The best way to learn a software is to continually challenge yourself in new ways. To help aid that process, I’m going to begin posting some SOLIDWORKS obstacle courses for you to test your modeling skills on. The first challenge is to figure out the fastest way to remove all the holes from this imported (i.e. featureless) model. You can download the 2015 SOLIDWORKS model here to try it for yourself, or you can scroll down to find numerous answers below.
The reason challenges like this are so useful is because they force you to explore many possible solutions. The more you find, the more you’ll have at your disposal for future challenges. They’re all great options, but only one is the fastest (and fair).
FeatureWorks (20 seconds)
FeatureWorks (available in every seat of SOLIDWORKS Professional and Premium) is a tool used to automatically build a parametric feature tree for imported geometry. It’s often a useful way to manage and modify legacy CAD files that were originally modeled in another CAD application. In this case, we can use it to recognize the holes as features and then suppress them. Here’s how:
- Right click on the model > FeatureWorks > Recognize Features
- In the PropertyManager, uncheck all options under ‘Automatic Features’ except ‘Holes’
- Click ‘OK’
- Select the first hole feature in the FeatureManager
- Hold the SHIFT key while selecting the last hole to select all of the hole features
- Click the ‘Suppress’ icon in the top left corner of the context sensitive pop-up menu
Defeature (15 seconds)
Defeature is a tool used to eliminate the level of detail associated with your part or assembly model. Some purposes of the tool include creating an ultra-efficient version of your model to be used in assemblies, or to remove proprietary information from your model before you share it with your customers/vendors. In this case, we can use it to remove all the holes by following the steps below:
- Select Tools > Defeature (or search for it in the command search in the top right corner of your interface)
- Select at least two of the inside planar faces for the ‘Features to Keep’ selection box. Otherwise, the Defeature command will take it one step too far and fill the entire volume with solid material.
- Click the blue ‘Next’ arrow to view a preview of the resultant geometry
- Click the ‘Next’ button one more time
- Optional: You can save a copy of the simplified model
- Click ‘OK’
Power Select / Delete Face (10 seconds)
Power Select (available in every seat of SOLIDWORKS Professional and Premium) is a very convenient yet seldom-used tool. In fact, all of the alternative selection tools available on the selection drop-down list are very underrated and underused. In this case, the Power Select tool can be used to quickly select all of the cylindrical faces (or, if they weren’t perfectly cylindrical, all of the non-planar surfaces).
Delete Face is a simple surfacing command that is the secret behind many solid modeling tricks. In this case, you can delete all of the pre-selected cylindrical faces and patch over them in one swift command. Here’s how:
- Activate ‘Power Select’ from the selection drop-down menu
- Select ‘Faces’ in the ‘Select what’ section of the Power Select’s Task Pane tab
- Select ‘Surface type’ in the ‘Filters and parameters’ section
- Select ‘Cylinder’ below that
- Click the ‘Search’ button to make the selection
- Click the ‘Close’ button to accept it
- Activate the ‘Delete Face’ command on the ‘Surfaces’ tab of the CommandManager
- Select the ‘Delete and Patch’ mode
- Click ‘OK’
Cheating (5 seconds)
With any competition, you always have to keep an eye out for cheaters. In this case, sneakily prepping the model by adding a Selection Set could be a major competitive advantage. Selection Sets (new in SOLIDWORKS 2015) are used to save common selections of all types of geometry for repeated future use. In this case, here’s how you can beat everyone else in your office with this challenge:
- Expand the ‘Selection Sets’ folder at the top of the FeatureManager Design Tree
- Select the ‘All Hole Faces’ selection set
- Run the ‘Delete Face’ command in ‘Delete and Patch’ mode (If you made a bet, add the ‘Delete Face’ and the ‘OK’ commands as Mouse Gestures for super-fast access)
I’m sure there are many more creative ways to conquer this challenge in SOLIDWORKS. If you discover them, please share your comments below!