Solide Documentation

Engineering and Technical Drawing Using Solid Edge Version 9 By Jerry Craig

SDC PUBLICATIONS

Schroff Development Corporation www.schroff.com

Solid Edge V9

2D Drawing

2D Drawing

21

2D Drawing

Solid Edge V9

2D Drawings may take two forms: 2D Sketches show the outlines and locations of multiple shapes or parts to be designed. 2D Profiles must be closed shapes with no entities inside or crossing the sketch. The sketch at the right may be used to create a part by selecting specific shapes then “cleaning up” the outline by trimming inner curves. The final shape must be a single series of connected lines and arcs.

Concept Sketch. (Cannot be used to create a part in this form).

Profile must be a closed figure with no internal lines.

Resulting 3D object with depth added.

Additional sketches were used to define the protrusion at the middle and the holes in the part after the initial shape was created.

22

Solid Edge V9

2D Drawing

Assembly Sketches (Layouts) These are used to define the critical geometry in a series of mating parts. Elements from the master sketch may be selected to create the individual parts. This assures that the parts are the correct size and are located in exactly the right place. Elements of the part sketches which are derived from the master sketch may be associated (linked) back to the master sketch. This means that any change in the master sketch will update all the associated parts.

Portions of the sketch were used to create the base of the roller assembly. Other portions of the same sketch will be used to create the opening for the wheel.

Modeling the wheel is done by selecting the large circle from the master sketch. The final assembly is shown with the parts modeled exactly as they fit.

As you can see, 2D sketches are the basis for much of the design and part creation process. These sketches can be very general at first then, exact sizes can be assigned later. All parts associated to the master sketches will re-size to the new dimensions.

23

2D Drawing

Solid Edge V9

Starting a 2D Sketch In this chapter all drawings will start from the Part Environment. Most of the commands and construction techniques are the same in other environments. If Solid Edge is already running, pop down the File menu .... Pick New … Select the More tab Use Normeng.par (inch)

For an introduction to 2D sketches, we will use the option to create a sketch. This option allows the designer to create an overall master outline showing major features of the part. When the actual part creation takes place, elements from the master sketch will be copied to the part outline sketch. • Selecting Sketch brings up the prompt: Watch the bottom left corner of the screen for instructions and prompts. • Pick the Front reference plane.

24

Solid Edge V9

2D Drawing 2D Sketch Window

2D Sketch Window Selecting a reference plane places a special window on the drawing. The view is looking straight at the selected reference plane. In this example the top and right planes appear as an edge and the front plane is the drawing surface.

Edge view of Right plane Edge view of Top plane

The profile will be created on the Front plane. The Drawing Tools Menu activates:

The sketch will be created on the surface of the Front plane.

Drawing Tools Menu Pick Tool Axis of Revolution Line* Arc Circle

DRAW

Rectangle Pattern* Fillet/Chamfer Trim/Extend

EDIT

Offset* Copy from Sketch* Construction/Entity Move* Smart Dimension Dimension

( Illustration from Solid Edge Online Help )

Explore the commands. Remember that each icon with a small arrow at the lower right corner has a Fly Out with additional commands.

Connect* Horizontal/Vertical* Tangent*

CONSTRAIN*

* Advanced concepts are discussed in the next chapter.

Equal*

25

2D Drawing

Solid Edge V9

Line Starting the line command displays the ribbon bar at the top of the screen. Click a start point and move the mouse. The length of the line and the angle will display.

Switch between line/arc

• You can type in a length and an angle in the dialog boxes. • While drawing a line you can switch to the arc command and back. Intent Zone

Line to Arc Clicking the arc button on the ribbon bar switches to the arc command. • An Intent Zone icon is displayed on the end of the line. Moving the mouse through the 4 sectors produces a different result for each sector.

Special Line Options Curve: Click points (square boxes) to define a series of tangent arcs. The radius of each arc is determined by the direction of the previous and next points.

Line

Curve

FreeSketch and FreeForm will be discussed in the next chapter.

26

FreeSketch

FreeForm

Solid Edge V9

2D Drawing

Arc From the fly out menu, 3 options are possible. Tangent

3 Points

Center, Start, End

Depending on the option chosen, (line or arc) exact sizes may be set using the ribbon bar. Note: In some constructions it is easier and more accurate to draw a full circle then trim to define an arc.

Circle 5 options are shown on the circle fly out. Center 3 Points Tangent Ellipse Ellipse Radius/ 3 Points Center Diameter 2 Points The ribbon bar accepts either diameter or radius. Tangent can be: • Tangent to one entity • Tangent to two entities including the reference planes. You can set the radius then move the circle tangent. Many options exist. Try different commands and ways of using the commands. Online Help gives excellent instructions for the use of each option.

27

2D Drawing

Solid Edge V9

Rectangle Three construction methods are available: • Use dialog boxes. Input Width, Height and Angle. • Click two points for the width and one point for the height. • Draw a diagonal sketch line with the mouse.

Sketch Diagonal Line

Rectangle Constructed

Sketch Editing Tools Select Tool

Used to select entities for editing. Hold down the CTRL Key to select multiple entities. To delete an entity, select it and press the Delete Key

Fillet/Chamfer

Fillet will round a corner or add an arc between two entities. Often, Fillet is the easiest way to create an arc when the start/end/center points are not well defined. Chamfer will bevel a corner. The bevel can be the same angle or distance on both sides or, the bevel may be a different distance or angle on each side. Note the expanded ribbon bar.

A

Small rounds, fillets and chamfers should usually be added to the solid model after the major shape has been created.

B

28

Solid Edge V9

2D Drawing

Trim/Extend Trim line Trim

Trim

Extend

Trim is used to remove segments of entities. The segments are defined by intersections on the sketch. Multiple segments may be trimmed by sketching a line through each entity. Extend will cause entities to intersect. extend will not work if one entity does not provide a stop for the entity being extended. • You can extend a line by selecting the line and keying in a new length in the dialog box.

Construction Lines Any entity may be designated as a construction element. This means that it is used to define geometry but is not considered as a part of the outline shape.

Construction lines were used to locate the center for the circle. Converts entities to construction and visa-versa.

29

2D Drawing

Solid Edge V9

Move/Rotate/Mirror/Scale/Delete

Move Rotate Mirror Scale Delete Move. • First click the Select Tool. • Pick the object to move. (Hold down the CTRL Key to select multiple objects or use a window to select the objects within the window.) • Click where the object is now. • Click to set new location.

Dimensioning Smart Dimensions Use where one entity is to be dimensioned. • Line • Circle • Arc All the dimensions shown are Smart Dimensions. Standard Dimensions

Distance Angle Coor- Sym- Dimension Between dinate metric Axis To change the size of an entity on the drawing: • Select the dimension. • Type in a new size.

30

Solid Edge V9

2D Drawing

SketchPoint This is a drawing tool that allows entities to be placed in relation to another entity. • Select the Tools pop down • Click SketchPoint to turn on. SketchPoint will prompt for a target location. (Upper right corner of rectangle.) • Start a command (circle). • Set the diameter of the circle. • Move the mouse and note the distance reading. • Set exact distances using the SketchPoint dialog boxes.

SketchPoint Ribbon Bar

On/ Off

Set Target

Angle From Horizontal

Increments Set to .125 or ??

X-distance (Left/Right)

Y-distance (Up/Down)

Key in a distance or angle and press Enter to lock the value. To unlock the value, set the value to zero. • To turn off SketchPoint, press the ESC key or click the On/Off icon..

Display Commands As work progresses, the screen size may need to be changed. • Zoom Window - magnify • Zoom Out (shrink) • Fit (re-size to fit screen) • Pan (slide without changing size)

Main Toolbar- Top of Screen Zoom Zoom Fit Window Smaller

All allow for quick magnification, or re-sizing of the drawing image.

31

Pan

2D Drawing

Solid Edge V9

IntelliSketch

QuickPick

You may have noticed a number of symbols on the lines of the previous examples. These are geometric indicators which constrain the geometry. As you draw these symbols appear. The check box turns the momentary indicators on/off.

QuickPick is a tool used to sort out the correct item when several possibilities exist due to stacked geometry. Park the mouse for a few seconds and dots will appear. Left click for the selection box. Geometry highlights as numbers are selected.

Geometric Relationships As you draw some of the relationships are automatically set. Sketches must have the proper relationships between entities in order to create actual parts. Sketches must be properly constrained to create the intended objects.

Connect

Concentric

Tangent

Horizontal/Vertical Co-Linear Parallel Perpendicular • Remove a relationship by deleting the marker. • Add a relationship by selecting from the Relationships menu. This menu is near the bottom of the Draw Toolbar.

Equal

32

Symmetric

Symmetric Axis

Solid Edge V9

2D Drawing

Tutorial - Accurate layout approach Draw the sketch for: Shaft Support Bracket. Refer back to this drawing as you complete the tutorial.

Shaft Support Bracket

__ Start Solid Edge Part __ Select Sketch from the left menu.

__ Select the Front plane for this drawing.

__ Start SketchPoint

33

2D Drawing

Solid Edge V9

__ Set the SketchPoint Target at the mid-point of the horizontal reference plane. Watch for the IntelliSketch mid-point icon and click to set the target.

Start Mid-point icon

__ Start the Line command. __ Using the dialog boxes in the SketchPoint ribbon bar, start a line at X= -2.000, Y= .500

On/ Off

End

Set Target

X distance from Target

__ Draw the line vertical down to Y = 0.000 __ Continue the line. Set the length to 5.000. __ Continue the line up a length of .500 as shown on the drawings above. Right-click to stop.

Y distance From Target

Note: Work with both the active ribbon bars to draw the lines. Click a box to make it active so numbers can be input.

34

Solid Edge V9

2D Drawing

__ Start the Circle command. __ Set the radius for .875 __ Use SketchPoint to lock the center at X=000, Y=3.000. Type each value in the dialog box and press Enter. Click to place the circle.

__ Draw a short horizontal line from the upper end of the leftmost .500 length vertical line as shown. Be sure the IntelliSketch icon indicates a connect and horizontal conditions. __ Reset the SketchPoint target to the lower right as shown. __ Start a circle. Set the radius = .750. __ Keyin X= -.6250 and Y= 1.250. Click to set the circle.

__ Turn off SketchPoint. (Click the On/Off icon). __ Draw the three lines shown. The diagonal line should be tangent to both circles. The horizontal line should connect at the right and be tangent at the bottom of the right circle. The vertical line should connect to the top circle.

35

2D Drawing

Solid Edge V9

__ Start the Fillet command. Set the radius to .500. Pick the two lines as shown to create the radius. The Fillet command will extend or trim the lines to create the correct radius. Fillet

Save the drawing as Tutorial1

__ Use the Trim command to remove the excess arcs from the construction.

Trim

__ Draw the 1.000 diameter circle. Start the circle command. Move your mouse over the top arc then toward the center of the arc. A special icon will show when the center is selected. Click and set the circle size to 1.000. __ Use SmartDimension and regular dimension commands to place the dimensions on the drawing as shown. Remember to move your mouse over an arc or circle before you try to place a dimension to the center. __ Save the Drawing as Tutorial1.

36

Solid Edge V9

2D Drawing

• The sketch is complete. It can be used to create a solid part by selecting geometry from the layout. • At this time we will create a preliminary 2D drawing. This is often done for design approval. • Copy the sketch and dimensions to the Clip Board.

