Introduction

This self-paced tutorial is modeled on portions of the book titled "Inside ProENGINEER" by James Utz and W. Robert Cox (Onword Press). Typical time required to complete the tutorial is 1-2 hours. READ the instructions CAREFULLY during the exercise, especially the part about saving your work. Pro/ENGINEER is a feature based, parametric solid modeling program. As such, it's use is significantly different from conventional drafting programs. In conventional drafting (either manual or computer assisted), various views of a part are created in an attempt to describe the geometry. Each view incorporates aspects of various features (surfaces, cuts, radii, holes, protrusions) but the features are not individually defined. In feature based modeling, each feature is individually described then integrated into the part. The other significant aspect of conventional drafting is that the part geometry is defined by the drawing. If it is desired to change the size, shape, or location of a feature, the physical lines on the drawing must be changed (in each affected view) then associated dimensions are updated. When using parametric modeling, the features are driven by the dimensions (parameters). To modify the diameter of a hole, the hole diameter parameter value is changed. This automatically modifies the feature wherever it occurs - drawing views, assemblies, etc. Another unique attribute of Pro/ENGINEER is that it is a solid modeling program. The design procedure is to create a model, view it, assemble parts as required, then generate any drawings which are required. It should be noted that for many uses of Pro/E, complete drawings are never created. A typical design cycle for a molded plastic part might consist of the creation of a solid model, export of an SLA file to a rapid prototyping system (stereolithography, etc.), use of the SLA part in hands-on verification of fit, form, and function, and then export of an IGES file to the molder or toolmaker. A toolmaker will then use the IGES file to program the NC machines which will directly create the mold for the parts. In many such design cycles, the only print created will be an inspection drawing with critical and envelope dimensions shown.

This tutorial is designed to introduce you to several of the basic features of Pro/E by creating a model of a car body. You will create a datum system, extrude a solid shape, add edge rounds, form a shell, and cut out the windows and wheel openings. Although there are no prerequisites, some familiarity with PC's and the Windows operating system is helpful.

Login Insructions

Room E 301

login New X session.

select Kahuna.

enter password.

When your CDE window pops upopen a new terminal and, with a Kahuna prompt displayed, enter

/usr/local/bin/pro18.

You are now in Pro/E.

Remember, files are saved in your account directory.

Room E 101A

Turn on the computer and monitor. After the machine boots, there will be a message telling you to press CONTROL-ALT-DEL to log on. After you press these keys, the next prompt will be for a user name and password. Consult the instructor for the current info. Login will bring you to an introduction screen. Pro/E will use a default directory for storing your part files if you do not specify another one. During the semester, many files are generated and purged, so save your files on your own floppy if possible. Next use the "PRO_E v.18" icon to start Pro/ENGINEER. The Pro-E icon is located under the PTC program group which is under PROGRAM MANAGER.

After Pro-E starts, switch to your personal directory (on a floppy). Under the MAIN menu click on Misc then Change Dir. There will be a prompt on the command line at the bottom of the screen to Enter NEW DIRECTORY name: - enter the path of your personal directory - something like a:\ will put files onto your floppy. A message should appear "Successfully changed to (your directory)". Entering a ? will allow you to browse for a new path.

We are now ready to start a part. First though, note that throughout the tutorial intended menu command choices will be represented by the capitalized names of the menu choices you should use all separated by hyphens. Thus, under the menu Main and then Mode, the two commands Part-Create should be clicked with the mouse one after the other to start your new part. A prompt to name the part will appear in the message window at the bottom of the screen. Type in a part name and press Enter (simply pressing Enter will accept the default part name).

After starting a part, saving it is a good idea. Under MAIN click DBMS then Save. A prompt will appear in the message window to enter the file name to save. Your current file name will be the default. Press Enter to accept the default. Frequent file saving is recommended - after each successful feature creation is a good idea in the beginning. This will allow you to recover your previous work if you encounter a major problem and have to bail out when creating the next feature.

