datum axis that

is parallel to the axis of the cone.

ÉÉÉ

Creating the Impeller Ć Part 2, Trimming the Blades

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Enter the following values:

X Length = 7.5

Y Length = 1.250

Z Length = 2.372 (2, accounts for the radius of the hole)

Floor Radius = .0625

Locate the pocket as shown below.

First, use Line onto

Line between this

datum plane and the

pocket's XC centerline.

Second, use Horizontal

between this arc's

center point and this

edge of the pocket

with a value of 0 (zero).

NOTE: Blades are not shown for clarity.

Step 8 Set the Modeling Preferences Body Type back to Solid.

Step 9 Save the assembly and all component parts; close all

parts.

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Creating the Impeller Ć Part 2, Trimming the Blades

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ÉÉÉ

Creating the ImpellerĆPart 3, Adding Blends

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Creating the ImpellerĆPart 3, Adding Blends

Section 7

The design intent in this section of the impeller creation is:

Each blade will have the same blends.

Impeller

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Creating the ImpellerĆPart 3, Adding Blends

Design Applications Using

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Step 1 Open the ***_impeller_assm part file.

Step 2 Create a .5 fillet at the base of all the blades.

.5 blend

Step 3 Create a .25 x 45

chamfer on the edges as indicated

below.

This edge

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Creating the ImpellerĆPart 3, Adding Blends

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7-3

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Step 4 Create a variable radius blend on the end of each blade.

Assign the variable radii as illustrated below.

R .5 at the end of

this edge.

R .0625 at the

end of this edge.

R 1.25 at the

end of this edge.

Step 5 Save the assembly and all component parts; close all

parts.

ÉÉÉ

Creating the ImpellerĆPart 3, Adding Blends

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ÉÉÉ

Creating the ImpellerĆPart 4, Mating the Assembly

Design Applications Using

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8-1

EDS

Creating the ImpellerĆPart 4, Mating the Assembly

Section 8

The design intent in this section of the impeller creation is:

Build associativity in the assembly so that the impeller maintains the

correct location and orientation.

Impeller

ÉÉÉ

Creating the ImpellerĆPart 4, Mating the Assembly

Design Applications Using

Unigraphics Workbook

8-2

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EDS

Step 1 Open the ***_impeller_assm part file.

Step 2 In the assembly part file, replace the current reference

sets of the ***_IMPELLER and

***_HOUSING_BOTTOM component part files with the

BODY reference set.

Step 3 Mate the impeller to the housing.

Center the impeller to the bottom housing using the faces

shown below.

First, select the

face of the cone

feature on the

impeller.

Second, select

the cylindrical

face of the

flange.

ÉÉÉ

Creating the ImpellerĆPart 4, Mating the Assembly

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8-3

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Assign a distance constraint with a 4" offset between the

impeller and housing using the faces shown below.

First, select

this face.

Second, select

this face.

Step 4 Edit the color of the assembly components.

In order to better distinguish between the components, the color attributes will

be edited.

The bottom housing will remain green however, the top housing will be edited

to be cyan and the translucency will be changed to allow the viewing of

impeller. The impeller will be edited to pink.

Edit the color of the top housing to Cyan with a Translucency

of 35. See the note below.

NOTE: If your part is not translucent, go to the General

Settings tab in the Preferences"Visualization Performance

pulldown menu and toggle the Disable Translucency option OFF.

Edit the color of the impeller to be pink.

Step 5 Review the assembly using View

→

Operation

→

Section.

Step 6 Save the assembly and all component parts; close all

parts.

ÉÉÉ

Creating the ImpellerĆPart 4, Mating the Assembly

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ÉÉÉ

Creating the Shaft SubĆAssembly

Design Applications Using

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9-1

EDS

Creating the Shaft SubĆAssembly

Section 9

The design intent of the shaft subĆassembly is that the Shaft_Impeller

component will control the diameter of the other shaft subĆassembly

components. This will be achieved by linking an edge of the shaft_impeller

component to the shaft_extension component. Another aspect of the design

intent is that the wall thickness of the shaft_extension is always 0.375.

Shaft Impeller

Shaft Load

Shaft Extension

ÉÉÉ

Creating the Shaft SubĆAssembly

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9-2

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Creating the Impeller interface of the Shaft SubĆAssembly

In this approach you will model the first component of the shaft assembly in the

ShaftĆSubĆAssembly part file. You will then create a component part file in the

shaft assembly and add the existing solid body to it.

Step 1 Using the dau_seedpart_in part file, create the

subĆassembly part file called ***_shaft_sub_assm.

Step 2 Create a 4.0" diameter x 11.0" long primitive cylinder in

the orientation shown below. The WCS shown is oriented

to the Absolute CSYS.

ÉÉÉ

Creating the Shaft SubĆAssembly

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Step 3 Create a 6.0" diameter x 2.0" long boss positioned Point

onto Point to the cylinder as shown below.

Step 4 Create a boss that will maintain a diameter that is 0.75

less than that of the boss created in the previous step and

has a height of 1.0. Position the boss Point onto Point to

the solid body as shown below.

Step 5 Create the chamfers and fillet as shown below.

.125 x 45

Chamfer

.25 x 45

Chamfer

.5 Radius

ÉÉÉ

Creating the Shaft SubĆAssembly

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Step 6 Create the keyĆway.

Create the two datum planes as shown below.

Create this datum plane

first thru the cylindrical

axis of the cylinder feature.

Create this datum plane second,

tangent to the cylindrical face of

the first feature and 90

to the

previous datum plane.

Create a Rectangular Pocket by selecting the placement face

and horizontal reference as shown below.

Horizontal reference

Placement Face

Use the following values for the pocket:

X Length = 10

Y Length = 1.25

Z Length = .524

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Creating the Shaft SubĆAssembly

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Locate the pocket as shown below.

Line onto Line

Horizontal from this

arc center to this

edge of the pocket

with a value of 0

(zero).

Step 7 Create a 2" radius automatic cliff edge blend by selecting

the edge shown below.

The reason it is an automatic cliff edge is that, when using the Blend function

with the blend type set to Edge and one of the adjacent faces has a height less

than the radius value, tangency will not be possible for that face and so it will be

cliffed.

Select this edge.

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Step 8 Create a .0625 blend on the edges of the keyĆway as

shown.

Blend these four edges.

Step 9 Create the hole shown below and locate it concentric to

the shaft.

1.0" diameter x 3.0" deep

with a 118

tip.

The part is now complete. The next step is to create a component part file and

add the part to it.

Step 10 Create a component part file called ***_shaft_impeller

and add the solid body to it.

There should now be a component part file in the ***_shaft_sub_assm part file.

The new component part file, ***_shaft_impeller, consists of the solid body and

all of the features used to create it, only the component object remains in the

subĆassembly file.

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Creating the Shaft SubĆAssembly

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Step 11 In the ***_shaft_sub_assm part file, replace the

***_shaft_impeller's current reference set with the BODY

reference set.

Step 12 Save the ***_shaft_impeller and ***_shaft_sub_assm

part files.

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Creating the Center Section of the Shaft SubĆAssembly

Next you will create the center section of the shaft subĆassembly. You will start

by creating an empty component part file in the subĆassembly and then link an

edge of the ***_shaft_impeller part to it. In this way the ***_shaft_impeller

part will control the diameter and orientation of the center section.

Center section of the

Shaft SubĆAssembly

Step 13 In the ***_shaft_sub_assm, create an empty component

part file called ***_shaft_extension.

Step 14 Link the edge of the component shown below to the

***_shaft_extension part file.

Select this edge.

Do not select the edge of

the chamfer.

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Creating the Shaft SubĆAssembly

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Step 15 In the ***_shaft_extension part file extrude the linked

geometry using the values below.

Enter:

Start Distance =

End Distance = 36

First Offset = 0

Second Offset =.375 (The sign, +/-, of this value should

create an edge that has a larger diameter than the generator

curve.

ÉÉÉÉÉ

Shaft_Extension slips

over Shaft_impeller.

If the shaftĆimpeller's feature, that interfaces with the extension, changes size,

then the extension diameter will also change and maintain the .375 wall

thickness.

Step 16 Create the two .25 x 45

chamfers as illustrated.

Chamfer

Step 17 In the ***_shaft_sub_assm part file, replace the

***_shaft_extensions' current reference set with the

BODY reference set.

