Quit the Sketcher and select the profile to be extruded.
Click Drafted Filleted Pad
The Drafted Filleted Pad Definition dialog box appears and the
application previews the pad to be created.
Enter 30 as the length value.
Selecting a second limit is mandatory. Select Pad1
top face as the second limit.
Note that planes can define second limits too.
Let's go on with the draft
definition. Enter 7 as the draft angle value.
Drafting faces is
optional. If you do not wish to use this capability, just uncheck the
Check the Second limit option to define the
So, Pad1 top face is also used as the neutral element.
Enter a radius value for each edge type to define the
Lateral radius: defines the fillets on
First limit radius: defines the round
Second limit radius: defines the filets
on the edges of the second limit.
edges is optional too. If you do not wish to use this capability, just
uncheck the options.
Clicking Preview previews the pad, the draft
and the fillets and display them in the specification tree. If you have
deactivated the draft or fillet options, the draft or the fillets are
then displayed as deactivated features in the tree, i.e. with red
Click OK to create the features.
If you look at the specification tree, you will note that you have
- one pad
- one draft
- three fillets
This means that for edition purposes, you need to
double-click the appropriate feature. This is your new part: