Reference Sheet for Pro/DESKTOP

Pro/DESKTOP Features
Page 100
Reference Guide for Pro/DESKTOP Features
Extrude Profile Feature
Concept: Extruding a 3D shape requires a valid 2D sketch. A valid sketch is a closed profile, that is, a continuous
line that encloses a space. A simple example of a valid profile is a circle or a rectangle. You can create much more
complex valid 2D shapes by overlapping circles, ellipses, squares, rectangles, and other shapes, but you must delete
lines that do not form a valid profile of a shape. The exception to the valid profile requirement is the “Thin”
command explained on page 100.
•
Draw a shape using the “Drawing Tools”.
(Multiple profiles can be extruded at the same time, as long
as they do not overlap)
Hint: Holding the shift key while using the rectangle tool
produces a square
•
Click on the “Extrude icon” in the Features window or select
from the Menu Bar, Feature > Extrude Profile.
•
Click and drag the yellow handle up until you get the Extruded shape
you want.
Or, you may enter a value in the Distance box in the
dialogue box.
•
Click and drag the green handle to add a taper (inward or outward) to
the shape.
Or, you may enter a value (in degrees) for the taper angle.
•
Click OK. (Notice that all the dimensions
are automatically placed in the dialogue
box)
Pro/DESKTOP Features
Page 101
Advanced Features of Extrude
Thin Command
•
•
•
•
•
Any non-enclosed shape or profile may
be Extruded using the “Thin” Command
in the Extrude Dialogue Box.
Draw a line using the Spline Tool.
Click on the Extrude icon or select it
from the Menu Bar, Feature >
Extrude Profile.
Check the Thin button and
define a Thickness for the
Extrusion.
If the Symmetric button is
checked then the Thickness (in)
will be even on both sides of the
path drawn.
•
If you unclick the Symmetric
button you can specify the
Thickness of the material on
both sides of the path drawn.
•
The red arrow in the drawing
window specifies the side of the
path where the material will be
added. To reverse this, click on
Other Side.
•
To sketch without entering
dimensions, click and drag the
yellow handle to Extrude a
shape. Use the orange handles
to define a “Thickness” and the
green handle to add a taper to
the shape.
Pro/DESKTOP Features
Page 102
Using the Intersect Material Command
•
•
Draw and Extrude a shape. Use the Select Faces tool to
highlight and select the top surface of the Extruded shape.
•
Add a New Workplane and a New Sketch to
the selected face. (Just right click and select
New Sketch; a New Workplane will automatically be
added because you selected and highlighted a face)
•
Draw a profile (in this case a circle).
•
Click the Extrude Profile icon and select
Intersect Material and Below the Workplane.
•
Drag the yellow handle down past the bottom
or specify a dimension in the Dialogue Box.
Finished Intersected Shape
Click OK.
Pro/DESKTOP Features
Page 103
Subtracting Material Using The Thin Command
•
•
•
•
You can also subtract material along a path from a
shape using the Thin command.
Add a New Sketch and a New Workplane to a face and
draw a path.
Select Subtract Material and Below the Workplane and
define a Thickness in the Dialogue Box.
Drag the yellow handle (turns blue on mouse-over) or
define a depth for the Extrusion in the Distance part of
the Dialogue Box.
Finished Thin Subtraction
•
Click OK.
Tips:
•
•
Drag the dialogue box away to uncover the workplane.
The handles turn blue on mouse-over.
Project Profile Feature
Concept: The Project Feature either adds or subtracts material from a solid. Unlike the Extrude command, no
distance dimension is required. Instead, with the Project command you specify the extent of the projection in one
of three ways: to the next face of the object; thru the entire object; or to a selected face of the object. Like the
Extrude command, there is a Thin option.
•
On an Extruded shape, select a face by clicking on
the Select Faces icon and highlight an outside
edge of the side you wish to select. (The selected
face will turn red).
Pro/DESKTOP Features
Page 104
•
Add a New Workplane and a New Sketch to the selected face.
(Just right click and select New Sketch - a New Workplane
will automatically be added because you selected and
highlighted a face)
•
Enter a label in the Name box for this New Sketch and New
Workplane for future reference.
•
Click OK.
•
Click on a “Drawing Tool” and draw the shape you wish to
Project on the new sketch. In this case it is a circle.
Click on the Project icon in the Features Window or
from the Menu Bar select Feature > Project Profile.
•
Give the Project Profile Feature a name for future reference
and choose Add or Subtract material from the dialogue box.
Pro/DESKTOP Features
Page 105
•
Choose Above Workplane or Below Workplane from the dialogue box.
(The new green arrow will define the
direction of the projection).
•
Select how far the Projection
should go.
•
Click OK.
Finished Projected Hole
Pro/DESKTOP Features
Page 106
Using the Thin Command with Project
•
Extrude a shape and place a new Workplane and Sketch on the side.
•
Draw a shape on this Sketch/Workplane.
•
Project Profile
•
Select Subtract Material and Below Workplane.
