Chamfer

Chamfer

Use the Chamfer command to bevel the edges of one or more bodies.

Depending on the orientation of the edges to be chamfered, chamfers can add or subtract material.

You can define the cross section of the chamfer by specifying:

• One symmetric offset distance.
• Two asymmetrical offset distances.
• An offset distance and an angle.

You can specify:

• Edge sets to define chamfers with different dimensions and cross sections within a single chamfer feature.
• Length limits to span the chamfer less than the entire length of an edge.

Where do I find it?

Application	Modeling, Sheet Metal, and Flexible Printed Circuit Design
Command	Chamfer
Graphics window	Right-click an edge of a body→Chamfer

Create a chamfer with asymmetric offsets

This example shows how to create two chamfers with asymmetric offsets in a single Chamfer feature.

Choose Home tab→Base group→Chamfer .

Select the edges to chamfer.

In the Edge group, set the following:

• Cross Section = Asymmetric .
• Distance 1 =
• Distance 2 = .

For this example, the distance values of 10 and 5 are used.

If the offset distances are measured on the wrong side of the selected edges, click Reverse Direction .

In the Edge group:

1. Expand the List.

List
Chamfer1

The current parameters of the chamfer are listed here. 2. Click **Add New Set ** .

List
Chamfer1
Chamfer2

A new set is created. It is currently empty, but will list the parameters of the next chamfer you create.

Select edges for the second chamfer.

The defining parameters of the first chamfer are remembered and applied to the second chamfer. For this example, we will use the same parameters. The new set of parameters populates the List.

List
Chamfer1
Chamfer2

Click OK to create the chamfer.

In this example, notice the exterior chamfer removes material and the interior chamfer adds material.

When a chamfer is created, a feature is created in the Part Navigator. The Details panel displays the parameters of the respective chamfers. The parameters are editable here. Note that you can have more than one chamfer in a Chamfer feature.

Part Navigator Chamfer (n)
Details
Parameter
= Chamfer 1 Distance 1
= Chamfer 1 Distance 2
= Chamfer 2 Distance 1
= Chamfer 2 Distance 2

Create a chamfer with length limits

This example shows how to use the datum planes to limit the length of chamfers.

Choose Home tab→Base group→Chamfer .

Select the edges to chamfer.

Set the following:

In the Edge group:

• Cross Section = Symmetric
• Distance =

For this example, a value of 2 is used.

In the Length Limit group:

• Limit Object = Plane

You can select an existing plane or create a new plane to limit the length of a chamfer.

For this example, we will create a new plane.

• Plane list = On Curve

For this example, a top exterior edge is selected.

Do the following:

1. Select an edge to create a plane.

For this example, a top exterior edge is selected. 2. Set the Arc Length scene dialog to specify the location of the plane on the edge.

In the Length Limit group, click **Add New Set **.

NX creates a new set. It is currently empty, but the next plane you create appears in this set.

List
Set 1
Set 2

Select another edge to create one more plane, and specify the location of the plane on the edge to control the length of the chamfer.

Click OK to create the chamfer with length limits.

The chamfers do not span the entire length of the selected edges.

Chamfer dialog box

Edge
Select Edge
Cross Section
Distance Distance 1 Distance 2
Angle
Reverse Direction
Add New Set
List
Chamfer1
Chamfer2

Length Limit

Limit Object

Lets you select the object to limit the chamfer length:

Limits the chamfer length with one or more points in point sets.

Specify Point

Lets you specify points to limit the length.

Limits the chamfer with one or more planes in plane sets.

Specify Plane

Lets you specify planes to limit the length.

If the plane intersects the chamfer in multiple locations, you can specify a point that defines the region to trim. The plane normal determines the side to trim. You can select the Trim to Limit Object check box and then specify a point.

Limits the chamfer length with one or more faces in face sets.

Select Face

Lets you specify faces to limit the length.

You can clear the Trim to Limit Object check box to limit the length at the first intersection point between the face and the chamfer.

Limits the chamfer length with one or more edges in edge sets.

Select Edge

Lets you specify edges to limit the length.

Add New Set

Lets you create object sets to define multiple length limits.

List

Displays the list of object sets created to limit the chamfer length.

Each set contains a single limiting object.

List
Set 1
Set 2

Settings

Tolerance

Specifies the tolerance value that is used to find the nearest face, which is then used to define the offset distance of the chamfer.

Offset Method

Available for the Symmetric and Asymmetric cross section types.

Specifies a method to define the edges of the chamfer faces using the offset distance values.

Defines the edges of the chamfer face by measuring the offset distance from the apex point.

This option produces accurate results when the faces adjacent to the edge are not analytic or not conveniently orthogonal.

Defines the chamfer by offsetting the faces adjacent to the edge you select by the specified distance(s), and then projecting the intersection of the offset faces normal to the original faces.

This option gives you more control over the accuracy of the chamfer, especially with complex cross sections.

	Cross Section = SymmetricDistance = 0.55
	Cross Section = AsymmetricDistance 1 = 0.55Distance 2 = 0.15