Virtual parts are awesome. You can create hundreds of these models without creating a single file. You can dramatically improve your designing speed by skipping some of administrative tasks involved with storing files.
Just make sure you are aware of the trade-offs.
Virtual parts are parts that you can quickly add, edit and delete without much hassle. You don’t need to come up with a name for them. They are quite content with their assigned name Part1^assembly12.
You can only use virtual parts in assemblies. You create a new one by selecting Insert > Component > New Part or by clicking these buttons in the Command Manager:
SolidWorks will now prompt you for a reference plane, without really telling you. The plane you select will coincide with the Front Plane of the new part. I want the front plane of my assembly to represent the frontal view of the machine that I am designing. That is why I carefully choose my front plane orientation when creating every single part of a large machine. By giving it a few seconds of thought right now, the assembly will snap together quickly later on.
After the selection of the front plane location, SOLIDWORKS will go into ‘Edit Component’ mode and it will start a new sketch on the Front Plane. It will also add a mate. The type of mate depends on what buttons you click in what order. More on that below.
When you add virtual parts to an assembly, SOLIDWORKS will help you fixing them in space. You can create three types of mating schemes:
This is default behavior, SOLIDWORKS fixes the part until you give it a better option. If you abort the process of assigning the front plane, the fixed relation remains. It’s not really a mate though.
This happens when you have selected the option ‘No External References’ in the Sketch toolbar before creating the new virtual part. Note that this option is only available in Edit Component mode. That means you might have to go into that menu once just to make sure your next virtual part will be created without mates.
No mates are added whatsoever when you disable external references, so the part can freely float in space. In previous SOLIDWORKS versions, a fixed icon (f) will appear before the new part’s name when editing the first sketch. That icon disappears after you exit that sketch and return to the assembly.
You have apparently not selected the option No External References before creating the virtual part. An InPlace mate will automatically replace the fixed relation when you select a front plane. That plane can either be a plane in the assembly or a face of another part.
InPlace mates are special mates for virtual parts and they appear in very few situations. They lock your part in place with regards to another part or assembly and you cannot edit them. You can only delete them and and replace them with a set of proper mates. I advise you to do just that, don’t leave them lingering around in your assembly.
You don’t have full control of the storage location of virtual parts. SOLIDWORKS will save the current version in a temporary folder somewhere on your pc. You only truly save your design when you save the assembly that contains the virtual part. When you close the assembly, you will close all virtual parts from that assembly automatically.
That is because virtual parts are saved inside the assembly in which they are created. When you save the assembly, SOLIDWORKS will save all virtual parts internally and the files in the temporary folder are deleted. You can check the references for a part (File > Find References) and it will show <save internal to assembly>.
The name of virtual parts can be edited in the tree by selecting the part and pressing F2 or by slowly double clicking the part name. As long as they are virtual, the suffix of a power sign (^) and the assembly name will appear in the part name.
Virtual parts are perfect in the concept phase of a design process. That’s the time where you create (I wouldn’t call it ‘design’ just yet) hundreds of parts, where probably 95 of them won’t make it into the final design. Using virtual parts instead of real parts will relieve you of having to save all parts using an unique file name (or a number if you’re doing things properly). You also won’t clog up your file system or PDM system with files that you will never use again.
You can also create perfect moving models for purchase parts. You only need to save one assembly file for a complete pneumatic actuator that consists of multiple parts. All that you need is an assembly, a few virtual parts plus a few mates.
There are a few caveats though. Product Data Management (PDM) systems are usually unable to see individual virtual parts, they just see the assembly. That means the parts might not appear on your bill of materials, and they are invisible when you use PDM functions like finding references.
You can not make drawings of virtual parts. If you really want to, you have to save them as an actual file first. I think this makes sense, since you should only use them in the first phases of the design process or for moving standard parts.
You can save a virtual part when you have it opened, but this doesn’t actually do a lot. Only when you save the assembly is when the parts will get saved (I just checked to make sure). This doesn’t make a lot of sense and I’ve seen it cause a lot of frustration. You can lose a lot of work when SOLIDWORKS crashes and you haven’t regularly saved the assembly.
I have also seen cases were virtual parts were somehow not saved properly. Somehow changes just disappeared when reopening the assembly. We had no idea what happened here, we’ve just seen it happen a few times.
When you add a standard part (that is, a part with a file name) to an assembly, you can turn it into a virtual part by right clicking it (in the tree or in the modeling area) and selecting Make Virtual.
Going the opposite route is something you have to do for all of remaining parts eventually. You can do this by right clicking the part and selecting Save Part(in External File).
So, virtual parts. Do you hate them or do you love them? They have some real advantages for quickly mocking up designs, just as paths do (check out our blog post on paths here). I think virtual parts are perfect for modeling purchase assemblies while keeping them in a single file.
If you trained your fingers to press Ctrl-S every minute without you even noticing, you lower the risk of losing work substantially. If you don’t do that, you risk a little more when the program crashes.
All in all, I think virtual parts are a great feature. I save a few clicks for every parts, which saves me hundreds of clicks per day, and I don’t have to name every single shaft and plate. No more inspirationless part names.
Speaking of inspiration, allow me to make a small sidestep. How awesome would it be if you could see your mechanical design right in front of you in real 3D? Augmented reality and virtual reality glasses like the HTC Vive will make that possible, hopefully within a few short years. When motion tracking with a simple desk device like made by Leap Motion becomes fully supported by major CAD packages, I’m in. I’m still considering buying a Leap motion controller, because tracking the movement of your hands can do a bunch of great things for CAD software. Just take a look at what they can do already in this video: