The greatest challenge faced when collating a bunch of best practices is to differentiate them from tips and tricks. Best practices come from practical experience and experience is simply the name we give to our mistakes.
Also, we spend very less time assembling in Solid Edge compared to part modeling and drafting. Whereas part modeling mistakes are a great deal easier to rectify when problems are found in downstream drafting, simulation or rendering, the same cannot be said about the assembling process which necessarily calls for meticulous planning.
My best practices articles The 10 Golden Rules of Solid Modeling and
Surfacing: Techniques from the Trenches were followed by a flurry of requests for synchronous best practices, assembly, sheetmetal and draft best practices. I am no sheetmetal expert and drawing best practices would be a never-ending saga since it is difficult to demarcate what could possibly constitute the best 6 or top 10 drafting best practices in Solid Edge.
Further, assembly best practices could be easily confused with ‘large assembly’ management tips but skimming through the articles on solid and surface modeling best practices, you can easily catch the drift.
So what follows are neither:
- Solid Edge
LARGEassembly best practices, nor
- Solid Edge assembly productivity tips that will fetch you success overnight.
Without a doubt creating assembly relationships form the bulk of activities when assembling components, so 5 of 12 best assembly practices shared below revolve around managing them.
Model a part in the same orientation as its layout in the assembly. This gives the solver engine a better chance of snapping components into the right location.
Agreed this is not always possible since there could be times when a part is placed in different orientations. Reorient components into the approximately close orientation before dropping them into the assembly.
Solid Edge provides a beautifully thought out and executed functionality to achieve this by allowing to reorient the part in the preview area itself. Watch and listen to a video created recently which illustrates this:
Number of Relationships
Relationships consume memory and take longer to solve. So it goes without saying to use only as many relationships as are needed to control component position and movement. See tip #1 in this set of tips which shows how to easily lookup the status of a component in the Pathfinder.
Though Solid Edge allows redundant relationships and the animation in the first tip in this set shows how to further explore each relation in detail, suppress or delete any redundant relationships.
Use the Flashfit relationship when applicable, which not only reduces the number of steps required but also automatically applies the optimum or least number of relationships required to fully define or constrain the part.
Join symmetrical assemblies to a mid-plane or axes. If you are dropping the first part into the assembly which is known to be a symmetric one, make sure you don’t end up relating its reference planes with the base reference planes in the assembly. This will necessitate creating additional reference planes for mirroring it.
This however holds good when the entire assembly is symmetric on one side of a plane. In some cases though, as seen in the image below, it is a good practice to not only model parts symmetric about the base reference planes but also relate the base plate to the base reference planes of the assembly.
In short, keep your eyes open and be opportunistic.
The axes of the base coordinate systems in Solid Edge can also act as virtual reference planes when the mouse is hovered in the space between them, but the underlying idea of symmetry remains the same.
Use a common reference if possible. Joining all components to a common component or reference geometry is a good practice since it reduces complexity.
For example, insert the typical base plate, main frame or the chassis as the first component and try to add relationships of subsequent components all to this single part when possible. The zone_try_it assembly in the training folder is a good example where the compressor, cooling unit and the fuel tank are all connected directly to the frame structure.
Alternatively use the base coordinate system to locate components in an assembly whenever possible.
Long chains of components take longer to solve and are more prone to relationship errors, unless you are modeling a kinematic link chain of components like a robotic arm.
It is a good practice to add PMI dimensions at the assembly level. These can always be extracted in the drawing using the Retrieve Dimension command. This way you can save time adding them again should you decide to use the 3D model for animation, rendering or to comply with model based definition practices that are introduced later.
This in turn involves some planning in terms of selecting the plane or view within the assembly since the GA layout can retrieve dimensions only in the view they were originally placed in the assembly. This means PMI dimensions applied in a top or its parallel plane cannot be retrieved in the front view in the assembly drawing.
Always organize part files in a folder structure. Avoid storing all assembly files in one folder. When Solid Edge must search through hundreds or thousands of files in a single folder to find the correct file, it could take longer to open files. When there are fewer files in a folder, the file is located and opened more quickly. If possible, place all subassembly components in the same sub-folder.