You can re-edit a sketch after you click finish.

__ Pick Edit. __ Pick Select All (All the elements on the drawing should change color). __ Click Copy. This places the selected elements on the Clipboard. This is one way of reusing a sketch in different Solid Edge environments. __ Pick Finish to close the sketch.

__Click the sketch. __Click Edit __ Click the sketch icon.

Note: Save the Part as Tutorial1

Creating a Drawing

__ Set Size for “A” wide. __ Click Background and set for “A” __ On the Main Ribbon Bar click Fit View.

In the next steps we will: 1. Open a Solid Edge Draft document. 2. Set the correct sheet size and title block. 3. Paste the drawing from the Clipboard. __ On the File menu pick New. __ Select Normal.Dft The default sheet size and background are too big. __ At the bottom of the screen Right-Click the word Sheet. __ Pick Sheet Setup. Use “A” horizontal and “A” background.

37

2D Drawing

Solid Edge V9

__ Turn on the Draw Toolbar Select View Toolbars Toolbars Place a checkmark in the Draw box.

__ On the Edit pop-down click Paste. The sketch will appear but in the wrong place.

__ Use the Move (Draw Toolbar) command to move the sketch to the middle of the title block. Click any place on the sketch then drag the sketch as shown.

Move is on a fly-out with several other commands. You may have to look for it if another command is current.

38

Solid Edge V9

2D Drawing

__ Use the Text Tool to place text in the Title Block as shown. Input your own school/company and name.

Note: Place the text approximately then use the Select Tool to drag it to the desired location. Text height is .125”

Put your own name in the DR BY box.

__ Save the drawing. __ Print the drawing. Printing/Plotting will vary depending on the output devices available. Check with your instructor. __ Click Properties for more settings. You may have to turn the drawing to a horizontal direction (Landscape). 39

2D Drawing

Solid Edge V9

Exercise 1. __ Layout the sketch in the Part Environment. __ Dimension the sketch. __ Set up an “A” size sheet in the Draft Environment. __ Use the Clipboard to copy the sketch onto the A-size title block. __Move the sketch to the center of the sheet. You may need to turn on the Draw Toolbar in order to move the sketch to the middle of the title block. __Fill in the Title Block as shown. Use your name in the DR BY: box. __Save and print the drawing.

40

Solid Edge V9

2D Drawing

Exercise 2. Create the sketch for the part shown below. Follow the steps as shown in Exercise 1. Create a drawing, dimension and print.

41

2D Drawing

Solid Edge V9

Exercise 3. Layout the sketch as shown. Dimension as shown. Create a drawing.

42

Solid Edge V11

2D Drawing

2D Drawing

25

2D Drawing

Solid Edge V11

2D Drawings may take two forms: 2D Sketches show the outlines and locations of multiple shapes or parts to be designed. 2D Profiles must be closed shapes with no entities inside or crossing the sketch. The sketch at the right may be used to create a part by selecting specific shapes then “cleaning up” the outline by trimming inner curves. The final shape must be a single series of connected lines and arcs.

Concept Sketch. (Cannot be used to create a part in this form).

Profile must be a closed figure with no internal lines.

Resulting 3D object with depth added.

Additional sketches were used to define the protrusion at the middle and the holes in the part after the initial shape was created.

26

Solid Edge V11

2D Drawing

Assembly Sketches (Layouts) These are used to define the critical geometry in a series of mating parts. Elements from the master sketch may be selected to create the individual parts. This assures that the parts are the correct size and are located in exactly the right place. Elements of the part sketches which are derived from the master sketch may be associated (linked) back to the master sketch. This means that any change in the master sketch will update all the associated parts.

Portions of the sketch were used to create the base of the roller assembly. Other portions of the same sketch will be used to create the opening for the wheel.

Modeling the wheel is done by selecting the large circle from the master sketch. The final assembly is shown with the parts modeled exactly as they fit.

As you can see, 2D sketches are the basis for much of the design and part creation process. These sketches can be very general at first then, exact sizes can be assigned later. All parts associated to the master sketches will re-size to the new dimensions.

27

2D Drawing

Solid Edge V11

Starting a 2D Sketch In this chapter all drawings will start from the Part Environment. Most of the commands and construction techniques are the same in other environments. If Solid Edge is already running, pop down the File menu .... Pick New … Select the More tab Use Normeng.par (inch)

For an introduction to 2D sketches, we will use the option to create a sketch. This option allows the designer to create an overall master outline showing major features of the part. When the actual part creation takes place, elements from the master sketch will be copied to the part outline sketch. • Selecting Sketch brings up the prompt: Watch the bottom left corner of the screen for instructions and prompts. • Pick the Front reference plane.

28

Solid Edge V11

2D Drawing 2D Sketch Window

2D Sketch Window Selecting a reference plane places a special window on the drawing. The view is looking straight at the selected reference plane. In this example the top and right planes appear as an edge and the front plane is the drawing surface.

Edge view of Right plane Edge view of Top plane

The profile will be created on the Front plane. The Drawing Tools Menu activates:

The sketch will be created on the surface of the Front plane.

Drawing Tools Menu Pick Tool Axis of Revolution Line* Arc Circle

DRAW

Rectangle Pattern* Fillet/Chamfer Trim/Extend

EDIT

Offset* Copy from Sketch* Construction/Entity Move* ( Illustration from Solid Edge Online Help )

Smart Dimension Dimension

Explore the commands. Remember that each icon with a small arrow at the lower right corner has a Fly Out with additional commands.

Connect* Horizontal/Vertical* Tangent*

CONSTRAIN*

* Advanced concepts are discussed in the next chapter.

Equal*

29

2D Drawing

Solid Edge V11

Line Starting the line command displays the ribbon bar at the top of the screen. Click a start point and move the mouse. The length of the line and the angle will display.

Switch between line/arc

• You can type in a length and an angle in the dialog boxes. • While drawing a line you can switch to the arc command and back. Intent Zone

Line to Arc Clicking the arc button on the ribbon bar switches to the arc command. • An Intent Zone icon is displayed on the end of the line. Moving the mouse through the 4 sectors produces a different result for each sector.

Special Line Options Curve: Click points (square boxes) to define a series of tangent arcs. The radius of each arc is determined by the direction of the previous and next points.

Line

Curve

FreeSketch and FreeForm will be discussed in the next chapter.

30

FreeSketch

FreeForm

Solid Edge V11

2D Drawing

Arc From the fly out menu, 3 options are possible. Tangent

3 Points

Center, Start, End

Depending on the option chosen, (line or arc) exact sizes may be set using the ribbon bar. Note: In some constructions it is easier and more accurate to draw a full circle then trim to define an arc.

Circle 5 options are shown on the circle fly out. Center 3 Points Tangent Ellipse Ellipse Radius/ 3 Points Center Diameter 2 Points The ribbon bar accepts either diameter or radius. Tangent can be: • Tangent to one entity • Tangent to two entities including the reference planes. You can set the radius then move the circle tangent. Many options exist. Try different commands and ways of using the commands. Online Help gives excellent instructions for the use of each option.

31

2D Drawing

Solid Edge V11

Rectangle Three construction methods are available: • Use dialog boxes. Input Width, Height and Angle. • Click two points for the width and one point for the height. • Draw a diagonal sketch line with the mouse.

Sketch Diagonal Line

Rectangle Constructed

Sketch Editing Tools Select Tool

Used to select entities for editing. Hold down the CTRL Key to select multiple entities. To delete an entity, select it and press the Delete Key

Fillet/Chamfer

Fillet will round a corner or add an arc between two entities. Often, Fillet is the easiest way to create an arc when the start/end/center points are not well defined. Chamfer will bevel a corner. The bevel can be the same angle or distance on both sides or, the bevel may be a different distance or angle on each side. Note the expanded ribbon bar.

A

Small rounds, fillets and chamfers should usually be added to the solid model after the major shape has been created.

B

32

Solid Edge V11

2D Drawing

Trim/Extend Trim line Trim

Trim

Extend

Trim is used to remove segments of entities. The segments are defined by intersections on the sketch. Multiple segments may be trimmed by sketching a line through each entity. Extend will cause entities to intersect. extend will not work if one entity does not provide a stop for the entity being extended. • You can extend a line by selecting the line and keying in a new length in the dialog box.

Construction Lines Any entity may be designated as a construction element. This means that it is used to define geometry but is not considered as a part of the outline shape.

Construction lines were used to locate the center for the circle. Converts entities to construction and visa-versa.

33

2D Drawing

Solid Edge V11

Move/Rotate/Mirror/Scale/Delete

Move Rotate Mirror Scale Delete Move. • First click the Select Tool. • Pick the object to move. (Hold down the CTRL Key to select multiple objects or use a window to select the objects within the window.) • Click where the object is now. • Click to set new location.

Dimensioning Smart Dimensions Use where one entity is to be dimensioned. • Line • Circle • Arc All the dimensions shown are Smart Dimensions. Standard Dimensions

Distance Angle Coor- Sym- Dimension Between dinate metric Axis To change the size of an entity on the drawing: • Select the dimension. • Type in a new size.

34

Solid Edge V11

2D Drawing

SketchPoint This is a drawing tool that allows entities to be placed in relation to another entity. • Select the Tools pop down • Click SketchPoint to turn on. SketchPoint will prompt for a target location. (Upper right corner of rectangle.) • Start a command (circle). • Set the diameter of the circle. • Move the mouse and note the distance reading. • Set exact distances using the SketchPoint dialog boxes.

SketchPoint Ribbon Bar

On/ Off

Set Target

Angle From Horizontal

Increments Set to .125 or ??

X-distance (Left/Right)

Y-distance (Up/Down)

Key in a distance or angle and press Enter to lock the value. To unlock the value, set the value to zero. • To turn off SketchPoint, press the ESC key or click the On/Off icon..

Display Commands As work progresses, the screen size may need to be changed. • Zoom Window - magnify • Zoom Out (shrink) • Fit (re-size to fit screen) • Pan (slide without changing size)

Main Toolbar- Top of Screen Zoom Zoom Fit Window Smaller

All allow for quick magnification, or re-sizing of the drawing image.

35

Pan

2D Drawing

Solid Edge V11

IntelliSketch

QuickPick

You may have noticed a number of symbols on the lines of the previous examples. These are geometric indicators which constrain the geometry. As you draw these symbols appear. The check box turns the momentary indicators on/off.

QuickPick is a tool used to sort out the correct item when several possibilities exist due to stacked geometry. Park the mouse for a few seconds and dots will appear. Left click for the selection box. Geometry highlights as numbers are selected.

Geometric Relationships As you draw some of the relationships are automatically set. Sketches must have the proper relationships between entities in order to create actual parts. Sketches must be properly constrained to create the intended objects.

Connect

Concentric

Tangent

Horizontal/Vertical Co-Linear Parallel Perpendicular • Remove a relationship by deleting the marker. • Add a relationship by selecting from the Relationships menu. This menu is near the bottom of the Draw Toolbar.

Equal

36

Symmetric

Symmetric Axis

Solid Edge V11

2D Drawing

Tutorial - Accurate layout approach Draw the sketch for: Shaft Support Bracket. Refer back to this drawing as you complete the tutorial.

Shaft Support Bracket

__ Start Solid Edge Part __ Select Sketch from the left menu.

__ Select the Front plane for this drawing.

__ Start SketchPoint

37

2D Drawing

Solid Edge V11

__ Set the SketchPoint Target at the mid-point of the horizontal reference plane. Watch for the IntelliSketch mid-point icon and click to set the target.