The next step is to create a datum system in three dimensional space. Under Mode- Part-Retrieve type in a part name and then select Feature-Create-Datum-Plane-Default. The screen will show three orthogonally intersecting planes called Datum. These are features of your design that anchor it in the program's working space.

We will now start to create features of a part by choosing a sketching plane and reference plane. Under MODE-PART-FEATURE-FEAT select Create-Solid-Protrusion-Extrude-Solid-Done (Extrude and Solid are default highlighted selections). The next menu will be ATTRIBUTES with the choice of One Side or Both Sides. Select One Side then Done. The SETUP SK PLN menu will appear. Select Setup New-Plane-Pick then click on the part window on the tag "DTM2". A red arrow will appear on the screen to show the direction of next feature creation and the DIRECTION menu will come up with the choices Flip or Okay - pick Okay. The next step is to establish a reference plane to orient the sketching plane. Under SKET VIEW select top then on the screen click on the tag "DTM3". The datum screen will now be replaced with the Sketcher screen. Sketcher is where the 2 dimensional outline of a feature is drawn and dimensioned. The outline is then extruded (or revolved, or swept, or blended) to form a 3-dimensional solid. It's now time to sketch the outline of the shape which will then be extruded to form the car body.

The default menu choice in Sketcher is Mouse Sketch. Place the cursor at the intersection of the datum planes in the center of the screen and click the left mouse button. Sketch the outline as shown, using the left mouse button to end each line segment. Click the center button to stop drawing lines. If you wish to delete any segments, click the right button to stop drawing lines, choose Delete under SKETCHER, and click on any segments that you wish to remove. When finished deleting, choose Sketch under SKETCHER to resume Mouse Sketch mode.

When the outline sketch is completed it must be attached to the datum system and dimensioned. The first step is alignment. Under SKETCHER select Alignment. You will align the left end of the body to DTM1 and the bottom edge to DTM3. Click twice on the line segment that forms the left end of the car. The word ALIGNED should appear in the message window at the bottom of the screen. If you were successful (and I really hope that you were), proceed to align the bottom segment to DTM3 by clicking where shown in Figure 3. If not, keep trying to click on the coorect line segment. The sketch should now be "attached" to the reference datum system. All the dimensional parameters may now be added. Under SKETCHER select Dimension. For simplicity, all dimensions will be referenced to the datum system and intersection points in this sketch. First place the vertical dimensions. Begin by left clicking on the datum line (shown as(1)) then left click on the first intersection (shown as (2)). To place the dimension, position the cursor where shown (3) then click the center mouse button. Dimension lines will be drawn and the symbol sd2 will be shown instead of a numerical dimension. Don't worry about the value of the dimensions, they will be modified after Regeneration in which the computer redraws the part model. Continue to place all the dimensions as shown.

After all the dimensions are placed it's time to perform the first Regeneration. During Regeneration the program analyses the sketched view, alignments, and dimensions to determine if the sketch is properly constrained. A properly constrained sketch is one where there are sufficient (but not too many) dimensions and alignments to define the geometry of the sketch and to locate the sketch to the existing part. In this case, the existing part is the datum system. (Note: This means that the sketched feature is a child of the datum system and the datum system is a parent of this sketched feature. Although we will address these relationships only briefly here, they are a very important factor when designing with Pro/E.) To Regenerate, select Regenerate under SKETCHER.

If you have followed the instructions carefully the message "Regeneration completed successfully." will appear in the message window, the sketch will look as shown with the dimension codes replaced with numerical values, and the command Modify highlighted under the SKETCHER menu. This is a Good Thing. The other possibility is that the message "Regeneration failed..." with some explanatory text appears. This is a Bad Thing and must be corrected before the program will let you proceed. Failure to Regenerate may be the most common and frustrating problem encountered by beginning Pro/E users. Often the problem is simple - for instance finding and fixing an omitted or double dimension. Other problems may be so obscure that the only recourse is to exit SKETCHER (Quit-...) and redo the sketch. All I'll say here is good luck and do what you have to to successfully Regenerate. If you must exit SKETCHER, you'll usually come out at the point where the datum planes have been created and then select Create-Solid-Protrusion....

