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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.

 

How to Export Quality Images in Drafting

Stephen Rose - Tuesday, January 03, 2017

Introduction:

 

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

 

Requirements:

 

  • 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

How to: Reverse Engineer a Feature from a Round Surface

Manny Marquez - Tuesday, December 08, 2015

 

More videos here: https://www.youtube.com/EdgeCanada


NX Isocline Series.Part I of III, the General Isocline Split

Stephen Rose - Wednesday, September 23, 2015

Overview

 

There are common poor-practices in the moulding industry, in this series we will shed light on some.

 

They often occur due to:

 

Lack of internal company best practices; attempting to rush though a project to meet the common compressed deliveries of today’s industry; lack of available tools in competitor software products; lack of awareness by the designer; or sometimes due to lack of training in the functions/tools available to the designer.

 

In this series we will cover several scenarios where the right feature functions, and the right training, can create a better finished product and more stable steel conditions.Stable steel conditions allow the mould to stand up to high production volume and eliminate production downtime due to pulling the mould for repair.Having more of the finished parts being passed through QC inspection, and having less downtime of the mould, both contribute into a lower life cycle cost of the project.

 

The scenarios we are going to cover in this series include:


  • I)The general Isocline split (This entry)
  • II)The corner contoured split
  • III)Mechanism lead in and angled Isocline.


What is an Isocline?


For those unfamiliar with the term Isocline, here is the dictionary definition: i-soc-line, noun, a line connecting points of equal gradient or inclination.


Where to find it

 

The Isocline Feature can be found several ways.If you are familiar with the traditional NX menu you will easily find it under Menu->Insert->Derived Curve->Extract

 

If you are more comfortable with the NX Ribbon style interface first you will need to have the Advance Role loaded, or your own customized Role where you have already added the Extract Curve to your ribbon. In the Advanced Role you will find it in CURVE->More Gallery->Derived Curve group->Extract Curve

There is always the command finder where you can search the Isocline feature and access it directly.

 

Use: Part I, The General Isocline Split

Here we have a moulded part with a full radius around the periphery of the wall-stock edge.

 


 

This is a close-up view of the radius following the outer wall-stock edge.

 


 

Common Poor-practice for Building Parting-line Split

The common poor-practice seen in the moulding industry is pulling off the parting-line split from the edge of the radius.Typically this is seen on somewhat vertical walls where the low draft angle doesn’t show much deviation from the radius edge to the true tangent apex of the radius (as compared to the die-draw).

 


 

From this close-up section below (and using iso-view above) you can see the designer selected the radius edge as the split for the mould.However based on the vertical die-draw axis (+Z) you can see that the radius actually bulges out past this split point to become slightly under-cut to die-draw.This causes a die-lock condition for the moulded part.

 

Several reasons why this goes unnoticed in the manufacturing process can be attributed to, but not limited to:

 

A)The undercut condition is very small and as the moulded part shrinks it releases itself from the under-cut and is no longer die-locked.

 

B)The mould was cut vertically in the Z axis so the cutter never actually cuts in the under-cut condition—thus leaving the customer with a blunted radius.

 

C)The mould is cut as shown but during hand polishing operations the top lip of the core is polished away leaving open draft—This then creates a mis-match condition where the core steel is stepped out past the cavity edge, and then polishing of the cavity edge is necessary to bring it over to the new core position.

 


 

Best-Practice for Building Parting-Line Split

First enter the Extract menu from either the traditional Menu button or through the Ribbon interface and choose Isocline.

 

Menu button:

 


 

Ribbon Interface:

 


 

Once in the Isocline dialog box:

 

1. We select the die-draw axis either using the default inferred vector selection, or any of the options in the Vector drop down list.If necessary you can then use the reverse vector orientation option. Note:after selecting the axis the dialog still shows 0 for the selection even though you have defined it, at this point hit OK to accept the vector selection.