Start Mid-point icon

__ Start the Line command. __ Using the dialog boxes in the SketchPoint ribbon bar, start a line at X= -2.000, Y= .500

On/ Off

End

Set Target

X distance from Target

__ Draw the line vertical down to Y = 0.000 __ Continue the line horizontally. Set the length to 5.000. __ Continue the line up a length of .500 as shown on the drawings above. Right-click to stop.

Y distance From Target

Note: Work with both the active ribbon bars to draw the lines. Click a box to make it active so numbers can be input.

38

Solid Edge V11

2D Drawing

__ Start the Circle command. __ Set the radius for .875 __ Use SketchPoint to lock the center at X=000, Y=3.000. Type each value in the dialog box and press Enter. Click to place the circle.

__ Draw a short horizontal line from the upper end of the leftmost .500 length vertical line as shown. Be sure the IntelliSketch icon indicates a connect and horizontal conditions. __ Reset the SketchPoint target to the lower right as shown. __ Start a circle. Set the radius = .750. __ Keyin X= -.6250 and Y= 1.250. Click to set the circle.

__ Turn off SketchPoint. (Click the On/Off icon). __ Draw the three lines shown. The diagonal line should be tangent to both circles. The horizontal line should connect at the right and be tangent at the bottom of the right circle. The vertical line should connect to the top circle.

39

2D Drawing

Solid Edge V11

__ Start the Fillet command. Set the radius to .500. Pick the two lines as shown to create the radius. The Fillet command will extend or trim the lines to create the correct radius. Fillet

Save the drawing as Tutorial1

__ Use the Trim command to remove the excess arcs from the construction.

Trim

__ Draw the 1.000 diameter circle. Start the circle command. Move your mouse over the top arc then toward the center of the arc. A special icon will show when the center is selected. Click and set the circle size to 1.000. __ Use SmartDimension and regular dimension commands to place the dimensions on the drawing as shown. Remember to move your mouse over an arc or circle before you try to place a dimension to the center. __ Save the Drawing as Tutorial1.

40

Solid Edge V11

2D Drawing

• The sketch is complete. It can be used to create a solid part by selecting geometry from the layout. • At this time we will create a preliminary 2D drawing. This is often done for design approval. • Copy the sketch and dimensions to the Clip Board.

You can re-edit a sketch after you click finish.

__ Pick Edit. __ Pick Select All (All the elements on the drawing should change color). __ Click Copy. This places the selected elements on the Clipboard. This is one way of reusing a sketch in different Solid Edge environments. __ Pick Finish to close the sketch.

__Click the sketch. __Click Edit __ Click the sketch icon.

Note: Save the Part as Tutorial1

Creating a Drawing

__ Set Size for “A” wide. __ Click Background and set for “A” __ On the Main Ribbon Bar click Fit View.

In the next steps we will: 1. Open a Solid Edge Draft document. 2. Set the correct sheet size and title block. 3. Paste the drawing from the Clipboard. __ On the File menu pick New. __ Select Normal.Dft The default sheet size and background are too big. __ At the bottom of the screen Right-Click the word Sheet. __ Pick Sheet Setup. Use “A” horizontal and “A” background.

41

2D Drawing

Solid Edge V11

__ Turn on the Draw Toolbar Select View Toolbars Toolbars Place a checkmark in the Draw box.

__ On the Edit pop-down click Paste. The sketch will appear but in the wrong place.

__ Use the Move (Draw Toolbar) command to move the sketch to the middle of the title block. Click any place on the sketch then drag the sketch as shown.

Move is on a fly-out with several other commands. You may have to look for it if another command is current.

42

Solid Edge V11

2D Drawing

__ Use the Text Tool to place text in the Title Block as shown. Input your own school/company and name.

Note: Place the text approximately then use the Select Tool to drag it to the desired location. Text height is .125”

Put your own name in the DR BY box.

__ Save the drawing. __ Print the drawing. Printing/Plotting will vary depending on the output devices available. Check with your instructor. __ Click Properties for more settings. You may have to turn the drawing to a horizontal direction (Landscape). 43

2D Drawing

Solid Edge V11

Exercise 1. __ Layout the sketch in the Part Environment. __ Dimension the sketch. __ Set up an “A” size sheet in the Draft Environment. __ Use the Clipboard to copy the sketch onto the A-size title block. __Move the sketch to the center of the sheet. You may need to turn on the Draw Toolbar in order to move the sketch to the middle of the title block. __Fill in the Title Block as shown. Use your name in the DR BY: box. __Save and print the drawing.

44

Solid Edge V11

2D Drawing

Exercise 2. Create the sketch for the part shown below. Follow the steps as shown in Exercise 1. Create a drawing, dimension and print.

45

2D Drawing

Solid Edge V11

Exercise 3. Layout the sketch as shown. Dimension as shown. Create a drawing.

46

Engineering and Technical Drawing Using Solid Edge V15 By Jerry Craig

Series V15

SDC

PUBLICATIONS

Schroff Development Corporation www.schroff.com www.schroff-europe.com

Solid Edge V15

2D Drawing

2D Drawing 2D Sketches Chapter 2

2D Profiles

2D Sketches

Using 2D Sketches

Create Part

Create Assembly

Reference Planes

Selecting

Profile View

Entity Objects

Lines

Arcs

Dimensioning

Smart Dimensions

Standard Dimensions

Sketch Point

Starting

Setting Reference Point

Key-In Values

Display Commands

Zoom Window

Zoom Smaller

Fit

Pan

IntelliSketch Settings

Geometric Relations

Editing Sketches

Selecting Entities & Deleteing

Fillets and Chamfers

Trimming and Extending

Construction Lines

Tutorial

Accurate Layout

Creating Drawings

Adding Text and Dimensions

Printing

Problems

25

Circles and Ellipses

Rectangles

2D Drawing

Solid Edge V15

2D Drawings may take two forms: 2D Sketches show the outlines and locations of multiple shapes or parts to be designed. 2D Profiles must be closed shapes with no entities inside or crossing the sketch. The sketch at the right may be used to create a part by selecting specific shapes then “cleaning up” the outline by trimming inner curves. The final shape must be a single series of connected lines and arcs.

Concept Sketch. (Cannot be used to create a part in this form).

Profile must be a closed figure with no internal lines.

Resulting 3D object with depth added.

Additional sketches were used to define the protrusion at the middle and the holes in the part after the initial shape was created.

26

Solid Edge V15

2D Drawing

Assembly Sketches (Layouts) These are used to define the critical geometry in a series of mating parts. Elements from the master sketch may be selected to create the individual parts. This assures that the parts are the correct size and are located in exactly the right place. Elements of the part sketches which are derived from the master sketch may be associated (linked) back to the master sketch. This means that any change in the master sketch will update all the associated parts.

Portions of the sketch were used to create the base of the roller assembly. Other portions of the same sketch will be used to create the opening for the wheel.

Modeling the wheel is done by selecting the large circle from the master sketch. The final assembly is shown with the parts modeled exactly as they fit.

As you can see, 2D sketches are the basis for much of the design and part creation process. These sketches can be very general at first then, exact sizes can be assigned later. All parts associated to the master sketches will re-size to the new dimensions.

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2D Drawing

Solid Edge V15

Starting a 2D Sketch In this chapter all drawings will start from the Part Environment. Most of the commands and construction techniques are the same in other environments. If Solid Edge is already running, pop down the File menu .... Pick New … Select the More tab Use Normeng.par (inch)

For an introduction to 2D sketches, we will use the option to create a sketch. This option allows the designer to create an overall master outline showing major features of the part. When the actual part creation takes place, elements from the master sketch will be copied to the part outline sketch. Watch the Status Bar for instructions and prompts.

2D Sketch selected

Front · Pick the Front reference plane.

Top

Right

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Solid Edge V15

2D Drawing 2D Sketch Window

2D Sketch Window Selecting a reference plane places a special window on the drawing. The view is looking straight at the selected reference plane. In this example the top and right planes appear as an edge and the front plane is the drawing surface.

Edge view of Top plane

Edge view of Right plane

The profile will be created on the Front plane. The Drawing Tools Menu activates: The sketch will be created on the surface of the Front plane.

Drawing Tools Menu Pick Tool Line Free Form Arc

Draw

Arc Circle Rectangle Fillet/Chamfer Trim/Extend

Edit

Offset*

Copy from Sketch*(Include)/ Construction Entity flyout Move* Smart Dimension

( Illustration from Solid Edge Online Help )

Other Dim

Horizontal/Vertical*

Explore the commands. Remember that each icon with a small arrow at the lower right corner has a Fly Out with additional commands.

Tangent*

* Advanced concepts are discussed in the next chapter.

Connect*

Constrain*

Equal*

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Line Starting the line command displays the ribbon bar at the top of the screen. Click a start point and move the mouse. The length of the line and the angle will display. · You can type in a length and an angle in the dialog boxes. · While drawing a line you can switch to the arc command and back.

Switch between line/arc Intent Zone

Line to Arc Clicking the arc button on the ribbon bar switches to the arc command. · An Intent Zone icon is displayed on the end of the line. Moving the mouse through the 4 sectors produces a different result for each sector.

Point - Available from the fly out menu. Click to place or input coordinates. Points are placed as Construction Elements.

Free Sketch. Use mouse to

Line Point

Free Sketch

Freehand drawing converted to geometry

draw outline. Solid Edge converts to geometry. (Usually needs a lot of editing).

Curve Menu. Draws or converts to BSPLINE geometry. Click curve to edit inflection points. Freehand courve or Bspline input points.

Convert to Bspline

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Solid Edge V15

2D Drawing

Arc From the fly out menu, 3 options are possible. Tangent

3 Points

Center, Start, End

Depending on the option chosen, (line or arc) exact sizes may be set using the ribbon bar. Note: In some constructions it is easier and more accurate to draw a full circle then trim to define an arc.

Circle 5 options are shown on the circle fly out. Center 3 Points Tangent Ellipse Ellipse Radius/ 3 Points Center Diameter 2 Points The ribbon bar accepts either diameter or radius. Tangent can be: · Tangent to one entity · Tangent to two entities including the reference planes. You can set the radius then move the circle tangent. Many options exist. Try different commands and ways of using the commands. Online Help gives excellent instructions for the use of each option.

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Rectangle Three construction methods are available:

· Use dialog boxes. Input Width, Height and Angle. · Click two points for the width and one point for the height. · Draw a diagonal sketch line with the mouse.

Sketch Diagonal Line

Rectangle Constructed

Sketch Editing Tools Select Tool

Used to select entities for editing. Hold down the CTRL Key to select multiple entities. To delete an entity, select it and press the Delete Key

Fillet/Chamfer

Fillet will round a corner or add an arc between two entities. Often, Fillet is the easiest way to create an arc when the start/end/center points are not well defined. Chamfer will bevel a corner. The bevel can be the same angle or distance on both sides or, the bevel may be a different distance or angle on each side. Note the expanded ribbon bar.

B A

Small rounds, fillets and chamfers should usually be added to the solid model after the major shape has been created.

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Solid Edge V15

2D Drawing

Trim/Extend Trim line Trim

Trim

Extend

Trim is used to remove segments of entities. The segments are defined by intersections on the sketch. Multiple segments may be trimmed by sketching a line through each entity. Extend will cause entities to intersect. Extend will not work if one entity does not provide a stop for the entity being extended. · You can extend a line by selecting the line and keying in a new length in the dialog box.

