Pro/ENGINEER  WildFire 4

 

Getting Started:

 

All students enrolled in an Engineering course have automatically an account setup for them in the Instructional Computer Facility. The userid for this account is formed by taking the first 6 letters of the student’s last name and adding their first and second initial to form the account name with a maximum 8 characters. The default password is created by taking the rightmost 6 characters/numerals of the students SIS#.

To start the logon-process on the Win XP workstations you must use the CONTROL+ALT+DELETE sequence. All three keys need to be pressed down together. A login-panel will pop up; enter your username and password to login. (Do not forget to logoff once you are done with your session.)

 

The next step (step #1) needs only to be done once, when you start using ProEngineer for the first time.

 

1.      Create the user ProEngineer file-folders. Bring up the Command Prompt-window:  (Start – Run – CMD)

Type in its window  config_proe   and the Enter-key.

This will create the local ProE subdirectory tree.

You will find also a new icon on your desktop. This icon is labeled ProE and will be used to start Pro/ENGINEER.

Note: Always use the icon created by this step to start Pro/E.

Do not use the shortcut from Start – Programs – Mech+Struct for working in ENGN1740!

 

2.      Now you can start ProEngineer by double-clicking its icon on your desktop. The process of starting ProEngineer is not instantaneous, be patient it will take about 90 seconds for ProE to be completely loaded and ready.

3.      After ProE has started you can open an existing design file or create a new one. When creating a new one, you must decide at this time what type of file you want to create. (The possible types of files one can create range from 2D sketch, part, assembly, drawing to sheet metal and mold design).

 

NOTE: When logging-in the first time, you may experience difficulties with your account. Either you don't know your proper userid or the password is invalid. In this case contact Jim Scheuerman at xt31500, or by email  James_Scheuerman@brown.edu.

 

Pro/ENGINEER Mouse Commands

 

 

 

Main Pro/Engineer Window

 

 

 

 

Dashboard Area of Pro/E Window

 

 

 

Define Sketche →

 

 

Creating a New Design File (see also step 3 on page 1)

 

 

Introduction to the Sketcher

 

In Pro/ENGINEER, the sketch is a 2D section of the feature being created. Essentially all features are created by this method. You create sections with the Sketcher. Note that before you can begin creating a section, you need to select, or create a plane which defines the location and orientation of the sketch in space. This plane can be any flat entity, such as a face of an existing solid geometry or a datum plane.

The Sketcher with its Intent Manager is a powerful geometry engine that is capable of "assuming" things about your input sketch that impact your design intent. The assumptions are embodied in a number of rules (see table below) that the Sketcher will invoke if necessary in order to successfully regenerate your sketch. It will only do this if the specified dimensions and/or alignments are not sufficient to completely define the geometry. You should become familiar with these rules, and learn how to use them to your advantage. Conversely, if you do not want a rule invoked, you must either:

(a)    use explicit dimensions or alignments, 

(b)   exaggerate the geometry so that if fired, the rule will fail,

(c)    force Pro/E explicitly to disable the constraints.

 

For example, if a line in a sketch must be 2o away from vertical, draw it at 75o and explicitly dimension it, otherwise it will be assumed to be exactly vertical. After the sketch regenerates, you can modify the dimension to the desired 2o value.

 

Rule

Description

Equal radius and diameter

If you sketch two or more arcs or circles with approximately the same radius, the system may assume that the radii are equal.

Symmetry

Entities may be assumed to be symmetric about a centerline.

Horizontal and vertical lines

Lines that are approximately horizontal or vertical may be considered to be exactly so.

Parallel and perpendicular lines

Lines that are sketched approximately parallel or perpendicular may be considered to be exactly so.

Tangency

Entities sketched approximately tangent to each other may be assumed to be tangent.

Equal segment length

Lines of approximately the same length may be assumed to have the same length.

Point entities lying on other entities or collinear with other entities

Point entities that lie near lines, arcs, or circles may be considered to be exactly on them. Points that are near the extension of a line may be assumed to lie on it.

Equal coordinates

Endpoints and centers of arcs may be assumed to have the same X- or the same y-coordinates.

 

When a sketch is regenerated, the rules that have been fired are indicated on the graphics window using one or more symbols beside each effected entity.

 

 

Sketcher Toolbar

 

The Toolbar is shown with each pull-out menu expanded.

 

Constructing your first Solid Part

 

As the first exercise with Pro/ENGINEER we will create a simple solid. The arcs and straight line segments shown below right define the profile of our solid. By ‘revolving’ this profile of line segments along a vertical axis a solid can be created. We will sketch the profile in the x-y or FRONT plane. The base will sit on the x-z or TOP plane and the profile will be swept around the y-axis to form the solid.

