The term “large assembly” means different things to different people, so how do we define a large assembly? Large assemblies are not defined by the number of components or physical properties; rather, they have two primary characteristics. An assembly is considered large if: It uses all your system resources. It hurts productivity.

These characteristics can be further divided and be caused by many of the following traits:

Physically large

• Requires some layout or other engineering input to position all the components properly.

• Has so many components that their management, calculation, and memory requirements are large enough to be a detriment to productivity

Complex

• Has many parametric relationships

• Has a large number of mates.

• Taxes your computer resources.

• It contains many different components that need to be managed and can slow down the processing speed of even large, fast computers.

• Has imported data that has to be located and loaded.

• Has geometric complexity that is difficult to rebuild– Requires best practices for large assembly design at the assembly level and at the part and drawing stage of work.

Uses multiple systems or disciplines. These could include:

• Mechanical components • Custom components

• Toolbox parts

• Library parts

• Weldments

• Routed systems

• Components from outside vendors and subcontractors

• Customer files the truth is not bigger and better hardware can fasten assembly performance but the slow performance is a combination of many factors in design.

Slower performance can be seen in following areas:

• Opening, Closing & Saving time

• Rebuild time

• Creating drawing

• Rotating, panning & viewing

• Inserting components

• Switching between parts, assembly, drawings

• Mating, etc…

Major performance issue arise from modeling practices than any software or hardware issues.

• Things under Solidworks control are 20%; they are bugs, algorithms, code efficiency.

• Things under user control are 80% as,

• Software and data management option and setup fail to plan things in the most efficient way affects performance.

• It’s good to buy Solidworks certified hardware or equivalent to maximizing performance.

• Best modeling practice needs to adapt to guide your work by avoiding lengthy modeling processes.

Slower performing assemblies are an accumulation of many small fixes there is no easy fix for such assemblies. Fact is when Solidworks models start running slow user wants to jump to the bigger and faster computer which is waste of money for keeping nonprofessional drivers on board. With a proper strategy of design root, the cause can be controlled to a low problematic end irrespective of how good your computer maybe (I am not against powerful Pc’s but against wrong practices).

Things to consider while creating large assemblies

File management

• All design team members of project needs access to files as required

• Protect files from accidental overwritten from non design team members

• Ensure file properties/metadata are filled correctly

Don’t allow to create situations where parts, assemblies, & drawings are stuck down by

• Inability to locate files

• Working on the wrong version file

• Modeling problems

• Hardware problems

• Network problems

Produce parts, assemblies, & drawings efficiently

• By using in-context features at design as appropriate

• Breaking in-context relationships & the problems of part origins

• Sharing data between engineering, manufacturing, & design team without any problem

• Its ideal to limit configurations to two to three at component level

• Design simplified parts

• Ideal to use parasolid bodies or simplified parts for library or purchased parts and assemblies

There is no quick fix method for slower large assemblies therefore significant methods and steps need to follow while designing to improve large assemblies.

Best Design Practice

Its important to know how thing in Solidworks background is working.

Effective modeling parts

• Proper origin

• Easy build features

• Removal of in-context relationships

• Removal of circular references

• Simplified versions

Effective modeling assemblies

• Sub-assemblies orginazition

• Proper level of detail

• Proper mates

Reducing information loaded into memory

• Quick open

• Light weight

• Large design review

• Simplified configurations

• SpeedPak

• Draft quality drawings

Data sharing (Must for designers)

• Access to all necessary files

• Access to the most current version

• Make changes to files with responsibility

• Protect from others to overwrite files.

How to Implement a Strategy

The way you will implement and enforce the strategy should be part of the strategy development. Things to consider when implementing your strategy for the design:

• Document the approach Procedures that are not written down can be more easily misunderstood and varied. The time required to properly document a plan is less than the rework time (and cost) caused by people not following the plan. Having written documentation of procedures also allows for accountability when members of the team deviate from the plan.

• Make it readily accessible No matter how good a plan is, it is useless if the people that need the information cannot see it. Have it posted on the engineering intranet, or on some common location where it can be easily viewed by the entire team.

• Communicate with users Make sure the procedures are discussed at planning meetings. Stress the consequences of not following the plan. Remind people of the procedures as soon as any deviation is noted.

• Document templates and document level settings Have everyone use the same templates. Well—designed part, assembly, and drawing templates can save time by automatically filling in required data directly from the models. Document templates also set the document properties to insure consistency between all the members of the design team.

• Custom properties Custom properties can be very useful as they can be automatically read and used to fill in data in bills of materials (BOMs) and forms in the PDM system. They can also be used as search criteria to more quickly locate files by helping to filter components during “advanced selection” to aid in assembly visualization and performance. Many custom properties can be included in the document templates to make it easier to include all the properties that are required for the project.

• System-level settings System-level settings can make a significant difference in system performance. Provide guidance to the design team on setting these.

Planning and File Management

• Understand the need to plan ahead when creating large projects.

• Understand the key elements required in a data management plan.

• Understand the benefits of a file management system such as PDM.

Large Project Design Planning

The more complicated a design, the more planning that needs to be done before the first part is created. Failure to plan and have everyone using the same methods can result in lost data, long rebuild times, and higher costs due to problem resolution. The planning of a large assembly follows the same general rules as any large project: you need to plan ahead and have structured progress. Some things to consider when starting the project:

• Have an understanding of the approximate size and makeup of a typical data set.

• Because you will be dealing with large data sets, develop a strategy before you start to model the parts and assemble them.

• Decide which tools and techniques you will utilize to make your assembly as manageable as possible,

• Determine which of the two primary techniques you will use:

• Skeleton model technique for large assemblies, usually used for machines, plant-t designs, paper processing allows visualizing and selecting important interfaces at all sub-assembly and even part levels.

• Master model technique Usually used for consumer products as ducts, car body, and the like, allows using complex surfaces as the base for components , Results in many multi-body parts.

• Decide how you are going to name parts and handle revisions.

• Each file name should be unique. Are you going to use intelligent part numbering or dumb part numbering?

• What will the revision scheme be and how will revisions be captured in the files?

• What is the workflow for documents?

• How are in-context relationships going to be used and managed? Keep in-context relations as simple as possible and keep to one master model where feasible.

Efficient large assembly design is a combination of many smaller things that when combined, can make a big difference. You must have disciplined modeling, assembly, and drawing technique. Plan before starting work, as the time to react is not when there are 15,000 parts in the assembly.

File Management

File management can help to save significant time during the design process. File management is a topic that needs to be decided on early in the process and is not something you slowly ease into. The methods and procedures need to be determined, implemented, and enforced if you are to gain any benefit. Starting a project with the idea that you can just start designing, naming and storing files without a well- thought-out procedure is a recipe for disaster. It takes much less time (and costs less) to plan the process and rules, than it does to fix the problem afterwards.

Managing and Sharing Data

To set up and manage files it is important to start with a set of goals. So, what are our goals when managing our files? These are some general goals that are usually included:

• Multiple users must have access to the same files.

• Users must be prevented from overwriting each other’s work.

• Everyone must know what the current version of each part is.

• Different work styles must be accommodated.

• Files need to be stored for maximum productivity by keeping them stored locally.

SolidWorks File Structure

The SolidWorks file structure is a single point database. This means that each piece of information is stored in only one file. Any other file that needs that piece of information must reference the file where it is stored rather than copy the information into itself. This means that SolidWorks creates compound documents by establishing external references.

External References

External references are the links between documents. There is no separate database to list the references. Instead, a pointer in the file header lists the referenced files and their location. These are absolute references, in other words, they are a complete path such as K:\myfiles\appliedproject.sldprt.

Where Used

There are no reverse file pointers in SolidWorks. While an assembly knows what files are used in the assembly, the individual components do not know that they are used in that assembly. This presents a management problem when modifying files that may be used in different assemblies. Data manager PDM systems keep track of these relationships, which makes it easier to determine the effects of changes to parts. Without a data management system, SolidWorks Explorer can be used to locate “where used” relationships; however, this can be slow as it must literally search through all the files in the specified search paths to determine if there is a reference.

The Manual Data Management Method

If you have a PDM system, how are you going to manage all the files for your large project? Different companies have tried different methods, but they generally reduce to two primary methods.In the first method, all files are stored in a central location. Users open the files across the network from the central location as needed and save the files when done making changes. SolidWorks collaboration options help to prevent multiple users from having write access to the same files at the same time.  There are several problems with this method:

• No history Any history as to changes, or who opened or saved the files, must be kept manually.

• No revision or version control, Tracking revisions must be done manually. Methods such as appending the revision to the file name are sometimes used and can cause additional file management problems.

• Easy to violate the rules There is nothing to stop users from copying files to their local drives to speed up their work, but this in turn violates the rules of only one person having write access to a file. If you are not strict with all users, someone will break the rules at the worst possible time and cause a loss of data.

• Opening files across a network Opening files across a network is a sure way to reduce productivity. With the large number and size of the files, network bandwidth can significantly slow the opening, saving and closing of files. Most PDM systems cache files locally on the user’s hard drive to speed open and save times.

• Search Without a PDM system, searches are left to SolidWorks and Microsoft® searches, In the second method, files are stored in a central location and users copy the files they need to their local workstation. After making changes, they save the files back to the central location. This ls the “Wild West” approach as nothing in the system enforces the rules. All control is lost except for what can be done through procedures enforcement. Whoever saves a file back to the network location last, overwrites the previous version, even if the last saved file is older than the file it is overwriting.

Product Data Management

While a single engineer or designer may be able to organize, store, and keep track of changes without a data management system, as soon as a second engineer is added, some form of data management is necessary. Data management is a prevention, not a cure. Some people will resist using a PDM system because they think that it is too hard, or they don’t want to learn something new, or they feel that it takes too much time, among other reasons. Yet, they are also the ones complaining when they can’t find all the files for the assembly they are working on because someone moved them, or their latest changes were overwritten by an older version of the same file when someone else saved the file on top of their work. There are several product data management systems on the market from workgroup level through enterprise, so the method or product you choose can be matched to the size of your data and budget. The bottom line is that you need to manage your data efficiently either by using a PDM system or through manual brute force. Not managing your data is costly in time, money, and human frustration.

Goals of Data Management

When selecting a data management method or system, you should keep in mind the goals of any data management system. They are to be able to do the following:

• Search and find referenced files

• Easily create a bill of materials listings and locate where files are used

• Enable collaboration and change control

• Track revision history and provide secure vaulting

SolidWorks Workgroup PDM

As the name implies, this PDM system is made for workgroups at a single location. Depending on the size and structure of the design team, SolidWorks Workgroup PDM may be used, but generally the size and makeup of the design teams that are required for large projects call for an enterprise solution.One key difference between SolidWorks Workgroup PDM and an enterprise solution is the single vault structure. if your design team works in multiple off-site locations, SolidWorks Workgroup PDM is not the best solution, as connectivity requirements would require excessive time to check files in and out of the vault. Some key features provided by SolidWorks Workgroup PDM

• Revision control

• Single workflow

• Tracks all changes to the files

• Can store any type of file

• File access is controlled through permissions

SolidWorks Enterprise PDM

With very large file sets, SolidWorks Enterprise PDM is usually the best choice for file management. SolidWorks Enterprise PDM uses an SQL database and can replicate the vault to multiple locations so that data can be synchronized regularly to avoid delays due to network bandwidth or slow internet transmission speeds. As the vault is stored as an SQL database, searches are fast.Some key features provided by SolidWorks Enterprise PDM.-

• Both revision and version control

• Multiple revision schemes

• Multiple workflows

• Tracks all changes to the files

• Can store any type of file

• File access is controlled through permissions

• Can provide notifications of changes

The Choice

The decision to use PDM is up to end users & companies requirements, as without PDM any data loss may significantly affect productivity and increase the cost of the system and of training the users.

Solidworks Part Modeling Technique

Parts

Good efficient assemblies start with good efficient parts. As parts are core elements of large assemblies, they need to be model sensibly and efficiently. Part design always has to start with a plan as to how to model it efficiently, with properly placed reference geometry. One key element when modeling parts is to establish the design intent. Once this is done, you can plan part construction by considering these elements.

• Origin – Where should the origin be? – How does the origin affect the mating of the parts in the assembly?

• Symmetry – Is there symmetry? – If so, how many planes of symmetry? Generally, the origin is on all the planes of symmetry. or even less of the part and then either. Using symmetry, you can model half or quarter or even less of the part and then either mirror or pattern the rest. mirror or pattern the rest.

• Features – Decide which elements should get their own features in the FeatureManager design tree. Will any features need in-context relationships?

• Configurations – Configurations can be used to create both the maximum (full detail) and minimum (only the detail needed to mate the part into the assembly) conditions of the part.

• Patterns – Patterns can reduce the amount of work to create the part and can also be used at the assembly level to automatically add fasteners.

• Views – Which view of the model Will be the Front View when detailing? – Will detailing require special views?

• Mating requirements – How will this part be mated in the assembly?

• Properties – What properties need to be attached to to the part for accurate assembly weights, BOMs, part callouts and the like?

• Templates – Right template can save time by having repetitive information and proper settings already entered. Consider creating specific templates for different customers.

• Document settings – Document settings will control the speed and ease of the design process. What image quality and display settings will allow us to see the design easily without slowing us down?

Features

Plan ahead before modeling to reduce the number of features. Combine features sensibly because you should also keep in mind the need to change the model in the future.

Put the fillets and chamfers at the end and combine them into the minimum number of features consistent with the need to make later changes. By placing these features at the end of the FeatureManager design tree you get two benefits. First, the model rebuilds faster when we are adding features before the fillets and chamfers. Second, you can easily group the fillets and chamfers into folders to suppress/unsuppress them quickly. Use the Feature Statistics tool to determine which features are slowing the rebuild time to see if they can be suppressed while working on other parts of the model. Feature Freeze Feature Freeze can be used to keep some or all features of a part from rebuilding. This can significantly reduce the rebuild time for complex parts. Setting the Feature Freeze bar at the bottom of the FeatureManager design tree will keep all features from rebuilding and make configuration changes much faster.

Feature Statistics / Performance Evaluation

The Performance Evaluation / Feature Statistics tool can be invaluable for locating features that are taking a long time to rebuild. You can use this tool to help determine which features should be suppressed in a simplified configuration.

Mate References

For parts that are only inserted into an assembly once, creating mates manually is a reasonable method to place the part. When parts are used many times, however, you can save significant time by establishing mate references on the reusable parts.

Patterns

Patterns can save time when used correctly, or they can slow a model rebuild time if not. The advantage of feature patterns is that they can be used as a source for other patterns at the  assembly level (feature—driven patterns). Patterns can also be used as a source to add fasteners to assembly using Smart Fasteners. This has the advantage of faster rebuild times as pattern controls the position of the fasteners instead of mates.

Avoid patterning on top of other patterns. Instead, make a single pattern with all the features.

Move big patterns as far down the FeatureManager design tree as possible. This allows the other features to be built first and also allows the pattern to be suppressed without worrying about parent/child relationships.

Remodeling Parts

Parts sometimes have inefficiencies caused by adding and deleting features, or features added to correct an earlier error while searching for the correct final form. At some point, these inefficiencies should be removed and the part recreated from scratch. It is usually difficult to make the decision to rebuild a part from scratch when you are under a tight deadline, but you need to weigh the cost in both time and money of remodeling the part against potential for problems that may be caused by the model. It certainly takes a finite amount of time to remodel the part, but usually not as long as you think because you know exactly what the final model will look like. With an inefficient model, a simple change could cause the model to fail to rebuild. While a single inefficient part in a large assembly may not have a huge effect on rebuild time, rebuild times will be affected by many parts that are inefficient. The other consideration is whether this is a single, one-time-use part, or it will be used in this and future designs. You may consider not recreating a one-time-use part, but reusable parts should be created efficiently.

Symmetry

Taking advantage of symmetry when creating a part can reduce the number and complexity of mates that need to be added at the assembly level. This is particularly true when parts need to be centred on each other. Using symmetry can also speed the rebuild time for individual parts when you mirror bodies. When mirroring bodies, surfaces are patterned instead of having to rebuild the geometry for each feature.

Templates

Having a proper set of templates can save time in all phases of modeling. The benefits of good templates include:

• Document properties are setHaving the document properties set in the template allows you to move ahead to modeling without having to make adjustments to the settings.

• Visual and physical properties are setVisual properties such as the model and background appearance can be set to eliminate the need to change it later. The proper and consistent material can already be added to the part before the first geometry is created.

• Custom properties are setMany items can be prefilled such as company name, address, the person creating the file, and other information established to capture model properties (material, weight, etc.).

Part Origins

Part origins are normally located based on the geometry of the part and its symmetry. There are two general exceptions: first is to locate the origin so that the part lines up in a layout grid at the correct position, without mates; second is when the part is created in-context and the origin is located by projecting the assembly origin onto the Front plane of the new part.

Having the origin based on the geometry of the part is the most common method and found in most best practices documents. Creating the geometry of the part off the origin for alignment purposes is generally not done in smaller assemblies or with parts that may go into different assemblies, but can be useful in a larger assembly as the part is inserted at the assembly origin and fixed. This approach reduces the number of top level mates. In many cases, if you properly locate features of the part on the origin, your mating planes already exist. For example, by placing the absolute center of a sketch for a Wide Flange Beam on the origin, then extruding from midplane, you get a Top plane in the middle of the beam, a Right plane in the middle, and a Front plane in the middle without having to do any extra work.

When a part is created in the assembly, the origin could be at some location well away from the part geometry. This is generally unacceptable and can be fixed, or as we will see later, the in-context relationships can be created differently to avoid the origin being off the part.

Part Configurations

Part configurations can have an effect on the speed and performance of large assemblies. There are productivity gains to be realized using configurations and consequently having fewer files to manage, but they can increase the file size of parts and assemblies. You have to decide if the benefits of using configurations outweigh the associated file size issues for their particular application and decide what will be best for them. Configurations allow you to control many variables within a part or an assembly in a fast and easy manner. The use of design tables takes this further still. However, when a configuration is activated, the data for that configuration is generated and stored in the file (e.g., preview, lightweight data, and body information). This is done to avoid performance problems in complex parts. There would be delays if configuration data had to be built every time a configuration is accessed. Because the data is stored the file size will grow as more configurations are activated. If the files are being opened across a network or copied across a network to a local working folder, the large file sizes will slow performance as more data will have to be copied across the network. When a part is used in an assembly, only the information of the configurations of the part used in the assembly is loaded into memory. For example, if a part with 200 configurations, all of which had been activated in the part, were used in the assembly, the data for that part’s active configuration would be loaded into memory. If a second instance of the part were inserted into the assembly using a different configuration, the data for the second configuration would also be loaded into memory. The data for the remaining 198 configurations would not be loaded into memory.

