SOLIDWORKS Lightweight Mode [VIDEO]

Article by Jim Peltier, CSWE updated November 4, 2013


Greetings, fellow SOLIDWORKS users! I’m here to help clear up some of the ambiguity of SOLIDWORKS Lightweight Mode that causes many users to shy away from using it. I myself used to be guilty of this because the first thing I would do after opening an assembly involved “Set Lightweight to Resolved.” Like many SOLIDWORKS users, I had been duped by the FUD regarding it. It certainly isn’t helped by what the help file says about it:

When a component is lightweight, only a subset of its model data is loaded in memory. The remaining model data is loaded on an as-needed basis.

What exactly is in this “subset of model data,” anyways? I decided to put it to the test this week and see what I could do and what I couldn’t.

Firstly, and most importantly, it loads the part model geometry as is appeared at the last save of the part. This was independent of whether the assembly was open during the last save or not, which was myth #1 cleared up. However, I recall having holes not lined up properly even after a rebuild when I used SOLIDWORKS Lightweight Mode in the past. I decided to test this behaviour next. Since it’s difficult to explain, I made this video demonstrating the problem (and a solution):


And this limitation makes perfect sense. SolidWorks isn’t loading the feature tree for the parts, so it does not notice that my Cut-Extrude has an external reference (indicated by the -> on the sketch). Because it doesn’t load the feature tree, it just loads the geometry, which means it will not update when I move the propane tank. The fact that it moved when I used an assembly-level feature makes sense, since the assembly-level features are shown regardless of lightweight status. This is perhaps the best argument in favour of assembly-level features!

Of course, don’t get carried away with this. Assembly-level features have their own quirks and are by no means the solution to every SOLIDWORKS modeling challenge. However, in this instance it provided a fix to my lightweight problem. I also forgot to select Propagate feature to parts, which would have shown me the cutout when I had just the Base Shelf open. Not choosing that option would only show it at the assembly level (useful if I want to cut this after my BBQ is assembled). This is fairly typical of what happens when I try to build an actual BBQ in real life.

As I had mentioned, parts loaded in SOLIDWORKS lightweight mode come in with the geometry as it was last saved, but does not load the feature tree. This helps speed up rebuild time and load time, which is why lightweight mode is largely beneficial. While a component is in lightweight mode, it is effectively a “dumb solid,” which is a term used to describe geometry in SOLIDWORKS that *cannot be modified due to a lack of features, such as an imported file. (*Dumb solids can actually be modified with a little persistence). Anything that you can do to a dumb solid at the assembly level (section view, apply mates) can be done to a lightweight component.

You can still run many of the tools on the Evaluate toolbar while in Lightweight mode: Interference Detection, Measure, Mass Properties, Section Properties, Assembly Xpert, and Clearance Verification. However, there are some that will not run or will nor run correctly with Lightweight components: Hole Alignment, Assembly Visualization, Curvature, and Symmetry Check.

It’s also worth mentioning the other modes that exist for opening an assembly: Large Assembly Mode and Large Design Review. Large Assembly Mode will override your Large Assembly threshold as defined in your settings (Tools > Options, System Options tab, Assemblies from the list on the left) and just open the assembly in Large Assembly Mode. Large Design Review opens the assembly’s geometry as it was last saved within the assembly. In terms of functionality, it’s more like an eDrawing than a SolidWorks assembly (you can see the parts, the geometry, take measurements, hide parts, create a section view). The obvious advantage is that it opens really, really fast. A less-obvious advantage is that if someone sends you only the .SLDASM file without any of the parts and you just want to see what the assembly looks like, you can open it using this method and see the assembly.

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Jim Peltier, CSWE

Jim has been using SolidWorks since 2001, and has spent most of that time working in the design of industrial automated manufacturing equipment. He has been working as an Applications Expert at Javelin Technologies in Oakville, Ontario since July 2012 and is a Certified SolidWorks Expert (CSWE).