Thursday, March 27, 2008

Profile Overview - SolidEdge

Profile Overview

clip_image002


clip_image003

Overview: After creating a new document, the first thing to create is the base profile. In most cases, you are going to start with a feature that adds material, such as a protrusion or a revolved protrusion. Play the video to see how to create and constrain a profile. This is a sound video, so please adjust your volume accordingly. clip_image004


clip_image005

Select a Plane

When you start with a protrusion or revolved protrusion, the first step is to define a plane that is the base of the feature. This plane will be created 'on the fly' and will be coincident with the front reference plane. clip_image006

clip_image008

clip_image005[1]

Create the Profile

Now that the plane is established, you are placed into the profile environment. The Draw toolbar and the Features and Relationship toolbar become active. Start by creating the curves for the profile. There are several tools on the Draw toolbar for creating a profile. Most profiles are created using lines and arcs, but there are several curves available. clip_image006[1]

clip_image010

clip_image005[2]

Constrain the Profile

After the profile is created, the next step is to add geometric constraints. It is important to get the shape constrained before dimensioning. If the shape is geometrically constrained, the profile will behave in a more predictable manner when dimensions are added. clip_image006[2]

clip_image012

clip_image005[3]

Dimension the Profile

Add dimensions to establish the physical size of the profile. clip_image006[3]

clip_image014

Wednesday, March 26, 2008

Profile Terminology- SolidEdge

In this unit ...

  • The following video will show you some of the highlights in this unit. This file contains sound, so be sure to adjust your volume accordingly. clip_image002
  • This unit:
    - Familiarizes you with the different types of profiles.
    - Shows you how to create the most common curves.
    - Demonstrates how to apply constraints on a profile.
    - Shows how to dimension a profile.
    - Demonstrates how to modify a profile.

clip_image003

Prerequisites

  • User interface experience

clip_image004

Completion Time: 2 hours

Profile Terminology

Second image

s


Overview: Profiles are used extensively in Solid Edge. A profile is a collection of curves and constraints that define a shape. The use of profiles is widespread throughout Solid Edge. You can create a profile in every module of Solid Edge, including Drafting.
Play the video to get an overview of how profiles work. This is a sound video, so please adjust your volume accordingly. clip_image002[1]


clip_image005

Closed Profile

A closed profile is a set of curves forming a closed loop without any overlapping lines. Closed profiles are used in any one of the following protrusion types: Protrusion, Revolved, Lofted, Swept, or Helical.

Third image

clip_image005[1]

Base Profile

A base profile is a closed profile on the first solid feature created in the part. Solid and Sheet Metal parts require the creation of base feature.

clip_image005[2]

Nested Profile

A nested profile consists of one closed profile completely enclosed within another closed profile, with none of the closed profiles intersecting at any point. If the feature is a protrusion, the outside profile defines the exterior extent of the solid, and the inside profile defines the interior extent of the solid, creating a cutout in the solid. If another profile nests inside the first nested profile, it creates a second solid that is not connected to the first. clip_image006

clip_image005[3]

Open Profile

Open profiles help you create features with additional design intent incorporated, and come into play after you create the base solid. Only use open profiles once you fully understand how they work.

clip_image008

clip_image005[4]

Constraints

Solid Edge uses two different types of constraints, geometric and dimensional. Geometric constraints are used to control the shape of a profile. Tangent, Horizontal and Vertical, Connect, and Collinear are just a few types of common geometric constraints. Dimensional Constraints, or Dimensions, are used to define the size of the profile. Most dimensions can be edited to change the size of the profile. clip_image006[1]clip_image006[2]

clip_image010

clip_image012

Tuesday, March 25, 2008

Reference Plane Project-SolidEdge

Project: Creating Reference Planes

clip_image001


clip_image002

Completion Time: 15 Minutes

clip_image004


clip_image005

Prerequisites

  • An understanding of creating reference planes.

clip_image006

Objective: Create three reference planes to serve as a base for a new feature.


clip_image007

Instructions

clip_image008

1: Open planes_project.par and save a copy to your local hard drive or a network drive where to can store parts. clip_image009

Step 1 - Details

1.1 clip_image010 Click Open. Use the Look In option to navigate to the folder where planes_project.par is located. Select the planes_project.par and click the Open button.

1.2 Select File | Save As… Use the Look In option to navigate to the folder where you can save the part. Type in a name for the new file. It would be recommended to keep it the same name.

clip_image008[1]

2: Create the first plane to it is parallel to the Front plane and passes through the center of the arc on the front of the mouse. clip_image001[1]clip_image009[1]clip_image012

clip_image008[2]

Step 2 - Details

2.1 clip_image013 Click Parallel Planes from the Plane pull-down menu on the Features toolbar.

2.2 Pick the Right plane in the graphics window.

2.3 Click Keypoints from the ribbon bar.

2.4 Select Arc Center from the Keyppoints pull-down.

2.5 Select the arc on the front of the mouse. clip_image014

clip_image015

clip_image008[3]

3: Create the second reference plane at a 60 degree angle from the first reference plane created and the bottom planar face of the part. clip_image001[2]clip_image009[2]clip_image017

clip_image008[4]

Step 3 - Details

3.1 clip_image018 Click Angled Planes from the Plane pull-down menu on the Features toolbar.

3.2 Pick the first reference plane you created.

3.3 Pick the bottom planar face of the part.

3.4 Move the cursor to get the horizontal and vertical orientation to the lower left corner of the plane.

clip_image020

3.5 Click in the graphics window to set the orientation.

3.6 Enter 60 in the angle text box on the ribbon bar.

3.7 Click in the graphics window to create the plane.

clip_image008[5]

4: Create the third reference plane 40mm from the second reference plane. Be sure the reference plane is above the part.

clip_image021]

clip_image008[6]

Step 4 - Details

4.1 clip_image013[1] Click Parallel Planes from the Plane pull-down menu on the Features toolbar.

4.2 Pick the angled plane in the graphics window.

4.3 Enter 40 in the distance text box on the ribbon bar.

4.4 Click above the part to create the parallel plane.

clip_image022

Review: Creating reference planes is useful for features that require compound angles or multiple offsets. If a feature only requires a single plane, then is it best to create it on-the-fly. This way, the plane is embedded into the feature and reduces the amount of features displayed on the Feature PathFinder. It also reduces the amount of objects displayed in the graphics window.