Step 18 Save the ***_shaft_extension and ***_shaft_sub_assm

part files.

ÉÉÉ

Creating the Shaft SubĆAssembly

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Creating the Final Section of the Shaft SubĆAssembly

The part that you are about to create is the final component of the shaft

subĆassembly. The modeling approach will be similar to that of the center

section, in that you will link geometry from the center section to this

component. Therefore, when the first component of the subassembly, the

***_shaft_impeller, changes in diameter, the center section also changes

followed by an update in the final component.

Final section of the

Shaft SubĆAssembly

Step 19 In the ***_shaft_sub_assm, create an empty component

part file called ***_shaft_load.

Step 20 Link the edge of the component shown below to the

***_shaft_load part file.

Select this edge.

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Creating the Shaft SubĆAssembly

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NOTE: When creating the extruded features in the next two

steps, pay close attention to the vector directions. You may need to

alter the polarity of the values given below.

Step 21 In the ***_shaft_load part file extrude the linked

geometry in the -Y direction (WCS oriented to the

Absolute CSYS) using the values below.

The extrusion starts with a negative value. This negative value will provide the

1.0" interface into the ***_shaft_extension with an 8.0" length outside the

extension.

Start Distance = -1

End Distance = 8

First Offset = 0

Second Offset =0

Step 22 Extrude and unite the edge shown below using the

following values.

Select this edge.

Start Distance = 0

End Distance = 8

First Offset = 0

Second Offset =-.375 (The sign, +/-, of this value

should create an edge that has a larger diameter than the

generator curve

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Creating the Shaft SubĆAssembly

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Step 23 Create the four flat faces.

First create the reference features as shown below.

NOTE: Do not be concerned if your datum axis does not point in

the same direction as illustrated above.

First, create this datum

plane thru the face axis

of the second extrusion.

Second, create this

datum plane parallel to

the first and tangent to

the cylindrical face.

Third, create this

datum axis thru the

face axis of the

second extrusion.

Create a Rectangular Pocket by selecting the placement face

and horizontal reference as shown below.

Select this datum plane

as the placement face.

Select this

datum axis as

the horizontal

reference.

ÉÉÉ

Creating the Shaft SubĆAssembly

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Use the following values for the pocket:

X Length =

Y Length =

Z Length =

.75

Corner Radius =

Floor Radius = .5

Create the first positioning constraint by using

Line onto Line and selecting the datum axis and the pocket's

XC centerline.

Create the second positioning constraint by using Horizontal

and selecting the edges shown below.

Select this

edge.

Select the arc

center of this

edge.

Notice that the pocket is presently hanging over the back edge of the extrusion.

You will enter a negative value to position the pocket on the opposite side of

the arc's edge.

Enter -2.

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Creating the Shaft SubĆAssembly

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Model the other flats as illustrated below by creating a

circular instance array about the datum axis.

Four flats

Create the chamfers on the edges as directed below.

.25 x 45

Chamfer

.125 x 45

Chamfer

ÉÉÉ

Creating the Shaft SubĆAssembly

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Step 24 Save the part.

Step 25 In the ***_shaft_sub_assm part file replace the reference

set of the ***_shaft_load component with the BODY

reference set.

Step 26 Save the subĆassembly part.

Step 27 Add the ***_shaft_sub_assm, using its BODY reference

set, to the ***_impeller_assm. Don't worry with

orientation or position, that will be dealt with in the next

step.

Step 28 Mate the shaft subĆassembly to the main assembly.

The shaft subĆassembly is probably not in the correct orientation. This step will

orient the subĆassembly to the impeller. Keep in mind that the shaft and the

impeller have a keyway in common.

ÉÉÉ

Creating the Shaft SubĆAssembly

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Apply Mate to the faces shown below.

First, select

this face.

Second, select

this face.

Apply Center to the faces as shown below.

First, select

this face.

Second, select

the internal

cylindrical face.

ÉÉÉ

Creating the Shaft SubĆAssembly

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EDS

Apply Align to the faces of the keyways as shown below.

TIP

You may need to apply Alternate Solution.

First, select

this face.

Second, select

this face.

The shaft subĆassembly should now be mated to the impeller.

Step 29 Edit the color of the three shaftĆsubĆassm components.

Change the ***_shaft_impeller to blue.

Change the ***_shaft_extension to orange.

Change the ***_shaft_load to yellow.

Step 30 Save and close the assembly and all component parts.

ÉÉÉ

Creating the Shaft SubĆAssembly

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ÉÉÉ

Adding Hardware to the Assembly

Design Applications Using

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10-1

EDS

Adding Hardware to the Assembly

Section 10

In this section of the activity you will add the required hardware using different

part families. After adding the hardware you will then mate them to the

appropriate component. When adding the fasteners that hold the lower and

upper housing together, you will use the Feature ISET function to populate all

the holes of a circular array.

Housing Fasteners

Impeller Key

Impeller

Socket Head

Cap Screw

ÉÉÉ

Adding Hardware to the Assembly

Design Applications Using

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10-2

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EDS

Step 1 Open the ***_impeller_assm part file.

Step 2 Add a 1.25" wide x 4" long key to the impeller assembly by

selecting a family member out of the dau_key part file.

Use the BODY reference set.

Step 3 Mate the key to the keyway.

Mate the faces as shown below.

Second,

select this

face.

First, select

this face.

ÉÉÉ

Adding Hardware to the Assembly

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10-3

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Mate the faces as shown below.

First, select

this face.

Second, select

this face.

Mate the faces as shown below.

First, select

this face.

Second, select

this face.

ÉÉÉ

Adding Hardware to the Assembly

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Step 4 Fasten the Impeller to the shaft subĆassembly using a 1.0"

diameter x 6" long socket head cap screw. Do this by

selecting a family member out of the dau_shcs part file.

Use the BODY reference set. Mate the fastener to the

counterĆbored hole in the impeller.

Step 5 Add the first bolt that will hold the upper and lower

housing together.

Add a 0.75" diameter x 2.5" long Hex head bolt. Do this by

selecting a family member out of the dau_bolt part file. Use

the BODY reference set.

Mate the bolt to the assembly as shown below.

Mate the bottom

of the bolt head

to this face.

Center this cylindrical

face with the cylindrical

face of the hole in the

bottom housing

NOTE: The alignment must be made to the hole in the bottom housing.

The first bolts used to hold the two halves of the housing together on each side

of the assembly need to have at least one mating condition to the hole feature

in the circular array of the bottom housing. The holes that appear in the top

housing do not belong to a circular array because the top housing was created

by a mirroring function. By mating the bolt as instructed above, the Feature

ISET function may be used later to populate the remaining holes with bolts.

This practice will also be applied to the first washers and nuts.

Step 6 Add the first lock washer.

Add a 0.75" diameter lock washer to the assembly file. Do

this by selecting a family member out of the

dau_lock_washer part file. Use the BODY reference set.

ÉÉÉ

Adding Hardware to the Assembly

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Mate the washer as instructed below.

Mate the top face of the

lock washer to the bottom

face of the bottom

housing's flange.

Center the cylindrical face of

the lock washer with the

cylindrical face of the hole in

the bottom housing

NOTE: The alignment must be made to the hole in the bottom housing.

NOTE: Bolt not

shown for clarity.

Step 7 Add the first nut that will hold the upper and lower

housing together.

Add a 0.75" diameter nut to the assembly part file. Do this

by selecting a family member out of the dau_nut part file.

Use the BODY reference set.

Notice that one side of the nut is beveled and the other side is flat.

Mate the flat side of the nut to the bottom face of the lock

washer.

Center the nut by selecting the nut's cylindrical face and the

cylindrical face of the hole in the bottom housing and choose

OK.

ÉÉÉ

Adding Hardware to the Assembly

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Step 8 Save the mating constraints for the bolt, lock washer, and

nut.

Step 9 Add the rest of the fasteners to this side of the housing

using the From Feature ISET" function.

NOTE: To be successful in the use of the From Feature ISET"

function, a couple of points must be kept in mind.

First, at least one mating constraint must be related to the circular

array. In this activity, the circular array is only present in the

***_housing_bottom part file. The hole pattern in the upper housing

is part of the feature that was created with Wave Geometry Linker

and is not recognized as an instance array.

Second, the mating constraints must be related to the first instance

of the array.

Step 10 Continue by adding the fasteners to the opposite side of

the housing, by applying the same methods as used on the

previous side.

