As an experienced SOLIDWORKS user, I know sometimes there are frustrating situations throughout my design process. I have found myself making up excuses or justifications when including explode lines to my explored view; have been unable to mate two sets of holes that are not perfectly concentric and have questioned why my assemblies are slow. If like me, you’ve found yourself in any of these situations, then this blog article is for you. I will share with you some of my favorite features from SOLIDWORKS 2018 onward that have helped increase my productivity. These features will allow you to retire your clever workarounds for workflows you might use daily or during specific phases of your projects.
Smart Explode Lines
Most users refrain from the extra step of adding explode lines because it tends to be unpleasantly tedious (unless you’re hourly).
Smart Explode Lines alleviate the dread of being tasked to include explode lines to exploded views. With as few as two clicks, you can completely populate your existing exploded view with Smart Explode Lines. These lines trace the exploded component’s complete path (even paths defined across multiple explode steps).
The property manager of the Smart Explode Lines tool allows you to:
- Easily include or exclude components assigned to explode steps
- Locate how the Smart Explode Line attaches to your component through:
- Bounding Box Center
- Component Origin
- Selected Point
Any changes made to the Smart Explode Line reference point of one instance of a component reveals a button to Apply to all component instances. This allows you to easily propagate this change to all other exploded copies of the same configuration of this component.
But wait, there’s more! These Smart Explode Lines will also accurately update when you make changes to the paths of components in your exploded view.
Selecting Over Geometry
The Select over Geometry tool lets you drag a box or lasso over a model without needing to start the drag from a blank region of the graphics area.
This feature is helpful when you cannot start the first click of a selection drag from a blank region in the graphics area. Use Select over Geometry when the model fills the graphics area or when unwanted items would be included in the selection. Now you can drag a box or lasso around components without having to juggle the hide/show settings of larger components filling the view in the background.
There are three ways to activate this feature:
- Click on Select over Geometry from the Selection tool drop-down
- Click on Tools > Select over Geometry
- Press and release the letter T
Some quick tips while Select over Geometry is active:
- Did you drag a selection box/lasso around the wrong components? No problem! Drag a box/lasso to clear the current selection and simultaneously select different items
- Shift + drag a new box/lasso to add items to the current selection
If you have components with two holes, you can use two sets of concentric mates to align those components even when the holes are not the same distance apart.
This capability is incredibly useful when one or both components are not easily available for editing.
|Source for these images: SOLIDWORKS Portal||
In the images above, apply a concentric mate to one set of holes (as per usual). After Ctrl-Selecting the second pair of cylindrical faces, when you click on the Concentric Mate type you’ll notice the Misaligned option will appear in a second row of the Mate Context Toolbar popup. Click on the Misaligned button to the left of the text Align Linked mate to apply the Misaligned mate type.
Your mate folder will look like this:
The two sets of holes will be nested under a single misaligned mate in the Mates folder. Editing one of the mates will reveal options to control which sets of holes will be truly concentric or to split the misalignment difference symmetrically between both sets. This is also where you can find the value of the maximum deviation.
You can enable or disable the creation of misaligned mates:
- Tools > Options > System Options > Assemblies > Allow creation of misaligned mates
You can set a document property for defining maximum deviation allowed and the misalignment preferences for either leaving the first set of concentric faces truly concentric, leaving the second set of concentric faces truly concentric or distribute the misalignment symmetrically between both sets:
- Tools > Options > Document Properties > Mates
Tab and Slot
A costly part of the manufacturing process is creating fixtures. This might encourage designers to manually create self-fixturing design features to reduce assembly and set up costs in the manufacturing process.
The new Tab and Slot feature allows designers to incorporate fully associative alignment and fit features for easier, quicker and more accurate fabrication. This tool would see immediate application for sheet metal and weldments users, but it is not limited to bodies created with these tools. Tab and Slot features can be used on a single solid body (a sheet rolled into a tube), multi-bodies and in the Edit Component mode in an assembly.
The Tab and Slot feature creates tabs on one body and slots (holes) on another body to interlock the two bodies. You can specify how the tabs and slots look and how they are distributed along the selected entities.
These features can be utilized in productivity features like Linear Pattern, Circular Pattern and Mirror.
Tab and Slot enhancements in SOLIDWORKS 2019 include:
- Group linking (like structural members)
- Apply tabs to circular edges
- Slot corner shapes (sharp, filleted, chamfered or circular corners)
- Controlling the slot length and width for desired clearances
- Control whether the slot will be a through-all cut or not
The only Tab and Slot enhancement included in SOLIDWORKS 2020 is allowing negative values for defining Slot Length Offset and Slot Width Offset.
Assembly Visualization Enhancement: Performance Analysis
We seem to be addicted to creating large assemblies but vehemently dislike the corresponding hit to performance. There is no universal “make it faster” button (yet), but SOLIDWORKS is making it easier for you to identify the culprits bogging down your assemblies.
Assembly Visualization (on your Evaluate tab) was introduced in SOLIDWORKS 2010. This tool allows you to map customizable identification colors onto your assembly for properties found in the Mass Properties tool, Custom Properties and even file properties.
The Performance Analysis button in this tool grants you single-click access to a set of predefined columns to help troubleshoot your assembly performance. You can view the open and rebuild times for the components and the total number of graphics triangles for all instances of components. With these components now identified, you can dig further to make your engineering and design judgement to whether you’re willing to accept the computational load of complex features or models in your top-level assembly.
The assembly above is sorted by the SOLIDWORKS-Rebuild Time column as noted by the downward arrow under the column title with customized colors.
I hope the enhancements to these features help you have a better and faster design experience. Some users are incredibly proud (and very good) at their workarounds. SOLIDWORKS 2018 enhancements to pre-existing tools and new features allows your mental bandwidth to be used for more designing and less “MacGyver-ing”.
Ready to explore more of the features in SOLIDWORKS 2018? Head over to our blog, where we provide a summary of each one of these features and guide you through them.