Construction Lines Any entity may be designated as a construction element. This means that it is used to define geometry but is not considered as a part of the outline shape.

Construction lines were used to locate the center for the circle.

The Construction toggle is on the flyout with the Include command.

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Move/Rotate/Mirror/Scale/Delete

Move Rotate Mirror Scale Delete Move. · First click the Select Tool. · Pick the object to move. (Hold down the CTRL Key to select multiple objects or use a window to select the objects within the window.) · Click where the object is now. · Click to set new location.

Dimensioning Smart Dimensions Use where one entity is to be dimensioned. · Line · Circle · Arc All the dimensions shown are Smart Dimensions. Standard Dimensions

Distance Angle Coor- Sym- Dimension Between dinate metric Axis To change the size of an entity on the drawing: · Select the dimension. · Type in a new size.

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Solid Edge V15

2D Drawing

SketchPoint

Sketch point provides a temporary origin to measure relative to existing geometry.

This is a drawing tool that allows entities to be placed in relation to another entity. · Select the Tools pop down · Click SketchPoint to turn on. SketchPoint will prompt for a target location. (Upper right corner of rectangle.) · Start a command (circle). · Set the diameter of the circle. · Move the mouse and note the distance reading. · Set exact distances using the SketchPoint dialog boxes.

SketchPoint Ribbon Bar

On/ Off

Set Target

Angle From Horizontal

Increments Set to .125 or ??

X-distance (Left/Right)

Y-distance (Up/Down)

Key in a distance or angle and press Enter to lock the value. To unlock the value, set the value to zero. · To turn off SketchPoint, press the ESC key or click the On/Off icon..

Display Commands As work progresses, the screen size may need to be changed. · Zoom Window - magnify · Zoom Out (shrink) · Fit (re-size to fit screen) · Pan (slide without changing size)

Main Toolbar- Top of Screen Zoom Zoom Fit Window Smaller /Larger

All allow for quick magnification, or re-sizing of the drawing image.

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Pan

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Solid Edge V15

IntelliSketch

QuickPick

You may have noticed a number of symbols on the lines of the previous examples. These are geometric indicators which constrain the geometry. As you draw these symbols appear. The check box turns the momentary indicators on/off.

QuickPick is a tool used to sort out the correct item when several possibilities exist due to stacked geometry. Park the mouse for a few seconds and dots will appear. Right-click for the selection list.

Geometric Relationships As you draw some of the Connect Concentric Tangent relationships are automatically set. Sketches must have the proper relationships between entities in order to create actual parts. Sketches must be properly constrained to create the Horizontal/Vertical Co-Linear Parallel Perpendicular intended objects. · Remove a relationship by deleting the marker. · Add a relationship by selecting from the Relationships menu. This menu is near the bottom of the Draw Toolbar.

Equal

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Symmetric

Symmetric Axis

Solid Edge V15

2D Drawing

Tutorial - Accurate layout approach Draw the sketch for: Shaft Support Bracket. Refer back to this drawing as you complete the tutorial.

Shaft Support Bracket

__ Start Solid Edge Part __ Select Sketch from the left menu.

__ Select the Front plane for this drawing.

__ Start SketchPoint

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__ Set the SketchPoint Target at the mid-point of the horizontal reference plane. Watch for the IntelliSketch mid-point icon and click to set the target.

Start Mid-point icon

__ Start the Line command. __ Using the dialog boxes in the SketchPoint ribbon bar, start a line at X= -2.000, Y= .500

On/ Off

End

Set Target

X distance from Target

__ Draw the line vertical down to Y = 0.000 __ Continue the line horizontally. Set the length to 5.000. __ Continue the line up a length of .500 as shown on the drawings above. Right-click to stop.

Y distance From Target

Note: Work with both the active ribbon bars to draw the lines. Click a box to make it active so numbers can be input.

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Solid Edge V15

2D Drawing

__ Start the Circle command. __ Set the radius for .875 __ Use SketchPoint to lock the center at X=000, Y=3.000. Type each value in the dialog box and press Enter. Click to place the circle.

__ Draw a short horizontal line from the upper end of the leftmost .500 length vertical line as shown. Be sure the IntelliSketch icon indicates a connect and horizontal conditions. __ Reset the SketchPoint target to the lower right as shown. __ Start a circle. Set the radius = .750. __ Keyin X= -.6250 and Y= 1.250. Click to set the circle.

__ Turn off SketchPoint. (Click the On/Off icon). __ Draw the three lines shown. The diagonal line should be tangent to both circles. The horizontal line should connect at the right and be tangent at the bottom of the right circle. The vertical line should connect to the top circle.

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__ Start the Fillet command. Set the radius to .500. Pick the two lines as shown to create the radius. The Fillet command will extend or trim the lines to create the correct radius. Fillet

Save the drawing as Tutorial1

__ Use the Trim command to remove the excess arcs from the construction.

Trim

__ Draw the 1.000 diameter circle. Start the circle command. Move your mouse over the top arc then toward the center of the arc. A special icon will show when the center is selected. Click and set the circle size to 1.000. __ Use SmartDimension and regular dimension commands to place the dimensions on the drawing as shown. Remember to move your mouse over an arc or circle before you try to place a dimension to the center. __ Save the Drawing as Tutorial1

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Solid Edge V15

2D Drawing

· The sketch is complete. It can be used to create a solid part by selecting geometry from the layout. · At this time we will create a preliminary 2D drawing. This is often done for design approval. · Copy the sketch and dimensions to the Clip Board.

You can re-edit a sketch after you click finish.

__ Pick Edit. __ Pick Select All (All the elements on the drawing should change color). __ Click Copy. This places the selected elements on the Clipboard. This is one way of re-using a sketch in different Solid Edge models.

__Click the sketch. __Click Edit __ Click the sketch icon.

Note: Save the Part as Tutorial1

Creating a Drawing

__ Set Size for “A” wide. __ Click Background and set for “A” __ On the Main Ribbon Bar click Fit View.

In the next steps we will: 1. Open a Solid Edge Draft document. 2. Set the correct sheet size and title block. 3. Paste the drawing from the Clipboard. __ On the File menu pick New __ Click the More tab. __ Select Normeng.Dft The default sheet size and background are too big. __ At the bottom of the screen Right-Click the word Sheet. __ Pick Sheet Setup. Set “A” background.

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__ Turn on the Draw Toolbar Select View Toolbars Toolbars Place a checkmark in the Draw box. Note: This method of creating drawings is useful for quick 2D sketches. It may be used with WORD and other editors for report writing. Except for these exercises we will use other tools to create detail drawings. __ On the Edit pop-down click Paste. The sketch will appear but in the wrong place.

__ Use the Move (Draw Toolbar) command to move the sketch to the middle of the title block. Click any place on the sketch then drag the sketch as shown.

Move is on a fly-out with several other commands. You may have to look for it if another command is current.

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Solid Edge V15

2D Drawing

__ Use the Text Tool to place text in the Title Block as shown. Input your own school/company and name.

Note: Place the text approximately then use the Select Tool to drag it to the desired location. Text height is .125”

Put your own name in the DR BY box.

__ Save the drawing. __ Print the drawing. Printing/Plotting will vary depending on the output devices available. Check with your instructor. __ Click Properties for more settings. You may have to turn the drawing to a horizontal direction (Landscape). 43

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Exercise 1. __ Layout the sketch in the Part Environment. __ Dimension the sketch. __ Set up an “A” size sheet in the Draft Environment. __ Use the Clipboard to copy the sketch onto the A-size title block. __Move the sketch to the center of the sheet. You may need to turn on the Draw Toolbar in order to move the sketch to the middle of the title block. __Fill in the Title Block as shown. Use your name in the DR BY: box. __Save and print the drawing.

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Solid Edge V15

2D Drawing

Exercise 2. Create the sketch for the part shown below. Follow the steps as shown in Exercise 1. Create a drawing, dimension and print.

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Exercise 3. Layout the sketch as shown. Dimension as shown. Create a drawing.

Exercise 4. Do the Tutorial. Save a copy as Ch2-Ex-4. Make a drawing. See Tutorial page 65.

46

Engineering and Technical Drawing Using Solid Edge V16 By Jerry Craig

Series V16

SDC

PUBLICATIONS

Schroff Development Corporation www.schroff.com www.schroff-europe.com

Solid Edge V16

2D Drawing

Copyrighted Material 2D Drawing

2D Sketches Chapter 2

2D Profiles

2D Sketches

Using 2D Sketches

Create Part

Create Assembly

Reference Planes

Selecting

Profile View

Entity Objects

Lines

Arcs

Dimensioning

Smart Dimensions

Standard Dimensions

Sketch Point

Starting

Setting Reference Point

Key-In Values

Zoom Smaller

Fit

Pan

Copyrighted Material Circles and Ellipses

Rectangles

Copyrighted Material

Display Commands

Zoom Window

IntelliSketch Settings

Geometric Relations

Editing Sketches

Selecting Entities & Deleteing

Fillets and Chamfers

Trimming and Extending

Construction Lines

Accurate Layout

Creating Drawings

Adding Text and Dimensions

Printing

Copyrighted Material

Tutorial

Problems

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2D Drawings may take two forms:

2D Sketches show the outlines and locations of multiple shapes or parts to be designed.

2D Profiles must be closed shapes with no entities inside or crossing the sketch. The sketch at the right may be used to create a part by selecting specific shapes then “cleaning up” the outline by trimming inner curves. The final shape must be a single series of connected lines and arcs.

Concept Sketch. (Cannot be used to create a part in this form).

Copyrighted Material Profile must be a closed figure with no internal lines.

Resulting 3D object with depth added.

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Additional sketches were used to define the protrusion at the middle and the holes in the part after the initial shape was created.

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Solid Edge V16

2D Drawing

Copyrighted Material

Assembly Sketches (Layouts)

These are used to define the critical geometry in a series of mating parts. Elements from the master sketch may be selected to create the individual parts. This assures that the parts are the correct size and are located in exactly the right place. Elements of the part sketches which are derived from the master sketch may be associated (linked) back to the master sketch. This means that any change in the master sketch will update all the associated parts.

Copyrighted Material

Portions of the sketch were used to create the base of the roller assembly.

Other portions of the same sketch will be used to create the opening for the wheel.

Copyrighted Material

Modeling the wheel is done by selecting the large circle from the master sketch. The final assembly is shown with the parts modeled exactly as they fit.

As you can see, 2D sketches are the basis for much of the design and part creation process. These sketches can be very general at first then, exact sizes can be assigned later. All parts associated to the master sketches will re-size to the new dimensions.

Copyrighted Material 27

2D Drawing

Solid Edge V16

Copyrighted Material

Starting a 2D Sketch

In this chapter all drawings will start from the Part Environment. Most of the commands and construction techniques are the same in other environments. If Solid Edge is already running, pop down the File menu .... Pick New … Select the More tab Use Normeng.par (inch)

Copyrighted Material

For an introduction to 2D sketches, we will use the option to create a sketch. This option allows the designer to create an overall master outline showing major features of the part. When the actual part creation takes place, elements from the master sketch will be copied to the part outline sketch.

Copyrighted Material

Watch the Status Bar for instructions and prompts.

· Pick the Front reference plane.