• If a new file is created using File, Save As, only the data for the active configuration is retained, which may reduce the file size significantly.

One way to increase assembly performance is by using simplified configurations that can be selected when opening the assembly.

Simplified Configurations

Simplified configurations are used to reduce the amount of data that must be loaded into RAM when the assembly is opened. This configuration should be created so that only the key information about the part is unsuppressed.

What information is important?

• Mating surfaces All surfaces will be needed to mate the part into the assembly. This requires some planning to make sure the correct surfaces are included.

• Interference surfaces All surfaces that show the volume of the part and its boundaries. This information is needed to make sure this part does not interfere with the surrounding parts.

What information is not important?

• Cosmetic featuresCosmetic features such as fillets, chamfers, engraving should not be included in a simplified configuration.

• Detail featuresSmall details of the part design are not necessary for the assembly and cause additional problems with graphics performance as they require many small triangles to be formed to display the shaded surface. This is analogous to creating a mesh in FEA.

Naming Simplified Configurations

One very effective way to use simplified configurations is to have an assembly configuration that opens all components in their simplified configuration. This assembly configuration is easy to create when opening an assembly by using an Advanced option because you can select the name of the configuration you wish to open for each component if it exists.

The important thing is that you can select only one configuration name. So you need a company standard for each engineer to create a simplified configuration with the same name. Also remember that capitalization is considered, so Simple and simple are two different configuration names.

The Simplify Tool

One difficulty in creating a simplified configuration is locating and selecting small features. The Simplify command allows the selection of features based on their size relative to the part.

From the Results list, you can individually select features and then click Suppress, or select All and then Suppress to suppress the features found in the Results list. A derived configuration will be created with those features suppressed.

Where to find it:

• Menu: Tools, Find/Modify, Simplify

• Tools toolbar: click Simplify

Fasteners and Toolbox

The toolbox can be set up to work two different ways:

• Master partsIn the master part setup, Toolbox retains a set of master parts. When you insert a fastener into an assembly. The toolbox will create a configuration of the master part based on the size you are using. The advantage of this is that the size of those part files increases as additional configurations are created. In a company environment, the Toolbox part files are normally kept on a network drive, which means that the files have to be opened across the network, slowing down performance.

• Copied parts In a copied part setup, new part files are created when you insert a fastener into an assembly. The advantage of this method, for large assemblies, is that these files can be stored with the assembly and have only a single configuration. While this method creates more files, the files can be stored locally and can be smaller because they only need to have a single configuration.

Toolbox parts can have three different thread displays. Because fasteners are purchased parts, there is no need to show the threads unless you need them for display purposes. For performance gains use a Simplified thread display. If you need the threads to display for a rendering, choose Cosmetic to have a thread appearance applied to the surface.

Level of Detail for Purchased Components

When you use purchased components in your designs, you need models of these components to fit into your assembly. Depending on the source for the component model, there could be a wide range of detail provided. How much of this detail is necessary for you to work on your design? Generally no more than what was listed above for the simplified configuration. To speed the design at the assembly level, a lot of detail can be stripped from the model.

Level of Detail

Too much detail causes excessive rebuild times. Below are some suggestions on ways to remove detail.

• Do not model threads. Model only functional threads. There are considerable regeneration times associated with modeling the helical threads. If you need a visual representation of the threads, Toolbox has an option to show threads as a texture map.

It takes more than five times the number of triangles to represent the surface of the bolt when you add helical threads.

If you need to see visual threads, use the Cosmetic option in Toolbox.

• Avoid using text for features. Do not model text unless it is part of casting or will be machined into the part. SolidWorks uses TrueType fonts in Windows. Text can have hundreds of entities, sometimes per letter. You can evaluate the impact of modeled text by opening a part with extruded text and using the Performance Evaluation tool previously known as Feature Statistics to list rebuild the times.

Below are the rebuild times for the simple part shown on the right. Notice that it took 0.00 seconds to rebuild with the text suppressed and 0.16 seconds to rebuild with the text unsuppressed. If we compare the geometry, the part without the text has just six faces but with the text, there are 530 faces.

If the text is not to be machined into the part, such as labels that will be affixed to the part, consider using decals because they do not create additional geometry.

• Minimize unnecessary detail.

Combine fillets of equal size or function.

• Avoid Lofts and Sweeps if you can create the geometry with an extrude or revolve feature. Lofts and sweeps take longer to generate.

• Do not model springs unless absolutely necessary. Like helical threads, sweeping along a helix creates a large file due to the complexity of the surface. Instead, use a cylinder that forms the bounding shape of the spring. This can be mated and used to detect interference while solving very quickly.

If you need more of a visual representation, consider adding either a decal or a thread appearance.

• Fully define sketches. Leaving sketches under defined may be acceptable when you are still in the early part of the design process for a part. Before using that part in an assembly, you should have it fully defined to avoid rebuild errors and to avoid unintentional changes.

Additional Consideration for Parts

In addition to the above techniques for part construction, there are several other considerations for efficient parts.

• Level of Detail for Manufactured PartsWhat level of detail is required for manufactured parts? Generally, there is one required level of detail and several optional levels. These levels of detail are controlled through modeling and configurations.

• Full (Default) ConfigurationAny part that you are going to manufacture must contain all the information necessary to actually make it. All the detail may also be required if renderings of the part will be necessary for marketing purposes.

• Simplified (Assembly) ConfigurationTo get the most out of simplified configurations, the company should establish a mandatory name to be used for this configuration. The reason to have a mandatory name is so that when you open an assembly, all components that have a simplified configuration can be opened in that configuration.

• Drawing ConfigurationIn many parts, there are features that should be suppressed before creating a drawing. These usually feature such as fillets that create tangent edges.

• SpeedPak ConfigurationSpeedPak configurations offer a huge saving in computational and memory requirements. Consider making the creation of a SpeedPak configuration the general rule for all assemblies.

• Analysis Configuration If the part needs to be analyzed, the person doing the analysis will make this configuration since deciding which features to suppress involves more than simply suppressing small fillets.

Common Tools

When you build parts in the context of the assembly, sketching is the same as in the part mode with the added benefit that you can see and reference the geometry of the surrounding parts. You will use Convert Entities and Offset Entities as well as add dimensions to geometry.