•
Check the Thin box and Symmetric box and type in a dimension for the Thickness.
•
Click OK.
Finished Thin Projection
Tip: If the Project Profile reports an error message, check to see if you have specified the proper direction
of the Projection (Above or Below the Workplane).
Revolve Feature
Concept: The revolve Feature produces a solid similar to the way a lathe produces an object. A profile is revolved
around an axis. Two sketches are required - one for the axis and one for the profile. These Sketches need to be on
the same Workplane.
•
•
In a New Sketch draw an axis line around
which the profile will be revolved.
(Hold down the shift key to draw a straight line
along the x or y axis of the drawing)
Rename the Sketch axis to so you can keep
track of which sketch is which.
Pro/DESKTOP Features
Page 107
•
Add a New Sketch to this Workplane and name it
profile for future reference.
(Note that only a New Sketch is added, not a New
Workplane)
•
Draw the profile of a shape to be Revolved.
The profile must not have any intersecting lines; it must be a valid profile.
•
Click on the “Delete Line Segment” icon to cut out lines to produce a valid profile, as in the
illustration above right.
•
Click on the Revolve icon in the Features Window or pull down from the Menu Bar
Feature > Revolve Profile and drag the yellow handle
around to complete the revolve.
(The yellow handle turns red on mouse-over)
•
You can also specify Add material or
Subtract material and the Angle of
Revolution in the dialogue box.
•
Click OK.
Pro/DESKTOP Features
Page 108
Finished Revolve
Tip: If the Revolve Profile does not work, make sure that you have specified a New Sketch before drawing
the profile of the Revolve.
NOTES
Pro/DESKTOP Features
Page 109
Sweep Feature
Concept: The Sweep Feature allows you to add or subtract material along a path that you create. It can also be
used to add or subtract material along an existing edge of an object.
The Sweep Feature requires two sketches on two workplanes: a path sketch on one workplane and a profile sketch
on another workplane. It also requires that the profile be perpendicular to the path – which is sometimes difficult.
•
Draw the path of the shape you wish to Sweep.
If you can, start at
the 0,0 coordinate
as indicated under
Snap to Grid.
•
•
•
Click Select
Workplanes.
Select the Workplane that bisects the profile you have drawn,
click on it to highlight.
Add a New Sketch to this Workplane and label it as profile.
(Just right click and select New Sketch)
•
Pro/DESKTOP Features
Shift-W to change the view onto this Workplane.
Page 110
•
Draw the profile of the shape you wish to Sweep.
You can use the cursor keys to angle it slightly so
you can see the path.
•
•
Click on the Sweep icon or pull down from the Menu
Bar, Feature > Sweep Profile.
Click OK.
Finished Sweep
Modifying the Sweep Shape
•
•
You can change the path or the profile of the Sweep after rendering by clicking on the Select Lines icon
(as long as you do not change the perpendicular relationship).
Highlight the path or profile by double clicking on it till it turns red:
Pro/DESKTOP Features
Page 111
Resize Circle Icon
Move Circle Icon
•
Make changes to the path or the profile.
•
Click on the Update icon:
•
The new path or profile will be recalculated and updated:
Tip: If the sweep brings up an error message, check to see that you don’t have any intersecting shapes or
a shape that wraps back on itself too tightly. Another common problem is that of having the profile shape
exactly perpendicular to the path. This can only be practically achieved by using intersecting workplanes.
Pro/DESKTOP Features
Page 112
Loft Feature
Concept: Lofting is a familiar term to the boat building industry, where a number of cross-section shapes are used
to form the shape of the hull. In Pro/DESKTOP, the Loft Feature is used to create a solid using two or more crosssection sketches drawn on separate workplanes.
•
Draw a shape on the Base Workplane.
•
From the pull down Menu Bar select Workplane > New Workplane and click Offset.
•
Drag the yellow handle up to create an offset
Workplane (or you can enter an Offset
distance).
•
C
l
ick OK and add a New Sketch to this Workplane. Notice
that the Offset Dimension appears in the dialogue box.
(Right click to Add Sketch)
•
Draw a second shape on this New Work Plane.
Pro/DESKTOP Features
Page 113
•
Use the Select Lines tool to select all the lines used for
the loft.
(Hold down the Shift Key to select multiple lines)
•
In the Menu Bar Click on
Feature > Loft Through Profiles and
select Add material. Make sure that all
the Sketches are listed that you wish to
Loft through.
•
If there is a mathematical problem with
the profiles, you can try moving the path of the Loft by
double clicking on the initial sketch in the dialogue box
and dragging the yellow handle until it intersects the
profiles correctly.
•
Click OK.
Finished Loft
NOTES
Pro/DESKTOP Features
Page 114
Tips: Check to see if all the shapes to be Lofted are showing in the dialogue box.
On profiles with more complex shapes you may need to manipulate the loft line. By selecting the profile
sketch in the dialogue box, a yellow square will appear, and it can be dragged to the appropriate corner of
the sketch. You might need to experiment with complex shapes to get a valid loft.