Front

Copyrighted Material Top

Right

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2D Sketch selected

Solid Edge V16

2D Drawing

Copyrighted Material

2D Sketch with Grid. Selecting a reference plane for the 2D sketch creates a 2D drawing screen. Turning on the Grid displays the Grid Tool Bar and places a grid on the screen.. Grid Icon

Grid Tool Bar

Face View of Front X - Z plane

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Edge View of Right Y - Z plane

Edge View of Top X - Y plane

Zero Origin Point

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Grid Settings Tool Bar

Grid Options

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Snap To Grid

Grid Off/On

Reset Origin To Zero

Move Origin

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Grid Options Dialog Box Grid settings may be adjusted for the type of sketch to be created. Major lines might be 1 inch while minor lines might be: 8 lines/inch = 1/8 inch (.125) 10 lines/inch = .10 inch, etc.

Snap To Grid locks the drawing geometry to the grid. This creates accurate geometry quickly without keying in distances as long as the points can be set to the grid locations.

Show Readouts turns on the X - Y display showing the cursor distance from the current Origin.

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Show Alignments projects a dashed line when the cursor is in line with existing geometry. Grid as Points. The grid may be displayed as points if prefered. Cursor Position Display. X and Y pointer locations are displayed as points are set. The distance is from the Origin.

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Resetting the Origin is often necessary during 2D drawing construction.

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New Origin

Default Zero Origin

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Solid Edge V16

2D Drawing

Copyrighted Material 2D Sketch Window

2D Sketch Window

Selecting a reference plane places a special window on the drawing. The view is looking straight at the selected reference plane. In this example the top and right planes appear as an edge and the front plane is the drawing surface.

Edge view of Top plane

Edge view of Right plane

The profile will be created on the Front plane. The Drawing Tools Menu activates:

Copyrighted Material

The sketch will be created on the surface of the Front plane.

Drawing Tools Menu Pick Tool Line

Free Form Arc

Draw

Arc Circle Rectangle

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Fillet/Chamfer Trim/Extend Offset*

Edit

Copy from Sketch*(Include)/ Construction Entity flyout Move* Smart Dimension

Connect*

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Horizontal/Vertical* Tangent* Equal*

( Illustration from Solid Edge Online Help )

Other Dim

Constrain*

Explore the commands. Remember that each icon with a small arrow at the lower right corner has a Fly Out with additional commands. * Advanced concepts are discussed in the next chapter.

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2D Drawing

Line

Solid Edge V16

Copyrighted Material

Starting the line command displays the ribbon bar at the top of the screen. Click a start point and move the mouse. The length of the line and the angle will display. · You can type in a length and an angle in the dialog boxes. · While drawing a line you can switch to the arc command and back. Line to Arc

Switch between line/arc

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Clicking the arc button on the ribbon bar switches to the arc command.

· An Intent Zone icon is displayed on the end of the line. Moving the mouse through the 4 sectors produces a different result for each sector.

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Point - Available from the fly

out menu. Click to place or input coordinates. Points are placed as Construction Elements.

Free Sketch. Use mouse to

Line Point

Free Sketch

Freehand drawing converted to geometry

draw outline. Solid Edge converts to geometry. (Usually needs a lot of editing).

Copyrighted Material

Curve Menu. Draws or

converts to BSPLINE geometry. Click curve to edit inflection points. Freehand courve or Bspline input points.

Convert to Bspline

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Intent Zone

Solid Edge V16

Arc

2D Drawing

Copyrighted Material

From the fly out menu, 3 options are possible.

Tangent

3 Points

Center, Start, End

Depending on the option chosen, (line or arc) exact sizes may be set using the ribbon bar.

Copyrighted Material

Note: In some constructions it is easier and more accurate to draw a full circle then trim to define an arc.

Circle

5 options are shown on the circle fly out. Center 3 Points Tangent Ellipse Ellipse Radius/ 3 Points Center Diameter 2 Points

Copyrighted Material

The ribbon bar accepts either diameter or radius.

Tangent can be: · Tangent to one entity · Tangent to two entities including the reference planes. You can set the radius then move the circle tangent.

Copyrighted Material

Many options exist. Try different commands and ways of using the commands. Online Help gives excellent instructions for the use of each option.

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2D Drawing

Rectangle

Solid Edge V16

Copyrighted Material

Three construction methods are available:

· Use dialog boxes. Input Width, Height and Angle. · Click two points for the width and one point for the height. · Draw a diagonal sketch line with the mouse.

Copyrighted Material Sketch Diagonal Line

Rectangle Constructed

Sketch Editing Tools Select Tool

Fillet/Chamfer

Used to select entities for editing. Hold down the CTRL Key to select multiple entities. To delete an entity, select it and press the Delete Key

Copyrighted Material

Fillet will round a corner or add an arc between two entities. Often, Fillet is the easiest way to create an arc when the start/end/center points are not well defined. Chamfer will bevel a corner. The bevel can be the same angle or distance on both sides or, the bevel may be a different distance or angle on each side. Note the expanded ribbon bar.

Copyrighted Material B

Small rounds, fillets and chamfers should usually be added to the solid model after the major shape has been created.

A

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Solid Edge V16

2D Drawing

Copyrighted Material

Trim/Extend/Break

Trim line

Trim

Trim Extend Break Corner

Trim is used to remove segments of entities. The segments are defined by intersections on the sketch.

Copyrighted Material

Multiple segments may be trimmed by sketching a line through each entity.

Extend will cause entities to intersect. Extend will not work if one entity does not provide a stop for the entity being extended. · You can extend a line by selecting the line and keying in a new length in the dialog box.

Copyrighted Material

Break will slice an entity into two parts.

Construction Lines

Any entity may be designated as a construction element. This means that it is used to define geometry but is not considered as a part of the outline shape.

Copyrighted Material

Construction lines were used to locate the center for the circle.

The Construction toggle is on the flyout with the Include command.

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Move/Rotate/Mirror/Scale/Stretch/Delete

Move Rotate Mirror

Scale Stretch Delete

Move. · First click the Select Tool. · Pick the object to move. (Hold down the CTRL Key to select multiple objects or use a window to select the objects within the window.) · Click where the object is now. · Click to set new location.

Dimensioning

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Smart Dimensions

Use where one entity is to be dimensioned. · Line · Circle · Arc All the dimensions shown are Smart Dimensions.

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Standard Dimensions

Distance Angle Coor- Sym- Dimension Between dinate metric Axis

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To change the size of an entity on the drawing: · Select the dimension. · Type in a new size.

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Solid Edge V16

2D Drawing

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Fill places a pattern or solid in a closed area. Fill Ribbon Bar:

Copyrighted Material Display Commands As work progresses, the screen size may need to be changed. · Zoom Window - magnify · Zoom Out (shrink) · Fit (re-size to fit screen) · Pan (slide without changing size)

Main Toolbar- Top of Screen

Copyrighted Material Zoom Zoom Fit Window Smaller /Larger

Pan

All allow for quick magnification, or re-sizing of the drawing image.

A "Wheel Mouse" may be used for fast zooms by activating the wheel.

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2D Drawing

IntelliSketch

Solid Edge V16

Copyrighted Material

QuickPick

You may have noticed a number of symbols on the lines of the previous examples. These are geometric indicators which constrain the geometry. As you draw these symbols appear. The check box turns the momentary indicators on/off.

Copyrighted Material QuickPick is a tool used to sort out the correct item when several possibilities exist due to stacked geometry. Park the mouse for a few seconds and dots will appear. Right-click for the selection list.

Copyrighted Material

Geometric Relationships

As you draw some of the Connect Concentric Tangent relationships are automatically set. Sketches must have the proper relationships between entities in order to create actual parts. Sketches must be properly constrained to create the Horizontal/Vertical Co-Linear Parallel Perpendicular intended objects.

Copyrighted Material

· Remove a relationship by deleting the marker. · Add a relationship by selecting from the Relationships menu. This menu is near the bottom of the Draw Toolbar.

Equal

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Symmetric

Symmetric Axis

Solid Edge V16

2D Drawing

Copyrighted Material

Tutorial - Accurate layout approach

Draw the sketch for: Shaft Support Bracket. Refer back to this drawing as you complete the tutorial.

Shaft Support Bracket

Copyrighted Material Copyrighted Material

__ Start Solid Edge Part __ Select Sketch from the left menu. __ Select the Front plane for this drawing.

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__ Turn ON the Grid.

__ Set the Grid for: 1.00 inch major lines, 8 minor (0.125 inch) lines. Activate Grid Snap

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__ Start the Line command.

__ Using the Grid Readout start the line at __ X= -2.000, Y= .500 __ To X= -2.000, Y= 0.000 __ To X=3.000, Y= 0.000

X=-2.000 Y=.500

__ To X= 3.000, Y=.500

X=3.000 Y= .500

Zero on Grid

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__ Right-click to stop the line.

Start

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Auto Re-size

Grid - Resizing __ Click on the Grid border.

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__ Drag the border to a new size. A Grid Size dialog box appears. Key in X,Y sizes or click the Auto-Resize icon.

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__ Start the Circle command. __ Set the radius for .875

__ Use Grid readouts to position the center at X=000, Y=3.000. Click to place the circle.

__ Draw a short horizontal line from the upper end of the leftmost .500 length vertical line as shown. Be sure the IntelliSketch icon indicates a connect and horizontal conditions.

Copyrighted Material

__ Reset the Grid Origin to the lower right (X=3.00, Y=0.000) as shown. __ Start a circle. Set the radius = .750. __ Place the center at X= -.6250 and Y= 1.250. Click to set the circle.

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__ Pick Tools ... IntelliSketch Set the dialog box as shown

New Grid Origin

Watch for the Allignment Icons "Point On" and "Tangent"

Turn Off the Grid

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__ Draw the Vertical and Tangent lines as shown.

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__ Start the Fillet command. Set the radius to .500. Pick the two lines as shown to create the radius.

The Fillet command will extend or trim the lines to create the correct radius.

Fillet

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Save the drawing as Tutorial1

__ Use the Trim command to remove the excess arcs from the construction.

Trim

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__ Draw the 1.000 diameter circle. Start the circle command. Move your mouse over the top arc then toward the center of the arc. A special icon will show when the center is selected. Click and set the circle size to 1.000. __ Use SmartDimension and regular dimension commands to place the dimensions on the drawing as shown.

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Remember to move your mouse over a arc or circle before you try to place a dimension to the center.

__ Save the Drawing as Tutorial1

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Copyrighted Material

· The sketch is complete. It can be used to create a solid part by selecting geometry from the layout. · At this time we will create a preliminary 2D drawing. This is often done for design approval. · Copy the sketch and dimensions to the Clip Board.

You can re-edit a sketch after you click finish.

__ Pick Edit. __ Pick Select All (All the elements on the drawing should change color). __ Click Copy. This places the selected elements on the Clipboard. This is one way of re-using a sketch in different Solid Edge models.

__Click the sketch. __Click Edit __ Click the sketch icon.

Copyrighted Material Note: Save the Part as Sketch1

Set Size for “A” wide: __ Click Background and set for “A” __ Zoom to full screen: On the Main Ribbon Bar click Fit View.

Creating a Drawing In the next steps we will: 1. Open a Solid Edge Draft document. 2. Set the correct sheet size and title block. 3. Paste the drawing from the Clipboard.

Copyrighted Material

__ On the File menu pick New __ Click the More tab. __ Select Normeng.Dft

The size tab should show "A-Wide"

The default sheet size and background are too big. __ At the bottom of the screen Right-Click the word Sheet.

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__ Pick Sheet Setup. Set “A” background.

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__ Turn on the Draw Toolbar

Select View Toolbars Toolbars Place a checkmark in the Draw box. Note: This method of creating drawings is useful for quick 2D sketches. It may be used with WORD and other editors for report writing by pasting from the clipboard.

Copyrighted Material

Except for these exercises we will use other tools to create detail drawings. __ On the Edit pop-down click Paste. The sketch will appear but in the wrong place. Click the sketch and hold down the left mouse key. Drag the sketch to the middle of the title block.

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If necessary, use the Move (Draw Toolbar) command to move the sketch to the middle of the title block. Window the sketch then drag the sketch as shown.

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Move is on a fly-out with several other commands. You may have to look for it if another command is current.

44

Solid Edge V16

2D Drawing

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__ Use the Text Tool to place text in the Title Block as shown. Input your own school/company and name.

Note: Place the text approximately then use the Select Tool to drag it to the desired location. Text height is .125” SAVE the drawing. This will insert the designer's name and date. School lab computers may not show the correct information. Use TEXT to put your name and date on the page as assigned.

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__ Save the drawing. __ Print the drawing. Printing/Plotting will vary depending on the output devices available. Check with your instructor.

Copyrighted Material Copyrighted Material

__ Click Properties for more settings. You may have to turn the drawing to a horizontal direction (Landscape). 45

2D Drawing

Exercise 1.

Solid Edge V16

Copyrighted Material

__ Layout the sketch in the Part Environment. __ Dimension the sketch.

__ Set up an “A” size sheet in the Draft Environment. __ Use the Clipboard to copy the sketch onto the A-size title block. __Move the sketch to the center of the sheet.

You may need to turn on the Draw Toolbar in order to move the sketch to the middle of the title block.

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__Fill in the Title Block as shown. Use your name in the DR BY: box. __Save and print the drawing. Drawing Name: Baffle Plate

Copyrighted Material Copyrighted Material 46

Solid Edge V16

Exercise 2.

2D Drawing

Copyrighted Material

Create the sketch for the part shown below.

Follow the steps as shown in Exercise 1. Create a drawing, dimension and print.

Copyrighted Material Copyrighted Material Copyrighted Material 47

2D Drawing

Solid Edge V16

Copyrighted Material

Exercise 3. Layout the sketch as shown. Dimension as shown. Create a drawing.

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Part Name: TEMPLATE

Exercise 4. Do the Tutorial.

Copyrighted Material Copyrighted Material 48

Engineering and Technical Drawing Using Solid Edge Version 17 By Jerry Craig Images from Solid Edge Gallery

SDC Schroff Development Corporation www.schroff.com

www.schroff-europe.com

Solid Edge V17 2D Sketches Chapter 2

Using 2D Sketches

Reference Planes

Entity Objects

Constraining Sketches

IntelliSketch Settings

Editing Sketches

Grid

Tutorial

2D Drawing 2D Profiles

2D Sketches

Create Part

Create Assembly

Selecting

Profile View

Copyrighted Material Copyrighted Material Lines

Arcs

Circles and Ellipses

Smart Dimensions

Standard Dimensions

Geometric Constraints

Copyrighted Material

Rectangles

Geometric Relations

Selecting Entities & Deleteing

Fillets and Chamfers

Trimming and Extending

Settings

Re-Setting Origin

Key-In Values

Copyrighted Material Accurate Layout

Creating Drawings

25

Adding Text and Dimensions

Construction Lines

Printing

2D Drawing

Solid Edge V17

2D Drawings may take two forms:

Copyrighted Material

2D Sketches show the outlines and locations of multiple shapes or parts to be designed.

2D Profiles must be closed shapes with no entities inside or crossing the sketch. The sketch at the right may be used to create a part by selecting specific shapes then “cleaning up” the outline by trimming inner curves. The final shape must be a single series of connected lines and arcs.

Complete Master Sketch. (Cannot be used to create a part in this form).

Copyrighted Material Profile must be a closed “loop” with no internal lines.

Resulting 3D object with depth added.

Copyrighted Material

Portions of the Master Sketch are copied when creating individual part features.

Copyrighted Material 26

Solid Edge V17

2D Drawing

Assembly Sketches (Layouts)

Copyrighted Material

These are used to define the critical geometry in a series of mating parts. Elements from the master sketch may be selected to create the individual parts. This assures that the parts are the correct size and are located in exactly the right place.

Elements of the part sketches which are derived from the master sketch may be associated (linked) back to the master sketch. This means that any change in the master sketch will update all the associated parts.

Copyrighted Material

Portions of the sketch were used to create the base of the pillow block assembly. Other portions of the same sketch will be used to create the opening for the bearing. Modeling the bearing is done by selecting the inner circles. The bronze bearing is created as a separate part.

Copyrighted Material

The final assembly is shown with the parts modeled exactly as they fit.

As you can see, 2D sketches are the basis for much of the design and part creation process. These sketches can be very general at first then, exact sizes can be assigned later. All parts associated to the master sketches will resize to the new dimensions. Each part will be the right size and in the right place.

Copyrighted Material Bronze Bearing

Exploded Assembly view.

27

2D Drawing

Solid Edge V17

Starting a 2D Drawing

Copyrighted Material

Any new object starts with a 2D sketch. Complex objects can be designed more efficiently by creating a master sketch with part geometry defined by a series of overlapping lines. As the part shape evolves the 2D lines are used to add material or cut away material.

Simpler shapes may be designed by staring directly with the Protrusion or revolved Protrusion icons. Master sketches give more control over the modeling process.

Component Sketches are placeholders for existing parts or for related items yet to be designed.

Copyrighted Material

Once Sketch is started, The Ribbon Bar displays prompts and options. A Reference Plane must be selected. Or, a new reference plane must be defined as a 2D drawing plane.

A pop down dialog box allow the selection of alternate planes for starting the sketch.

Copyrighted Material

Coincident Option starts a sketch on one of the existing reference planes.

Copyrighted Material 28

Solid Edge V17

• The Draw toolbar replaces the Main toolbar. • The drawing surface is now the Front (X-Z) plane. • The horizontal line is the edge view of the Top (X-Y) plane. • The vertical line is the edge of the Side (Y-Z) plane. Draw menu items may hve several options selected from pop down menus. The first tutorial (chapter 1) introduced the 2D drawing process.

Exercise:

Copyrighted Material Edge of Side (Y-Z) plane

A 2D drawing screen appears.

2D Drawing

Edge of Top (X-Y) plane

Copyrighted Material 2D drawing surface = Front (X-Z) plane

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√ Start Solid Edge. √ Click Sketch. √ Click the Front reference plane.

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Draw some shapes. Explore the pop downs

Press ESC key to stop a command.

When finished, click the RETURN button.

Exit Do not save the drawing.

29

2D Drawing

Solid Edge V17

Copyrighted Material

Draw Menu

Constraints Menu

Copyrighted Material

Drawn items may be changed by editing lengths, angles, diameter/radius, etc.

Edit Menu

When items are connected, changing one item may cause another entity to change in an unexpected or unwanted manner. Placing constraints on a 2D sketch helps to ensure Engineering Intent.

Copyrighted Material

Copyrighted Material

Constraining sketches is an important step in the design process. Many features may be changed as the design evolves. Making sure the master sketch changes in a predictable manner is critical. Constraints are a combination of geometric (parallel, vertical, concentric, tangent, etc.) and dimensional lengths. The first tutorial (chapter 1) introduced some of these ideas.

30

Solid Edge V17

2D Drawing

Line command. Starting a line displays the Line Ribbon Bar.

Copyrighted Material

Color

Active Line Style

Type Thickness

Toggle between line and arc

Alignment Indicator Many indicators will appear as a drawing is created. These help to insure good geometry.

Copyrighted Material

A straight line was drawn then the arc toggle was selected. The intent zone creates the arc based on how the mouse moves out of the intent zone.

Intent Zone

Alignment indicators flash when horizontal.vertical, extensions or other alignments are sensed.

Indicators may be turned On/Off by clicking Tools menu and clicking the selection buttons.

Copyrighted Material

Tools ... Intellisketch ... Relationships toggles various geomentric indicators on/off.

Alignment Indicators On/Off toggles.

Copyrighted Material 31

2D Drawing

Solid Edge V17

Copyrighted Material Distance Between dimension option was used to fix point location.

Point

Other options for Line are Point (used as a marker or place holder) and Freesketch.

Freesketch. Hold left moude button down and draw shape. Solid Edge will create straight lines and arcs.

Copyrighted Material

√ Place smart dimensions to constrain the shape.

Circle. Pop down provides options for drawing circles and ellipses.

The circle ribbon bar provides options for color, linetype and line thickness. Click either diameter or radius box to input size.

Tangent Circle

Copyrighted Material

A circle was placed at random tangent to two lines. The circle size may be set using the circle command or by placing a smart dimension.

Copyrighted Material 32

Solid Edge V17

2D Drawing

Arc.

Copyrighted Material

Three options are shown. The arc ribbon bar gives slightly different options for each arc type.

Curve. Click a series of points. A smooth curve is drawn. Curve has many settings and options. Check Help for more information.

Copyrighted Material

Rectangle.

Quick method: Select Rectangle. Hold down left mouse button and sketch diagonal line. Use smart dimensions to set size.

Copyrighted Material Copyrighted Material 33

2D Drawing

Solid Edge V17

Constraining Sketches.

Copyrighted Material

Constraints help to insure that changes to a sketch behave in a predictable manner. Editing causes shapes to change and parts often must be re-sized for weight, strength, appearance or other reasons. All of the changes can result in some weird shapes unless constraints are in place to control the changes. Two types of constraints are used: Dimension Constraints and Geometric Constraints.

Dimension Constraints

Smart Dimensions are applied to individual elements. A single pick will dimension a line, circle, etc.

Copyrighted Material

A pop down menu for other dimension types is shown. Distance between and angle between relate two items. Driving dimensions control a part feature. Driven dimensions are controlled by other dimensions. Each type is a different color on the screen.

Geometric Constraints

Copyrighted Material The geometric constraint icons are shown. Choosing and applying constraints is a matter of planning which elements must remain fixed in relation to other elements that are allowed to change.

Copyrighted Material

Turns display of geometric icons Off/On

34

Solid Edge V17

2D Drawing

Aligning Geometry

Copyrighted Material

The rectange is centered on the reference planes using connect constraint. (The first tutorial in chapter 1 used horizontal and vertical to do the same thing).

Copyrighted Material

Connect the mid-point of the horizontal line to the vertical (Y-Z) plane. Connect the mid point of the vertical line to the horizontal (X-Y) plane.

Changing the 2.000 and 3.000 dimensions will keep the rectangle centered.

A hexagon has been circumscribed about a circle. We want to be able to change the circle size and keep the hexagon shape.

Copyrighted Material

Lines are connect constrained and tangent constrained.

Changing the circle size produces in an unexpected result!

Copyrighted Material

What other constraints need to be added to fix the problem?

35

2D Drawing

Solid Edge V17

Editing 2D sketches.

Copyrighted Material

2D drawings are often constructed using basic shapes then editing the shapes to get the final forms. Fillet is a rounded corner. Chamfer is a beveled corner.

Offset may be one side or both sides.

Copyrighted Material

Sizes and locations may be fixed by placing dimensions. Objects may be moved or resized by changing the dimension value.