Alternatively, you can change the setting Do not create references external to the model in Tools, Options, External References, and the new feature or part will not be created with any external references. Converted geometry is simply duplicated in this case, with no constraints. No dimensions or relations to other components or assembly geometry can be added. Hole Series A Hole Series is a special kind of Hole Wizard hole that is created at the assembly level and automatically creates in-context holes in the referenced components. While these are very useful in the design process, remember that you are creating an in-context feature that must be solved at the assembly level.

In-Context Modeling

Parts can be created and built from within the assembly. These parts can also be inserted into the assembly as new parts and built using converted edges, offset edges and standard techniques. They are called Virtual or In-context parts. In-context modeling can be a great time-saver in the design phase of most projects. By using in-context features, you will be required to do much less work when changing dimensions of individual parts and features as the in-context relationships carry the changes through the in-context features in a predictable way. Generally accepted best practice is to remove in-context references before parts are released to manufacturing to avoid unintended changes from occurring; however, the point at which this occurs is not absolute. In some industries, in-context relationships may be left intact and locked if the customer is known to require changes after manufacturing has begun. When building parts in context, you can take advantage of other parts that exist. You can copy geometry, offset from it, add sketch relations to it, or simply measure to it.

While there are many advantages to using in-context features in your models, they can cause slower performance when solving the model and can create confusion for people working on the model later in the process. Additionally, creating in-context parts in an assembly can cause the part origin to be someplace other than the most desirable location.

Note: One of the things to consider before deciding to model a part in the context of an assembly is where that part will be used. In-context features and parts are best used for “one-of-a-kind” parts that will be used only in the assembly where they are modeled. Parts that will be used in more than one assembly should probably not be modeled in context. The reason for this is that the external references created by the in-context features are stored in and controlled by the assembly in which the references were established.

If a virtual or in-context part is to be reused in other assemblies, it is possible, with some work, to make a copy of the part and remove all of the external references. The part can also be created by purposely borrowing geometry but with no external references created.

In-Context Modeling and PerformanceHow do in-context features affect performance? With in-context features, the relationship between the current feature and the entity it is referencing is maintained at the assembly level. This is required because the relationships depend on the positions of the parts which are controlled by mates. In the assembly, we see these relationships as Update Holders. Therefore, in-context features create additional work when the assembly is solved. While one or two properly constructed in-context relationships may not make a noticeable difference in assembly rebuild speed, the more you have, the greater the slowdown could be. So, in addition to the other reasons for removing in-context relationships, we must consider the performance of the assembly.

Creating ln-Context Features

The method in which in-context parts are created as taught in the SolidWorks training classes is as follows:

• Adding new parts into an assemblyWhen you create a new part in an assembly, the part is given a default name and you select a plane (or planar face). The name is used as the temporary part name while the selected plane orients the Front reference plane of the new part. An InPlace mate is added to the assembly to maintain the position of the new part. The location of the origin of this new part is determined by projecting the assembly origin onto the Front plane of the new part.

• Building parts in an assemblyAs the new part is created, the selected plane face becomes the active sketch and the part is in Edit Part mode. The part is created using standard methods and references to other geometry in the assembly.

• Creating in-context featuresWhen you reference geometry that is in another part while creating a feature, you are creating what is called an in-context feature. For example, referencing the edge of a shaft when making its mating hole in another part creates a relationship between the shaft and the hole. A change to the diameter of the shaft would cause a corresponding change to the diameter of the hole.

InPlace Mates

The InPlace mates created automatically for in-context parts are there to prevent movement of the part. This is because the in-context part is attached to the geometry of parts in the assembly through external references, references that cross between parts at the assembly level. Changing the location of the part can cause changes to the geometry that may not be desired.

Replacing InPlace Mates You can remove InPlace mates using Delete, and remate the part using standard mate techniques. This technique gives you an option to leave a degree of freedom for movement. Generally, this works best if the face selected for the InPlace mate is perpendicular to the direction of motion, as this does not affect the part origin. Deleting InPlace Mates When you delete an InPlace mate, a warning message appears after the confirmation dialog.

The base sketch of the part located by the InPlace mate contains references to other entities in the assembly. These references may update in unexpected ways after this mate is deleted because the part will no longer be positioned relative to the assembly. Would you like to remove these references now? (No geometry will be deleted.)

Errors

Always resolve rebuild and import errors as they happen. it is much easier to solve a rebuild problem when it happens because you know where in the process the problem occurred. If you continue to build a part that has errors, the errors will just compound and can take many times more effort to solve than if handled immediately. Similarly, import errors should be fixed before editing the part further. Failure to solve the import problem immediately is like building a house on a foundation with structural problems.

Import Diagnostics

Whenever you import a model, SolidWorks will ask you if you would like to run Import Diagnostics. Running the diagnostics at this point is preferable to waiting as you can never anticipate the problems that may be caused by geometry with errors. if you add any additional features to the imported part, Import Diagnostics will no longer be available because it only works on an unmodified imported body.

Check Entity

Another valuable tool is Check. Check can be run on the model at any time and used to locate both errors in the geometry and undesirable geometry, such as short edges, that can cause other geometry to fail.

Where to find it:

• CommandManager: Evaluate>Check

• Menu: Tools, Check

External References

In-context parts and features create many external references which are used to create and maintain relations between parts at the assembly level. To break these references and keep the part intact, you must manually go through the in-context features and change the in-context references to local references.

When they are working properly, external references are considered in-context. When they cannot work properly, they are considered out of context and cannot update properly.

Out of ContextIn—context relationships are maintained through the assembly in the Update Holders 3. For the in-context feature to work correctly, the assembly must be open for the in-context feature to update. It is able to work properly and change through the propagation of changes only while the assembly is open.

Putting a Part Back into ContextTo put an out-of-context part back into context, open the externally referenced document. There is an easy way to do this: right-click the out-of-context feature and click Edit In Context.

Breaking and Locking External ReferencesThe flow of changes can be stopped temporarily or permanently using the Lock/Unlock and Break options. These options essentially suppress the Update Holder so that it is not solved. This helps to speed up the assembly rebuild. If you want to reuse the in-context part in another assembly, or use it as the starting point for a similar design or apply motion, you should remove the external references. By copying and editing the in-context part, you can create a duplicate part that is not tied to the assembly. Once the in-context features are created, it is a good idea to lock the external references. If changes are made that affect the in-context features, the external references can be unlocked, the assembly rebuilt, and then the external references locked again.