Create a shared network directory for components that can be accessed by many designers on many projects.
Another area of utmost importance is managing assembly files between projects. A highly-recommended practice is using the Revision Manager or its new avatar the Design Manager found on the Tools tab, Environs group on the ribbon bar.
The Design Manager enables you to rename documents while maintaining links, move documents to new locations, replacing one part with another, assign document numbers, revisions and project names.
Features – Plan Ahead
Avoid relationships between features that might be removed later in the design process. Also, if you are using a part parametrically driven using a suppression variable, pay attention to any of the edges or faces of the feature being used in the assembly relationship. When the feature is suppressed the relationship will fail.
Though everything cannot always be foreseen, in such cases it is a good practice not to delete or change the relationship parameters but instead locate and then suppress any relationship which you suspect might be caused due to feature related problems in the component part.
It is also a good practice to repair model errors before you even insert it in an assembly. This is especially true for imported parts using neutral formats which are either directly used in the assembly or after some modifications. The Optimize command can be used to identify and repair any such faulty geometry. See a related article which discusses this command in greater details.
A Stitch in Time Saves Nine
Remember that adding a relationship never fixes earlier relationships problems. If a component is causing problems, it is a good practice to suppress all its relationships and recreate them instead of diagnosing each one. This is especially true for conflicts related to flipping sides in the Mate and Planar relationships. Use ARM or simply the Assembly Relationship Manager to see the relationships for components.
Once the component is satisfactorily positioned, it is a good practice to go back and delete all suppressed relationships.
Whenever possible, create relationships in subassemblies rather than the top-level assembly to reduce the rebuild time of the top-level assembly.
Whenever possible, fully position each part in the assembly, unless you need that part to move for any assembly motion related studies. Assemblies with several interrelated uninhibited degrees of freedom take longer to solve and have less predictable behaviour when you drag parts.
Never Assemble in Perspective
Although this might be tempting to many, it is observed to be causing several problems picking edges and reference planes for adding relationships.
If you are creating assembly features like holes, the hole profile may appear jagged or polygonal instead of circular. Also selecting hole profiles in such states can become difficult.
Perspective can be turned off quickly by clicking its button on the ribbon bar’s View tab, Styles group and there is also a keyboard combination for this which this video illustrates.
Use Synchronous Models
This will allow you to modify multiple parts in the assembly without having to open them explicitly.
This ability is perhaps the most useful feature of Synchronous modeling outside the part and sheetmetal environments.
Synchronous edits at assembly level can save you hassle of establishing clumsy and difficult to maintain interpart relationships using linked variables or any other method.
If you want to see real Synchronous Technology in action and relish its true benefits, it is in the assembly environment, since late stage design changes can be made literally on-the-fly using synchronous edits at the asssembly level itself.
So it is a good practice in the long term to start investing in Synchronous models – both part and sheetmetal.
A Recently uploaded Video by Edger Alan Pope (what’s your forum name buddy?) of CAD Central illustrates this.
Use a Proper Template
A Template can be used to make sure that all assemblies created with a company standard and all parts in a project have identical properties. These may include units, dimension precision and custom properties to name a few.
Don’t Lose Sight of Manufacturing
It is easy to occasionally become so involved in the little details that we lose sight of the big picture. It is a good practice to step back, take a breath and try to remember who the consumers of the assembly are. These are typically the ones on the shop floor followed by those on the assembly line or people on site who would bolt or weld parts and machine them afterwards. Just a few good practices here:
- Rotate the assembly model periodically, then rotate it more and if you have a 3D mouse, rotate further. This will help spot errors of every kind which are easy to miss from just one viewpoint.
- Take sections using either the Section command on the PMI tab or using the Set Planes feature on the View tab. This will help spot overlaps.
- Use the Drag Component command with Detect collision mode to avoid any interference.
The Good, the Bad and the Best
Whereas good practices come from experience and experience comes from bad practices, the best practices emerge from the good ones only when we share and brainstorm.
So the aforelisted 12 suggestions could potentially be the best only when you approve of and certify or add your practical wisdom to them.
Use the comments section below to make these good practices the best ones!