Chamfer

This command allows you to create chamfers on the edges of a shape.

Creation Stages / Use:

Click the icon or select Shape > Chamfer... from the drop-down menu (or Modeling > Local Shapes > Chamfer in the assembly document).

Choose the chamfer creation type: Identical or different values (see details in the available options)
Choose the chamfer creation mode
Fill in the parameters corresponding to the mode chosen
Select the edges and/or faces on which to apply a chamfer with the value provided

Available Options:

Value:

Identical: in this mode, all of the edges/face selected will use the same values as the chamfer parameters. If the values are modified while in use, then the edges/sides already selected (and those selected thereafter) will use this same radius.

Different: in this mode, it is possible to assign different values to the edges/faces selected. Thus, when you change the value of a parameter, the edges/faces already selected will still use the value of this parameter which was entered when they were selected. The new edges/faces selected will use the new value.

This mode applies the different values to the chamfer, but it is not possible to change the creation mode.

Mode:

You can choose here the way in which the chamfer is parameterized:

Offsets	Distance Angle	Distances

Offsets: Offsets: This mode creates chamfers that are even, this being the case even on non-planar faces or those faces that do not have an constant angle amongst each other. It is therefore indispensable when a chamfer is made on non-planar faces.

Angle Distance: This mode only supports planar, cylindrical or conical faces. The chamfer will not function if the faces are complex (curves).

Distance: This mode only supports planar, cylindrical or conical faces. The chamfer will not function if the faces are complex (curves).

Distances and Angle Distance:

Supported edges must have neighboring faces type:

- Plane - Plane,

- Plane - Cylinder

- Plane - Cylinder/Cone

- Plane - Cylinder/Sphere

Edges:

The edges/faces selected will be appear in this list.

To delete elements from this list, it is possible to select them again in the graphic area or to select them from the list and then use the "Delete" key on your keyboard. If the selection contains multiple invalidities, the contextual command Delete Invalid Selections allows to remove them quickly.

You can invert the direction of the chamfer by clicking on the last column "Invert"

If the Values option is set on "different", then two new columns are displayed in this list. These two columns correspond to the value of the two parameters of the chamfer for the corresponding edge.

You can modify the value of the parameters by clicking in the cell.

By checking Shape edges, all edges of the shape are selected. Orientated chamfers (second distance or distance+angle) are not compatible with this mode.

Limits:

By default, the chamfer is applied on the complete selected edges. This option allows to define limits.

	Points: allows to select 2 points by segment or loop to limit the chamfer. These points can also be created on the fly by clicking "+".

	Limits: allows to select 2 planes,surfaces or faces of the shape by segment or loop to limit the chamfer. These planes can also be created on the fly by clicking "+".

The pink arrows allow to invert the side of the limit.

Advanced Options:

Keep the faces covered: When this option is checked, TopSolid stores in the memory the topology of the faces which disappeared after creation of the chamfer. This keeps you from losing operations that use these faces as a reference.

Below is an example illustrating the occurrence with a fillet. The principle is the same for a chamfer.

Here is a shape with a boss operation made on the upper face. The fillet makes this face disappear. Here the behavior difference is observed. The behavior is similar with a chamfer.

Initial shape	Option Disabled	Option Enabled

Modifications:

Double-click the chamfer to display and modify parameter values.