Perpendicular Constraint - SolidEdge

Perpendicular

Use this to ...

• Make two lines have a 90-degree angle between them.
• Play the video to learn how to add perpendicular constraints to profiles. Do not adjust your volume; there is no sound associated with this video.

Key Points

• The Perpendicular constraint displays as a small 90-degree angle symbol at inside the corner of the two lines.

Prerequisites

• Solid Edge must be in the Profile mode. Profile mode is automatically activated when creating a sketch feature or creating a profile for a feature.

Process: Creating a Perpendicular Relationship

1. Click Perpendicular on the Features and Relationships toolbar.

2. In the Graphics window, pick the first line.

3. Pick the second line. The first line moves perpendicular to the second line and a small 90-degree angle symbol displays inside the corner.

Parallel Constraint - SolidEdge

Parallel

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Use this to ...

• Makes two lines have the same angular alignment.
• Play the video for a demonstration on how to assign a parallel constraint. Do not adjust your volume; there is no sound associated with this video.

Key Points

• Makes the first line parallel to the second line
• Parallel displays as two small parallel lines on each object.

Prerequisites

• Solid Edge must be in the Profile mode. Profile mode is automatically activated when creating a sketch feature or creating a profile for a feature.

Process: Creating a Parallel Relationship

1. Click Parallel on the Features and Relationships toolbar.

2. In the Graphics window, pick the first line.

3. Pick the second line. The first line moves parallel with the second line and a small set of parallel lines display at the center of the selected lines.

4. Continue picking lines until all parallel constraints are assigned.

Concentric - SolidEdge

Concentric

Use this to ...

• Connect center points to each other.
• Play the video to see how to assign a concentric constraint. Do not adjust your volume; there is no sound associated with this video.

Key Points

• Attaches a center point of an arc/circle to the center point of another arc/circle.
• Concentric displays two small circles at the center point of the two selections.

Process: Creating a Concentric Relationship

1. Click Concentric on the Features and Relationships toolbar.

2. Pick the first arc/circle.

3. Pick the second arc/circle. The first selection moves to fit the second.

Advanced Constraints Overview - SolidEdge

Advanced Constraints Overview

Overview: In the Basic Profile Creation unit, you were shown some of the more commonly used constraints. Those constraints are used a high percentage of time when creating profiles. Play the video to see a demonstration of adding some of the advanced constraints. This is a sound video, so please adjust your volume accordingly.

Concentric

The Concentric command forces two circles or arcs to share the same arc center. It is located on the Features and Relationships toolbar. The concentric constraint is displayed as two circles at the arc center of the selected curves.

Parallel

The Parallel command makes two lines parallel to each other. This constraint does not need to be applied to lines that are already horizontal or vertical. The parallel constraint displays as two small parallel lines at the midpoint of a line.

Perpendicular

Perpendicular forces two lines to be at a 90-degree angle to each other. Again, this constraint does not need to be applied to lines that are already horizontal and vertical. This constraint is displayed in the graphics window with small box at the intersection of the two lines.

Equal

The Equal command makes two curves equal in size. The two curves must be the same curve type, so you cannot apply an Equal constraint between a line and an arc. This constraint is displayed as a small equal sign at the midpoint of each curve.

Trimming Profiles - SolidEdge

Trimming Profiles

Use this to ...

• Trim and/or delete lines in a profile.
• Play the video to see how to trim curves by selection and by dragging. Do not adjust your volume; there is no sound associated with this video.

Key Points

• Assigns the connect constraint between the curves being trimmed.
• Select the portion of the curve to remove.

Prerequisites

• Solid Edge must be in the Profile mode. Profile mode is automatically activated when creating a sketch feature or creating a profile for a feature.

Process: Trim by Picking

1. Click Trim on the Draw toolbar.

2. In the Graphics window, move the cursor over the curve. The segment to be trimmed highlights.

3. Pick the highlighted segment. The highlighted segment is trimmed.

Process: Trim by Dragging

1. Click Trim on the Draw toolbar.

2. In the Graphics Window, hold the cursor near the curves to trim.

3. Drag the cursor across the curve(s). A drag path displays.

4. Release the left mouse button. The curve(s) trim, extend and/or deletes.

Tips

• When trimming corners by dragging, be sure to drag over the portions of the curves you wish to keep.

Changing Curves to Construction - SolidEdge

Changing Curves to Construction

Use this to ...

• Convert curves in a profile to Construction.
• Convert reference curves back to regular curves.
• Play the video to see a demonstration of how to create curves and change them to construction curves. Do not adjust your volume; there is no sound associated with this video.

Key Points

• Construction curves are not included as part of the feature.
• These curves assist you when lining up other curves in the profile.
• When a curve converts to a construction, the line style changes from solid to phantom (dashed).

Prerequisites

• You must be in either the Sketch or Profile mode.