NOTE: When selecting the components for the From Feature

ISET function; select them in the graphics window. If selection is

made in the dialog box window, duplication of fasteners will occur

on the side that is already done.

Step 11 Save & close the assembly and its component parts.

ÉÉÉ

Editing the Assembly Part File

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11-1

EDS

Editing the Assembly Part File

Section 11

In this section of the activity you will change some assembly components'

parameters in order to edit the size and shape of the assembly. As you do this

you will be able to observe how the captured design intent maintains the

desired form, fit, and function. You will make the following edits:

Edit the moldline sketch

Change the number of holes in housings

Change the location of the impeller in the assembly

Change the number of blades on the impeller

Increase planar interface between shaft and impeller

Change the length of the shaft extension

Correct any interferences

ÉÉÉ

Editing the Assembly Part File

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Step 1 Open the ***_impeller_assm part file and load all

components fully.

Step 2 Change the inner moldline of the bottom housing by

editing the MOLDLINE sketch to the values shown below.

Step 3 Add the holes shown below to each of the top flanges by

editing the appropriate circular array. Maintain the

existing spacing.

New holes

Step 4 Review the Impeller assembly.

Did the upper housing and impeller update? If not, it is because these

components are only partially loaded.

ÉÉÉ

Editing the Assembly Part File

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If the upper housing and impeller components did not

update; open them using the Assembly Navigator. If the

components have updated, skip this action.

Notice how the impeller and upper housing have updated to reflect the changes

made in the lower housing. Also notice how the two new holes have been

populated with fasteners. This is because the holes are part of an array and the

From Feature ISET function was used to place the fasteners.

Step 5 Change the location of the impeller in the assembly.

Edit the mating constraint with the offset of 4 to 7 (or -4 to

-7, as appropriate), to move the impeller 3" further into the

housing. Apply the change before selecting OK.

An Update Error dialog pops up informing you that the system is unable to

update a blend in the ***_impeller part.

Choose Accept.

Notice that the variable radius is no longer present on the blades of the

impeller.

ÉÉÉ

Editing the Assembly Part File

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Here is what has happened. Examine the illustration below and your graphic

screen. Notice how one end of the impeller blade makes a transition across the

edge of two of the interior housing faces.

Before we continue, let's review how the blade was created.

The blade was extruded some distance. An interpart expression was then

created so that if the housing changed size the extrusion would always be long

enough to be trimmed to match the housing shape.

In order for the impeller to maintain shape and clearance to the inside moldline

of the housing, the lower housing moldline sketch was linked to the impeller

part file. From this linked sketch in the impeller part file, a sheet solid was

created and edited to provide the clearance between impeller and housing. The

impeller was then trimmed to this sheet solid, which is composed of 3 separate

faces.

In its original position, the blade was intersected by 2 faces of the sheet body

which generated 6 edges to which the blend was applied. When the impeller's

location in the assembly was changed, the blade only intersected one face of the

sheet solid, which caused 3 of the original edges to go away and one new edge

to be generated. The blend must be edited to include the new edge.

ÉÉÉ

Editing the Assembly Part File

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In addition, the edge where the 0.0625 radius of the variable radius had been

defined no longer exists. So the system looks for the next radius size which is

1.25 and attempts to apply it. Therefore, the location for the 0.0625 radius must

also be redefined.

Rear face

R 1.25

R .0625

This radius no longer exists

since the edge has been

redefined.

R .5

Sheet Solid used for

trimming the impeller

Radius assignments

for the variable radius

To resolve this error the new edge of the impeller needs to be added to the

variable radius blend feature and the location for the 0.0625 radius must be

specified.

For clarity, change the displayed part to the impeller.

Choose Edit

→

Feature

→

Parameters.

From the Edit Parameters dialog box select the blend that

was identified in the Edit During Update dialog box and

choose OK.

The edges and variable radii points are highlighted on the original blade to

which the blend was applied.

Notice that the back edge is not highlighted but three edge representations

from the impellers previous location are highlighted.

The CUE line prompts you to select edges, points, or snapshot curves.

ÉÉÉ

Editing the Assembly Part File

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Rotate your view and zoom in as necessary to deselect the

old edges of the blend as shown below. Once deselected,

choose OK in the Edge Blend dialog box and then Apply in

the Edit Parameters dialog box.

