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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



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.





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 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.




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: 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.




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: Future blog articles will provide further overviews of the other tools for dealing with large assemblies.


How to Export Quality Images in Drafting

Stephen Rose - Tuesday, January 03, 2017



  • This FAQ explains the steps to generate quality shaded image views in drafting, including the use of translucency. 




  • Understanding of Modeling and Drafting environments in NX


Step By Step Process…

  • 1.Generate your solid body, or load an existing solid part, and adjust translucency as required.
  • 2.Switch to the Drafting environment and generate a sheet.
  • 3.On the top ribbon select the <File> Tab, then choose Preferences -> Drafting



  • 4.Under the <View > expandable menu select <Workflow>, then scroll down until you see the Visual Settings group in the right-hand pane.In that group check <þ> Use translucency and <þ> Use Line Antialiasing then select <OK>.(n.b. See end of document for anti-alias impacts)
  • 5.Place a view of your choice on the sheet drawing (the default will be a wire-frame view.



  • 6.Select the drafting view boundary, right-click and choose Settings
  • .
  • 7.For best results, in the left-hand pane, under the <Common> expandable menu select <Configuration> , and in the Settings group in the right-hand pane set preference to Exact Representation, rather than Lightweight.You can specify the curve tolerance here also.



  • 8.Now scroll down further in the left-hand pane and select <Shading>, and in the Format Group in the right-hand pane change the Rendering style from Wireframe, to Fully Shaded.Make any other adjustments needed for surface Shininess, then in the Tolerance group select one of the default Tolerances, or chose Customize to edit manually.Then click <OK>.



  • 9.You will then see results similar to this:



  • 10.You can then set other view dependent preferences if you want hidden lines, or smooth lines, shown different than the default setting.      Default


      Smooth Edges lightened


      Hidden lines processed


  • 11.Once your views are set you can use File->Export->pdf, you can use File->Print to a pdf, (with Export shaded views as wireframe left Unchecked), or you can File->Plot to plot to a suitable configured printer--or even plot out to a graphics format such as TIFF.


n.b.Out of the Box the Graphic Plotting format resolution is set quite low.If you need a higher resolution you can go into the plotter administration and change the values.

  • 12.To set these Graphic Formats resolutions go to File->Utilities->Printer Administration, you are then prompted to Edit the printer setup or Create a new one.(See the Plotter Setup documentation for this initial setup.)Once you are in the Edit menu, you will see the <Graphics Default> tab, under that tab are the types of graphic formats for plotting to. You can edit each of their default resolutions here.



Anti-Alias Notes in Drafting Mode:


Anti-alias choices can make an impact on how well your shaded surface edges show up on the drawings.The two pictures directly below show the Drafting Preference setting “Use Anti-Aliasing”



Use Anti-Alias Unchecked (OFF)               Use Anti-Alias Unchecked (ON)


Adjusting Full-Scene Antialiasing toggle, can also sometimes improve results.


ST9 Assembly In context Contour Flange

Manny Marquez - Thursday, October 13, 2016


Check out our other videos here

Moldwizard Series

Stephen Rose - Thursday, October 06, 2016

Check out our 3 part MoldWizard Series


Part 1:



Part 2:



Part 3:




Ways to help with Keyshot

Cory Goulden - Wednesday, September 14, 2016


Have you have ever been asked to create an image or snapshot for any reason and the model that you created in SE does not have the level of detail required? Maybe there are holes in a sheet that are not there (for performance reasons for example). Maybe a hose is just a tube but you want it to appear to have a ribbed type look to it? Keyshot might be the solution.


We, as CAD designers, make a cognitive decision to keep things simple as best we can. Let’s take a look at how we can utilize Keyshot to do some of the heavy lifting in this case.


We can start with a simple tube in Solid Edge. We need to produce a picture of this tube but it needs to look corrugated. Quickly we can take it into Keyshot. This is where the fun starts.


              Start                                                                                                    Finish



This is easily accomplished by using the thread face style in Solid Edge and then going into Keyshot.



What’s that? Too easy or doesn’t look good enough. Okay we can apply a hard black plastic to it in Keyshot. That makes the cylinder look good but we need to apply a texture to it. On the left hand side of the Keyshot menu under the textures tab you can select the “Horizontal_Tubes_Normal”. As usual with Keyshot it is as simple as dragging and dropping onto our model. Next go to the right side menus of Keyshot and let’s edit the properties of this texture. From the Project menu under the Materials>Textures tab (As illustrated below) I changed the Scale to .1 and the Bump Height to 2. For this model those sizes give me what I want to see.





This looks great and I did not have to model the corrugation. A mistake some users can make. You may not need the information in the CAD model but you may need to show it in screenshots or documentation. Try doing it in Keyshot. I am sure you will have impressive results!


“But you also said holes in a sheet” is what you are thinking now….I know I know. Great tools here too.


For example, we design holes that have specific purposes. But let’s say we need a perforated sheet. We have a solid sheet in Solid Edge and take in into Keyshot.


First option here is to apply a material type (such as “Aluminum Circular Mesh) to the sheet. This gives us circular cut-outs in the material. Again you might need to adjust the parameters. As you can see, you can see right through it.



You could modify the colours from there is need be.


You could also apply a Texture to an applied material as we did before in the above steps.


This is a simple process to have fast performing models in Solid Edge and also be able to produce what might be required for presentations, documentation, or to others. Keyshot makes it easy!





NX CAM: Eliminate wasted cutting motions on overhanging blank material

John Pearson - Thursday, July 28, 2016


Regular readers of our blog may recall my last NX CAM article, where I stated that many improvements to the software are missed due to lack of upgrade training. I gave several reason for this, which I’ll not repeat. If you’re interested, you can read the article:


Continuing on the theme from that article, I’d like to highlight another recent improvement that may have been overlooked by some users. This improvement focuses on eliminating some wasted cut motions. My old boss, back in my CNC programming days, used to always remind me that machine time was more valuable than my time. It was his way of saying that he wanted us to make our programs as efficient as possible. So I was trained to always look for cutting efficiency. Perhaps that is why this enhancement caught my eye. This was introduced in NX9, so if you haven’t upgraded to NX9 or NX10, you have to do this manually. Let’s first look at the scenario.


I have a part to be machined, along with my defined blank geometry, as shown below.



Let’s assume that I rough out the bottom of the part first, using cavity mill.



Next I’ll want to rough out the top. I define my cavity mill operation and set the containment to use the IPW (in process workpiece). In other words, my blank becomes what was left after the last operation.



The image below shows the blank material after the bottom rough cut.



Prior to NX9, my cutting path would look like the following image.



Notice that the tool roughed the top, but it continued to cut the bottom half which had already been roughed away. In NX9 they added an enhancement which omits cuts that remove insignificant amounts of material from overhanging IPW’s. So in NX9, under the Strategy tab, you will see a new option called Cut Below Overhanging Blank.



If this is turned on, you will get the old pre-NX9 results, as shown above. If it is turned off, your path will generate as shown below.



Notice here that no cutting motions are wasted trying to remove the IPW left behind by the previous operation on the underside of the part. This could add up to some significant machine time savings for your company.


I will continue to highlight some of the newer NX CAM enhancements in future blog articles. But keep in mind that this is a slow way to learn about improvements. For example, had you attended an NX9 upgrade course, you would have learned this enhancement and more, almost 2 years ago. Imagine how much machine time that could have been saved; definitely enough to pay for the course and much more.


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, For our training schedule, please visit our events page at,


For more information and quotes, contact your Account Manager, or contact us at


NX CAM: Options for selecting cut areas

John Pearson - Thursday, May 26, 2016


With the daily grind to meet production schedules, it is often difficult to keep up with all the changes to NX CAM software. I have spoken with many users who are basically still using methods that they learned from their first CAM course(s), despite the fact that there now exist more efficient ways of doing things. The primary reason for this is that they have not received any update training. Some companies expect the users to learn on their own, yet fail to provide time to do so. Others don’t see the value in upgrade training, or insist that their users simply don’t need it. Whatever the excuse, training always seems to be the lowest priority, until issues arise. I have even known companies who have even investigated changing software, when the far less expensive option of training would provide them with all that they need.


With this in mind, I thought it may be ideal to review some of the newer and more efficient ways of doing things in NX CAM. For this blog article I’d like to focus on the new options for cut area selection, added to the fixed and variable contour operations, in NX9. You can now define Cut Areas, for these operations, by selecting a seed face and bounding edges that form a closed loop.


Example 1 : Let’s start by looking at a simple example where I use a seed face inside a single loop. Here I have a Contour Area operation for the part you see below.



I start by selecting the Specify Cut Area option. I then use the new selection method that has been added. This method is labeled as Edge Bounded Region, and is found in the Selection Method list.



With this new option selected, all I have to do is select a seed face, as shown below.



Then I select the bounding edge as shown below.



Tip: To ensure the selection of the tangent curve, I make sure that the selection intent, on the Top Border Bar, is set to Tangent Curves .



I then click on Preview Region, and notice that I have selected this entire region with minimal mouse clicks.



Example 2: This example shows the selection of a single seed face that is found between two containment loops. Using the same part and operation as in Example 1, I start by selecting Specify Cut Area. I select the Edge Bounded Region option from the Selection Method list. This time I select the seed face shown below.



As before, I use the Tangent Curves selection intent to select the top closed loop.



I then select the bottom closed loop.




These two closed loops form the exterior and interior containment loops and when I select Preview Region , I am shown the selected area.



If you expand the Region Options on the Cut Area dialog, you will see 2 other options, the Traverse Interior Edges option, and the Use Tangent Edge Angle option.



The next two examples will look at these options.


Example 3 : Using the Traverse Interior Edges option.


In this example, I expand on Example 1, where I have already selected the faces as shown below.



But in this example, a boss and an additional edge blend has been added to the model.



If I use the same selection method as in Example 1, but also toggle on Traverse Interior Edges, the Preview Region shows me the following selection area.



Example 4 : Using the Use Tangent Edge Angle option.


In this final example, I have modified the part by removing the top edge blend. By removing the edge blend, the normal vectors between the faces now form a 30-degree angle.



I start by selecting Specify Cut Area. I select the Edge Bounded Region option from the Selection Method list. For my seed face I select the bottom face.



For the bounding edge I select the four exterior edges shown below.



Next, I toggle on the Use Tangent Edge Angle option and set the Angle Tolerance to 25.0000, as shown.



When I generate my operation, I notice that the top planar face is ignored. This is because the normal vectors between tangent faces exceed the specified 25-degree Angle Tolerance, therefore the adjacent face is not included in the cut area.



Rule: If the normal vectors between tangent faces equal or exceed the user specified Angle Tolerance, the adjacent face is not added to the contained area to be machined.



As you can see, these new options are more efficient than the previous method for selecting a cut area. And this is just one of the many new tools added in recent years. NX CAM continues to improve its technology, but it is up to you, the user, to learn about these improvements. It has been my experience that this does not happen unless the user is allowed the time to learn. The most cost effective way for users to improve is through professional training. Update and custom courses are available through either Siemens Training or through Designfusion. For more information, contact your Account Manager or contact us at



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.