When the List External References dialog is active, there are options available to Lock All or Break All references. These options allow you to change the relationship between the in-context part and referenced files.

Lock All Lock All is used to lock or freeze the references until they are unlocked at a later date using Unlock All These changes are reversible after the UK is clicked. Until the references are unlocked, changes will not propagate to the part. When Lock All is selected, SolidWorks displays a message:

All external references of the model “Part Name” will be locked. You will not be able to add any new external references until you unlock the existing references.

The FeatureManager design tree lists the locked references with “->*” symbols. Using Unlock All later will restore the “->” symbols.

No additional external references can be created while the part is in the locked state.

Break AllBreak All is used to break all references with the controlling files. Clicking the button launches a message that indicates the change is not reversible after OK is clicked.

When Break All is selected, SolidWorks displays a message: All external references of the model “Part Name” will be broken. You will not be able to activate these references again.

The FeatureManager design tree lists the broken references with “->x” symbols. Changes will no longer propagate to the part.

Once the references are broken, they can be listed only by using the List Broken References check box in the List External References dialog.

Break All does not remove the external references. It simply breaks them, and once broken, they can never be fixed. Because Break All is irreversible, you should use Lock All in almost all situations.

Do not confuse the command List External References with File, Find References. In a part document, the command File, Find References only lists the name of externally referenced documents, if they exist. It does not provide feature, data, status, entity, or component information.

Removing External

References Options like Lock All are useful to interrupt the flow of changes to an in-context part, but the best way to stop the changes permanently is to use File, Save As with the Save As Copy option to copy the part and remove the references. Why Remove External References? When parts are built in-context they contain references. If mates are removed or in-context parts are used in other assemblies (out of context), unexpected changes could occur. Here are some reasons why you might remove external references.

• Component Movement – The In-Place mate prevents movement and although it can be removed, the features remain in-context.

• Re-use of Data – Component parts can generally be used in multiple assemblies. If a part contains in-context references, they must be removed prior to out-of-context use.

• Assembly Performance – Because the Update Holders are at the top level of the assembly, they must be resolved when the assembly is rebuilt. If they are not removed, they should be locked until they need to be updated.

Solidworks performance and system options

In order to reduce the lag time (the time from when you execute a command until it completes) in design software like SolidWorks, it is important to adjust settings both within the software and the operating system. There isn't a one-size-fits-all approach to setting up SolidWorks, so it's crucial to understand how different settings can impact performance and make informed choices. Often, better performance may mean sacrificing some model image quality.

Remember that SolidWorks options are grouped into system options and document properties. System options are for SolidWorks as a whole, while document properties only apply to the open document and are initially set by the document's template. Some settings are personal preferences, but many affect system performance and may need to be adjusted. In the next section, we'll explore the system options that impact performance and suggest some recommended settings. We won't cover SolidWorks options that don't significantly affect performance and are purely user preferences.

Solidworks general options

General

The general options to Show thumbnail graphics in Windows Explorer and to Show the latest news feeds in the task pane should be cleared as both take up processing power and CPU time that can be better spent on assembly performance. Enable Freeze bar should be selected as this function can be used to prevent features in components from being rebuilt unnecessarily.

Solidworks Drawings options

Drawings

The highlighted options relate to drawing speed.

Show contents while dragging drawing view causes SolidWorks to continually update the graphics inside drawings views as you drag the view. if you clear this option, the contents of the view have to be recalculated only when you stop dragging it, eliminating a lot of real-time calculations.Allow auto-update when opening drawings. If you clear this option, drawings will open faster as the information in all the views will not update until you rebuild the drawing.

Automatically hide components on view creation. This Option hides components that are not visible in the view, such as components completely enclosed within another component. SolidWorks must calculate the visibility of each component in the view to determine which components are not visible, and that takes valuable time to do. This option is off by default in Large Assembly Mode. Save tessellated data for drawings with shaded and draft quality views. If you clear this option, file size is reduced, which reduces the amount of data that is loaded when the drawing is opened. If this data is in the drawing it will be loaded from the model. The disadvantage of this option is that the views will be empty in view—only mode and when viewed with eDrawings®.

Drawings, Display Style, select draft quality so that all new views are created in draft quality. While you might expect a large increase in performance, this setting will have only a small effect as High quality views are processed in the background.

Colors change the Background appearance to plain. This avoids using other movable backgrounds that have to be recalculated as the model viewpoint is changed.

Select use specified color for drawings paper color as this has the same effect on drawings as the background appearance had for parts and assemblies.

Display/ Selection, set the Assembly transparency for in-context edit to Maintain assembly transparency. As calculating transparency is intensive, keeping at the assembly at the same level.

Solidworks Default Templates Options

Default Templates

Certain operations in SolidWorks automatically create a new part, assembly, or drawing document. Some examples are:

• Insert, Mirror Part

• Insert, Component, New Part

• Insert, Component, New Assembly

• Form New Subassembly Here

• File, Derive Component Part

In these situations, you have the option of either specifying a template to use or having the system use a default template. This option is a matter of preference; however, it is generally faster to have a default template specified as it will save a few mouse clicks by having the template defined. It will also ensure that the correct template is used if you have several templates but use only one. If, however, you use multiple templates because of different requirements for different customers, select Prompt user to select document template and you will have a choice each time a new file is created.

Solidworks Document Properties Options

Document Properties

These are established in the templates used to create SolidWorks files. It is important to remember that the option setting described here should be set in the templates to ensure their use in future files. The most important document property with respect to performance is Image Quality. The slider affects the shaded display of the assembly and part and controls the tessellation of the curved surfaces for shaded rendering. The farther to the right the slider is adjusted, the smoother the edges will appear and the slower the performance. The basic rule is to set the sliders as far to the left as you can tolerate. In most cases, two or three tick marks from the left side are acceptable to most people.

In the example below, moving the slider from Low to High cause more than 2,500 times more triangles to be calculated, which causes a significant slowdown in performance.Note: The triangles shown in the images are not clearly visible to the viewer; they are generated for the purpose of illustration only.

When you are working in an assembly, the image quality for each component is controlled by the document properties of the individual components. When you select Apply to all referenced part documents, the resolution of the individual parts can be changed to a common resolution.