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 


Perspective View of finished Solid

 

 

Procedure:

 

·         To begin we must create a new Part file. Select File – New and name it vessel. Make sure you uncheck the ‘Use default template’ box and click OK. The next window popping up is the ‘New File Options’ window. Select start_mmns as your template file and you can enter a description and your initials in the two parameter text fields. This will base the new part file on a template file, which has predefined datum planes, coordinate system, saved views and has the working units defined as mm, N and s.

·         When starting to create a solid we need to pick the appropriate tool. Click on the Revolve Icon with the left mouse button. It is found in the Base Tool section of the Feature Toolbar on the right side of the Pro/E window.

·         See the Dashboard below the Navigator window become active. Click (left mouse button) on the Placement icon in the Dashboard and a small window will open, called ‘Sketch’. Click on the Define icon. Next a new window pops up again called ‘Sketch’ in the upper right corner.

·         We use the FRONT datum plane as our sketching plane. Select it by clicking on its name ‘FRONT’. Leave all the defaults (yellow arrow as View direction, RIGHT as Datum Reference and Right as Orientation). Click the Sketch icon, or middle mouse-button to close this window.

·         We are now in the ‘Sketcher’ and  ready to begin sketching the profile:

Note a new set of icon appear on the right edge of the graphic window; these are the sketcher tools.

Notice further, we are working now in 2-D mode in the Front datum plane, but our view is still the original 3-D view. You can obtain a direct straight on 2-D view by clicking on the ‘Orient Sketching plane parallel to the Scren’-icon.

 

Sketching the Profile:

1.         First we draw a line segment starting from the origin, (at x=y=0 – the intersection of x and y axes) along the x- axis as the radius of the base.

Select the Line tool, if it isn’t is automatically selected. We need only to make two left button mouse clicks to place the line. Next click the middle mouse button to end placing line segments. We place the second horizontal line segment again with x=0, but at some distance above the first, to represent the radius of the mouth. Next connect the two starting points with a vertical line. Pro/E requires us to ‘close’ our section profile along the axis of revolution.

2.         Notice all three lines are automatically dimensioned. We will change these dimensions to their correct values with the Modify command, or by double clicking their values and then editing them.

Move the cursor to a dimension and select it by clicking left. Notice how it changes color to red when selected. Next click on the Modify icon from the Sketcher Toolbar. A window pops up, enabling you to change the selected dimension’s value. Modify all three line segments to the proper value. Do the vertical segment last!

3.         Next we use the 3-point Arc tool to place bottom arc.

Select from the Sketcher Toolbar – Arc (3point or tangent end).

Begin at the right endpoint of the base line segment. Place the second point above the first point, about a little more than half the vessel’s height and a little closer to the y-axis. The third point is defining the curvature of the arc. Place it somewhat to the right of the first point for the x-direction, but in the middle between the first and second point in the y-direction. Click again the middle mouse button to terminate the process.

4.         Double-click the radius dimension to change it to the proper value ( 90 ).

5.         Modify the horizontal dimension to specify the distance of the center of the arc from the vertical axis. The value is 45.

6.         The final arc is made with the same Arc  tool.

Select from the Sketcher Toolbar – Arc (3point or tangent end).

Select the end point of the first arc as the starting point, and the right end point of the line segment representing the mouth as the arc’s end point. When selecting the first point move away from it in a direction that is tangential to the first arc. Click again the middle mouse button to terminate the process. Modify its value to 40.

7.         To finish the sketch for our revolved solid we must define an axis of revolution.

Use Sketch - Centerline and place it along the y-axis. Click again the middle mouse button to terminate the process. We have completely defined the profile for our solid.

We are now ready to leave the sketcher: click on the Check mark icon on the Sketcher toolbar.

8.         Click on the ‘Check’ icon on the Sketcher toolbar to exit the Sketcher.

·         Returning to the Dashboard, we need only to specify the angle of rotation that the profile is required to rotate to complete the solid. Select 270 degrees and click on the ‘Check’ icon.

 

You can change your viewing orientation to better see the model just created. Move the mouse in the main window, while depressing the middle mouse button for a dynamically changing view.

 

Don't forget to save your part, we will use it again later.

 

You can also experiment modifying the part:

Right-click ‘Protrusion’ in the Model Tree and select Edit Definition in the popup-menu.

Modify a dimension, or the angle of rotation.

 

 

 

RETURN