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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.

 

ST9 Assembly In context Contour Flange

Manny Marquez - Thursday, October 13, 2016

 

Check out our other videos here

New – Standalone Advanced Draft Course

John Pearson - Thursday, July 07, 2016

 

As Solid Edge’s capabilities expand, so too must we expand our ability to utilize the latest capabilities. With this in mind we have created a new, standalone advanced draft course. We use to teach advanced draft capabilities as part of the advanced modeling course. However, we felt that it wasn’t doing the topic justice. So we have created a 2-day course focused on the Solid Edge Draft environment.

 

This new course builds on the draft training from the fundamentals course. It takes the user to new and deeper levels of knowledge and expands their capabilities. Upon completion, students will be able to create, and manipulate, draft templates. They will also have a greater understanding of how to manage and manipulate the views, dimensions, annotations, styles, and tables, in the Draft environment. The course content includes:

 

Day 1

 

Module 1: Draft Templates 

– Draft Templates

  • Global Settings

  • Background Sheet

  • Boundaries, Title Blocks, and Logos

  • Callouts

  • Working Sheet

  • Saving the template

  •        • Template locations

 

Module 2: Advanced View Control 

– Advanced View Control

  • DV Wizard saved settings

  • Rapid population of draft template

  • Draft Quality drawing views

  • Drawing View Display Depths

  • Locking a drawing view

  • Modify a drawing view cropping boundary

  • Advanced Detail View option

  • View Alignment of Break Lines

  • Drawing View Styles

 

Module 3: Advanced View Editing 

– Advanced View Editing

  - View Activation

  - View properties

  - Track Dimension Changes

  - Drawing View Tracker

  - Force Drawing Views to Update

 

Module 4: Advanced Dimensions 

– Advanced Dimensions

  • Smart Dimension Hot Keys

  • Coordinate Dimension options

  • Symmetric Dimensions

  • Attach Dimensions

  • Add Jogs to Dimension

  • Insert a vertex in a leader

  • Dimension Styles

  • Copy Attributes

 

 

Day 2

 

Module 5: Advanced Annotations 

– Advanced Annotations

  • Advanced control over center lines and center marks

  • Stacked Balloons

  • Special Symbols

  • Reference Text

  • Technical Text note

  • Format Code

  • Annotation Alignment Shape

 

 

Module 6: Parts List and Tables 

– Parts List and Tables

  • Parts List Properties in detail

  • Tables Styles

  • Pull Assembly or Model Out of Assembly Context

  • Hole Table

  • FOP Tables

  • User-defined Tables

 

 

Module 7: Automated Draft Tools 

– Automated Draft Tools

  • Dimension Alignment

  • Dimension Automatic Arrangement

  • Automatic Centerlines

  • Perspective Views

  • QuickSheet Template

  • Sheet Compare

  • Batch Printing

 

Module 8: Miscellaneous Tools 

- Layers

  - Blocks

  - Symbols

  - Revision Manager

 

This advanced knowledge will allow the student to improve on both qualities of, and efficiency in, their draft documents.It significantly advances the capabilities in creating and modifying draft documents, and has been professionally designed to maximize return on investment.

 

This course, which is unique to Designfusion, adds to our list of courses already offered by our professional trainers. For a complete list of our courses, please visit our technical training page at, http://www.designfusion.ca//technical-training.html. For our training schedule, please visit our events page at, http://www.designfusion.ca//events.html.

 

For more information and quotes, contact your Account Manager, or contact us at info@designfusion.com.

 




How to copy a whole set of files from a project

Dominic Benoit - Tuesday, May 03, 2016

Depending on the folder structure used in your company, links between Solid Edge files can sometimes be spread all over the file system. The task to consolidate all files may seem impossible, but often essential for various reasons. You must already have tried to copy all using Windows Explorer, but you always keep the feeling of having forgotten well-hidden part files.

 

The Revision Manager is the ideal tool in order for grouping, or even for restructuring files.

 

Method of grouping: (such as for sending by e-mail)

Only downlinks will be found and copied.


  • 1-Open the general assembly

 


 

  • 2-Starting from the left to the right, click the buttons in the following order :
  •    a.Expand All
  •    b.Select All
  •    c.Copy
  •    d.Set Path

 


 

  • 3-Select the destination folder. Create one if necessary with the New Folder button.
  • 4-Confirm that all actions are properly prepared.

 


 

  • 5-Click Perform actions


 

Your documents are copied to the specified single folder.

 

Copying method, keeping the original structure :

Only downlinks will be found and copied.

  •     1-Open the general assembly

 


 

  • 2-Starting from the left to the right, click the buttons in the following order :
  •     a.Expand All
  •     b.Select All
  •     c.Copy

 


 

  • 3-You must now change the path of your copy:
  • a.Click on Replace 

  •  
  • b.Enter the beginning of the path that is common to all files in the Find What box.
  •     i.Ex 1. F:\00_Demos\Quicklooks
  •     ii.Ex 2. F :
  • c.Enter the beginning of the destination path for all files in the Replace with box.
  •     i.Ex 1. G:\Copy
  •     ii.Ex 2. G :
  • d.Click on Replace All

 


 

  • 4-Confirm that all actions are properly prepared.

 


 

  • 5-Click on Perform Actions.

  •  
  • 6-You then have a message offering you to create missing folders in the destination. Answer Yes, the folders will be created as specified in step 4.

 

Your documents are copied to the specified folder by creating the structure.

 

Full copy method:

 

The downlinks and uplinks will be found and copied.

  •     1-Open the general assembly

 


 

  • 2-Starting from the left to the right, click the buttons in the following order :
  •     a.Expand All
  •     b.Select All
  •     c.Copy

 


 

  • 3-Do a Where Used to find the .DFT documents referring to these 3D models.
  •     a.Tools-> Where Used
  •  


 

  • 4-Identify the folders to crawl for the search.
  •     b.Click Add to include the desired folders in the right column.
  •     c.Click on Process Options to select only the .DFT file type.

 



  •  
  •     d.Click on Next to start the search.
  •     e.Selected AND found files will be listed at the bottom of the screen.
  •  
  • 5-Use one of the previously proposed methods to specify the destination of copies.
  • 6-Click in the lower pane, you need to select the .DFT files to apply the same copy / destination strategy.
  •     f.Click on Select By Type.


 

  •     g.Choose the .DFT files, then OK
  • 7-Click the action button Copy, and use a previously proposed method for specifying the destination of copies.

 


 

  • 8-Confirm that all actions are properly prepared.
  • 9-Click on Perform Actions.

  •  
  • 10-You then have a message offering you to create missing folders in the destination. Answer Yes, the folders will be created as specified in step 4.

 

Your documents are copied to the specified folder by duplicating all the structure.

 

 


How to copy a whole set of files from a project

Dominic Benoit - Tuesday, March 08, 2016

Depending on the folder structure used in your company, links between Solid Edge files can sometimes be spread all over the file system. The task to consolidate all files may seem impossible, but often essential for various reasons. You must already have tried to copy all using Windows Explorer, but you always keep the feeling of having forgotten well-hidden part files.

 

The Revision Manager is the ideal tool in order for grouping, or even for restructuring files.

 

Method of grouping: (such as for sending by e-mail)

Only downlinks will be found and copied.


  • 1-Open the general assembly

 


 

  • 2-Starting from the left to the right, click the buttons in the following order :
  • a.Expand All
  • b.Select All
  • c.Copy
  • d.Set Path

 


 

  • 3-Select the destination folder. Create one if necessary with the New Folder button.

  • 4-Confirm that all actions are properly prepared.

 


 

  • 5-Click Perform actions 
  •  

Your documents are copied to the specified single folder.

 

Copying method, keeping the original structure :

Only downlinks will be found and copied.

  • 1-Open the general assembly

 


 

  • 2-Starting from the left to the right, click the buttons in the following order :
  • a.Expand All
  • b.Select All
  • c.Copy

 


 

  • 3-You must now change the path of your copy:
  • a.Click on Replace 

 

  • b.Enter the beginning of the path that is common to all files in the Find What box.
  • i.Ex 1. F:\00_Demos\Quicklooks
  • ii.Ex 2. F :

  • c.Enter the beginning of the destination path for all files in the Replace with box.
  • i.Ex 1. G:\Copy
  • ii.Ex 2. G :

  • d.Click on Replace All

 


 

  • 4-Confirm that all actions are properly prepared.

 


 

  • 5-Click on Perform Actions
  •  
  • 6-You then have a message offering you to create missing folders in the destination. Answer Yes, the folders will be created as specified in step 4.

 

Your documents are copied to the specified folder by creating the structure.

 

Full copy method:

The downlinks and uplinks will be found and copied.