Process: Creating a Construction Curve

1. Click Construction on the Draw toolbar.

2. In the Graphics window, pick a curve. The normal curve converts to a construction curve.

Process: Converting a Construction Curve

1. Click Construction on the Draw toolbar.

2. In the Graphics window, pick a construction curve. The construction curve converts to a normal curve.

Creating Ellipses - SolidEdge

Creating Ellipses

Use this to ...

• Create a full ellipse by select three points.
• Create a full ellipse by picking the center point and radius point.

Key Points

• Creates an ellipse by picking three points.
• Creates an ellipse by picking the center point, the primary axis point, and the secondary axis point.
• Play the video to see a demonstration of how to create two different types of ellipses. Do not adjust your volume; there is no sound associated with this video.

Prerequisites

• Solid Edge must be in the Profile mode. Profile mode is automatically activated when creating a sketch feature or creating a profile for a feature.

Process: Creating an Ellipse By Three Points

1. Click Ellipse by 3 Points from the Circle fly-out on the Draw toolbar.

2. In the Graphics window, pick the first point of the ellipse. A dashed line displays connecting the point to the cursor.

3. Pick the second point, an ellipse displays between the two points.

4. Pick the third point to define the height and create the ellipse.

Process: Creating an Ellipse By Center and Endpoints

1. Click Ellipse by Center from the Circle fly-out on the Draw toolbar.

2. In the Graphics window, pick the first point of the ellipse. A dashed line displays connecting the point to the cursor.

3. Pick the second point, an ellipse displays between the two points.

4. Pick the third point to define the height and create the ellipse.

Tips

• Ellipses are difficult to fully constrain. Use them only if necessary.

Filleting Profiles - SolidEdge

Filleting Profiles

Use this to ...

• Round corners in a profile.
• Play the video to learn how to create two fillets using two different methods. Do not adjust your volume; there is no sound associated with this video.

Key Points

• Creates a tangent arc between two curves in profile.
• Use this option as a last resort. Use a round feature on the model afterwards.

Prerequisites

• Solid Edge must be in the profile mode. Profile is automatically activated when creating a sketch feature or creating a profile for a feature.

Process: Dynamically Creating a Fillet on a Profile

1. Click Fillet from the Fillet fly-out on the Draw toolbar.

2. If necessary, click No Trim on the ribbon bar.

3. In the Graphics window, pick the first curve to highlight it.

4. Pick the second curve to highlight it and display the fillet.

5. Move the cursor to the desired location.

6. Pick to create the fillet.

Process: Creating a Fillet on a Profile by Dragging

1. Click Fillet from the Fillet fly-out on the Draw toolbar.

2. In the Graphics Window, hold left mouse button close to one of the curves to fillet.

3. Drag the cursor across the two curves.

4. Release left mouse button to create the fillet.

Tips

• It is strongly encouraged to apply fillets as round features in the model. This practice gives you more flexibility for editing, deleting, or redefining the fillet.
• Dragging across the two lines you want to modify also places a fillet. This modifies the lines to the cursor's approximate intersect position; however, this is very inaccurate.
• The two curves being modified don't have to connect to perform this operation. The Fillet operation connects the two curves to the fillet.

Sketch Tools- SolidEdge

Ellipse

An ellipse creates a circle that is shortened on one axis. They can be handy in a profile, but can also be a little tricky to constrain. There are two methods for creating an ellipse, By Center and By Three Points. Either method uses the same technique for creating them. When you create an ellipse, you pick the first location of the ellipse, pick the location of the primary axis, then pick the location of the secondary axis.

Trimming

It is sometimes required to trim curves that overlap or need extending. The Trim functions on the Draw toolbar provide the capability of trimming curves. The command trims back the portions of curves that are selected. This can be done by picking curves individually or by dragging the cursor across the curves to remove. The trim options also apply geometric constraints to the trimmed curves. Using the trim options can be very useful when importing profiles from other CAD packages, such as AutoCAD.

Construction Curves

There are times when you need to create curves in a profile that are helpers in constraining a profile. These curves are called construction curves. To create a construction curve, simply create the required curve or curves as regular geometry. After the geometry is created, you convert the geometry using Construction. This option converts regular curves to construction curves. After the curves are converted, they display in a phantom line font. Construction can also convert a construction curve back into a regular curve.

Profile Basic - SolidEdge

Profile Basic - SolidEdge

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In this unit ...

• The advanced profile creation unit exposes you to more complex curves and constraints. This unit provides you with different techniques for quickly creating curves, constraints, and dimensions. In addition, you will learn additional tips for modifying a profile. Play the video for an overview of what will be covered in this unit. This is a sound video, so please adjust your volume accordingly.
• This unit: - Introduces you to more profile terminology and settings. - Shows you how to create the additional curves. - Demonstrates how to apply more constraints on a profile. - Shows how to rapidly dimension a profile. - Demonstrates how to modify a profile.

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Prerequisites

• Basic Profiles knowledge

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Completion Time: 2 hours

Advanced Profiles Overview

Overview: There are several curve types available when creating a profile. The Advanced Profile Creation unit exposes you to most commonly used curve types. In the next few topics, you will be shown how to use these curve commands. Play the video to see an overview of the advanced tools available when creating a profile. This is a sound video, so please adjust your volume accordingly.

Rectangle

Located on the Draw toolbar, Rectangle creates a series of 4 lines. There are two different methods for creating a rectangle. The fastest method is by dragging the cursor across the graphics window. A rectangle is created between two locations of the drag. The second method uses three points. The first point is the base point, the second point defines the length of the rectangle, and the third point defines the height of the rectangle. This is useful for creating rectangles at an angular orientation.

Project: Basic Profile Creation Project - SolidEdge

Project: Basic Profile Creation Project

Completion Time: 30 Minutes

Objective: Complete the three sketches to re-enforce the topics described in this unit.

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Instructions

1: Create a new metric part in a location where you can save parts. Save the part and name it flanged_elbow.

Step 1 - Details

1.1 Click File | New.

1.2 Select the More tab and select Normet.par from the list.

1.3 Click OK on the New dialog.

1.4 Click File | Save.

1.5 Click OK on the Properties dialog.

1.6 Use the Look In option to navigate to the folder where the part is top be saved.

1.7 Type in flanged_elbow in the file name text box.

1.8 Click OK on the Save As dialog.

2: Create the first sketch Top plane. The profile consists of an arc with two small lines on each side. The arc center is constrained to the mid point of one of the reference planes and the ends of the arc are connected to the corresponding reference plane. The two short lines are both 10mm long. Complete this profile to the shape and size of the following picture.

Step 2 - Details

2.1 Click Sketch from the Features toolbar.

2.2 Pick the Top plane in the graphics window.

2.3 Click Line on the Draw toolbar.

2.4 Draw the following curves.

2.5 Click Tangent. Apply tangency between all lines and arcs that do not have it.

2.6 Click Connect. Pick the arc center and the mid point of the reference plane. Pick the endpoint of the lower portion of the arc and select the horizontal reference plane. Pick the endpoint of the upper portion of the arc and select the vertical reference plane.

2.7 Click Equal. Pick the two small lines.

2.8 Click Smart Dimension. Pick the arc and dimension it to a value of 60mm. Pick one of the lines and dimension it to a value of 10mm.

2.9 Click Return on the ribbon bar.

2.10 Click Finish on the ribbon bar.

3: Create the second sketch on the Front plane. The profile consists of a circle. The circle is connected to the end point of one of the short lines in the first sketch. Complete this profile to the shape and size of the following picture.

Step 3 - Details

3.1 Click Sketch from the Features toolbar.

3.2 Pick the Front plane in the graphics window.

3.3 Click Circle by Center from the Circle Fly-out on the Draw toolbar.

3.4 Draw the following circle.

3.5 Click Connect. Pick the circle center and the end point of the short line from the first sketch. The cursor should look like this when you select the end of the curve.

3.6 Click Smart Dimension. Pick the circle and dimension it to a value of 96mm.

3.7 Click Return on the ribbon bar.

3.8 Click Finish on the ribbon bar.

4: Create the third sketch on the Right plane. The profile consists of two lines and two arcs in the shape of an oval. The arc centers are aligned vertically with the end point of one of the short lines in the first sketch. The mid points of the lines are aligned horizontally with the mid point of the Top plane. Complete this profile to the shape and size of the following picture.

Step 4 - Details

4.1 Click Sketch from the Features toolbar.

4.2 Pick the Right plane in the graphics window.

4.3 Click Line on the Draw toolbar.

4.4 Draw the following curves.

4.5 Click Tangent. Apply tangency between all lines and arcs that do not have it.

4.6 Click Horizontal – Vertical. Pick the arc center the top arc and pick the end point of the short line in the first sketch. Pick the mid point of the left vertical line and pick the mid point of the reference plane.

4.7 Click Smart Dimension. Activate Tangent Display in the ribbon bar. Pick the top arc and the bottom arc and dimension it to a value of 96mm. Pick the left vertical line and the right vertical like and dimension it to 60mm.

4.8 Click Return on the ribbon bar.

4.9 Click Finish on the ribbon bar.

5: When you have completed the sketches, save the part. Remember the location of this part for future use.

Step 5 - Details

Click File | Save.

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Challenge Task: To ensure the second and third profiles are connected to the first profile, edit a dimension in the first profile. Modify the radius dimension to a value of 120mm. Look to see if the second and third profiles move with the change. If not, revisit the profiles and set the connection to the first profile.

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Review: In this project, we positioned the second and third profiles relative to the first profile. If the first profile is modified, the location of the other two will automatically update. This is an effective method for capturing Design Intent.