Shell Command
Concept: Many manufactured shapes are shells, such as the case for a cell phone. Pro/DESKTOP automates the
development of a shell with this command. You may specify an open face into the interior space by selecting that
face before you use the command. If you do not select a face, the object will be hollow.
•
Select any face of an extruded object using the Select Faces tool. If you do not click on a face and use the
Shell Solids tool, you will create a hollow object.
•
Click on the Shell Solids icon.
Pro/DESKTOP Features
Page 115
•
Click and drag the yellow handle to the desired wall thickness or type in an Offset dimension in the
dialogue box.
•
Click OK.
Finished Shell
Solid
Pro/DESKTOP Features
Page 116
Sweep Profile Along Helix
Concept: Creating springs, internal or external threads is relatively easy in Pro/DESKTOP by creating an axis line in
one sketch and a profile shape in another sketch. The length of the axis line will determine the length of the helix.
You can either add or subtract material with this feature.
•
Shift – W to view onto workplane and then draw an axis line to Sweep the Helix around.
(Hold the Shift Key down to draw a straight line)
•
Create a New Sketch
on this Workplane.
•
Draw the profile of the
shape to Sweep Profile
Along Helix. In this
case, a rectangle.
•
Select Feature > Sweep Profile > Along Helix.
•
Drag the yellow handle to the desired pitch.
•
Click OK.
Finished Sweep
Along Helix
Tip: As with the other Features, you can modify the size, shape and pitch of the finished Sweep by clicking
on Select Lines tool and double clicking on the lines to be changed:
Click the Update icon to render.
Pro/DESKTOP Features
Page 117
Compressing and Sending Files Via E-Mail
To Compress Individual Files for E-Mailing:
(Do this for each file in your project)
•
•
Open all the .des files in
Pro/DESKTOP.
Select Features in the
Browser Window.
•
Click and drag the finish flag to the top
(arrows below).
•
Click on Update light then click Select lines tool
to show the part geometry.
All the necessary information associated with the
part is included without the large file size
after rendering in
3-D.
Pro/DESKTOP Features
Page 118
Part geometry
without 3D
rendering
•
Save and send as an E-Mail attachment.
To Open a Compressed File:
(Reverse order from compressing files)
• Open the file.
• Select the Features Window in the Browser.
• Drag the finish flag to the bottom.
• Click on the update light.
• The file will render in 3-D.
To Send a Completed Assembly Along With the
Associated Files:
•
Open the assembly file you have created.
•
Go to File> Save Copy As
Pro/DESKTOP Features
Page 119
•
In the dialogue box (Do you want to save copies of all the reference files?), Click Yes.
•
Define a location (Desktop) for the folder and give the folder a name (in this case, Fred’s Files).
•
Click OK.
• Attach to E-Mail and send.
Pro/DESKTOP Features
Page 120
Shortcut Keys
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
Arc Drawing Tool = [T]
Autoscale = [Shift + A]
Autoscale Selection = [Shift + S]
Circle Drawing tool = [C]
Components Browser = [Shift + C]
Configurations = [Alt + 3]
Constraints = [N]
Delete Line Segments = [D]
Design Rules = [Alt + 2]
Dimension Constraint = [Z]
Duplicate = [CTRL + D]
Edges, Select = [ E]
Ellipse Drawing Tool = [I]
Enhanced View = [F12]
Faces, Select = [F]
Feature Browser = [Shift + E]
Features, Select = [A]
Front Elevation = [Shift + N]
Half Scale = [Shift + H]
Hide Other Sketches = [CTRL + H]
Isometric View = [Shift + I]
Line, Select = [L]
Manipulate View = [Space Bar]
New File = [CTRL +N]
New Sketch = [CTRL + K]
New Workplane = [CTRL + L]
Next View = [ALT + Right Cursor]
Onto Face = [Shift + F]
Pro/DESKTOP Features
Page 121
Onto Workplane = [Shift + W]
Open = [CTRL +O]
Parts, Select = [P]
Plan View = [Shift + P]
Previous View = [ALT + Left Cursor]
Print = [CTRL + P]
Rectangle Drawing Tool = [R]
Right Elevation = [CTRL +R]
Save = [CTRL + S]
Select All = [CTRL + A]
Shaded View = [F10]
Spline Drawing Tool = [B]
Straight Line = [S]
Toggle Construction = [CTRL + G]
Toggle Fix = [CTRL + F]
Toggle Reference = [CTRL +R]
Toggle Sketch Filled = [CTRL + Shift +F]
Toggle Sketch Rigid = [CTRL + Shift + R]
Transparent View = [F11]
Trimetric View = [Shift +T]
Tumble = [Shift + W]
Undo = [CTRL + Z]
Update Design = [F5]
Wireframe View + [F9]
Workplanes Browser = [Shift +Z]
Workplanes, Select = [W]
Zoom In = [Shift + Z]
NOTES
Pro/DESKTOP Features
Page 122