  • 1-Open the general assembly

 


 

  • 2-Starting from the left to the right, click the buttons in the following order :
  • a.Expand All
  • b.Select All
  • c.Copy

 


 

  • 3-Do a Where Used to find the .DFT documents referring to these 3D models.
  • a.Tools-> Where Used

 


 

  • 4-Identify the folders to crawl for the search.
  • b.Click Add to include the desired folders in the right column.
  • c.Click on Process Options to select only the .DFT file type.

 



 

  • d.Click on Next to start the search.
  • e.Selected AND found files will be listed at the bottom of the screen.

  • 5-Use one of the previously proposed methods to specify the destination of copies.

  • 6-Click in the lower pane, you need to select the .DFT files to apply the same copy / destination strategy.
  • f.Click on Select By Type.

 


 

  • g.Choose the .DFT files, then OK
  • 7-Click the action button Copy, and use a previously proposed method for specifying the destination of copies.

 


 

  • 8-Confirm that all actions are properly prepared.
  • 9-Click on Perform Actions
  •  
  • 10-You then have a message offering you to create missing folders in the destination. Answer Yes, the folders will be created as specified in step 4.

 

Your documents are copied to the specified folder by duplicating all the structure.

 


Solid Edge and Keyshot : how does it work? Chapter 2

Francis Robert - Tuesday, February 23, 2016

Here is the conclusion of the article on the interaction between Solid Edge and Keyshot.Make sure to read Chapter 1 first!

 

To simplify the text, SE = Solid Edge and KS = Keyshot…


  • 1. Take advantage of Keyshot’s behavior

 

We saw that KS reads SE files and reproduces the assembly / sub-assembly / part structure tree.Keyshot also adds another level based on the SE Face Styles used in the CAD model, most of these colors were added with SE’s Part Painter tool.

 

This will allow you to « cheat » easily the look of parts without the need to double part count or any other acrobatics. Note that multi-body SE files don’t change KS’ behavior.


  • 2. How about a concrete example?

 

We want to show a single part with machined faces. To do this in Keyshot, first use Solid Edge Part Painter and apply different face styles to the machined faces, prior to send to KS. The actual color doesn’t matter but remember that KS has a powerful search and select tool that can read Face Styles’ names.Use it to your advantage!

 

Example: First steps in Solid Edge: on the left side, a single part containing multi-bodies on which we used the Part Painter. On the right side, also a single part containing multi-bodies but they have a single color.

 


 

Let’s see how the structure looks like when you send the model to Keyshot:

 


 

We can clearly see the « main » structure (one top-assembly, two parts). We also see the additional level KS created, based on the Face Styles used in SE. The left side multi-body partshows each face style used under the « Material » column (Grip, Orange, Blue, etc). The right-side multi-body part only shows a single level since we used a single face style for both bodies in SE (Teal).

 


 

Keyshot will be able to apply a material to each face sets shown in the « Material » column. Because of this, the right-side part is condemned to use a single color.Keyshot 6 Pro offers a way to split bodies and faces (see below) but you’re stuck if you don’t have this version of KS.As it stands right now, the right-side part bodies can only have the same color.

 

Example: We applied some materials to the left-side part. It contains multi-bodies but we also used Part Paitner on some faces.By using the right technique, we were able to apply a “machined” material to one of the face of the cube, as well as a textured black rubber grip on the orange handle.

 


 

  • 3.I still want to split bodies on the right-side part to apply different colors. What can I do?

 

The answer depends on which Keyshot version you are using!


  • a.Keyshot for Solid Edge (SE Classic or Premium)
  • i.Go in SE, using Part Painter apply a different face style to each face you want to individually control.Use different colors for each face sets as they   will be grouped in KS.Update your render.

  • b.Keyshot Pro 5 and previous
  • i.There are no other solutions than editing the source geometry file.If your source files are Solid Edge, or can be edited by SE, use the Part Painter technique defined above.

  • c.Keyshot Pro 6
  • i.Use the brand new « Geometry Editor » tool which allows you to split elements (face, bodies, tesselation triangles) directly in your KS session.This tool is really cool and will save you tons of time! We can also change the face vector, for example, to control grain direction.

 

Using KS 6 Pro Geometry Editor, we choose which operation we want to execute:

 


 

We graphically choose which body or face we want to split from the main group:

 


 

Hit “Done” and we can now apply different materials on each body:

 


 

  • ii.Please note that this process will break the « Live Linking » with the Solid Edge model.You will be prompted with a warning message.If you want to maintain the live link with the SE model, use the Part Painter method instead.

