SolidWorks Tech Tip: Deleting "Things"

SolidWorks Tech Tip: Deleting Things

Most people know that you can delete lines from a sketch, or features from the Solidworks feature Manager, by pre-electing the object(s) and then simply hitting the DELETE key. But did you know, that over the last 4 years, the programmers have enhanced the intelligence behind the DELETE key, allowing it to react differently in the following situations:

BODIES: If what you have pre-selected are Solid or Surface Bodies, the DELETE key will instead launch the function INSERT - FEATURES - DELETE BODY.

PATTERNS: If what you pre-selected were members of a feature Pattern, the DELETE key will pop-up a dialog asking you if you really wanted to delete the entire pattern, or if instead you wanted to add the selected pattern members to the "SKIP LIST".

SURFACE EDGES: If what you pre-selected was an edge curve from an interior 'hole' in a surface face, the DELETE key will automatically run the function INSERT - SURFACE - UNTRIM, which will 'heal' the surface to eliminate the hole.

SolidWorks Tech Tip: What's Old is New Again: Dynamic Editing

SolidWorks Tech Tip: What's Old is New Again: Dynamic Editing

A function was added in SolidWorks 99 that allows you to dynamically edit features without having to Edit Sketch or Edit Feature definition. This functionality is still there, lurking in the software, waiting to be rediscovered by today's SolidWorks user!

First, to access Move/Size Features, you need to add an icon to your toolbars: Open a part file. Go to Tools - Customize... Click on the Commands tab. Select the Features category of icons. In the third row of icons, look for two small green spheres with four black arrows. Drag and drop that icon onto your toolbar of choice.


Now that you have the icon available, what can you do with it? To use any of the Move/Size Features capabilities, turn on the function by clicking the icon once to activate it. Now, here's what you can do:


Activate the Move/Size Features icon. All of the following behavior will only occur if Move/Size Features is active. Click the icon to activate or deactivate the function:

Move Features. Click on the face of a feature and drag/drop it onto another face (or edge). This works with Extrude, Revolve, Fillet and Chamfer. You have now reassigned the location of the feature to either a new sketch plane (or new edge to fillet/chamfer). Normally you can only drag/drop to move features in this manner if you hold down the Shift key, but with Move/Size Features active you do not need the Shift key.


Size Features. Select the face of an Extrude. Three small green sphere "handles" appear. Drag the one that has two straight arrows sticking from it and you can dynamically change the extrude depth without having to Edit Feature. Cursor feedback tells you the length of the extrude as you drag it. Moving your cursor nearer or further from the extrusion centerline alters the drag increment.



Resize Sketches. Click on the face of a feature, such as an Extrude, that is built from an underderfined sketch. You will see the outline of the sketch highlight in green. You can now immediately drag underdefined sketch geometry to resize the feature without the requirement of using Edit Sketch first.

Modify Sketches. Be very careful with this next use of Move/Size Features since it is difficult to reverse except with Undo. Select a face of an extrude feature. If you drag and drop one of the other two green sphere "handles" (either the one with four arrows or the one with two curved arrows) then you will invoke the Tools - Sketch Tools - Modify command. This allows you to move the sketch of the feature around freely, thus repositioning and/or reorienting the sketch origin.


Dynamic Sketch Editing. Saving the best for last here... If your Move/Size Features icon is active, then you can Edit Sketch immediately by double-clicking the sketch in the FeatureManager. While editing, you will see a golden preview of the feature that updates real-time as you make changes to the sketch.