“Did You Know…” Tips and Tricks I Learned at SolidWorks World 2015 – part 2

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Below are all the Tips and Tricks I picked up on during the Technical Training Sessions day 2 of SolidWorks World.

On Tuesday I attended:

  • “The World Is Still Flat: Everything You Need to Know About Drawing Views” presented by Rachel Diane York of Fisher Unitech
  • “An Introduction to SOLIDWORKS Industrial Conceptual” presented by Justin Burton (and about a dozen helpers) of SolidWorks. (I won’t list any tips here, since this is an entirely new product.)
  • “Introduction to SolidWorks MBD” presented by Steve Ostrovsky of TPM.

 Did you know…

  • You can insert a drawing view in a non-standard orientation without creating a new orientation view. Go to Insert >> Drawing view >> Relative to model to creating a drawing view based on faces. This command isn’t on the CommandManager by default, so it’s easy to miss.
  • You can toggle the Lock View Focus setting through the right-click menu or by double clicking on an empty space within a view. When the view focus is locked, any new items (sketch entities, annotations, etc.) are attached to that drawing view.
  • When adding projected views, you can hold Ctrl to break the automatic alignment.
  • If you have an auxiliary drawing view that’s tilted at an angle, you can right click on it and select Align drawing view. Your view will be nice and level, and a rotation label will automatically be applied.
  • You can dimension to break lines in drawings, so that the break always stays in the same place, even if the part changes shape. The dimensions are then automatically hidden.
  • To use a non-circular detail view profile, sketch your desired shape first, then activate the Detail View command. Choose any profile style other than “Per Standard” and then select “Profile” to use the sketched shape.

  • The broken-out section view is very tricky. After clicking the button, the only feedback you’ll get is a Spline symbol next to your cursor (which you won’t be able to see if you’re still hovering over the CommandManager). Draw a spline around your desired area. As soon as you close the spline by clicking on the first point again, the Broken-out Section View Property Manager appears.
  • To create a broken-out section view up to the center of a hole or other feature, click on that feature in a projected or parent view. Activate the preview to see the position of the section line.
  • Hit the “A” key to toggle between the various versions of a sketch entity (such as Corner Rectangle, Center Rectangle, 3-Point Rectangle, etc.)


Did you know…

  • In some instances, moving to a Model-Based Definition environment paid for itself within a year by reducing paper costs by almost $5000.
  • Even if you don’t have the SolidWorks MBD package, using DimXpert dimensions is a huge step in the right direction. It keeps your 2D and 3D data in sync, makes drawing creation much easier, and will make the move to MBD a snap in the future.
  • If you use DimXpert dimensions, and keep them orderly in the part, you can make 2D drawings in just a few seconds by choosing “Import DimXpert Annotations” from the View Palette.
  • When using DimXpert, press the tilde (~) key to quickly move selected dimensions to a different annotation view.
  • The best way to use DimXpert is to use the Auto Dimension Scheme command on a few features at a time.
  • The Geometric Tolerance properties are smart when using DimXpert, but dumb in 2D drawings. For example, trying to add two parallel datums, or using the same datum twice for a GD&T feature will result in an error.

  • When using MBD, specific 3D views can be saved to your part and assembly templates, making view creating that much faster. (For example, a plain isometric view, a view with all dimensions, or a view with notes.
  • If you’re concerned that your partners aren’t ready for MBD, don’t worry. 3D PDFs can be printed just like a regular drawing, so vendors who still need 2D/paper drawings can use your MBD output (apparently GE Power does this).
  • MBD was just released last week, on 2/12/15.

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