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 prefer 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.
You can turn a standard part (that is, a part with a file name) into a virtual part.
Just right click it (in the tree or in the modeling area) and select Make Virtual.
You might use virtual parts in the concept phase. In the next phase, you will have to convert all virtual models to normal files.
You can do this by right clicking the part/assembly and selecting Save Part(in External File).
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. You cannot edit InPlace mates. 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.
When you save the assembly, the virtual models are stored inside the assembly. SOLIDWORKS will also delete the files in the temporary folder.
When you close the assembly, you will close all virtual parts as well.
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.
You can check the references for a part (File > Find References) and it will show <save internal to assembly>.
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, the virtual 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.
Virtual parts are perfect in the concept phase of a design process.
That is when you create (I wouldn’t call it ‘design’ just yet) hundreds of parts and 95% of them won’t make it into the final design.
Using virtual parts instead of real parts will saves you from 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 create perfect moving assemblies, like pneumatic or hydraulic actuators, using virtual parts.
Now you only need a single assembly file.
Just create an assembly, add a virtual parts and a few mates.
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.
Virtual models can be used in assembly drawings. The components also show up in a BOM.
You cannot make a drawing for a single virtual part or assembly. This popup will tell you:
If you really want to make a drawing of a virtual model, 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.
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 also think they 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 substantially lower the risk of losing work. 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 while doing mock-ups. 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: