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NX Draft Feature

Stephen Rose - Wednesday, July 29, 2015

Overview


Most users are familiar with the need to draft walls of parts or tooling to a certain angle. For those that are not familiar: It is used in manufacturing to allow de-mold of plastic parts and castings, a design requirement of some sort of functional fit, or so that the cutter and possibly the holder have clearance when machining down in deep-draw cavities.

 

The NX Draft Feature command has different sub-types when applying draft angle to a model.In this example we will use the two simplest types From Edges and Tangent to Faces types.

 

Where to find it

 

The Draft Feature can be found several ways.If you are familiar with the traditional NX menu you will easily find it under Menu->Insert->Detail Featureà->Draft

 

If you are more comfortable with the NX Ribbon style interface you will find it in HOME->Feature Group->Draft

 

There is always the command finder where you can search the Draft feature and access it directly.


Use


Here we have an unfinished (yellow) part with vertical side walls as our starting body.First we want to add a simple draft angle to the side walls.

 


 

We access the Draft Feature command, either from the Menu or the Ribbon Bar interface.

 


 

Ribbon Interface

 


 

Once in the Draft Feature:

 

1. We select Type of Draft from the drop-down list and pick From Edges.

 

2.We define the Draw Direction, in this case the Z axis.

 

3.We proceed to select the bottom periphery edge of the part.

 

4.We set the angle to 5° and then with the preview option turned on we see the model updates to having 5° draft around the entire edge.(NX is smart enough adjust the upper radii

without the need to remove the radii and reapply after the draft command.)We use OK to apply this draft and exit the dialog box.

 


 

With the body drafted we now want to add a Hole Feature.In this example we set the Counter Bore Diameter large enough, and the position of the hole far enough over, so that the Counter Bore breaks out the side of our body.

 


 

With the C’bore subtracted the resultant part shows that there would be sharp material conditions where the holes break out the side of the body walls.(Note: In this picture we have also mirrored over the feature for better clarity of the conditions)

 


 

We want to clean up this condition by straightening the C’bore surface so they end up breaking out 90° to the side walls.

 


 

We enter the Draft Feature once again:

 

1. We select Type of Draft from the drop-down list and pick Tangent to Faces.

 

2.We define the Draw Direction, in this case the axis must point away from the concavity of the c’bore-Y axis (not into it as +Y) as indicated by the orange arrow .

 


 

3. We then select the C’bore face that is to be drafted.

 


 

4.We set the angle to 0° and then with the preview option turned on we see the model update to having 0° draft to the axis, but starting tangent to the C’bore face.

 


 


 

After hitting OK to accept the draft we end up with the modified part body as shown.(Note: In this picture we have also mirrored over the feature for better clarity of the conditions)

 


 


 

This type of modification can be very useful in part/product design to clean up features and eliminate sharp corners in a mold. It can also can play a part in the tooling industry by opening up areas for milling machines. Opening up various break out areas on tooling can increase the amount of machining strategies available to complete a particular feature.In this case access to the side of the feature is now possible.Efficiency could be realized by allowing use of profile or other machining methods to complete the majority of this part, rather than having to mill down the vertical axis of the feature only.

 


 


If you would like to learn more about this operation and other advanced operations, you should attend one of our advanced NX CAD courses. To arrange for advanced training please contact your Account Manager, or contact us directly at info@designfusion.com.



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