Pro/DESKTOP is a feature based solid modelling and assembly modelling package with an inbuilt feature-based drafting package designed to run on a PC.

Version 8 differs from previous versions as it is built on the same platform as Pro/Engineer and because of this files can now be transferred between these two packages.

The software has three major parts to it being 3D Design, 2D drafting and a 3D Album or visualisation package. All three parts of the software interact and changes made to one effect the others. This is the meaning of Parametric Design.

The first package we will look at is the 3D design.

Pro/DESKTOP can be controlled using descriptive menu bars or by selecting the options from regular windows pull down menus.

The Views Toolbar
• Wire Frame	• Shaded
• Transparent	• Enhanced
• Trimetric	• Section
• Auto-scale	• Auto-scale selection
• Zoom in	• Zoom Out
• View options	• Toggle back through views
• Toggle forward through views	• Tumble
View Options Drop-down menu

Pro/DESKTOP has comprehensive help tutorials available. These can be used in conjunction with this manual to help understand the software. These tutorials can be found under the Pro/DESKTOP help menu.

There are some simple rules when relating to selection within Pro/Desktop which are common to all areas of the software. It is important to understand these rules before you proceed with the rest of the course. When selecting any line, edge, face, component or in fact anything within the software the selection tool must first be found and selected from the Design toolbar.

Once this is selected, move the cursor over the item to be selected and you will see it turns BLUE. This means it is PRESELECTED. The item colored blue will be selected if you click the mouse. Once you have clicked the mouse, the line, edge, face or whatever you selected will now be colored in RED. Red indicates an item is SELECTED.

If you now want to drag or move the item you move back over it with the cursor and wait for the cursor to change to indicate the item can be manipulated.

No edges selected	Edge Pre-Selected
Edge Selected

To be able to use Pro/DESKTOP you must have an understanding of Features, Sketches and Workplanes.

The best way to think of workplanes is to think of them as drawing boards. If you want to draw on a face of an object or anywhere in a design first you need to create a workplane or drawing board. When you open a new design, you get 3 workplaces by default. They are the Base, Frontal and Lateral.

Sketches are like sheets of tracing paper and are placed on drawing boards. You cannot have a sketch unless it is on a drawing board or Workplane. You can have multiple sheets of tracing paper or sketches on the same drawing board. When you are drawing on one sketch, you can see the lines drawn on other sketches. The active piece of paper or sketch is always highlighted in black in the sketch list.

Features relate to solids within a design. A sketch is used to define a feature. If you create a feature from a sketch then any changes made to that sketch in the future will change the feature. If the sketch is deleted the feature will no longer be able to exist.

When looking at the menu bars on the screen you will notice that several of the icons are colored yellow. Yellow icons refer to Solids or Features. They allow you to create a feature or select a face, edge or part of a feature.

If you open a new design then draw a rectangle this is a sketch. The shading or "fill" indicates that the "Sketch is Valid" or is OK to use to create an extrusion.

With a new design there is an initial sketch created on the base Workplane by default. By looking in the Workplane design tree you can see the active sketch is called initial and is located on the base Workplane.

If a sketch is NOT VALID because lines overlap or the profile is not a closed boundary then the shading is not shown. The sketch is invalid and must be corrected before you try to make a feature from it.
Invalid Sketch	Valid Sketch
If you draw a rectangle then extrude it the resulting solid is a Feature and appears in the Feature list at the top left of the screen.
You can reselect a Feature and modify it from this Feature List.
Feature List showing Extrusion	Right Click to Modify
As designs are created you can select any feature in the list and redefine it at any time. Once the feature is changed you must refresh the design for the change to take effect.
Click to Refresh design when Green
If you now draw a circle it will be added to the active sketch, which is in this case the initial sketch.
Circle added to initial sketch
The Extrusion we defined is applied to all items drawn on the initial sketch, so as soon as we add to or modify the sketch the Green refresh light comes on. This indicates that the sketch defining a feature has changed and so the design needs to be updated. If we click the Update light the design is updated and the modified feature is shown.
	Click to Refresh design when Green
	Updated Feature
Example 2: Creating New Sketches and Workplanes
When you create a new design the software automatically creates three Workplanes and adds a sketch to the base Workplane. If we draw a rectangle on the initial sketch on the base Workplane and extrude this up we now have a block.
If we wanted to draw another item and extrude it higher than the block we have we must create a NEW SKETCH to define the new feature. If we add to the existing initial sketch then whatever we draw will be extruded to the same height as the block. Add a sketch to an existing Workplane We need to add a sketch to the base workplane. This is like adding another sheet of paper onto the base drawing board. To do this move the cursor over the Workplane folder named base and Right Click the mouse. Select New Sketch
You can now draw some additional geometry on the new sketch and create a new extrusion using the new sketch. The sketch can overlap lines on other sketches an will remain valid. The new extrusion can be any height.
The Workplane tree and Feature tree show the additional sketches and features.
Add a sketch and create a new Workplane If you want to draw on the top of the cylinder we need to add a sketch to the top face of the cylinder. To do this we must create a workplane or drawing board on this face and add a sketch or sheet of paper to the drawing board. If you try to add a sketch to a face where there is not already a drawing board then Pro/DESKTOP will automatically create this for you. Extrusion 2 New sketch can overlap other sketches First select the Face Selector tool from the Design toolbar and select the top face of the cylinder. Note as you move near the edge of the face it pre-highlights in Blue.
With the face pre-highlighted, left click the mouse and the face will be selected and colored in red. Right click the mouse anywhere on the screen or go to the workplane menu then select New Sketch.
The new sketch window appears and automatically suggests that a new Workplane is also created. You can now name the new sketch and Workplane or accept the default suggestions then click OK. Note: sketch 2 is in bold type so is the active sketch.
Now draw a rectangle on top of the cylinder Once the rectangle is drawn it can be extruded as shown.
Select the top face of the cylinder with the face selector tool.
From the Feature Menu or toolbar select the Round Edges feature and set the radius to 8mm
The Chamfer Edges feature works in the same way as the Round Edges feature. Just select the edges or faces prior to selecting the feature. Multiple edges or faces can be selected by holding down shift during the selection process.