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How to SHIFT More CTRL to the SOLIDWORKS User (using CTRL, SHIFT and ALT keys)

Article by Jim Peltier, CSWE created/updated March 5, 2014

Man using a SolidWorks keyboard

SolidWorks Keyboard Control

Greetings, fellow SolidWorks users. A question we are sometimes asked is for a comprehensive list of all the things that Ctrl, Alt, and Shift keys are used for in SolidWorks, since this isn’t exactly documented in the shortcut keys.

CTRL

  • Ctrl+Drag: You can use this to copy in many situations. In sketch mode, you can copy a sketch entity. In part mode, you can use it to copy a feature. In assembly mode, you can use it to copy a part. You can also copy a sub-assembly if you use the Feature Tree. In a drawing you can copy a view to the same sheet or another sheet if you use the tree.
  • Ctrl+Drag (middle mouse button): You can use this to pan in any mode. Ctrl+arrow keys work for this as well.
  • Ctrl+Click: This will allow multiple selections. I mention this one because it is so important in SolidWorks to be able to select multiple things (entities, geometry, parts, etc)
  • Ctrl+Q: This is the Force Rebuild command. You will find it nowhere on the toolbars, nor in the menus, nor in the command manager, nor in the Customize tab, but it is very important. This command rebuilds everything in the feature tree, making it more powerful than the standard Rebuild (Ctrl+B).
  • Ctrl+B: This is the default Rebuild command (can be changed). This will rebuild only features that have changed since the last rebuild. Long-time SolidWorks users may remember when the default hotkey for this was R. Be warned that there may be unseen errors in your part that will not be rebuilt or seen using this method (see Ctrl+Q above)
  • If you hold down Ctrl while sketching, it won’t add the automatic sketch relations that it typically would (a temporary workaround to disabling “Automatic Relations” under Tools > Options, then under the System Options tab, select Relations/Snaps from the list on the left).
  • Ctrl+Spacebar: Activates the View Selector regardless of the setting when you only press Spacebar.
  • Ctrl+Tab: Switch between open documents. Works in other Windows programs as well.
  • Ctrl+C and Ctrl+V: Copy and Paste respectively (not unique to SolidWorks). In a sketch, you can copy entities using this method or the Ctrl+Drag mentioned earlier. In part mode, you can copy a sketch (does not work with the Ctrl+Drag method). In a drawing, you can enjoy greater control over where you place your view if you use this method over Ctrl+Drag. In an assembly, you need to select a part/assembly from the tree to copy it, but it still works. Another really cool thing you can do in an assembly with this is that you can select a part’s feature from the tree, do a Ctrl+C and Ctrl+V to make a copy of the same feature as an assembly-level feature!

SHIFT

  • Shift+Drag: In a part, you can do this to a feature to move it (great for fillets or moving a feature from one face to another). In a drawing, this will move projected views along with the view you have selected together, as though they are one view. Also in a drawing, you can move a dimension to a different view.
  • Shift+Drag (middle mouse button): Zooms in and out smoothly. When zooming in, it zooms in to the centre of the screen.
  • Shift+Arrow Keys: Rotates your view 90°, regardless of what your view rotation setting is for your arrow keys (Tools > Options, under the System Options tab select View from the list on the left and adjust the Arrow Keys field in the View Rotation pane). Works in part, assembly and sketch modes.
  • Shift+Click: In a feature tree this will select everything between two selected items. When applying dimensions to an arc or circle, it will snap the dimension to the max or min position depending on where you select the arc or circle. When selecting parts in the graphics area, it allows multiple selections (same as Ctrl).
  • Shift+Click: When sketching, it will temporarily enable Snap To Grid (otherwise accessible via Tools > Options, under the System Options tab select Relations/Snaps from the list on left and check the Grid option), but it does it in a much more intuitive way.

ALT

  • Alt+Drag: In an assembly, this activates the Smart Mates command (mentioned in this blog article). When making an exploded view, you can Alt+drag the little ball in the triad and drop it onto a planar, cylindrical, or conical face or circular edge to get it to align to that face or axis.
  • Alt+Drag: In a drawing, you can move a view without having to hover over the edge of the drawing view first. Same thing with a table
  • Alt+Drag: In a sketch, you can adjust both handles of a control point of a spline in a symmetric manner.
  • Alt+Drag (middle mouse button): Rotates the view in a plane which is parallel with the viewing plane. Alt+arrow keys does this as well.
  • Alt+Scrollwheel: When you have the magnifying glass (default hotkey G) active, this will enable a section view which is parallel with your viewing plane. This allows you to see inside a part within a magnified region.
  • Alt+Click: While in the View Selector, pressing Alt will allow you to select back faces of the virtual cube shape.
  • Alt+Click: When placing a dimension or annotation in a drawing mode, this will temporarily disable alignment with other dimensions/annotations.
  • Alt+0176 on numberpad: Makes a ° symbol. Also Alt+0216 makes Ø, Alt+0177 makes ±, Alt+0181 makes µ. These are standard Windows Alt Characters. You can find them listed in the bottom corner of Windows Character Map, but I’ve listed the ones you are most likely to use in SolidWorks (they also work if you’re typing an e-mail).

Of course, SolidWorks is always adding more and more of these each year and this is by no means a complete list.

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Jim Peltier, CSWE

Jim has been using SolidWorks since 2001, and has spent most of that time working in the design of industrial automated manufacturing equipment. He has been working as an Applications Expert at Javelin Technologies in Oakville, Ontario since July 2012 and is a Certified SolidWorks Expert (CSWE).

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