 


 

2.In this case we make sure the Single option is selected as we only want one set of curves.(The family option lets you generate multiple sets of curves between a range and angle step over.)

 

3.We then set the angle requirement--from the die-draw axis-- to create the isocline at.In this case when creating the outer parting split normal to the +Z axis we set this value at 0°.Then click OK to accept the angle and progress to the face selection dialog.

 


 

4.We then select all the faces we wish to process for Isocline creation.This can be done by single on screen selections, or the other selection options presented in the dialog box.Depending on how you intend to use the Isocline command in your process you may want to select all faces in body if you think the data will change enough that all faces need to be processed, however if you are quite sure it will only be these local faces to be accommodated then it’s best to only select the needed faces to reduce the amount of faces processed during updates.After selecting the faces needed in this set click OK.

 



You will be returned to the first Isocline menu again in order to create further Isocline definitions, but in this case click Cancel.

 

An Isocline representing the parting-split is generated (Red Line below).You can see the difference between A) the original radius edge, and B) the position of the Isocline split.

 


 

We now can develop a parting-split surface from the Isocline curve.

 


 

From this close-up section below (and using iso-view above) you can see that the parting-split surface lies at the 0° draft location of the radius and that the split now represents the outermost extent of the radius surface data.This split location ensures open draft to each half of the Core and Cavity.

 


 

If you would like to learn more about this operation and other advanced operations, you should attend one of our advanced NX CAD courses. To arrange for advanced training please contact your Account Manager, or contact us directly at info@designfusion.com.





New Template control in ST7

John Pearson - Monday, October 20, 2014

Many of you have received the new ST7 version of Solid Edge. With over 1300 customer requests addressed, in this new release, I feel it’s worth covering the highlights over the next few blog articles. We also offer a “What’s new in ST7” course, for those of you who prefer a more instructed hands-on approach.

I’d like to start with the new template control. When you launch ST7, you’ll notice the newly designed startup screen.



Notice the list of default templates. These templates are populated based on the standards selected in the initial installation. In previous versions it has been a tedious process to change the standard of the default templates. The template folder and template control mechanism has been restructured to make this much easier. Let’s explore this new mechanism.

From the startup screen, click the Edit List link.



Notice that the new Template List Creation dialog appears.



From the Standard Template column, on the left hand side, select the ANSI Inch standard.


Click OK, and notice that the default templates have been updated to the ANSI Inch standard.



This new approach allows for users to set and change their own template standards, regardless of the initial setup standards.

For you users, that may have existing custom templates, it’s very easy to reuse them with this new mechanism. Simply tell Solid Edge where your custom template folder resides. This is the same process as in previous versions. Bring up the Solid Edge Options > File Locations tab.


Select the User templates header and click the Modify button.



Browse to where your custom template folder resides, in your data base. In this example I’m using a “My custom templates” folder.



Click OK to accept the folder location. Then click OK to close the Solid Edge Option dialog.



Notice that the startup screen now contains my custom templates. If you click on the Edit List link again, you’ll notice that the User Templates have been added to the left column, above the Standard Templates.



Again, this new approach allows for users to set and change between their own template standards, including custom templates, regardless of the initial setup standards.

Another new option is the ability to mix templates into a custom list. Suppose that your job requires you to create a series of mechanical drawings. You could create a custom list of different draft templates to allow you to select different standards directly from the startup screen.

To set this up, click on the Edit List link. At the bottom of the Template List Creation dialog, click the create new list button.



In the List name field, type in Draft Templates.



Click OK, and notice that the Draft Templates header is added under a Custom Templates header.



Using the Browse button, located beside the Add Template field, browse to the ANSI Inch Templates and select the “ansi inch draft.dft” file



Click OK. In the Displayed name field, type in ANSI Inch Draft and click the Add button. Notice that you can also add a description if you wish.



Repeat this step and add as many draft templates that you will need. In this example I added the following Draft templates:

o ANSI Metric Draft

o DIN Metric Draft

o ISO Metric Draft



Click OK. Notice the list has been added to the Startup screen.



Click on the Edit List link again. Notice the other options at the bottom of the dialog.



1. You can rename a list.

2. You can delete a list.

3. You can save a list without having it appear on the startup screen.

Even with the creation of a list, you can always switch back to other standards as your need requires.

This is just one of the many useful and time saving enhancements in Solid Edge ST7. If you’d like to learn more, feel free to contact us sales@designfusion.com, or attend one of our upcoming “What’s new in ST7” courses.

Solid Edge University 2014

John Pearson - Monday, April 28, 2014

Join us at Solid Edge University 2014 and Re-imagine What’s Possible

If you haven’t already registered for this annual event, there is still time to join us in Atlanta from May 12-14, 2014. Designfusion will have 5 members of our team present at this year’s event. Three of them will be presenting as guest speakers. This conference continues to grow each year, and this year is no different. This year users can:

    •      - Obtain New Solid Edge Certification
    •      - Learn about the new capabilities of Solid Edge ST7
  •      - Meet the Solid Edge development team
  •      - Network with peers and Designfusion technical experts
  •      - Attend numerous training sessions, and
  •      - Discover a range of complimentary applications from our best-in-breed technology partners.

Attendees will be welcomed at the Westin Peachtree Plaza, in Atlanta, GA, on Monday May 12 with a Welcome Reception from 6 pm to 8 pm. But the real excitement starts on Tuesday May 13, with the launch of ST7. Below are the tentative schedules for Tuesday and Wednesday.

 

 

 

 

You can see that, with this jam packed schedule, the learning potential is huge. This is not a marketing conference but a conference designed to educate users. This is why we call it Solid Edge University. So if you haven’t already registered, there’s still time to do so at http://solidedgeu.com/. We hope to see you there.

An overview of Sensors in Solid Edge

Manny Marquez - Thursday, April 24, 2014

During a benchmark last week I demonstrated sensors. It had been a very long time since I have used that functionality and after seeing the usefulness it could provide for a prospect I decided to write a review for the blog. One such use is when constructing parts and assemblies, you often need to keep track of critical design parameters.


For instance, when designing a shield or shroud that encloses a rotating part, you must maintain enough

clearance for maintenance and operational purposes. You can use sensors to define and keep track

of design parameters for your parts and assemblies.

Types of sensors:

          • • Minimum distance sensors
      • • General variable sensors
      • • Sheet metal sensors
      • • Surface area sensors
      • • Custom sensors
A Sensor Assistant keeps track of sensor alarms that have been triggered by changes
to the model. It quickly accesses the affected sensor definition information so you can
review it and fix the alarm or the model as needed.

You can activate or deactivate the Sensor Assistant and alarm notification
in the graphic window using the Show Sensor Indicator option on the Helpers
tab of the tools options dialog box. This does not affect the operation
of the sensors themselves.

Alarm Types

Displays a bitmap indicating the type of sensor alarm:

  • A sensor violation alarm indicates a design threshold has been exceeded 
  • A sensor warning alarm indicates an element has been deleted:
  • Click the alarm hyperlink to jump to the specific sensor definition information.


We will be using a sample model from the training folder in solid edge.

1. Open the sheet metal assembly located in C:\Program Files\Solid Edge ST6\Training \ (seaabbf.asm) folder.


Minimum distance sensors

Minimum distance sensors are used to track the minimum distance between any two elements.
For example, you can track the minimum distance between two part faces in an assembly.
You define a minimum distance sensor similar to how you measure the minimum distance
between two elements with the Minimum Distance command in the assembly from one part to another.

2. Click on the command, and then select one surface of the chassis part and the other surface from powsup.par part.



3. Enter the name of sensor and values as shown.

4.          

Once done with creating this sensor, we will get back to this sensor on how to trigger the alarm.


