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Working with Large Assemblies – Part 2

John Pearson - Wednesday, March 29, 2017

 

In this article, I will continue to focus on some of the Solid Edge tools used to deal with large assemblies. As mentioned in the previous article, “Working with Large Assemblies – Part 1”, If you are a Solid Edge user, hopefully you are aware of the following tools for dealing with large assemblies:

 

  • •Simplified Parts
  • •Simplified Assemblies
  •     ○Visible Faces
  •     ○Model Command
  • •Selection Tools
  • •Display Tools
  • •Queries
  • •Zones
  • •Configurations
  • •Limited Update
  • •Limited Save
  • •Assembly Open As options
  • •Assemblies made of synchronous parts.
  •  
  • Combine these tools with some best practices and other tips and tricks, and you’ll find that large assemblies behave more efficiently and are more reliable in Solid Edge, than any other mainstream CAD package.
  •  
  • In this article, I’d like to focus on display tools, configurations, and zones. I’ll look at how they work, how to create them, and some best practices for using them. First, we’ll look at display tools.
  •  
  • Display Tools
  •  
  • One of the easiest ways to improve display performance, when working with large assemblies, is to control which parts in the assembly use physical memory resources. This can be achieved by inactivating components, hiding components and unloading components.
  •  
  • When you first load a part into the assembly environment, using default settings, the part is visible and active. That is to say that both the display data, and underlying math data, is loaded into the assembly file. The more components that are added the more data that is loaded. The more data that gets loaded, the more physical memory is used. The following paragraph is an excerpt from the Solid Edge Help document, and explains how available memory affects performance of the program:
  •  

The amount of physical memory available on your computer affects the performance of all your Windows applications, not just Solid Edge. When the physical memory is completely allocated, some operations are swapped to virtual memory. Virtual memory is disk space on your hard drive allocated for use when physical memory resources are not available.

 

Virtual memory is much slower than physical memory. When any application has to swap information between virtual memory and physical memory to complete a task, system performance slows down considerably. You can improve performance by increasing available physical memory in the following ways:

 

   Reduce the demand for physical memory

   

    Install additional physical memory in your computer

 

Note

See the readme.htm file in the Solid Edge folder for additional information on memory recommendations for Solid Edge.

 

You can reduce the demand for physical memory in 3 different methods:

 

Hide components: This allows you to unload the display data of the components. It also makes your display less cluttered, allowing you to work more efficiently with the displayed parts.

 

Unloading Components: Once the components are hidden, you can unload them using the Unload Hidden Parts command. This unloads the part from memory, freeing up the memory for other tasks.

 

Inactivate components: This allows you to unload the underlying math data on components, but still maintains the display data. You can see the component and the component will maintain any attached assembly relationships.

 

Of course, if you hide a component, you can also show the component at any time. Likewise, you can activate a component when you need to perform any task that requires the underlying math data.

 

 

Configurations

 

When working with a large assembly, it is common to work on specific areas or sections of the assembly, at different times. Configurations allow you to capture and control isolated displays of those specific work areas or sections. For example, if you are working on a large vehicle assembly, you may want to focus on the rear wheel mechanism. You can inactivate, hide, or even unload, the rest of the assembly. Thus, only showing the components of the rear wheel mechanism. Then you can create a configuration, and call it Rear Wheel Mechanism.

 

 


 

Once you’ve defined the configuration, you can use the Assembly Configuration list in the Home tab > Configuration group, to apply the specific display configuration. This allows you to quickly display, hide, inactivate, and unload specific components.

 


 

Furthermore, when you open an assembly, you can select it to open to a specific display configuration.

 


 

You can also place the configuration into a drawing view, by selecting it from the Drawing View Wizard options.

 

 

 


 

Zones

 

Zones are similar to configurations, but provide additional intelligence, to aid the user. A zone is a defined work envelope, which allows you to see either all the components inside the zone, or all the components inside and overlapping the zone. For example, imagine that you are responsible for the modeling of a conveyer belt sub-assembly, on a large machine assembly. Inside the large machine assembly, you can create a conveyer zone, as shown below:

 

 


 

Like a configuration, you can display only the components inside of the zone.

 

 


 

But you can also display any overlapping components.

 


 

This provides the additional advantage of seeing any components that interfere with your zone, that may have been added by another user. Thus, making zones an ideal tool for large assemblies that are created and modified by multiple users. You also have the same added benefits offered with configurations, allowing you to open an assembly into a specific zone, and allowing you to place specific zones into a drawing view.

 

Summary

 

Display tools, configurations, and zones, are just a few of the tools in Solid Edge, used to accelerate work and improve performance in large assemblies. This article has been a brief overview of these tools. There are many additional options and benefits not covered in this article. Further information can be found in the Solid Edge Help documents, or you can attend one of our Advanced Assembly courses, where we teach all of the methods to deal with large assemblies, plus many more tools for creating, editing, and managing assemblies. The complete course syllabus can be found on our training page, at the following link: http://www.designfusion.ca//technical-training.html. Look for the third part of Working with Large Assemblies in the near future.

