Love or hate it sketching is the foundation for most of your models within Solidworks (and really any parametric 3D modeler). How efficient you are at Solidworks Sketching can impact your overall modeling performance. Having a bad sketch is like building a house on a poor foundation… your house will start off ok, but something bad is bound to happen.

I can’t stress enough that regardless of the modeling software you are using, you should always follow the golden KISS rule… Keep It Simple Stupid Silly! The moment your sketch becomes work, you’ve made it waaaaayyyy too complicated. Don’t try to do it all within one sketch… keep it to one sketch per feature. Stability comes before size… add relationships before dimensions. Leave fillets & chamfers to where they belong… as features NOT in the sketch!

As you are learning software, you are bound to pick up tips, tricks, suggestions, and other goodies from a wide variety of sources. The trick is to keep an open mind and never stop learning. The absolute worse thing to do is assume that even after years of using Solidworks there is nothing left for you to learn. I’m going to share some tips & tricks I’ve picked up in regards to sketching in Solidworks. Where did I get these from? Social media, reading the help (yes really), using other training material,  youtube, and watching others.

Solidworks Sketching Tips

To quickly define a sketch plane normal to an edge, select the edge and start the sketch feature (#1). Solidworks defines a sketch plane normal to the selected with the origin coincident to the end of the edge. All this in one simple operation

Solidworks is not the first modeling system I learned. One of the first things that I learned (and really have grown to appreciate) is that you can initiate the desired sketch feature (Extrude, revolve, etc) and if no sketch exists it will prompt for the sketching plane and put you into full out sketching mode (#2). Once you complete the sketch and exit the sketch environment it resumes with the sketch feature operation.

Ctrl + 8 is the shortcut for Normal To (#3), my favorite zoom tool for working with sketches. By using Normal To the view is rotated so that you are looking directly at the select object (sketch) making sketches much easier. Normal To is also available in the Standard Views toolbar.

Solidworks Normal To Button Location

Trim is fine, but I need more power! With the Trim feature active, drag across the segments you want removed and they are trimmed back to the nearest boundary (#3). If you hold shift while dragging it extends opposed to trim (#4). While in trim, drag an endpoint to extend the object (#5)

I’m a big fan of using splitting over trimming. Trimming objects tends to remove relationships, but with split I still get the desired profile, but don’t lose the relationships. Split Entities (#6) is not shown by default, so the quickest way to access it is doing a Command Search. You can always drag-and-drop it onto the ribbon if you want easier access in the future.

Solidworks Sketch Search Split Entities

Mirror is a feature that creates mirrored copies of selected objects as well as applying symmetrical relationships so the copied objects remain in symmetry with the original.  To dynamically mirror objects as you create them enable Dynamic Mirror (#7) from the Tools menu

Solidworks Dynamic Mirror Menu Location

SWx Dynamic Mirror3

With colinear lines, delete the coincident point between the lines to auto-merge the objects into one (#8).

SWx Sketch Merge Two Lines

After exiting the sketch, right-click on it within the Feature Manager and select Sketch Color (#9). With this, you can change the color of the sketch, beneficial when you have multiple sketches (unconsumed) within the model.

Rapid Fire (#10)….

  • When sketching lines click-and-drag with the left mouse button to create a single line. If entering size information double-click after picking the second point to end the line command
  • While in the line command, click-and-drag off a circle to generate a tangent line
  • While in the line command click-and-hold on the circle to make the quadrants appear. Move the cursor to the quadrant point and release to snap to the point.
  • Press A to cycle through the active sketch tool’s styles, for example, Circle to Perimeter Circle, or switch to Arc while drawing lines… beats going all the way over the side of the screen!
  • To move an object hold Ctrl as you start to drag the object, to Copy the object hold Ctrl throughout the dragging process
  • Done sketching? Double-click in the graphics window to exit the sketch

Automatic Relations (#11)

Having the system automatically detect and apply relations is not always a good thing, especially when it happens when you didn’t want it!

  • When you need to create geometry at “shallow” angles, say close to horizontal or vertical over-exaggerate the line so there is no chance of the horizontal or vertical being applied. You can always dimension the angle after.
  • When an endpoint destination is too close to an existing endpoint or midpoint adjust the object past the desired location and use Trim. By trimming a line, a coincident constraint is automatically applied
  • Hold Ctrl… this disables the relationship inference. When you release Ctrl Solidworks goes back to inferring relationships.

 

 

 

Feature Image 2013-0224 sketch 02