As indicated earlier, after successful Regeneration the default menu selection will be Modify. Regeneration is always a two (minimum) step process - define geometry then modify values. Select a dimension by left clicking. The dimension will change color from yellow to red and the prompt "Enter a new value:" will appear in the message window. Type in the new value (see figure) and press Enter. The modified value will show in white. After modifying all the dimensions, Regenerate again. If the successful Regeneration message appears (it should), select Done in the menu box directly under the SKETCHER menu box. The SPEC TO menu will appear - select Blind-Done. In the message window will be a prompt to enter depth. From the keyboard input 2 then under FEATURE EDIT select Done. The message window will say "PROTRUSION has been created successfully." To see the part in three dimensions, select View under MAIN then Default under ORIENTATION. Congratulations! You are now a Solid Modeler!

Okay, enough admiring your work. It's time to round the sharp edges. Again, for simplicity this will be done in several steps. The first edges to be rounded are the intersections of the hood with the windshield and the trunk with the rear window. Under FEATURE-FEAT select Create-Solid-Round-SIMPLE-DONE-CONSTANT-EDGE CHAIN-DONE-PICK -one by one-DONE then under RADIUS VAL select Enter. The prompt will appear in the message window to "Enter RADIUS". Input a value of .12 then press Enter. Now, round the front and rear edges of the roof. Use a value of .15 here. On your own, round the front edge of the hood and the rear edge of the trunk to .25. The last edges to be rounded are the left and right top edges. Enter a value of .25 to complete the rounding. Note that sometimes the value you may choose for a round is forbidden by some of the choices already made for other features. Also, dimensioning to a feature location where a round becomes tangent or merges into some other feature is very bad practice. Find another location for that dimension.

At this point we'll investigate one of the most fun options - the Spin command. Spin allows you to use the mouse to spin your model on the screen in three dimensions. Under MAIN select View-Orientation-Spin then position the cursor in the center of the model and click the center mouse button. Movement of the mouse will now spin the model in various directions. Experiment with different movements to find out how to control the orientation. (Note: if the cursor is moved out of the active window, spinning will stop but Spin is still active.) To cancel Spin, insure that the cursor is positioned inside the active window and click the middle mouse button again. When you are finished using Spin, leave the model with the bottom surface visible.

The next command -Shell- is very powerful. Shell allows you to remove the inside of almost any shape that you have created, leaving a constant-thickness wall. Under FEATURE-FEAT; select Create-Solid-Shell-pick (now select the bottom surface of the car shape with the mouse. This may require you to rotate the part to select that surface) -done select-pick-remove-done select-done refs. Now enter the thickness. Input .12 then Done. If you're not impressed with Pro/E at this point, then I don't know what will impress you. If you want, now is a good time to Spin the model again. The menu items to choose are View under MAIN then Orientation-Spin.

Well, your model is looking better all the time. Let's cut some more of it away. The Cut command is one of the most versatile in Pro/E and will be used three times to complete your model. The first cut we'll make is for the wheel wells. Choose View-Default to orient the part then under FEAT select Create-Solid-Cut-Extrude-Solid-Done. In the next set of menus select One Side-Done and use defaults. Select the tag for DTM2 for the sketching plane. The red arrow (direction of feature creation) on the screen should point "into" the model - if it does not, select Flip. When the arrow is pointing into the model select Okay. When prompted for a reference plane select Top and pick on the tag DTM3. Here we are, back in Sketcher.

