Draft

Draft

Use the Draft command to modify faces by changing the angle relative to a draw direction.

You can do the following:

• Specify multiple draft angles and assign an angle to a set of faces.
• Add a single draft feature to multiple bodies.

Before draft	After draft

The Draft command is typically used to apply slope to faces for use in molded or die cast parts, so that when the mold or die separates, the faces move away from each other rather than sliding next to each other.

Generally, the draw direction is the direction in which the mold or die must move to be separated from the part. However, if you are modeling a mold or die, it is the direction in which the part must move to be separated from the mold or die.

Where do I find it?

Application	Modeling
Command	Draft

Isocline and True Draft methods

Isocline method

The entire face you are drafting will have the same angle at any section you cut through. This is the default method for creating a drafted surface.

An isocline surface is a ruled surface where the surface tangent at any point has the same slope, and where slope is measured as an angle relative to the draw direction.

		Draw direction, parallel to the centerline of the trimming cones. Stationary edge. The half-angle of the cones equals the specified draft angle. The apex of the cones follows either the stationary edge, or the section curves that are created from the stationary plane and the original faces to be drafted.

True Draft method

The True Draft method is useful when the faces to be drafted have edges that are nearly parallel to the draw direction, or when the Isocline method cannot create the required draft.

A True Draft surface is defined by a set of lines that have the following characteristics:

		Plane through point on stationary edge, normal to the face to be drafted and parallel to the draw direction. Stationary edge Line through point on stationary edge and parallel to the draw direction. Line through point on stationary edge on the plane at an angle equal to the draft angle, plus 90 degrees to the line that is parallel to the draw direction. Draft angle plus 90 degrees.

Create a draft from a plane

1. Choose Home tab→Base group→Draft .
2. From the Draft Type list, select Face.
3. Click the middle mouse button to accept the default draw direction (+ZC).
4. In the graphics window, select the planar face as the stationary plane.
5. Select the faces to draft.
6. In the Angle box, type a value.

For this example, 10 is entered. 7. Click OK.

Create a draft from an edge

This example uses the True Draft method to draft edges that are not contained in a plane normal to the draw direction.

Choose Home tab→Base group→Draft .

From the Draft Type list, select Edge.

Define draw direction +ZC.

Select the stationary edge.

Draft Angle = 20

In the Settings group, from the **Draft Method ** list, select True Draft.

Create a draft tangent to faces

This example shows how to draft the selected faces while maintaining the tangency to the blend.

Choose Home tab→Base group→Draft .

From the Draft Type list, select Tangent to Face.

Define draw direction +ZC.

On the scene toolbar, select Single Face from the Face Rule list.

Select tangent faces.

Angle = 5

Create a draft to parting edges

This example shows how to create a draft at parting edges and create a ledge perpendicular to the reference direction and the edge.

Choose Home tab→Base group→Draft .

From the Draft Type list, select Parting Edge.

Define draw direction +ZC.

Define the stationary plane.

Define the parting edges.

** Angle** = 10

Draft dialog box

Type
Specifies the method you want to use to create the draft.
Face

Edge

The draft is from a stationary edge. This option is useful when the edges required to be stationary are not contained in a plane normal to the direction vector.

Draft from stationary edge

Tangent to Face

The draft is tangent to a face. This option is useful in molded or cast parts to compensate for possible die lock.

Draft moves side faces to maintain tangency with the top

Parting Edge

The draft is from a parting edge relative to a stationary plane. The stationary plane determines the cross section that is maintained. This draft type creates ledge faces perpendicular to the reference direction and the edge.

Draft creates a ledge at parting edge, defined by a datum plane

Draw Direction

The draw direction is the direction the mold or die moves to be separated from the part.

NX infers the draw direction based on the input geometry.

Draft References

Available when Type is set to Face.

Stationary Face

Lets you select a stationary face or multiple faces as the reference for the draft. The intersection curves of the stationary faces with the draft faces are used as referece to calculate the draft.

Parting Face

Lets you select single or multiple faces as the reference for the draft. The intersection curves of the stationary faces with the draft faces are used as reference to calculate the draft.

• The faces to draft are subdivided at the intersection curves with the stationary faces.
• Draft can be added to both sides if needed.
• If the parting face and the fixed face do not intersect, an error message displays warning that the draft reference does not intersect faces to draft.

Stationary and Parting Face

Lets you create a draft from the stationary face t the parting face. The intersection curves of the stationary faces with the draft faces are used as reference to calculate the draft. The faces to draft are subdivided a the intersection with the parting face.

Type specific options
Face
Edge
Tangent to Face
Parting Edge
Settings
Draft Method
True Draft

For more information, see Isocline and True draft.

Distance Tolerance

Lets you specify the maximum distance between the input geometry and the resulting body.

The default value is taken from the Modeling Preferences.

Angle Tolerance

This tolerance is used to ensure that the drafted surfaces are within the specified angle in relation to neighboring surfaces.

The default value is taken from the Modeling Preferences.