Copyrighted Material

Move pop-down displays several related editing commands.

Copyrighted Material

The rectangle shape was modified using the fillet editing command.

36

Solid Edge V17 Trim

2D Drawing

Copyrighted Material

Inner circular arcs were removed using trim.

Extend will only work if there is a “stopper” boundry.

Copyrighted Material

Extend would not work but Trim would work.

Construction Lines

Copyrighted Material

Regular lines may be toggled to construction line status (and back). Construction lines are not considered as part of a profile sketch. Using construction lines is a good way to anchor geometry and locate circle centers, etc.

Copyrighted Material 37

2D Drawing

Solid Edge V17

Grid and Grid Snap

Copyrighted Material

Placing a grid on the screen enables additional drawing accuracy controls. By setting a useful grid spacing and toggling Snap To Grid, the start and end points of lines, centers of circles, etc. can be placed accurately. Grid is very useful when an item must be placed relative to an existing point. Re-set the grid zero then measure over to the new point.

Toggle Grid On/Off with the screen icon or use Tools ...Grid Grid Ribbon Bar is shown.

Copyrighted Material

Grid settings dialog

Grid display On/Off

Snap to Grid On/Off

Set Grid 0,0 to new location

Set Grid to Origin

Copyrighted Material

Grid Options Dialog Box

Sets major line spacing, Minor spaces per major, colors, etc.

A typical decimal inch setting is shown. Working with architectural layouts, a typical setting might be: Major = 1 foot Minor = 12 (1 inch)

Copyrighted Material 38

Solid Edge V17

2D Drawing

Decimal inch grid setting shown.

Copyrighted Material

Grid Snap enabled so start and end points are on grid intersections.

Origin 0,0

X,Y locations may be set by clicking left mouse button or by keying in points.

Copyrighted Material

Re-Sizing the Grid Area

√ Click the Select Tool

√ Click near the outside of the grid. √ Drag the grid to a new area. A new ribbon bar for Grid Size Setting will appear at the top of the screen.

Copyrighted Material

An auto-resize option may be enabled.

Copyrighted Material 39

2D Drawing

Solid Edge V17

Tutorial - Shaft Support √ Start a new Part. Be sure to use More ... Normeng.par as the startup file √ Click Sketch √ Pick the Front (X-Z) reference plane. Refer back to this drawing for dimensions

Copyrighted Material Copyrighted Material Copyrighted Material

1. Set up a decimal inch grid as shown in the previous section. 1.000 inch major lines and 10 minor lines. 2. Draw the base of the part as shown. Start Line at -2.000,-0500 to -2.000, 0.000 to 3.000,0.000 to 3.000, 0.500 Re-size the grid if needed.

Copyrighted Material Origin 0,0

40

Solid Edge V17

2D Drawing

3. Draw two circles with center at X = 0.000, Y = 3.000

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The small circle is 1.000 diameter. ( Ø symbol = diameter)

The large circle is .875 radius. ( R = radius) Use the Tab Key to move the input to radius in the circle ribbon bar.

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4. Draw a line straight down from the side of the large circle. Make sure the line is tangent to the circle and is indicated vertical.

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5. Draw a short line across from -2.000, 0.500

6. Use the Trim Corner tool to close the corner.

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2D Drawing

Solid Edge V17

7. Re-set the grid origin to the end of the line at 3.000, 0.000

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Click the re-position origin icon on the grid ribbon bar.

Click the end if the line at 3.000,0.000.

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8. Draw the circle at -0.620, 1.250 Key in the center location in the X: and Y: boxes in the grid ribbon bar. Point to the center location.

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9. Draw line tanget to 2 circles as shown. Use tangent constraint to be sure line is tangent to both circles.

10. Draw line from 0.000, 0.500 tangent to the bottom of the right circle.

Save the drawing as ShaftSupport

Copyrighted Material 42

Origin 0,0

Solid Edge V17

2D Drawing

Copyrighted Material Copyrighted Material Copyrighted Material

The bottom of the large circle and the upper side of the right circle.

The .500 radius at the left side of the drawing. (We could have used Fillet at step 6.)

Place dimensions on the sketch as shown. Use dimension constraints to correct any location errors.

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Be sure the center of the two circles is in vertical alignment with the Side (Y-Z) reference plane.

Save the drawing.

(Next, we will make a part and a drawing).

43

2D Drawing

Solid Edge V17

13. Click the Return icon

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The sketch can be seen on the Front (X-Z) plane. 14. Click Protrusion

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15. Select the Front (X-Z) plane

16. Click Include Just O.K the dialog box.

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17 Click each of the lines and arcs that define the outline of the part. A Include icon will appear on each item. Do NOT include the reference planes.

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The final outline should be a closed loop.

44

Solid Edge V17

2D Drawing

Copyrighted Material

18. Click RETURN and set the depth of the part to 1.000

Copyrighted Material 19. Click Cutout

Select the Front (X-Z) plane. 20. Click Include Just OK the dialog box. Include the 1.00 diameter center circle.

Copyrighted Material Copyrighted Material 45

2D Drawing

Solid Edge V17

20. Click RETURN Click the Through Next option in the cutout ribbon bar. Use the mouse to point the cutout arrow toward the back of the part. Save the model.

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Part Properties.

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Collecting data for Bill of Material lists is an important documentation step. If your instructor provides data, fill in the dialog boxes. If not, just Cancel.

Making a drawing.

Be sure the part is saved from the previous steps. 21. Click New on the File Menu. Click the More Tab and select Normeng.dft

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A default drawing sheet will show.

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22. At the bottlom of the screen, Right Click the Sheet option.

46

Solid Edge V17

2D Drawing

23. Click the Background Tab and select A-Sheet (8 1/2 x 11 size)

Copyrighted Material Copyrighted Material

24. Select the ShaftSupport.par model from the folder where you save it.

25. Select Front for the key view.

Copyrighted Material Copyrighted Material 47

2D Drawing

Solid Edge V17

26. The Front view is selected by default.

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Click TOP , RIGHT and ISOMETRIC as shown.

Click Finish. The drawing will fit at a scale of 1:2 . Select that option before placing the views.

Click a view to move it on the sheet.

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Place some dimensions as shown.

Save and Print the drawing.

End of tutorial

Copyrighted Material Copyrighted Material 48

Solid Edge V17

2D Drawing

Problem 1.

Copyrighted Material

__ Layout the sketch in the Part Environment. __ Dimension the sketch.

__ Set up an “A” size sheet in the Draft Environment.

__ Place the views of the part as shown in the previous tutorial.

__Fill in the Title Block as shown. Use your name in the DR BY: box. __Dimension the drawing.

Copyrighted Material

__ Save and Print the drawing.

Thickness = 1.000

Copyrighted Material Copyrighted Material 49

2D Drawing Problem 2.

Solid Edge V17

Copyrighted Material

Create the sketch for the part shown below. Follow the steps as shown in Tutorial 1. Create a drawing,

dimension save and print.

Copyrighted Material Copyrighted Material Copyrighted Material

Thickness = .125

50

Solid Edge V17 Problem 3.

2D Drawing

Copyrighted Material

Create sketch and model. Make a drawing as shown in Tutorial 1. Dimension, Save and Print.

Copyrighted Material Copyrighted Material Part = Template

Thickness = .25

Copyrighted Material 51

2D Drawing

Solid Edge V17

Problem 4.

Copyrighted Material

Do the “Modeling Parts with Sketches” tutorial. Make a drawing as shown in Tutorial 1. Save and Print the model and the drawing.

Copyrighted Material Copyrighted Material Copyrighted Material 52

Engineering and Technical Drawing Using Solid Edge V18 by Jerry Craig Images from Solid Edge Gallery

Progressive Sheet Metal Die

SDC

PUBLICATIONS

Schroff Development Corporation www.schroff.com

www.schroff-europe.com

Solid Edge V18 2D Sketches Chapter 2

Using 2D Sketches

Reference Planes

Entity Objects

Constraining Sketches

IntelliSketch Settings

Editing Sketches

Grid

Tutorial

2D Drawing 2D Profiles

2D Sketches

Create Part

Create Assembly

Selecting

Profile View

Copyrighted Material Copyrighted Material Lines

Arcs

Circles and Ellipses

Smart Dimensions

Standard Dimensions

Geometric Constraints

Copyrighted Material

Rectangles

Geometric Relations

Selecting Entities & Deleteing

Fillets and Chamfers

Trimming and Extending

Settings

Re-Setting Origin

Key-In Values

Copyrighted Material Accurate Layout

Creating Drawings

31

Adding Text and Dimensions

Construction Lines

Printing

2D Drawing

Solid Edge V18

2D Drawings may take two forms:

Copyrighted Material

2D Sketches show the outlines and locations of multiple shapes or parts to be designed.

2D Profiles must be closed shapes with no entities inside or crossing the sketch. The sketch at the right may be used to create a part by selecting specific shapes then “cleaning up” the outline by trimming inner curves. The final shape must be a single series of connected lines and arcs.

Complete Master Sketch. (Cannot be used to create a part in this form).

Copyrighted Material Profile must be a closed “loop” with no internal lines.

Resulting 3D object with depth added.

Copyrighted Material

Portions of the Master Sketch are copied when creating individual part features.

Copyrighted Material 32

Solid Edge V18

2D Drawing

Assembly Sketches (Layouts)

Copyrighted Material

These are used to define the critical geometry in a series of mating parts. Elements from the master sketch may be selected to create the individual parts. This assures that the parts are the correct size and are located in exactly the right place.

Elements of the part sketches which are derived from the master sketch may be associated (linked) back to the master sketch. This means that any change in the master sketch will update all the associated parts.

Copyrighted Material

Portions of the sketch were used to create the base of the pillow block assembly. Other portions of the same sketch will be used to create the opening for the bearing. Modeling the bearing is done by selecting the inner circles. The bronze bearing is created as a separate part.

Copyrighted Material

The final assembly is shown with the parts modeled exactly as they fit.

As you can see, 2D sketches are the basis for much of the design and part creation process. These sketches can be very general at first then, exact sizes can be assigned later. All parts associated to the master sketches will resize to the new dimensions. Each part will be the right size and in the right place.

Copyrighted Material Bronze Bearing

Exploded Assembly view.

33

2D Drawing

Solid Edge V18

Starting a 2D Drawing

Copyrighted Material

Any new object starts with a 2D sketch. Complex objects can be designed more efficiently by creating a master sketch with part geometry defined by a series of overlapping lines. As the part shape evolves the 2D lines are used to add material or cut away material.

Simpler shapes may be designed by staring directly with the Protrusion or revolved Protrusion icons. Master sketches give more control over the modeling process.

Component Sketches are placeholders for existing parts or for related items yet to be designed.

Copyrighted Material

Once Sketch is started, The Ribbon Bar displays prompts and options. A Reference Plane must be selected. Or, a new reference plane must be defined as a 2D drawing plane.

A pop down dialog box allow the selection of alternate planes for starting the sketch.

Copyrighted Material

Coincident Option starts a sketch on one of the existing reference planes.

Copyrighted Material 34

Solid Edge V18

• The Draw toolbar replaces the Main toolbar. • The drawing surface is now the Front (X-Z) plane. • The horizontal line is the edge view of the Top (X-Y) plane. • The vertical line is the edge of the Side (Y-Z) plane. Draw menu items may hve several options selected from pop down menus. The first tutorial (chapter 1) introduced the 2D drawing process.