 


 

I hope this will help you better control your renderings and make you more efficient. Don’t hesitate to send me your questions and comments.Happy Rendering!

 


Solid Edge and Keyshot : how does it work? Chapter 1

Francis Robert - Tuesday, February 16, 2016

 

In this article, I will focus on the Solid Edge / Keyshot interaction and their capability to update a render rather than starting from scratch after a CAD change.Wheter you use the Keyshot for Solid Edge version (Classic and Premium licenses) or the Keyshot Pro version, you need to understand how these two applications work with each other.You’ll be able to use this behavior to your advantage.

 

In order to simplify the text, SE = Solid Edge and KS = Keyshot.


  • 1. « Live Linking » option

 

Make sure that this mandatory option is enabled in Keyshot.Go in the menus « Edit -> Preferences », select the « Advanced » section and validate that “Enabled Live Linking” is checked on.

 


 

  • 2. Keyshot and Solid Edge’s face styles

 

Keyshot reads Solid Edge’s face styles in its own fashion.Keyshot will maintain the assembly / sub-assembly / part structure you already defined in SE, but i twill also add another level.This additional level is related to the face colors (SE Face Styles), so it’s closely tied to SE’s Part Painter tool and how you used it.

 

We’ll go deeper into this topic in the next chapter.

 

Example: The geometry below comes from a single part file containing multi-bodies. Using the right technique, we were able to apply a machined texture to one a face on the cube and a textured rubber material on the orange handle.

 


 

  • 3.How should I prepare my Solid Edge model before sending to Keyshot?

  • a.Only the displayed geometry will be sent to KS. Make sure to show or hide the correct geometry before you launch KS.You can also display construction surfaces, they will go in KS.However, other construction elements like curves, sketches and PMIs will not go through.

  • b.Add required « scene » elements.Keyshot supplies a « ground floor » but do you need some walls, roof or other additional elements that will enhance your render? Add them in the CAD if you can before sending to KS.

  • 4. My Solid Edge model changed, what should I do with my Keyshot render?

 

There are two ways to update an existing KS render when the SE model changed.Note that saving is independent in both applications, so make sure to save your files in both SE and KS.


  • a.If you didn’t close your applications …

  • i. There is a « Keyshot Update » button in SE.This button is enabled only if SE and KS sessions were not closed.Simply click the button and the KS model will update.

 


 

  • b.If you closed your applications…

    • i.The « Keyshot Update » button will be disabled but the update feature is still available! First, open your BIP file in Keyshot.Then, open your SE model and hit “Keyshot Render”.

  • ii.Keyshot will recognize if the SE model was used in the KS session.You will see the following dialog box.You’ll have the option to update the current KS sessions (select Yes) or create a new render session (select No).

 


 

  • 5.I’m updating an existing render file, what should I expect?

  • a.Keyshot looks into what changed in the SE model and updates only what is required in KS. What changed in SE will be updated (dimensions, color, location, display state, etc).What didn’t change in SE will not be affected in KS.

  • b.Example 1: We applied a Material to a part in KS.We change the Face Style (color) in SE, then we update the render. Result: The part color will be extracted from the SE Face Style.

  • c.Example 2: We applied a Material to a part in KS. We make some changes in SE but we don’T change the part’s face style, then we update the render.Result : The part will maintain its association with the KS material and not change color.

  • d.Example 3: We moved a part in Keyshot. We make some changes on the SE geometry (dimensions, features, etc) which doesn’t affect the part’s face style, then we update the render.Result: The part will maintain its “overridden” location in KS but its geometry will be updated.

 

Come back here to see the next chapter on the Solid Edge / Keyshot interaction. Don’t hesitate to submit your questions or comments.Happy rendering!

 


 


Common mistakes in Rendering

Francis Robert - Tuesday, February 09, 2016

In this article, I’d like to expose common mistakes made by users when rendering their products. I saw too many bad images on web sites or other marketing documentation to state that modern rendering technology solved all problems.You have the tools to create really nice images; it’s up to you to use them to your advantage!

 

Everyone has a different level of artistic sense.It will obviously influence the result but I hope that by following these simple rules, you will create remarkable imagery.So, whether you’re the next Picasso or can’t draw a stick figure, you won’t have any excuses anymore.