Deselect the three old edges

Select the blend to edit again.

This time select the edge that is not highlighted.

New edge

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Editing the Assembly Part File

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Select the control point as shown below. Be sure that the

control point selected is the end point of the edge that was

just added to the blend feature.

Control point

In the variable radius text box enter .0625 and choose OK

twice.

Review the assembly part file.

NOTE: The removal of the old edges and the addition of the new

edge could have been completed in one step but was done in two

steps for clarity.

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Step 6 Change the number of blades on the impeller from 6 to 5.

Maintain equal spacing of the blades.

Step 7 Change the profile of the blade by editing the BLADE

sketch to the values shown below.

p78=6.625

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Step 8 Review the assembly.

Step 9 Increase the planar interface between the impeller and

shaft_impeller components of the main assembly.

Determine the current radial interface between the planar

faces of the two components.

Radial interface

between the two

components.

Impeller

Shaft_Impeller

The radial interface is 0.25, this value needs to be increased to 0.5. To achieve

this, a boss feature on the shaft_impeller will be edited.

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Editing the Assembly Part File

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Edit the boss feature shown below to have a diameter of 6.5.

Select this

boss feature.

Did the rest of the shaft subĆassembly update? If not, it is because these

components are only partially loaded.

If all of the shaft subĆassembly components did not update;

open them using the Assembly Navigator. If the components

have updated, skip this action.

Here is a good example of design intent captured. Observe how the shaft

extension and shaft_load components update in size. The shaft extension is now

6.5" in diameter and has maintained a wall thickness of 0.375. This was

expedited by two operations. First, the boss feature on the shaft_impeller

component that fits within the shaft_extension had its diameter expression

made associative to the first boss in order to maintain a 0.375 offset. Second,

the edge of the shaft_impeller was linked to the shaft_extension component.

Step 10 Change the length of the shaft extension to 24 inches.

Notice how the shaft_load component maintains its position relative to the

shaft extension. This is because the shaft_load component is linked to the

extension component.

Step 11 Perform a Clearance Check on the assembly.

Change the work part back to the ***_impeller_assm.

Choose Assemblies

→

Components

→

Check Clearances

Choose Select All in the Class Selection dialog box and

choose OK.

ÉÉÉ

Editing the Assembly Part File

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EDS

Notice the hard" and touching" interferences listed in the dialog box. We are

not concerned with the touching" interferences as they are simply face to face

conditions. However, the hard" interferences identify conditions that need to

be addressed.

Double-click on the interference between the Key_35 and

the ***_shaft_impeller.

Move the Interference Check dialog box to a location away

from the graphics window and Replace View to the Right

view.

Zoom in closely to one of the bottom corners of the keyway

on the impeller shaft and the key itself as shown in the figure

below.

To see this

Interference

Zoom in here

Notice the corner radius of the keyway is too large and interferes with the

chamfer on the key. To solve this problem we need to edit the blend radius of

the keyway in the impeller shaft.

Cancel the Interference Check dialog box.

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EDS

Step 12 Correct the Interferences.

Change the work part to the ***_shaft_impeller.

Edit the blend radius of the keyway to .03125

Change the work part back to the ***_impeller_assm.

Rerun the Check Clearance operation.

Notice that the previous hard" interference is listed as a new touching"

interference at the top of the dialog box.

DoubleĆclick on the interference between the Key_35 and

the ***_impeller.

Move the Interference Check dialog box to a location away

from the graphics window and Replace View to the Front

view.

Zoom in closely to the upper right corner of the keyway on

the impeller and the key itself as shown in the figure below.

Interference

The interference is this case is due to the mating condition applied between the

end face of the key and the rectangular pocket. This is an acceptable

interference because the key can be moved further into the keyway. You could

fix the interference by switching the mate constraint to a distance constraint

and entering an offset value.

ÉÉÉ

Editing the Assembly Part File

Design Applications Using

Unigraphics Workbook

11-13

EDS

Bring the Interference Check dialog box back to the graphics

screen and doubleĆclick on the interference between the

hex_head_.75x2.5 and the ***_housing_top.

Move the Interference Check dialog box to a location away

from the graphics window and, if necessary, Replace View to

the Front view.

Zoom in closely on the head of the bolt and the top housing

as shown in the figure below. (You may have a different bolt

displayed.)

Interference

Zoom in here

Notice the interference between the radius under the bolt head and the hole. If

you remember when creating the holes in the housing we only used the exact

diameter of the bolt as the hole diameter. It is obvious that we need to have

some clearance here. The top housing is a linked mirror of the bottom housing

so we will need to edit the hole diameter in the bottom housing to see the

change in both parts.

ÉÉÉ

Editing the Assembly Part File

Design Applications Using

Unigraphics Workbook

11-14

Unigraphics NX

EDS

Cancel the Interference Check dialog box.

Change the work part to the ***_housing_bottom.

When we created the bottom housing we established an expression name and

value for the hole diameter and used the expression when we created the thru

hole. We then created a circular array of the hole and added it to the mirror set

for the other side. Changing the value of the hole diameter expression will

effect all the holes in the part and maintain our design intent.

Edit the hole_dia expression to .875

Change the work part back to the ***_impeller_assm.

Rerun the Check Clearance function.

NOTE: Unless you moved the key away from the end of the

keyway on the impeller, the hard interference will still exist

between them.

Step 13 Save the assembly and all component part files

ÉÉÉ

Applying a Revision to the Assembly

Design Applications Using

Unigraphics Workbook

12-1

EDS

Applying a Revision to the Assembly

Section 12

In this last section of the activity, you are to assume that a particular phase of the

design has been declared frozen. Any changes after this point will have to be filed in

conjunction with a revision.

You will make several changes to the shaftĆload component and then do a SaveĆAs. In

this operation you will save the component, subĆassembly, and main assembly with

new names that indicate a revision has taken place.

ÉÉÉ

Applying a Revision to the Assembly

Design Applications Using

Unigraphics Workbook

12-2

Unigraphics NX

EDS

Step 1 Open the ***_impeller_assm part file, or change the

displayed part to ***_impeller_assm, whichever is

applicable.

Step 2 Change the number of flats on the ***_shaft_load

component from 4 to 6 and maintain equal angle.

Step 3 Edit the pocket feature to the values shown below.

Change these values :

Z Length =

.375

Floor Radius = .374

Step 4 Create a 0.375 wall in the hex area of the part.

In order to maintain associativity with the outside shape; the extrusion will be

created from associative offset curves.

.375 wall thickness

Create associative offset curves from the face shown below.

The offset value is .375 with the offset vector pointing toward

the interior of the solid body.

Select this face.

ÉÉÉ

Applying a Revision to the Assembly

Design Applications Using

Unigraphics Workbook

12-3

EDS

Extrude the curves 6" into the solid body and subtract.

Step 5 Create a 0.75 diameter thru hole as shown below. Locate

the hole Point onto Line relative to the datum axis and a

distance of 1.5" from the edge of the solid body.

Placement face

Thru face

Step 6 Save the part with a new name.

Since this is a revision, the part file needs to be saved with a different name so

that a history may be maintained.

Choose File

→

Save As.

An information window pops up informing you that this component is used in

the subĆassembly and main assembly.

Enter ***_shaft_loadĆa and choose OK.

ÉÉÉ

Applying a Revision to the Assembly

Design Applications Using

Unigraphics Workbook

12-4

Unigraphics NX

EDS

The Save Part File As dialog box reappears. The CUE line prompts you for a

new part file name for the subĆassembly.

Since a change was made to form, fit or function of the shaft_load component,

you will also be required to save the subĆassembly and main assembly with a

different name.

Enter ***_shaft_sub_assmĆa and choose OK.

The Save Part File As dialog box reappears. The CUE line prompts you for a

new part file name for the main assembly.

Enter ***_impeller_assmĆa and choose OK.

Next you receive the OK to SaveAs dialog box. This is Unigraphics' way of

saying, Do you really want to do this?". You do.

Choose OK.

NOTE: A change that does not affect the form, fit, or function of a

component, such as a drawing note, would not require a revision to

the assembly part files.

Step 7 Make the ***_impeller_assmĆa part file the displayed

part.

Step 8 Open the original ***_impeller_assm part file.

Step 9 Review the two assemblies. Shade the models and admire

your work.

There are now two assemblies of the impeller mechanism which document the

history at two different design phases.

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