 

Working with Large Assemblies – Part 1

John Pearson - Thursday, March 23, 2017

One of the most prominent issues, that has bogged down many CAD systems, is the ability to deal with large assemblies. Despite improved hardware and continuing CAD improvements, this issue is still a top complaint among many CAD users. In some cases, it is the CAD system’s architecture that causes the system to slowdown as the assembly size increases. However, with Solid Edge, most cases we encounter are the result of the user being unaware of tools and/or best practices for dealing with large assemblies. If you are a Solid Edge user, hopefully you are aware of the following tools for dealing with large assemblies:

 

 

  • • Simplified Parts
  • • Simplified Assemblies
  •      ○Visible Faces
  •      ○Model Command
  • • Selection Tools
  • • Display Tools
  • • Queries
  • • Zones
  • • Configurations
  • • Limited Update
  • • Limited Save
  • • Assembly Open As options
  • • Assemblies made of synchronous parts.
  •  
  • Combine these tools with some best practices and other tips and tricks, and you’ll find that large assemblies behave more efficiently and are more reliable in Solid Edge, than any other mainstream CAD package.
  •  
  • In this article, I’d like to focus on Simplified Parts and Simplified Assemblies. I’ll look at how to create them and best practices for using them. First, we’ll look at Simplified Parts.
  •  
  • Simplified Parts
  •  
  • Solid Edge defines a simplified part as:
  •  
  • A part that has had some of its features hidden using the commands in the Simplify Model environment. When you simplify a part, it will process faster in an assembly. You can control whether the simplified version or the designed version of the part is displayed in the assembly.
  •  
  • For an example of a simplified part, let’s look at the following part, which is the back of a clock.
 

 
  • Notice that this part contains, screw holes for attachment, and fill pattern of holes for ventilation. To simplify the part, you start by selecting Tools tab > Model group > Simplify option.

 


 

This creates a separate header in the PathFinder, similar to creating a flat pattern in the Sheet Metal environment.

 


 

You can now use the Delete Faces, Delete Regions, Delete Holes, or Delete Rounds commands to simplify your part. These commands are found on the Home tab, in the Modify group.

 


 

In this example, the Delete Holes command was used to create the following simplified part. Notice the Delete Holes feature under the Simplify header, in the PathFinder.

 


 

In the part environment, you can toggle between the two versions of the part, using the Tools tab > Modal group.

 

        

 

         

 

 

When placed in the assembly, you can select which version you want displayed by using the shortcut menu in the PathFinder.

 


 

This allows you to use the lighter weight, simplified version, in the assembly while you work. But you can easily toggle on the designed part for final display or any other time you may need it.

 


 

Simplified Assemblies

 

Similar to a simplified part, you can create a simplified version of a sub-assembly, to be used in the top-level assembly. Solid Edge provides two methods for creating simplified assemblies. Both have advantages and disadvantages, so it is up to the user to decide which will best suit their needs. Prior to selecting the method, you first have to tell the system that you want to create a simplified version of your assembly. To do this, go to the Tools tab > Model group, and select the Simplify option.

 

 

 

Now you must select either the Visible Faces command, or the Model command, which are the two methods used to create the simplified version of the assembly.

 


 

Visible Faces

 

The Visible Faces command has the advantage of rapid creation of the simplified version of your assembly. The disadvantage is that it is not associative to the designed version of the assembly. When you make changes to the designed version, you have to remember to update the simplified version. Solid Edge defines the Visible Face method as:

 

Creates a simplified representation of an assembly by processing the assembly to show only the exterior envelope of faces and by excluding parts, such as small parts. This improves interactive performance when you use the simplified representation of the assembly as a subassembly in another assembly or to create a drawing of a large assembly.

 


 

Essentially, you create an outer shell of the designed assembly with the option to hide any small components, such as hardware parts, exposed to the outer shell. This is ideal for assemblies with many internal components, that are not visible from the outside of the assembly.

 

Simplified Assembly Model (SAM)

 

The second method is the Model command. This command launches the Simplified Assembly Model environment, often referred to as SAM. Solid Edge defines the Model command as:

 

Creates a simplified representation of an assembly creating a solid representation of the simplified assembly. The solid model is stored as ordered solid geometry within the assembly.

 


 

The SAM environment allows users to create rapid enclosure of the model, and then use ordered modelling to modify the enclosures to better represent the assembly shape. These simplified models are associative to the designed assembly. Plus, you can create simplified version of framed or cage like assemblies, that would be poor candidates for the Visible Face method. The disadvantage is that this can take a bit longer to create, than the Visible Face method.

 

Using the simplified version

 

Whichever method you use, the simplified version can be shown, in a higher level assembly, using the shortcut menu in the PathFinder.

 


 

In the Solid Edge Help documents, under Controlling simplified assemblies, you will find the following table, illustrating the many ways to control simplified assemblies.

 


 

It is important to note that simplified assemblies should only be made if it is a sub-assembly, of a higher-level assembly. Creating them will actually add weight to the assembly itself. However, you can significantly reduce the weight, of the higher-level assembly, when used in the higher-level assembly. Solid Edge best describes this as follows:

 

Simplified assemblies and memory usage

 

When you create a simplified representation of an assembly, the data storage requirements for the assembly document increase because the surface data for the simplified representation is stored in the assembly document.

 

The size increase required to support the simplified representation is small when compared to the size requirements of all the documents that make up the assembly.

 

When you place a simplified assembly document as a subassembly into another assembly, the memory requirements required to display the higher-level assembly drop dramatically. This improves performance and also allows you to work with larger data sets more effectively.

 

This performance improvement also applies when creating a drawing of a simplified assembly. Because less memory is required to support the simplified data set, the drawing views will process quicker.

 

Summary

 

As mentioned in the beginning of the article, Simplified Parts and Simplified Assemblies, are just two methods of dealing with large assemblies. The intent here is to make sure you are aware of them and provide an overview of their benefits. The detailed creation and use, of these tools, require much more space than allotted for this blog. Further information can be found in the Solid Edge Help documents, or you can attend one of our Advanced Assembly courses, where we teach all of the methods to deal with large assemblies, plus many more tools for creating, editing, and managing assemblies. The complete course syllabus can be found on our training page, at the following link: http://www.designfusion.ca//technical-training.html. Future blog articles will provide further overviews of the other tools for dealing with large assemblies.