Save Tessellation with Part Document

Clearing this option may initially appear to be a good idea as it will reduce the size of the files. However, the downside is that you will lose visualization data. The tessellation data saved with the file provides the display information for view-only mode, the SolidWorks Viewer, and eDrawings.

SolidWorks Add-ins

Turn off all SolidWorks add-ins that you are not using. Each add-in consumes system resources.

Solidworks Assemblies Options

Assemblies

Large Assemblies Mode is a toggle that automatically changes certain settings when opening an assembly with more components than the threshold value. In large-scale design, Large Assemblies Mode is usually selected. The threshold value is a choice you make depending on the sizes of your assemblies and the capability of the hardware you are using.

The primary function of the Large Assembly Mode is to ‘ increase performance by turning off functions that require more computations.

• Do not save auto recover info, the periodic saving of your work in progress can be a great benefit if people do not routinely save their work or if you are experiencing frequent problems with computer crashes that you have not yet solved. These auto recover save operations can take a significant amount of time and interrupt the workflow.

• Hide all planes, axes, sketches, curves, annotations, etc. This option is the same as selecting Hide All Types in the View menu. By hiding all these entities, the computational load is diminished.

• Do not display edges in shaded mode, calculating all the edges in a large assembly can be time—consuming. This option just shows the components as shaded without edges.

• Suspend automatic rebuild, when assemblies are large, recalculating assembly and mates after every change can be very slow. By suspending automatic rebuild, you can make several changes and then do a single manual rebuild. While this speeds the input, if there is an error, it will not show up until the rebuild. This may make the troubleshooting process more difficult. You can also suspend automatic rebuilds when the assembly is open by right-clicking the top-level icon of the assembly and toggling Suspend automatic rebuild.

• Use Large Design Review, this is a toggle that causes assemblies above the threshold value of the number of components to be opened in Large Design Review mode. This should be selected and a toggle value determined based on the Size of the assemblies you normally open. This option can save a considerable amount of time when used.

Solidworks External References Options

External References

The settings under External References look very simple and unimportant, however, they can significantly affect the performance of opening and saving large assemblies.

Open referenced documents with read-only access, when you open an assembly as read-only, the component files are not opened read-only unless this is selected or the files have already been opened by someone else who has to write access to the files. It is a good idea to have this option selected. If not, when you open the assembly, you get write access to all the component files, even if you have no intention of making any changes to those files. This prevents other people from being able to change these files.

Don't prompt to save read-only referenced documents, if you select the option to Open referenced documents with read-only access, you should also select this option. If you do not, SolidWorks will prompt you several times for each component file when you try to save the assembly. In a large assembly, this can be very frustrating and time-consuming.

Load referenced documents, this option determines if documents that are referenced by components in the assembly should also be opened. Selecting Prompt will ask the user if these files should be opened when the assembly is opened. Depending on the stage of development, selecting Prompt is usually a good choice as it allows the user to only load references as necessary.

Search file locations for external references, this option turns on the search of the file locations listed in the File Locations, Referenced Documents list. This option should be cleared except when specifically trying to locate files that have been moved improperly. Leaving this option selected can cause a significant increase in file opening time if there is a long list and file paths.

Solidworks Image Options

Performance

Performance and Image Quality are related and have a button to quickly jump between the two settings.

Verification on rebuild causes each face in a model to be checked against all other faces in the model. When this option is cleared, each face is checked only against the surrounding faces. While it is important to make sure that you have a good model by using Verification on rebuild, you do not have to leave it on all the time. Instead, turn this option on periodically and do a forced rebuild (Ctrl+Q) to make sure the model builds without errors. Then clear the option. This allows you to work faster but also to check your models to avoid a catastrophic error.

Solidworks Transparency Options

Transparent surfaces require precise ordering and rendering of the model to accurately reflect what is visible behind the object. Both front and back faces need to be considered as well as colours.

Both options should be cleared to result in a lower quality. transparency display, both when the model is stationary and when moving. This will allow the model to be panned and rotated more quickly. Selecting High quality for normal view mode will cause the transparency to be high quality when the model is stationary. Selecting High quality for dynamic view mode will cause the model to be high quality when the model is being panned or rotated.

Automatically load components lightweight this is a choice that depends on the complexity and size of the assemblies you work on. There is a similar option in Large Assembly Mode that will load components lightweight when assemblies reach the large assembly threshold. If you routinely open assemblies below the large assembly threshold but only work on a few of the components, then this option should be selected. Level of detail, moving this slider to the far right will allow the model to be moved, panned and rotated faster. This option causes the smaller components to change to blocks when you move, pan, zoom, or rotate the assembly. Once the assembly stops moving, the components will again be displayed normally.

Always resolve sub-assemblies, this option should be cleared. If it is selected, subassemblies are automatically resolved when the top level assembly is opened, lightweight. This removes some of the advantages of opening the assembly lightweight.

Check out-of-date lightweight components, generally, you should make sure that components are up-to-date when working on an assembly to keep from working on something that has already been changed. Choosing the option Indicate will cause a flag to be shown in the FeatureManager® design tree for all out-of-date components. This allows you to update only components that are needed rather than all components and in doing so, increase performance.

Resolve lightweight components, if you load components lightweight but then need the component resolved to perform some task, setting this option to Always will save a step. Always will resolve the component automatically if the operation you are performing needs the component resolved. This saves time by not having to agree to resolve the component.

Rebuild assembly on load, this is an option that should be set to Always. This will rebuild the assembly when it is opened, avoiding the problem of working on out-of-date geometry. While it will take longer to open the assembly, this additional time is better than working on incorrect geometry, which can cost even more time.

Mate animation speed, if the mate animation speed is set to any position other than Off, SolidWorks must calculate intermediate positions for components between where they start and where they will be once mated. By turning this off the intermediate positions do not have to be calculated and the component will jump directly to the mated position.

Software OpenGL, with no files open, examine Use software OpenGL. If it is checked and greyed out, you need a new video card. When SolidWorks launches, it checks the video card against a list of video cards that meet the requirements for SolidWorks. If your card does not meet the requirements, SolidWorks will automatically select Use Software OpenGL. This means that instead of your video card running hardware OpenGL, the tasks will be done by the software. This further taxes the CPU and slows down your system. Here again, you are balancing the cost of new equipment against the time lost by not having it. As the assembly size grows, using Software OpenGL will result in significant lost time and user frustration.

