Tài liệu PUMP HOUSING CREATED USING SURFACE Pro/ENGINEER doc

Surface merges are created by selecting Feature, Create, Surface, Merge, and then selecting the two quilts to be combined through Intersect or Join.. Select Insert pull-down menu, then

ME-430 INTRODUCTION TO COMPUTER AIDED DESIGN

PUMP HOUSING CREATED USING SURFACE

Pro/ENGINEER Wildfire 2.0

Dr Herli Surjanhata

Create a part called pump_housing Delete the default coordinate system Right-click on PRT_CSYS_DEF, and select Delete

Create a coordinate system using Planes method by selecting icon, make sure you hold down Ctrl key while selecting the three default datum plane

3-Select the Orientation tab, make sure that coordinate system CS0 as shown in the figure below The X-Y plane of CS0 is aligned with RIGHT

Create the following datum curve

Select the CS0 coordinate system

Cylindrical – as the type of coordinate system

Editor window appears, and enter the following equation – see figure below:

r = 5 + 2.25*t

theta = -105 – 345*t

z = 0

Save and Exit the editor

Click OK to end the datum curve creation

*What is a surface quilt?

A surface quilt is a "patchwork" of connected surfaces A quilt may contain one or

more surface patches The external edges of a surface are yellow, and the internal

boundaries of the patches are displayed in magenta

*What is a merge?

A surface merge allows multiple surfaces to be combined into a single quilt Surface

merges are created by selecting Feature, Create, Surface, Merge, and then

selecting the two quilts to be combined through Intersect or Join Completion of

the merge operation will be visually evident by turning the yellow edges to magenta

Datum curve created using Equation

Select Insert pull-down menu, then

Sweep -> Surface

Select Traj

Pick the datum curve

Ok Done -> Okay Open Ends -> Done

Sketch the following arc:

Click , then select button - to end the creation

The resulted surface is shown below

*What is the difference between the Capped Ends and Open Ends options available

when creating surfaces?

Surface features created with Extrude, Revolve, Blend, or Sweep can be open or closed volumes If the surface is going to be open, select Open Ends from the ATTRIBUTES menu If the feature is required to enclose a volume, select Capped

Ends A tube can be created by extruding a circular section as Open Ends A closed

cylinder would be created by extruding the same section as Capped Ends

Create the new surface for housing outlet

Select the Datum Plane

tool

Click OK

Datum plane DTM1 is created

Select the Extrude tool

Pick the Extrude as Surface

Pick the datum plane DTM1, and for

Sketch Orientation, pick the RIGHT

datum plane

Click the Sketch button

Pick the right outer arc as reference

Pick this edge for reference for datum plane creation

Sketch the circle as shown in following figure

Click , then Enter Depth: 5

Click icon to finish the surface creation

The resulted surfaces are shown below

Merge both surfaces

*What is the difference between the Join and No Join options available when

creating swept surfaces?

Surface features created with Sweep, Var Sec Swp, or Swept Blend, by selecting

edges of a surface as a trajectory, will have the option to be merged with the

existing quilt If Join is selected from the SRFS JOIN menu, the feature will be

automatically combined into one quilt with the original surface This functionality saves the step of creating a new feature with Merge No Join simply means that the

feature is not to be merged with the quilt referenced for the trajectory

*What is the difference between Intersect and Join, from the SURF MERGE menu?

Intersect and Join are the two methods which combine surfaces into one quilt

Selecting Intersect from the SURF MERGE menu will merge two intersecting quilts

This should be used when quilts overlap one another Pro/ENGINEER will prompt the user to choose which portion of the selected quilts are to remain in the final merge

feature Join will merge two adjacent quilts into one A single-sided edge of one of

the quilts must lie on the other surface If a portion of one surface extends beyond the boundaries of the other surface, Pro/ENGINEER will prompt the user to select a portion of that surface to keep for the final merge feature

*What would cause a surface merge to not be created?

Pro/ENGINEER will be unable to create a surface merge if the selected quilts do not actually intersect Verify that the surfaces intersect by creating a datum curve by

Intr Surfs If the datum curve cannot be created, or is discontinuous, the surfaces

must be redefined They can be enlarged by selecting Extend from the QUILT SURFS menu

Merging both surfaces

From the Model Tree, select the first created surface (i.e Surface id 43 in this example), then hold the Ctrl key, and pick the second surface (i.e

Extrude 1)

Or pick the surfaces from graphics area

Pick the Merge Tool from the right toolbar panel Click

Options

Make sure the Intersect is selected

Click the Change side icon , then hold down the CTRL key, pick the other icon

Click the icon to finish the operation

Create a new surface with BOTH SIDES protrusion and 5.5 in extrusion depth The section is shown below

Select the Extrude tool

Pick the Extrude as Surface

As sketching pick the datum plane

RIGHT, and accept the default for

Sketch Orientation plane

Click the Sketch button

Click the icon

Select the Extrude on both sides icon

Extrusion depth = 5.5

Sketch a circle of 10.55 diameter

Merge the surface again with intersect Pick the two surfaces to be merged as shown in the Model tree, then select the Merge Tool

Click the Change side icon , then hold down the CTRL key, pick the other icon

The resulted surface is shown below

Select on Round Tool to create a 0.125” radius round at the intersection of the surface

Click the to complete the task

*What may prevent a solid use quilt feature from being created?

Features being created with the Use Quilt and Solid options from the SOLID OPTS

menu, must reference a quilt that completely encloses a volume to be added or removed Any gaps, represented by yellow edges, can hinder feature creation

Surfaces that have been successfully joined have magenta edges at their borders Any patches that are not continuous need to be joined with the Merge command

*What may prevent a thin use quilt feature from being created?

Features being created with the Use Quilt and Thin options, from the SOLID OPTS

menu, offset a selected quilt a user-defined distance and fill in that gap with solid material The offset distance and curvature of the selected quilt are the factors which determine creation Ensure that the chosen quilt can be offset to at least the

thickness value This can be verified by creating a surface through Feature,

Create, Surface, New, Offset, and entering the thickness It can also be

investigated through the INFO menu by selecting Analysis, Srf Analysis, Radius,

and selecting the surface The info tool will find the minimum radius of the quilt, which should equal the maximum offset distance in the indicated direction

Use the existing surface to create a solid object – pump housing, and the following commands will be used:

0.125” radius round

To create a thin solid from a surface quilt,

Select the surface quilt first from Model Tree,

then Edit -> Thicken Enter thickness 125 Click the to flip the direction

Click the button to continue

Create the following THIN 360-degree revolved protrusion, with 0.125” thickness

Select on the Revolve Tool , then

Use FRONT as Sketching Plane, and accept default for Sketch Orientation

Make sure

to select

the icon, and the

to change the direction

of thickening

Create another 360-degree thin revolved protrusion

Create the inlet flange shown below

Select on Datum Plane Tool to create a new datum plane that passes through the center axis of the housing and angled -30 deg from FRONT datum plane

Datum plane DTM2 is created

Create a 300 ° revolved protrusion by

using DTM2 as sketching plane, and pick

RIGHT datum plane as Top reference for

Sketch Orientation

Revolved angle = 300°

The inside edge of

this section is

aligned with the

edge of the hole

Select on the Hole Tool and

create the hole as shown below

Pattern the hole as indicated below

Pattern increment = 30°

Total number of holes = 10

Create the hole and pattern it as shown below

Pattern increment = 30°

Total number of holes = 10

Select on the Hole Tool and

create the hole as shown below

Don’t forget to add the necessary rounds – use any appropriate radius, for example 0.2” radius or else