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TOPIC: USING THE FILLET TOOL (FILLET FEATURE) - OVERVIEW
BEFORE YOU BEGIN
- If there is any concept you do not understand, check out previous lessons here.
INTRODUCTION
Fillets are smooth and round features commonly found on a edges of parts. Fillets are primarily used to reduce stresses on machine components/parts to reduce the potential of fatigue failure due to high stresses, and for aesthetic reasons. For the case of aesthetics, large filleted edges can be found on common household appliance e.g. coffee makers, reading lamps, hair dryers, phones, etc. These fillets help to improve handling experience (or ergonomics). So you can hold on to a phone without feeling acute pressure inside your palms because of the filleted edges of the phone.
The Fillet tool allows you to parametrically add a fillet feature to your part/component. This fillet could be a constant-radius fillet (where one radius is used to create the entire fillet) or a variable-radius fillet (where more than one radius is used to define the fillet along the edge). The Inventor Fillet tool offers an easy but powerful means of applying and modifying fillet features in your design.
OBJECTIVES
At the end of this lesson, the reader should be able to:
- Describe the purposes of fillets on parts/components.
- Explain the difference between fillets and rounds and give an example of how they are used.
- Use the Fillet tool to create constant radius fillets.
- State the guidelines for creating fillets.
LOCATING THE FILLET TOOL
The Fillet tool could be found on:
- RIBBON: Model tab > Modify panel > Fillet
- SHORTCUT: F
DEFINITION AND TYPES OF FILLETS
A fillet is defined by a single constant radius, or in the case of a variable fillet, by more than one radius. Technically, there are two types of fillets, namely, "Fillet" and "Round." The term "fillet" is used when a fillet is applied to an interior (or internal) corner/edge, (where the faces forming the corner/edge have an angle of 180 degrees or less between them). Fillets will also add material to your component/part. On the other hand, the term "round" is used when a fillet is applied to an exterior (or external) corner/edge. A round removes material from your component/part when created.
Figure 2 shows a part whose three (3) interior edges have been filleted, while Figure 3 shows a part whose exteior edges have been rounded. Note that both fillets and rounds are created with the Fillet tool.
CATEGORIES OF FILLETS
On the fillet dialog box, there are three important categories of fillets or rounds that can be created, namely:
- Edge Fillet,
- Face Fillet, and
- Full-Round Fillet.
EDGE FILLET
As the name implies, an edge fillet is created along an edge of a part. An edge is formed by two adjacent faces, therefore, the Fillet tool will reshape the two shared face to create the desired fillet or round. Figure 4 shows a part with a single edge fillet.
FACE FILLET
A face fillet adds a fillet or round between two selected face sets, which need not share an edge. Figure 5 shows part with a face fillet applied between the top face and the left face.
full-round fillet
A full-round fillet adds a fillet or round that is tangent to three selected adjacent faces. The center face set is replaced by a variable-radius fillet. As can be seen in Figure 6, as full-round fillet is applied between the top, right, and bottom face of the part. The center (right) face is totally replaced with a fillet, which is tangent to all the three selected faces.
CONSTANT-RADIUS FILLET OPTIONS
The Constant Filet tab of the Fillet Dialog box contains the following creation methods and options.
|
OPTION
|
DESCRIPTION
|
| 1. |
Edge |
Adds fillets or rounds to one or more edges of a part. All fillets and rounds created in a single operation become a single feature. |
| 2. |
Face |
Adds fillets or rounds between two selected face sets. The face sets do not need to share an edge. |
| 3. |
Full Round |
Adds fillets or rounds that are tangent to three adjacent faces. The center face is replaced by the fillet. |
| 4. |
Select Mode |
Mode selection enables easy selection of objects to fillet.
- Select Edge, for edge selection priority, enables you to select individual edges on the part. So you have control of what edge to select
- Loop, for face selection priority, allows you to select all edges on a particular face in one click.
- Feature, for feature priority selection, allows you to select what feature to apply the fillet to. This works on parts with multiple features, so it gives your control over which feature to apply the fillet to, thereby ensuring that your do not select edges any other feature.
|
| 5. |
Solids |
This button is only available when multiple solid bodies exist in the part file. When this is the case, the user can click the solids button to select one or more solid bodies to use with the All Fillets and All Rounds selection options. |
| 6. |
All Fillets |
Use the All Fillets check box to quickly select all fillet edges on the part. Select them both to have all edges on the part selected. |
| 7. |
All Rounds |
Use the All Rounds check box to quickly select all round edges on the part. Select them both to have all edges on the part selected. |
GUIDELINES FOR CREATING FILLETS
Although both fillets and chamfers are relatively simple shapes, they are often a challenge to create with consistency where multiple edges intersect. Following the guidelines presented here can improve your success in creating these features.
- Avoid creating all of your fillets with a single feature. You will have a greater success creating and changing features with less edges selected.
- Create these features on parallel edges of a part first. When you create additional features, you can select the resulting face to complete the remaining edges at the same time.
- Pressing CTRL while clicking removes geometry from the selection.
- Because fillets are considered finish features, consider creating them toward the end of the design process after all other features have been defined.
- Avoid including fillets in your sketch geometry and instead create them as part features.
In the next two lessons, we are going to look at how to create constant-radius and variable-radius fillets, face fillets, and full-round fillets.
REFERENCE
1. Autodesk Inventor 2010: Official Training Courseware.
