Virtual component why?
Virtual components were introduced with V17 to help designers give a good start to their design.
Like many human being when something is simple it must be good. This is the first assumption that will lead many designers to disaster or at least complicate their lives. This is also this assuption that will make them ignore good practices or usefull features.
Many of you who find 3D modeling easier/faster than making 2D sketches, have the bad habit to start modeling in 3D right at the beginning of a project. In many cases this is OK. BUT in others many cases, this is not the best approach.
Often these lead designers to paint themselves in the corner. It also leads to bad product structure and other problems along the way. And worst of them bad decisions that found their way to production where we ask to find solutions.
Virtual component when introduce wisely, they will help you plan and manage your product design at the DNA level🙂
The cycle of a virtual component start with a 2D representation
«….A sketch that is used to define the 2-D geometry for a pre-defined component in a virtual assembly. You create component sketches using the Component Sketch command in a part, sheet metal, or assembly document. You can create the graphics manually by drawing lines, arcs, circles, and so forth, or you can create a 2-D image from the 3-D model using the Component Image command. You can also use a combination of graphics that you create manually and graphics created with the Component Image command….»
From a traditional part environment, from the «Home» tab under the «Sketch» group you will find «Component sketch».
From there you will have access to «Tool» tab where «Virtual» group could be found. You will be able to start the «Component Image» command
At the part level there is not much work to do; SE will recognize the shape and create the virtual representation in the plane you specify. Once accept the image will be place in the pathfinder has a sketch.
Virtual image cannot be locate has it is a snap shot of the part when look at a certain point of view. It is meant to be light weight and to be use when a concept is layout, therefore no precision is need.
If you would like to place elements that can be locate. Simply draw geometry or use the «Project» command (include). From those elements you will be able to precisely place virtual component in a layout.
For assembly same technique is use. SE will recognize visible part to extract the visual image. Part can be select manually to create the image. Geometry can be create to have precise input when place virtual image of an assembly.
Good care should be taking when selecting the plane on witch you will place the virtual component sketch. That plane will serve has a reference further down the process.
There is no obligation to have virtual image inside existing part to use them in a virtual project, except that it will be hard to locate them. Like anything else good preparation help succes.
Creation of virtual project.
Once existing parts has their own virtual image we can launch the creation of our virtual project.
From within traditional assembly under the Home tab, «Assemble» group, launch «Component Structure Editor»
On the left you have explorer window to navigate and locate existing components.
Preview on the bottom let you have a first look at the select part. Preview window is interactive, it use the same command you are familiar with.
Above the principale zone, you will have the available virtual part. Once you select, the dropdownliat will populate itself.
How this list get populate?
In the «Solid Edge Options», under files locations their is an entry name:
It is a simple .txt file with instructions in the header. For each virtual type component, you enter the name you would like to display. Each project can have its own VCNames.txt.
Creation of virtual project – Add component type
To start adding component, slect the type, enter a name or pick one in the list then press «Enter». Your project structure will start to shape.
Using existing components (usually standard one), pick one in the explorer window and drop it at the right location in the product structure.
No worry you can reorganize them even if you drop it at the wrong place.
If you want to insert the real document instead of its virtual image, simply check the option bottom left.
How can I make the difference between an existing part and a virtual copy of that same part?
Look at the two «anchor.par»
In the top right corner there is one with a small flag representing a cube, that’s indicate a 3D file associate with the virtual image.
For the other copy of anchor standard icon is use. Small shaker indicate that the part is not fully constraint
Here a look at few icons use in the pathfinder.
Since this is a virtual structure, you can play with it without problem. You can promote or demote part or sub assembly to better suite your needs. Only component insert has real one could not be move around.
When finish click «OK»
Creation of virtual project – Make a template
Once ok button is click, you will be back in the Assembly file. From there you will be able to save that assembly file in our template folder for future reference.
When it comes time to start a similar project, this could be a huge time saver. No need to create complex structure create small one to give you more flexibility.