No Preview During Open if a preview is not shown when a file is opened, more memory can be dedicated to the resources to load the files into memory.

Solidworks View Options

View transitions are nice for presentations and can sometimes make it easier to see changes; however, this comes with a decrease in performance. When any of the transitions are set to something other than Off, SolidWorks must calculate intermediate positions or transparencies. This requires processing power that could be better spent in actual design.

Backup/ Recover, from a purely performance perspective, Auto-recover should be turned off as it can take a noticeable amount of time to save the files. This will usually occur just as you have a brilliant idea and are trying to implement it. If you are undisciplined in your work habits, turn on Auto-recover. However, if you save often, you can turn it off so that the save takes place when you want it to and does not interfere with your workflow.

File Explorer, like add-ins, only locations that you are routinely using should be selected. By selecting other locations, each time you select the File Explorer tab, those selected locations have to be read and populated into the File Explorer. If you are not using those locations, this is just wasted effort.

File and Model Search, when working on large assemblies and projects, you want the computer resources to be working on your design and not background tasks. Indexing should be performed when the computer is idle so as not to take computational resources away from our design time.

If dissection is scheduled, make sure it is set to run during nonworking hours.

Solidworks Windows options Options

Windows options

Different settings in Windows can also slow down your system as these settings affect everything you do. The following items in Windows Vista® and Windows 7 are effects that enhance the way things are shown on the screen. Each one takes additional graphics calculations that siphon resources away from SolidWorks.

• Aero, one clear indicator that Aero consumes resources is that in most laptop power management schemes, Aero is turned off when running on a battery.

• ClearType, is software technology that improves the readability of text on LCD screens.

• Windows Search, disable this option if you rarely do searches.

• Menu and Cursor Effects, windows have many effects that are used only to make the information on the screen look better but do not enhance performance. These include items such as pointer shadow, pointer trails, and cascading menus.

Performance Options

Choose the option Adjust for best performance rather than Adjust for best appearance or Let Windows choose.... While there are exceptions, the general rule is that if it is making the display loo better, it is taking resources that could be better used on performance.

System Maintenance

Proper system maintenance can help your hardware run better by allowing it to find files easier.

Defragment the hard drive(s) often. Loading files is harder for the computer when the file data is not stored in contiguous sectors.

Clearing Temp and Backup Files, temp files can build up and take away storage space and make it difficult for running programs to save their temporary data if there are a large number of unused temp files.

Uninstalling Applications, remove unused applications from your computer, particularly if they are programs that load on startup and stay active in the background. They are just using resources unnecessarily.

Windows Registry, as not all programs uninstall well and may leave registry entries, it is a good idea to Clean the registry periodically. There are several third-party or after-market registry cleaners available.

Service Packs provide updates to reported issues. These could be fixes to problems or refinements to make things run better. Some people load service packs as soon as they are available and others wait until the next service pack after the one they are loading has been released. With the complexity of the software, there is always a possibility of a bug being in a service pack; however, you should look at the release notes to see what has been fixed in each service pack. You will generally be much better off installing a service pack that fixes a problem affecting your day-to-day problems than maintaining an old service pack that is slowing you down.

Running Other Programs

CAD is a computer-intensive endeavour if speed is a problem, the computer should not be using its resources for other tasks such as playing music, or editing pictures. Dedicate the computer to the CAD task and shut down the other applications and processes that are running which cause interference and take away RAM, IO, and processing speed.

Virus Protection

In today’s world, some form of virus protection is required to protect our investment. One option is, of course, not to connect to the Internet in any way. While this may reduce the need for virus protection, you also have to consider the issue of file transfer and collaboration. What happens if you get a file from a vendor that is infected? Without some form of virus protection, you can run into a very costly problem with loss of data and the need to reformat one or more computers. Considering the cost of these consequences in time and money, virus protection is inexpensive. With large assemblies, you have to be careful as to how virus protection is set to run as different options can cause significant slowdowns in your system. There are different methods used to scan your computer depending on which virus protection program you use. Generally, these methods can be classified in three ways,

• Scheduled scans, as the name implies, scans are scheduled to take place at certain times and dates. Make sure that this is set for nonworking times such as the middle of the night or on weekends.

• On-demand scans, in this method, you manually initiate the scan. You can usually select which drives and types of files are to be scanned.

• Real-time scans can be used to check files as they are used by the computer. This can be a great benefit to protect your computer but can also significantly slow down your work when there are a large number of files in use. You will have to make a judgment call based on your working environment and the level of risk you face as to how much checking you want to have. Generally, you can exempt SolidWorks files from the real-time scans, which will allow better performance. Have the system scanned regularly. A computer with a virus can ruin more than your day. Lost or corrupted data can be expensive, and sending a file with a virus to a customer can result in the loss of future business.

Solidworks Rx Options

SolidWorks Rx is a tool located inside of SolidWorks that can be used for several tasks that can help SolidWorks run faster. To improve performance, the Diagnostics and System Maintenance tabs are the most important.

Diagnostics

Selecting the Diagnostics tab will cause SolidWorks Rx to examine the system and SolidWorks settings. The results will highlight things that should be fixed.

System Maintenance

The System Maintenance tab provides one place to run several maintenance tasks Simultaneously. This can be used to clean out temporary files from several locations as well as run Windows checkdisk and Defragmenter on multiple hard drives.

Once tasks are selected, you can choose to run the maintenance immediately, at a selected time, or on a regular schedule. Further refinements can be made through the Windows Task Scheduler.

Solidworks Saving Settings Options

Saving Settings

We examined various SolidWorks settings for increased performance, as these setting no need any maintenance once its set, but still have them saved in back up just in case any intentional or unintentional changes is made.

System Options, are saved as registry file by using the Copy Settings Wizard. The Copy Settings Wizard can be used to both save settings and restore settings. With it, you can save system options along with keyboard shortcuts, menus customization, and toolbar layout.

Where to find,

• Start, All Programs, SolidWorks Tools, Copy Settings Wizard

Document Properties

Document properties are stored with template files. As mentioned earlier, one should create a good set of templates with all the settings required for the different tasks or customers you have. Templates can also contain geometry (a start part), reference geometry, custom properties, and much more. A little time creating templates can save a lot of time by eliminating repetitive actions later.