Never include fasteners with modeled threads in your assemblies.

This is the reason the SolidWorks toolbox comes with three options for thread display when inserting fasteners into your assemblies: Simplified, Cosmetic, and Schematic.  The popular and recommended choice is ‘Cosmetic‘ – a healthy combination of detail and efficiency.

There are quite a few factors that can contribute to clunky and inefficient assembly models, but two very obvious culprits are the quantity/complexity of features and surfaces.  You can apply this concept to any type of model, but modeled threads are a perfect example to discuss both of these slow downs.  Though there are times when it makes sense to model threads within a part file, it’s rare that those threads are needed within an assembly file.

One of the coolest things about McMaster-Carr (besides their same day delivery of just about anything you can ever dream of) is that they offer 3D models of a majority of their products in a native SolidWorks file (i.e. feature tree, dimensions, and relations are included).  McMaster-Carr customers with SolidWorks have a huge advantage over the rest, because they’ll be able to quickly edit these files however they’d like.  Here’s an example…

• Download a 1” long ¼-20 SHCS from McMaster-Carr and notice that the part comes fully equipped with modeled threads.
• Click Tools > Feature Statistics and note the 0.80 second calculated rebuild time.
• Right mouse button (RMB) the “Cut-Sweep1” feature, and select “Configure Feature” from the menu.
• Create a “Simplified” configuration with the thread cut feature suppressed.

• Run the Feature Statistics tool one more time and you’ll see a 0.15 second rebuild time. Just by removing one feature, we managed to cut the rebuild time to less than a fifth of what it was.  This goes a very long way inside an assembly where many of these fasteners can exist.

Obviously, you can make “Simplified” configurations for any type of model (not just threaded fasteners).  You can suppress any type of feature that is not required to be present in the assembly (complex features, fillets, chamfers, etc.).  This is a great way to speed up large assembly performance.  All you have to do is activate the “Simplified” configuration of all the part files within an assembly.  “How?”, you might ask…

• Click File > Open within SolidWorks and browse to an assembly file.
• Before opening it, click the “Advanced” check box.
• When you click the “Open” button, select the following options on the pop-up menu.

Once you click OK, SolidWorks will find any part within the assembly (regardless of the levels of sub-assemblies) that has a “Simplified” configuration and activate it.  Simple (no pun intended)!  Why not create a simplified configuration for every part file?

Let’s start with the first part of that, “What is Instant3D”.  It lets you quickly create and modify geometry by using drag handles and scales.  You can use Instant3D in parts and assemblies.  To turn it on, select the “Features” toolbar and select “Instant3D” which is on the far right end of the toolbar.

The second part of the question, “Why would you want to use it” is a little more subjective.  If you need to change a dimension, you have the ability to just select the model face which will show the dimensions making it very quick to modify the model.

 This option is great when you are not “sure” of the design and you have some dimensions on the model.  The dimensions have a small blue dot at the end of the extension line which is what you left click and hold on.  Then a scale will show up that you can “drag-n-drop” on for your new dimensional value.

Another great way that you can use Instant3D is when you want to create an Extrude.  When you are done sketching and exit, select a segment of the sketch which will activate an arrow. 

This arrow will allow you to drag it away from the model, creating a boss extrude, or into the model creating an extrude cut.

This is just the basics of Instant3D.  I suggest you try it out and see how it can help you be more productive.

This is a really quick video demonstrating a basic workflow to create one part that closely references another part utilizing multi-body modeling techniques in SolidWorks 2011.  I created this video for a customer and figured I’d share it with the rest.  Some tips to pay attention to…

• Don’t judge me on the design, I wanted to keep it simple.  : )
• Ignore my non-use of the RMB (right mouse button) to exit commands.  I try not to use this shortcut in videos to keep things easier to follow.
• Leaving the ‘Break link to original part‘ check box in the ‘Insert Part’ command unchecked will allow changes made to the iPhone to propagate to my case design.
• I do not click in the graphics area to insert the part.  Instead, I simply click the green check mark to have it dropped precisely at the origin of the new part file (this works in assemblies too).
• I insert a ‘Weldment‘ feature so that my future part features do not automatically ‘Merge result’ and blend the solid bodies together.
• RMB’ing an edge and selecting ‘Select Tangency‘ can be a big time saver.
• A lot of times, people forget that you can shell outwards.
• When working with multi-body part files, always make sure to pay attention to the ‘Feature Scope‘ of your cut features.
• You can window select multiple corner points when using the ‘Sketch Fillet’ tool.  You can also drag the yellow preview to resize the radius.
• I could have added the 0.03125″ fillets more quickly by typing “1/32″ and by selecting the top face of the case and the cut face of the ‘Cut-Extrude2′ feature rather than selecting each individual edge.  Selecting a face will always apply a fillet to the face’s perimeter edges.
• In SolidWorks 2011 SP4, you can accelerate the PhotoView 360 preview rendering by scrubbing your mouse across the areas of interest.

• Multi-body sheet metal parts
• Multiple materials per part file
• Improved cut list organization
• Indented cut lists in BOMs
• Parametric move/copy bodies command
• Right click access to hide bodies in drawing views

With these enhancements (and plenty more), SolidWorks just converted the solid line between assemblies and multi-body part files into a construction line.  Think about it; nobody complains about using part files for weldments…  Why not everything else (from furniture to electronics)?  Rather than using multi-body part files exclusively for parts containing structural member features, what’s wrong with extrusions?  Revolves?  Sweeps?  Sheet Metal features?

Certainly, machine designers will stick with assemblies as they will need to take advantage of mates and degrees of freedom to allow for physical dynamics between all of their machine’s components.  However, any “assembly” that’s static now lends itself beautifully to multi-body part modeling.  Here are some of the benefits:

• Utilize all the in-context modeling techniques you can dream of without the hassle of external references!
• Simple file management – there’s just one file.
• No need to worry about defining parts’ locations via mates.
• Great for quick concept design as bodies can always be saved out to an assembly file with individual part files if need be (for drawing files or PDM purposes).  All you need to do is remember where they buried the “Save Bodies” command (Insert > Features > Save Bodies…).
• Show bodies in multiple positions using the parametric move/copy bodies command and control the distance/angle dimensions with a design table.  This method works great for controlling ‘open’ and ‘closed’ configurations of cabinet doors/drawers.
• Don’t forget, if you happen to have a library of commonly used part files, you can still use them in multi-body part files!  Just drag and drop them in as solid bodies and choose whether or not they should stay linked to the original library component.

Try it out.  I bet you could save a third of your design time by building a multi-body part file rather than an assembly file.

With the surface in the middle, you can thicken it and make it a solid.
This helps build in some “Design Intent” and intelligence into your model.

Anyways, if you haven’t seen it, just search “SolidWorks” on YouTube.  It’s called “Using the Wacom Cintiq with SolidWorks”, and it appears on the very first page of the search results!  Let it be a lesson to all that once you post a video to YouTube, there’s no further editing that can be done to that video (e.g. remove the intro!!).

Click here to view the embedded video.

…The first sketched line will produce unpredictable results because it passes over multiple surfaces.  The second sketch produces the 1.5mm measurement shown in the last image.