In this new assembly file, even if its parts are virtual, they behave the same as a real assembly file. From «Application menu», «File Poperties» you will have the entire set of properties, plus the ability to create custom one.
If your interest in knowing a little bit more about properties
In a more control environment (larger company) where we have engineer, designer and drafter, this will help assign task to group /department has discuss in a previous article.
Creation of virtual project – working inside the structure
Working inside a virtual structure is simple has sketching.
From the pathfinder of the assembly you will create plane at the correct distance from the base plan. Usually this will involve parallel plane creation to position sketches.
From within the sketch you will position you virtual image. Remember the icon with flag has a cube, RMB and choose «Position Virtual Component»
Remember the viewswe have create earlier, Solid Edge will ask you which one you would like to place, base on the orientation of the plane you are working choose the right one.
So gradually you will be able to start layout your existing part without having to deal with 3D part.
Once you start placing virtual image of real component, new information will be available in the Partfinder has a flag on each icon.
New command will be available in the contextual menu once a virtual part start it’s transformation into a real component.
What about those virtual parts that has no information?
It is simple has the other ones. From within a sketch start drawing the lines that will represent the part in the orientation you are working.
Example: plane is set parallel to front view, then draw the front representation of the part.
Once geometries are layout, RMB on the virtual component and choose «Edit definition»
SE will ask you to follow two steps:
First – Select the geometry you would like to assign to the virtual component.
Second – Define where the origin will be place and the view represent by the geometry.
At this point we are half way between virtual and real component. If we consider 3D modeling real🙂
I miss a part what i can do?
Stay inside the sketch, locate the part from the Pathfinder library and drag inside your sketch.
Yes it is possible to bring 3D part inside a sketch. I bet that you didn’t know this one….?
When doing this SE will aks you wich face should be parallèle to the skecth plane.
On the vertical Ribbon bar few options will be present to you..
From here you can decide if the part drive the sketch element
The skecth drive the part. This will allow you to use geometric constrain or dimension to precily locate the part.
If the part is alreay insert in the assembly, from within a assembly sketch environement, under the «Tools» tab, inside the group «Virtual» choose «Component Select Tool»
Creation of virtual project – Publishing virtual component
You have work hard it is now the time to be reward.
Once virtual parts has been create, then organize in logic subassembly, you have then layout your project to trace what will be the general direction.
You have use the properties manager to push has much informations possible into each virtual parts so those hungry data consumers will be happy.
Last step is to use the publish button
For each components you will have acess thru the contextual menu
to more commands
Up to the last minutes, you can change the name of the publish component
Decide the path where the file will be save
Decide if you would like to change the template the part will be base to be published. This is one of the reasons why having predefine 3D template is useful.
At the bottom you can ask to use simplify representation after publishing. At any time you will be able to toggle between the two representations in your design.
Remember the two steps where we associate 2D lines to a virtual part and setup origin… those lines will be transfer at part level so you won’t have to draw then twice and they will be place in the correct plane at the correct location versus the origin.
This tool will help plan and manage early in the process. From a simple project to a huge one you will have a bird view of the structure before commit yourself to (sometime) a rigid structure.
Designer has taking bad habit to model in 3D rapidly, integrating this in your daily routing will ask you to make some effort, who would like to change it’s old comfotable sliper🙂
Once master this tool will give you benefit.
1-Help capture design intent
2-Help for quotation
a.Better project startup
b.Help establish design method
c.Identify major component (master one)
d.Identify method/assembly sequence
4-Distribution of work among people relate to project
5-Facilitate the BOM numbering
6-Spread the load of each sub-assmebly ( less part per branch)
7-Help reuse existing parts
8-Help sequence the realisation of the project ( smaller orgaise sequence)
9-Help plan the manufacturing
10-… less frustration🙂 more organisation
Video card is down I operate with a spare one, when things get back to normal I will take few moment to build a video.
Until then have a nice design time. And remember to treat our CAD department like olympic athlete, training, training, training to keep designer on the Edge.
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