Favorite SolidWorks Trick

As Adam Heard said on 973, “What’s your favorite CAD trick?” or something to a similar effect. I actually don’t have one, but I’m curious to learn yours.

My favorite (Inventor) tool is the entire sheet metal system with it’s flanges and flat patterns.

I also just learned about the (Inventor) offset tool, which is really helpful in certain situations like pocketing.

Patterns. Pattern everything. Patterns in patterns. Patterns in patterns in patterns. Patterns of holes, patterns of everything. Favorite trick, favorite tool in Creo. One of the underclassmen asked me how I could CAD a drive train in 20 minutes: patterns.

Also center-rectangles and thin wall extrusions are great.

Generally, the newest thing I find that saves me time is my new favorite trick.

(I understand that these things might be old hat to a lot of people but we’re all at various points in our educations :P)

In my personal opinion patterns are one of the most powerful model/geometry creation tools in Creo-- learning how (and when) to use them and the limitations is probably a small book of knowledge.


I just found another great time saving thing. When doing sheet metal fillets (in inventor), you can select all of the corners in a specific feature by selecting choose by feature instead of choose by edge. Didn’t know about this until today and it’s going to save me a lot of time.

Probably not a “trick” but I like to use 3d sketches on Solidworks to create parts and structures very fast using the sheet metal tools. I also like that I can make my own “sheet metal” parts for other materials such as fiberglass angles and c channel.

In Solidworks if you want to select a bunch of sketch entities (like lines, circles, etc), if you click and draw a rectangle to the right it will only select things completely inside the rectangle selection and if you click and drag to the left it will select everything that is partially inside the rectangle selection.


I know this is basic, but projecting geometry in Inventor and the similar tool in Solidworks for asemblies.

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Design tables! Not only can you quickly toggle between various configurations of the same part but you have access to all the math tools of a spreadsheet and your critical dimensions in an easy to view area. You can really quickly and easily view and set relationships between dimensions across multiple sketches and features, and even drive a design with a quick and dirty GUI made in the spreadsheet.

It’s particularly a useful technique for stuff like gussets and brackets that you may need to frequently adapt and/or have a lot of common configurations of. Instead of a starting a whole new part file you just create a configuration with a row of dimensions inside a excel file.


Patterns, as stated. The loft tools are pretty obscure but useful for designing weird looking dog shifter dogs.

The thing I love about Solidworks is that you can get by with less than 12 functions, but learning the other functions saves time. So it’s good for anybody.

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Personally, I’m a fan of the Convert Entities tool. I use it when I want to copy a profile from the face of the three-dimensional object on which I’m sketching. It saves a lot of time when I need to offset sketch geometry.

My favorite inventor tricks:
The constrained orbit mode (found in the top right under the view cube)

Favorite inventor tools:
Rib tool (found under create in the 3D model tab)
Rule Fillet (found under plastic part in the 3D model tab)

I use the two tools above to make complex lightening patterns quickly without risk of the sketch exploding or my computer crashing. Maybe I should make a short video about it.

Getting to know the weldments tools is pretty clutch, even if you don’t plan on actually welding.

Making part libraries with materials and weights already assigned for common FRC parts saves a lot of time. Do it in the off-season to save hours during the build season.

Don’t waste time with chain patterns. It’s not robust enough yet.

Envelopes are useful to ensure you’re in your starting config/etc.

When using Solidworks I’ve found the following trick to be quite efficient.

Selecting the entities I want to make relationships between while holding the control key, releasing the control key, then moving my mouse towards the phantom menu that appears to the upper right of the mouse and then clicking the relation I want on the menu.

This instead of selecting multiple entities and choosing the relation on the Property Manager tab on the left.

Shift clicking on two faces/edges in an assembly and clicking enter will mate the components (coincident or concentric) without entering the mate menu.

When filleting with many edges, click the first edge and don’t move the mouse. A phantom menu appears with options to select all edges on the part based on various filters.

Use rollback mode to make features in parts while respecting the rebuild process. Helps avoid missing edges and holes when changing the part.

A clever use of split feature and cuts allows you to add tabs in perpendicular parts with only two features. Or wait until SW2018 for sheet metal to get tabs.

Parts with layout sketches can not be set to flexible. Don’t use layout sketches.

When doing dimensions across parts/assemblies, you can use smart dimension and click on another dimension to be automatically linked.

You can make a single hex shaft file for your entire robot assembly using configurations and multiple external references This is incredibly helpful for making drawings.

Parts can be made in an assembly and then have external references broken to make a top down approach without leaving an assembly.

You can design your entire robot in one part file. Not that you should but we did in 2017 and I finished that CAD much faster than 2018.

Assembly features that don’t cut all the targeted parts in the first feature will not show up when patterned despite the pattern intersecting those parts.

You can pattern components using pattern by sketch and then pattern the hole patterns using pattern by pattern. I used this to put holes for bearing blocks in the drive rails. This is mostly useless unless you’re doing machining work and don’t want to place thousands of holes manually.

Tab to hide a part. Shift tab to unhide.

I modeled our bellypan as a single solid body and then converted the body to sheet metal. I could specify the faces and bends and made and incredibly complex part very quickly.

Learn miter flange. Great for angled walls and weird shapes.

You can edit the sheet metal bend profile. Click the sketch under the feature or enter the feature and click edit profile.

You can use the fold/unfold features to add features on flat parts before flanges are added.

Saving faces as dxf creates a solidworks education stamp which your sponsor might not like. Use AutoCAD scripts to automatically edit this out.

You can change your dxf format settings to specify layers for holes and contours. Some sponsors compensate by layer automatically.

Make extrusion by using center rectangle and thin feature. Use the same approach of one part and configurations to keep all your extrusion to one part for ease of drawings.

I probably have a hundred more tips if you ask.


Disabling hyperthreading to increase SolidWorks performance.

The “S” keyboard shortcut brings up commonly used in-context tools right next to the cursor.


Multibody parts for anything and everything in a subsystem that doesn’t have relative motion. Everything in the system can be driven by a few sketches. Makes file management really easy and gives you a cut list that recognizes identical parts. Mirroring as virtual parts is really helpful for sheet metal stuff too so you don’t need a separate file for something that is cut the same but bends the opposite way.


Binding “m” to measure and “ctrl+m” to mate

Good 'ol relations. Equal, midpoint, tangent, concentric, parallel, co-linear, all find their uses in surprising ways.

This. A thousand times this.

Nobody seems to share my enthusiasm for the “S” key shortcut menu. I try to preach it to people, I show them how useful it is, but nobody ever uses it.

Any tool that anyone in this thread brings up (for SolidWorks) can most likely be added to this pop-up menu. It can be customized for parts, assemblies, drawings, and sketches. If you care about working efficiently in SolidWorks, this is for you

I have all of my commonly and semi-commonly-used tools and drop-downs on the shortcut menu and I’ve saved so much time. I don’t even know where the tools are in the main docked hotbars anymore because they’re just always right next to my mouse

Not a Solidworks thing but rather an Inventor thing:

Using the “Assemble” feature in assemblies to place parts into holes and other objects. I used to always use 2 to 3 mate/flush/concentric constraints to do the same process that Assemble does in one. I first learned it with fasteners, but I’ve been applying it more to other parts.

I also thought it was a neat trick on creating wires by drawing a 3D line using 2 planes to create the path and using the “Sweep” feature to create the bulk of the wire.