As before, the default in Sketcher is Mouse Sketch. The last time we drew straight lines - let's try some circles. In Mouse Sketch, the center button automatically draw's circles. Place the cursor at the center of the first wheel well (see fig.) and click the center mouse button once. This will place the center of the circle. Start moving the mouse and you will drag the diameter of the circle. Clicking the center button a second time will set the diameter. Place two circles, located as shown in the figure. Try to be as accurate as possible - this will allow you to utilize the assumptions in Sketcher. Although assumptions may be confusing at times, they can be very helpful. In this case, if the two circles are drawn the same size (use the grid marks as an aid) then only one will need a diameter dimension. After the circles are drawn, align them to the bottom of the car. Select Alignment then click twice on the crosshairs at the center of each circle. After each pair of clicks the word ALIGNED should appear in the message window. The aligning has taken care of the vertical location of the wheel wells. To locate the wheel cut-outs in the horizontal direction select Dimension. Again, for simplicity we will dimension to the datum plane. Click once on the center mark of each circle, once on datum 1, then place the dimension using the center mouse button. To dimension the diameter of the circle, left click twice on the perimeter of the circle (clicking once on a circle produces a radial dimension, two clicks produces a diameter). After double clicking on the circle use the center mouse button to place the dimension.

All dimensioned and aligned? Select Regenerate. If Regeneration is successful, modify the dimensions as shown then Regenerate again. If Regeneration fails, see previous comments regarding Failure to Regenerate. After successful Regeneration, modifying of dimensions, and Regeneration again select Done. An arrow will appear along with a prompt indicating that arrow points toward area to be removed. The arrow should point "inside" the wheel - if it doesn't, select Flip. When the arrow is pointing into the circle, select Okay. Since this cut will extend the complete width of the body, select Thru All under SPEC TO then Done-Done. Save the model, then Spin if desired. When finished spinning, select View-Default.

Next step is cutting out the windshield and rear window. Under FEAT select Create-Solid-Cut-Extrude-Solid-Done-One Side-Done then pick on the tag DTM1. The arrow for feature creation should point into the model - if not, Flip the arrow - then select Okay. For the horizontal reference plane select Top then pick on the tag DTM3. You are now back in Sketcher mode.

Using the left mouse button, sketch the box as shown. Select Dimension then dimension as shown. Regenerate, modify dimensions, and regenerate again.

We will now add the corner radii using the fillet command. Select Sketch-Arc-Fillet then pick the top horizontal line and the left vertical line approximately where shown. (Note: The distance from the corner that the fillet selection point is picked will determine how large the fillet is initially drawn. If all points are picked the same distance from their respective corners, all the fillets will be drawn the same size and only one will need to be dimensioned.)

Pick points to create the other three fillets then select Dimension and dimension one fillet (remember, single click on an arc to create a radial dimension). Note that dimnsions establish themselves relative to fillet centers. Regenerate, Modify the arc dimension to .05, Regenerate then Done. The arrow for material removal direction should point into the window - if not, Flip - then select Okay. Under SPEC TO select Thru All-Done-Done. The front and rear windows are now done - select View-Spin to rotate the model, select Default when finished admiring.

The last cut for this model will create side windows. Under FEAT select Create-Solid-Cut-Extrude-Solid-Done-One Side-Done then pick on the tag DTM2. The arrow for feature creation should point into the model - if not, Flip the arrow - then select Okay. For the horizontal reference plane select Top then pick on the tag DTM3.

Sketch as shown - try to make the angled front and rear lines as parallel as possible to the model edges. Dimension as shown, Regenerate, Modify dimensions, and Regenerate.

Add the corner fillets using Sketch-Arc-Fillet. As these lines meet at different angles it may be very difficult to create equal arcs. Because of this, dimension all four of the fillets as shown. Regenerate, Modify, and Regenerate. Verify that the arrow points inside the window then select Okay. To complete the Cut, Select Thru All-Done-Done.

For a final touch, let's view a shaded model. Under Main select Environment. Under Environment, click on Disp DtmPln and Disp Axes to turn off these options (the check marks will disappear). In the next box down select Shading, then Done-Return. The shaded model may be rotated under View-Spin.