Generation of 2D Engineering Drawings
Creating a 2D Drawing for the Component BASE
Figure 1 2-D Drawing of the Component BASE
A 2-D drawing of the component BASE is shown in Figure 1. This drawing can be produced
using Pro/ENGINEER 2001 through the following steps:
1. Naming the drawing and choosing drawing size/orientation
In the main menu, choose File → New, select Drawing in the radio button in New window,
enter a drawing name BASE, uncheck Use default template and click Ok to create a
drawing called BASE.DRW. In the pop-up New Drawing window, input the optional
default model that is base.prt in the Name window, select Empty for Specify template,
Landscape for Orientation, Standard Size A for Size, and click OK.
2. Framing the drawing automatically or manually
Choose DRAWING → Sheets, SHEETS → Format, DRAW FORMAT → Add/Replace,
Unblank, Open window will show the already-made frame, select a.frm and click Open.
The frame will frame the drawing screen.
If one draws the boarder lines and the tittle box of the draft, choose SKETCH → LINE.
3 Multiple view creation and layout
(1) Creating top view
In Manu Manager window, Choose DRAWING → Views, VIEWS → Add View,
VIEW TYPE → General, Full View, No Xsec, Scale, Done. Select the center point of
the top view in the working window, enter 0.4 in the command window as the scale for
the view, then Orientation window appears.
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In this window, choose Type → Orient By Reference, Reference 1 → Front, GET
SELECT → Pick, pick up the top surface of the component. Choose Reference 2 →
Bottom, pick up the front surface of the component, and click Ok.
(2) Creating front and right views
In Menu Manager window, choose DRAWING → Views, VIEWS → Add View,
VIEW TYPE → Projection, Full View, No Xsec, No Scale, Done. Select the center
point of the front view. Repeatedly, choose VIEWS → Add View, VIEW TYPE →
Projection, Full View, No Xsec, No Scale, Done, select the center point of the right
view.
(3) Creating an isometric view
Choose VIEWS → Add View, VIEW TYPE → General, Full View, No Xsec, Scale,
Done, select the center point of the isometric view, enter 0.3 in the command window as
the scale for the view. In the pop-up Orientation window, choose Ok. The three views
and an isometric view are in the drawing frame. VIEWS → Move View, pick up one
view to an appropriate place. Select the two scale labels and drag them to appropriate
locations using drag handles. The drawing is shown in Figure 2.
Figure 2 A drawing of the Component Base in the Drawing Process
4. Changing the drawing configuration
In Menu Manager window, choose DRAWING → Advanced, ADV DWG OPTS → Draw
Setup. Notepad text editor with the drawing configuration file is popped up and change the
following parameters:
Table 1 The Modified Drawing Configuration Parameters
Parameters Values
drawing_text_height 0.1
draw_arrow_style FILLED
text_orientation PARALLEL
draw_arrow_width 0.04
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draw_arrow_length 0.12
tol_display YES
Choose FORMAT → Decimal Places, enter number of decimal places for value as 1.
5. Showing the dimension, center lines and tolerance (drawing modification)
Choose VIEW from the Pro/E pull-down (model window) menu, → Show/Erase,
Show/Erase window comes up, click Show, in Type zone, choose the dimension button,
tolerance button, and Axis button. In Show By zone, choose Feature radio button, and
accept all default options in the window, click Show All. Confirm window pops up, Yes to
the question. Those items appear in the drawing. Then Accept All and close in Show/Erase
window. The dimensions, centerlines and tolerances are all there.
6. Cleaning the dimensions
Choose DRAWING → Tools → Clean Dims, and Clean Dimensions window is shown,
GET SELECT → Pick Many, PICK MANY → Pick Box, Inside Box. Drag the cursor
from one corner to the other diagonal corner of the rectangle draft area and form a
rectangle in which the dimensions will be relocated to clear visibility.
Erase some unimportant dimensions, choose VIEW→ Show/Erase, Show/Erase window
comes up, click Erase, in Type zone, choose the dimension button, in Erase by zone, choose
Selected Items. Pick those dimensions to be deleted, GET SELECT → Done Sel.
Add the user defined dimensions, choose INSERT→ Dimension → New References, use
the left mouse button to select two points or two lines, and middle mouse button to specify
the location of the dimension value, then select the dimension orientation. To dimension
the locations of the holes, one can select the circle and the edge, Pro/E 2000i2 will
automatically dimension the edge to the center of the circle. Pick up dimensions and move
them to appropriate locations using drag handles. Up to now, the draft is shown in Figure
3.
7. Switch the dimensions between the views
To evenly distribute the dimensions, pick the clouded dimensions one at a time, EDIT →
Switch to View, and pick one point in the other view, then the dimension switches to there.
Pick the dimension to an appropriate place or the dimension text around using drag
handles.
8. Flip Arrows
When the space is tight for the dimension arrow, flip the arrow by pick the dimension
arrow, click EDIT → Properties → Flip Arrows and the arrow will change its directions
for better looking.
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Figure 3 A Draft of the Base Part
9. Editing the dimension value and its tolerance
To change the dimension value and/or its tolerance, pick the dimension, choose EDIT→
Properties. In the Dimension Properties window, four different Tolerance Modes can be
selected, and Upper Tolerance and Lower Tolerance can be fed in new numbers, or even
one can change the Dim Format and Number of Digits. Click Ok. New dimension will
appear.
10. Documenting the draft
To make the notes of title and date, choose INSERT→ Note → Make Note, click the
desired location of the note on the screen, type in TITLE, and hit return key twice.
Following the same procedure, enter the note DATE.
To change the height of the texts and move them to the ideal locations, pick note TITLE,
EDIT → Properties. In the Text Style dialog box, click the Use Default check box regarding
Height parameter, and enter the value as 0.15, click Apply button and Close button of the
dialog box. Pick up the note TITLE: and move it to appropriate location using drag
handles. Following the same procedure, modify the height of note DATE: and move it to
the appropriate location. Choose DETAIL → Done/Return. (See Figure 4)
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Figure 4 A Standard Drawing of the Base Component
11. Saving the drawing to a file
Choose File → Save, or press the desktop saving icon, accept the drawing name
BASE.DRW.
12. Plotting the created drawing
Choose the main menu File → Print → MS Printer Manager → OK. One can also export
the drawing to other types of CAD model or to an image by choosing File → Save a copy.
13. Exit the window
Choose File → Exit.
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