Exercise:

Copyrighted Material Edge of Side (Y-Z) plane

A 2D drawing screen appears.

2D Drawing

Edge of Top (X-Y) plane

Copyrighted Material 2D drawing surface = Front (X-Z) plane

Copyrighted Material

√ Start Solid Edge. √ Click Sketch. √ Click the Front reference plane.

Copyrighted Material

Draw some shapes. Explore the pop downs

Press ESC key to stop a command.

When finished, click the RETURN button.

Exit Do not save the drawing.

35

2D Drawing

Solid Edge V18

Copyrighted Material

Draw Menu

Constraints Menu

Copyrighted Material

Drawn items may be changed by editing lengths, angles, diameter/radius, etc.

Edit Menu

When items are connected, changing one item may cause another entity to change in an unexpected or unwanted manner. Placing constraints on a 2D sketch helps to ensure Engineering Intent.

Copyrighted Material

Copyrighted Material

Constraining sketches is an important step in the design process. Many features may be changed as the design evolves. Making sure the master sketch changes in a predictable manner is critical. Constraints are a combination of geometric (parallel, vertical, concentric, tangent, etc.) and dimensional lengths. The first tutorial (chapter 1) introduced some of these ideas.

36

Solid Edge V18

2D Drawing

Line command. Starting a line displays the Line Ribbon Bar.

Copyrighted Material

Color

Active Line Style

Type Thickness

Toggle between line and arc

Alignment Indicator Many indicators will appear as a drawing is created. These help to insure good geometry.

Copyrighted Material

A straight line was drawn then the arc toggle was selected. The intent zone creates the arc based on how the mouse moves out of the intent zone.

Intent Zone

Alignment indicators flash when horizontal.vertical, extensions or other alignments are sensed.

Indicators may be turned On/Off by clicking Tools menu and clicking the selection buttons.

Copyrighted Material

Tools ... Intellisketch ... Relationships toggles various geomentric indicators on/off.

Alignment Indicators On/Off toggles.

Copyrighted Material 37

2D Drawing

Solid Edge V18

Copyrighted Material Distance Between dimension option was used to fix point location.

Point

Other options for Line are Point (used as a marker or place holder) and Freesketch.

Freesketch. Hold left moude button down and draw shape. Solid Edge will create straight lines and arcs.

Copyrighted Material

√ Place smart dimensions to constrain the shape.

Circle. Pop down provides options for drawing circles and ellipses.

The circle ribbon bar provides options for color, linetype and line thickness. Click either diameter or radius box to input size.

Tangent Circle

Copyrighted Material

A circle was placed at random tangent to two lines. The circle size may be set using the circle command or by placing a smart dimension.

Copyrighted Material 38

Solid Edge V18

2D Drawing

Arc.

Copyrighted Material

Three options are shown. The arc ribbon bar gives slightly different options for each arc type.

Curve. Click a series of points. A smooth curve is drawn. Curve has many settings and options. Check Help for more information.

Copyrighted Material

Rectangle.

Quick method: Select Rectangle. Hold down left mouse button and sketch diagonal line. Use smart dimensions to set size.

Copyrighted Material Copyrighted Material 39

2D Drawing

Solid Edge V18

Constraining Sketches.

Copyrighted Material

Constraints help to insure that changes to a sketch behave in a predictable manner. Editing causes shapes to change and parts often must be re-sized for weight, strength, appearance or other reasons. All of the changes can result in some weird shapes unless constraints are in place to control the changes. Two types of constraints are used: Dimension Constraints and Geometric Constraints.

Dimension Constraints

Smart Dimensions are applied to individual elements. A single pick will dimension a line, circle, etc.

Copyrighted Material

A pop down menu for other dimension types is shown. Distance between and angle between relate two items. Driving dimensions control a part feature. Driven dimensions are controlled by other dimensions. Each type is a different color on the screen.

Geometric Constraints

Copyrighted Material The geometric constraint icons are shown. Choosing and applying constraints is a matter of planning which elements must remain fixed in relation to other elements that are allowed to change.

Copyrighted Material

Turns display of geometric icons Off/On

40

Solid Edge V18

2D Drawing

Aligning Geometry

Copyrighted Material

The rectange is centered on the reference planes using connect constraint. (The first tutorial in chapter 1 used horizontal and vertical to do the same thing).

Copyrighted Material

Connect the mid-point of the horizontal line to the vertical (Y-Z) plane. Connect the mid point of the vertical line to the horizontal (X-Y) plane.

Changing the 2.000 and 3.000 dimensions will keep the rectangle centered.

A hexagon has been circumscribed about a circle. We want to be able to change the circle size and keep the hexagon shape.

Copyrighted Material

Lines are connect constrained and tangent constrained.

Changing the circle size produces in an unexpected result!

Copyrighted Material

What other constraints need to be added to fix the problem?

41

2D Drawing

Solid Edge V18

Editing 2D sketches.

Copyrighted Material

2D drawings are often constructed using basic shapes then editing the shapes to get the final forms. Fillet is a rounded corner. Chamfer is a beveled corner.

Offset may be one side or both sides.

Copyrighted Material

Sizes and locations may be fixed by placing dimensions. Objects may be moved or resized by changing the dimension value.

Copyrighted Material

Move pop-down displays several related editing commands.

Copyrighted Material

The rectangle shape was modified using the fillet editing command.

42

Solid Edge V18 Trim

2D Drawing

Copyrighted Material

Inner circular arcs were removed using trim.

Extend will only work if there is a “stopper” boundry.

Copyrighted Material

Extend would not work but Trim would work.

Construction Lines

Copyrighted Material

Regular lines may be toggled to construction line status (and back). Construction lines are not considered as part of a profile sketch. Using construction lines is a good way to anchor geometry and locate circle centers, etc.

Copyrighted Material 43

2D Drawing

Solid Edge V18

Grid and Grid Snap

Copyrighted Material

Placing a grid on the screen enables additional drawing accuracy controls. By setting a useful grid spacing and toggling Snap To Grid, the start and end points of lines, centers of circles, etc. can be placed accurately. Grid is very useful when an item must be placed relative to an existing point. Re-set the grid zero then measure over to the new point.

Toggle Grid On/Off with the screen icon or use Tools ...Grid Grid Ribbon Bar is shown.

Copyrighted Material

Grid settings dialog

Grid display On/Off

Snap to Grid On/Off

Set Grid 0,0 to new location

Set Grid to Origin

Copyrighted Material

Grid Options Dialog Box

Sets major line spacing, Minor spaces per major, colors, etc.

A typical decimal inch setting is shown. Working with architectural layouts, a typical setting might be: Major = 1 foot Minor = 12 (1 inch)

Copyrighted Material 44

Solid Edge V18

2D Drawing

Decimal inch grid setting shown.

Copyrighted Material

Grid Snap enabled so start and end points are on grid intersections.

Origin 0,0

X,Y locations may be set by clicking left mouse button or by keying in points.

Copyrighted Material

Re-Sizing the Grid Area

√ Click the Select Tool

√ Click near the outside of the grid. √ Drag the grid to a new area. A new ribbon bar for Grid Size Setting will appear at the top of the screen.

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An auto-resize option may be enabled.

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Tutorial - Shaft Support √ Start a new Part. Be sure to use More ... Normeng.par as the startup file √ Click Sketch √ Pick the Front (X-Z) reference plane. Refer back to this drawing for dimensions

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1. Set up a decimal inch grid as shown in the previous section. 1.000 inch major lines and 10 minor lines. 2. Draw the base of the part as shown. Start Line at -2.000, 0.500 to -2.000, 0.000 to 3.000,0.000 to 3.000, 0.500 Re-size the grid if needed.

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3. Draw two circles with center at X = 0.000, Y = 3.000

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The small circle is 1.000 diameter. ( Ø symbol = diameter)

The large circle is .875 radius. ( R = radius) Use the Tab Key to move the input to radius in the circle ribbon bar.

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4. Draw a line straight down from the side of the large circle. Make sure the line is tangent to the circle and is indicated vertical.

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5. Draw a short line across from -2.000, 0.500

6. Use the Trim Corner tool to close the corner.

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7. Re-set the grid origin to the end of the line at 3.000, 0.000

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Click the re-position origin icon on the grid ribbon bar.

Click the end if the line at 3.000,0.000.

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8. Draw the circle at -0.620, 1.250 Key in the center location in the X: and Y: boxes in the grid ribbon bar. Point to the center location.

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9. Draw line tanget to 2 circles as shown. Use tangent constraint to be sure line is tangent to both circles.

10. Draw line from 0.000, 0.500 tangent to the bottom of the right circle.

Save the drawing as ShaftSupport

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Origin 0,0

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The bottom of the large circle and the upper side of the right circle.

The .500 radius at the left side of the drawing. (We could have used Fillet at step 6.)

Place dimensions on the sketch as shown. Use dimension constraints to correct any location errors.

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Be sure the center of the two circles is in vertical alignment with the Side (Y-Z) reference plane.

Save the drawing.

(Next, we will make a part and a drawing).

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13. Click the Return icon

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The sketch can be seen on the Front (X-Z) plane. 14. Click Protrusion

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15. Select the Front (X-Z) plane

16. Click Include Just O.K the dialog box.

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17 Click each of the lines and arcs that define the outline of the part. A Include icon will appear on each item. Do NOT include the reference planes.

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The final outline should be a closed loop.

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18. Click RETURN and set the depth of the part to 1.000

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Select the Front (X-Z) plane. 20. Click Include Just OK the dialog box. Include the 1.00 diameter center circle.

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20. Click RETURN Click the Through Next option in the cutout ribbon bar. Use the mouse to point the cutout arrow toward the back of the part. Save the model.

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Part Properties.

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Collecting data for Bill of Material lists is an important documentation step. If your instructor provides data, fill in the dialog boxes. If not, just Cancel.

Making a drawing.

Be sure the part is saved from the previous steps. 21. Click New on the File Menu. Click the More Tab and select Normeng.dft

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A default drawing sheet will show.

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22. At the bottlom of the screen, Right Click the Sheet option.

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23. Click the Background Tab and select A-Sheet (8 1/2 x 11 size)

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24. Click the Drawing View Wizard. Select the ShaftSupport.par model from the folder where you saved it.

25. Select Front for the key view.

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26. The Front view is selected by default.

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Click TOP , RIGHT and ISOMETRIC as shown.

Click Finish. The drawing will fit at a scale of 1:2 . Select that option before placing the views.

Click a view to move it on the sheet.

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Place some dimensions as shown.

Save and Print the drawing.

End of tutorial

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Problem 1.

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__ Layout the sketch in the Part Environment. __ Dimension the sketch.

__ Set up an “A” size sheet in the Draft Environment.

__ Place the views of the part as shown in the previous tutorial.

__Fill in the Title Block as shown. Use your name in the DR BY: box. __Dimension the drawing.

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__ Save and Print the drawing.

Thickness = 1.000

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2D Drawing Problem 2.

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Create the sketch for the part shown below. Follow the steps as shown in Tutorial 1. Create a drawing,

dimension save and print.

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Thickness = .125

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Create sketch and model. Make a drawing as shown in Tutorial 1. Dimension, Save and Print.

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Thickness = .25

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Problem 4.

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Do the “Modeling Parts with Sketches” tutorial. Make a drawing as shown in Tutorial 1. Save and Print the model and the drawing.

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