SolidWorks Tips You May Have Never Seen Before!

Move Sketches… EASILY

These features are presented in no particular order, but I do consider this one of the most hidden yet easy to use tools when you are unsatisfied with the location of your sketches relative to the origin or anything else.

Moving Sketches while in Edit Sketch mode is not always the easiest task, ESPECIALLY when they are Under Defined Sketches or those that are Copy/Pasted from DraftSight or other 2D applications.

Where most users run into trouble is that they feel, and I don’t disagree, that you should just be able to window select all the sketch entities and then just grab a point and drag the whole group. While this sounds logical, it has simply never been the case.

Then you could try the Move Entities command, but it doesn’t always snap to the final location as you might expect.

The following technique is completely effective and very easy to do, you just have to know the sequencing of the clicks.

First, Window select the sketch entities you wish to move.

Second, hold the CTRL key on your keyboard then Pick and Drag the selected entities from one of the points in the sketch.

CAREFUL NOW… The trick here is that a CTRL + Pick and Drag in Windows is a Copy… and that is ‘initially true’ here too. Note the Cursor with the little (+) next to it. If you let go of the Left Mouse Button FIRST, you will COPY the Sketch.

Instead, while in the middle of the ‘Copy Sketch’ operation, release the CTRL KEY while still holding your Cursor. The little (+) goes away and the entire operation turns into a MOVE command.

Simply snap and release your cursor when your selected point is in the proper location, or snapped to the origin.

In summary, of the thousands of functions in the millions of lines of SolidWorks code, these are some of the more useful yet somewhat hidden functions I use frequently. I hope that you found something you didn’t know about that helps you improve your quality of designs, but most importantly saves you time and effort during your creative process.

Copy Surfaces

Copying a surface from one part to another is a very useful tool when you want to build In Context relationships between parts, especially when you get an unruly imported file with thousands of surfaces… .but you only need to ‘touch’ just a few.

I also use it for operations where I may want to simulate a Coating or Tape application on a part. Just Copy the Surface and Thicken it as a new Body.

What you may be asking yourself is: “That sounds great, Darin, but there is NO ‘Copy Surface’ Command”… .and you’d be absolutely CORRECT!

Many users try to use the KNIT SURFACE command, but this doesn’t work unless the faces you select are adjacent to each other and can form a single, ‘knitted’ surface.

However, there is a simple trick to this one, and it lies in the OFFSET SURFACE COMMAND.

Pick a face or faces, adjacent or disjointed, and select OFFSET SURFACES from the Surfaces Tab.

It will show the selection, and the title in the Property Manager will state “Offset Surface” until you set the distance to ZERO. Then the title changes to COPY SURFACE. That’s it!

You can use this in context of an assembly, and while editing a part you can select faces of other parts and Copy the Surfaces. This will create Associative Surfaces in the part you are editing.

This tool really has dozens of use cases.

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