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  • 1.Starting point
  •  

Where should I begin?An interesting model will be easier to work with, of course, but we can still make a rectangular welded frame interesting.First : what NOT to do…

 


 

Dont’ laugh!I still see these kinds of images in some Case Studies! A Solid Edge direct screen capture can still be acceptable in many cases but you need to make some sort of effort…

 

  • a.Hide construction elements (coordinate systems, reference planes, sketches, PMI, etc) unless they are absolutely necessary. A simple right-click in     the graphics zone will help you do this in seconds.
  •  
  • b.Crop the image so you don’t see the Edgebar, the Quick View Cube and how many Internet Explorer tabs you have opened.Focus on your product!
  •  
  • c.Use gradient background.Many of you miss the old Solid Edge V12 background but still…
  •  
  • d.Activate the high-quality display parameters. Raise the Sharpness and “anti-aliasing” levels.Activate floor reflection unless it causes distractions.Enable Perspective angle set to 35mm first, then tweak if required. Don’t hesitate to explore settings and save a 3D View Style to reuse later.

 


 

Let’s see what Solid Edge can look like, even without Keyshot:

 


 

Much better, isn’t it?

 

  • 2.Shifting in second gear!
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If you’re not satisfied with the image quality rendered by Solid Edge alone, level up by sending your model to Keyshot. In Solid Edge, go to the Tools tab and hit “Keyshot Render”.Let’s look at the “as-is” result, created by Keyshot by default:

 


 

Again, much better, no?Reasons why this is better are both simple and complex but one of the main reason is the lighting. By default, Keyshot lights up the model using its “Environment”.This is a rectangular high-resolution image wrapped on a sphere surrounding the model. Each pixel of this wrapped image acts as a light source, which gives a natural light and feels similar to what your eyes are used to see.

 

Moreover, the same environment image is used to generate reflections on the polished material present in the model. A simple change of environment can make a huge difference on the look of a render.Browse the Environment library, select an image you like and drag it in the graphic window of Keyshot.

 


 

Many control parameters are available to tweak the environment. See it for yourself in the Project section, Environment tab.For most users, simple parameters like contrast, brightness and rotation angle will be sufficient.Keyshot Pro adds a “HDRI Editor” tool, enabling you to modify the default environments supplied in the library and create your own.


  •  
  • 3. More materials, less reflections!

 

There is a lot to say about Materials in Keyshot.I use the word « Material » because this aspect regroups color, texture, reflection, transparency, refraction and even decals.It’s far from a simple color!Let’s see common mistakes made at the Material level:

  •  
  • a. Material mistake #1: Changing idea during the process…
  • The look of a material is strongly influenced by its environment and its camera point of view as well.This is even more obvious for “brushed” textures (stainless steel).Always define the cameras and environment before starting to tweak the materials.If you don’t, chances are you’ll have to start over again if you changed environment and point of view.
  •  
  • b. Material mistake #2: Sharp edges…
  • In many industries, we model parts quickly without « removing sharp edges ».This is good for production, not for the CAD guy, but for rendering, it’s almost always preferable to add fillets and radii everywhere.The result will be much better and natural looking reflections than with perfectly sharp edges.
  •  
  • c. Material mistake #3: Mirrors… mirrors everywhere!
  • You polished your model and applied mirror-like materials everywhere.This may have been a good idea at the time but your final image will hurt from this decision.One aspect is the render calculation performance going down a bit but mostly, it will be hard to distinguish the model surfaces, parts and even the background.

 

Let’s look at an example which combines mistakes #2 and #3.Polished material (Roughness is at 0.008) and sharp edge(zero radius):

 


 

Let’s add some rounds and fillets. You can do this in the CAD or with Keyshot Pro 6, use the “Rounded Edges” setting located on the bottom of the Scene tab (Project section).We also changed the Roughness value to 0.1 to reduce the mirror effect.See the difference with the image above:

 


 

  • 4.Conclusion
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Following these simple rules, you’ll be able to create beautiful realistic images of your products… without going to Art School!To conclude, let’s see the same model as our starting point rendered in Keyshot. The left side has sharp edges and polished material everywhere, the right side followed the guidelines. Happy rendering!

 

 

 

Using IFC files with Solid Edge ST8

Francis Robert - Tuesday, February 02, 2016

Solid Edge ST8 can now import and export « IFC » files. This “Industry Foundation Classes” format is actually a neutral 3D file which allows sharing geometry and properties between a CAD tool and “BIM” applications (Building Information Modeling).We could compare an IFC file with a STEP file for example; difference is that the IFC format also contains a suite of properties used in the Construction and Architecture industries.The IFC format is developed by an international committee and is not owned by any CAD vendor in particular, therefore the “neutral” file nickname.

 

Solid Edge ST8 supports two types of IFC files, IFC2X3 and IFC4. The IFC2X3 type doesn’t contain precise geometry (Brep is NOT supported) and less properties.This type is closer to a STL or JT (without precise geometry) file.Whenever it’s possible, it’s better to use the later IFC4 type.It’s more recent, does support precise geometry (Brep) and can carry more properties.These properties are closely tied to the Construction industry, like electrical consumption for example.The application that reads the IFC4 type will be able to add the geometry to its general layout, automatically going on the correct Field / Building / Story, adding the electrical consumption to the overall building consumption, for example.Please note that you need to install Solid Edge ST8 Maintenance Pack 3 in order to manage these additional properties.


1. Simplification

 

We strongly suggest simplifying the geometry before exporting the model to the IFC format.While you can always export the model as is, your partners and customers will appreciate the fact you took some time to remove unnecessary details (hardware, internal components, etc.). When your product is positioned into a building, you can remove details without impact.By simplifying geometry, the global performance will be much better and you won’t share all the fabrication details (and intellectual properties) with your customers.

 

Solid Edge offers efficient simplification tools at the part level as well as at the assembly level. This allows you to remove faces not required in the final model (chamfers, fillets, internal details, etc.) while keeping a single file per part to maintain.

 

Solid Edge will export the IFC model in its « as displayed » state. So if non-required parts are displayed, you should hide them before exporting, check the correct option, and the IFC model will look exactly as you want to.Same thing applies to the “Design” or “Simplified” display state of parts.


2. Properties management

 

Before exporting to IFC format, you need to make sure the properties are defined correctly.This is the primary purpose of this format.If there were no benefit in sharing properties, you could simply use existing neutral 3D formats like STEP and Parasolid.

 

For type IFC2X3, the list of properties is limited to Author, Organization, Program and Description). We access these properties via the IFC export options.In Solid Edge, select Save As, then the IFC format and the Options button will become available.

 


 

Type IFC4 is more recent and can carry as many properties as desired.Again, in the IFC export options, you can select « Include IFC properties ».This enables the link to an Excel spreadsheet used to define properties groups, names, types and values.We can have as many spreadsheets as required.

 


 

The default XLSX file supplied with Solid Edge is located in the Program sub-folder of the ST8 installation folder. There are instructions in the first tab and a suite of properties given as an example.We suggest backing up this file and using it as your foundation to define your own list of properties.

 

Each of the following tabs is used as a property group. Each group contains a list of properties, each with their name, value and type.You can create and remove groups and properties to make sure to cover the needs of each of your projects.For multiple customers with different needs, we suggest to create a spreadsheet for each one of them.You’ll only need to select the appropriate spreadsheet when exporting your model.


  • Portions of the default XLSX file supplied with ST8 MP3:



  • For example, group « Pset(Common) » contains general properties for every basic IFC file. Another groupe like “COBie” (Construction Operations Information Exchange) corresponds to generic properties used in the Construction industry without regards to actual geometry.


3. Export

 

Once the model is simplified and the properties correctly defined, you just need to hit « Save ».You’ll see file size compression in the process, especially with the older IFC2X3 format.


4.Import

 

Solid Edge ST8 can also import IFC files.You will probably see additional assembly levels than the model you exported. Since IFC format is aimed at Construction projects, it will add a couple of levels of sub-assemblies above the actual model.They correspond to Construction Site / Building / Story.This allows architects easier management of building components.

 

If you import an IFC2X3 type, you won’t be able to select the geometry in Solid Edge.This is because the geometry is faceted data, not precise geometry.You only have the « visual » portion; there is no « mathematical » portion (Brep).Therefore, the IFC2X3 usage is very limited when opened in a CAD tool but you can still use it as a reference. You will not be able to select a keypoint, create a draft, display visible edges or even do a boolean operation.This is similar to the usage of a STL or JT (without precise geometry) in Solid Edge.

 

If you import an IFC4 type, you will remove the limitations mentioned above. IFC4 contains the “Brep”, so there is precise geometry in the file.You’ll be able to use it as with any other imported CAD format, similar to a STEP or Parasolid.Even the parts’ colors will be imported.

 

As you see, we strongly suggest using the IFC4 type whenever you can.


5. Conclusion

 

With a couple of tries, you’ll be able to find the right balance in the level of details (what do you simplify?) and the list of properties to share with your customers and partners. You’ll be able to share your products intelligently with all architects on the planet in a complete and precise fashion.