Variables Sensors

You can use a general variable sensor to track variables, such as driving and driven dimensions. Let's say that your company only has machines that cuts or bends to a specific size. Ideally you want a safe guard so that you don’t design a part you can’t manufacture or don’t carry stock of that size. In this example we will track the overall height of the part being designed.



5. Edit the Chassis in place.

6. Select the variable sensor. Enter a name for the sensor, then select 552.61 cell. Click on the add variable icon then add values as shown below.

Observe the threshold and sensor range and compare that to the gauge and description. This should give you an idea on how the sensor will alert when it has been triggered.


Sheet Metal Sensor


You can use sheet metal sensors to track design parameters, such as the minimum distance between particular types of sheet metal features and part edges. You can create your own sheet metal sensors from scratch, or you can select from a list of predefined examples. Let’s say that we need to make sure a cutout does not get to close the outside edge, for reason that the heat sink will get hot and damage the component. Sheet metal sensors are available only in sheet metal documents.

7. Click on the sheet metal sensor; make sure to select the Face on the options on ribbon bar. Select surface on part as shown.


8. Select cutouts on (edge set 1) and exterior edges from (edge set 2). Set threshold at 20, therefore if a hole gets 20mm of an edge, a sensor will be triggered.

9.  

Notice the two sensors now; we are done creating this sensor, we will get back to this sensor on how to trigger the alarm.

Surface Area Sensor

You can use a surface area sensor to monitor a surface or a set of surfaces. Also you can monitor both the positive and negative surface area. A negative surface area sensor monitors the "holes" or internal boundaries in a surface.For instance, you may need to track the total area for a series of ventilation holes and cutouts in a surface.

10. Click on surface area sensor icon; select the negative area with face option then click on surface of part as shown.

11. Enter sensor name, with indicated values, again study the current value to the threshold and sensor range. Notice on the airflow gage how much it’s left to trigger the alarm.


Done with creating this sensor, we will get back to this sensor on how to trigger the alarm.

Custom Sensor

You can use a custom sensor to monitor any numeric result that is calculated from a custom program. For example, you could create a custom program that assigns a manufacturing cost to each feature type used for creating sheet metal parts. The program would then monitor the part features and give you the part cost of the completed model.

Note: you need to run the CustomSensorRegistration.exe from the custom sensor folder.

12. Select custom sensor then click on GetMass.



13. Note: If you did not add a material type, you will get this message. Simply go to the material table and add a material. See below.



14. Enter the sensors name and fill in the indicated values as shown below. The current value is 8.18 lbs, we set a threshold of 10 lbs and range between 5 lbs to 15 lbs. If the part goes over 11 lbs the sensor will set a warning alarm.

15.



Let's put all sensors to the test, starting with the clearance sensor, this will allow us to have a minimum distance from other parts on the assembly For example, if you don’t want the heat sink to get any closer to the side wall for it want allow proper flow.


16. Edit in place chassis.psm part. Select Hole 5, then click on dynamic edit, select dimension 62.50 and enter new value of 80. Since the sensor is a Assembly part, you need to (close and re-run) notice the sensor violation alarm indicates a threshold has been exceeded. (If don’t see indication, select on the tools tab click update all links)



17. Click on sensor violation alarm, for sensor details.


In real scenarios you will determine what actionsare needed to resolve the violation by making changes to the model.

In the following scenario we will only be triggering off the sensors to show sensor violations.


18. The following sensors will take place on the part environment (chassis.psm); we will trigger the Height sensor this time. Select the (contour flange 1) then click on dynamic edit. Enter 200mm value to see violation. Click on update all links.



19. We will trigger the holes to edge sensor now, select on the (Cutout 1) click on dynamic edit. Select dimension 30 enter new 15 value then enter.



20. Next will be the Airflow sensor, select on the (Cutout 1) click on dynamic edit. Click on the 94 dimension, enter 90.




21. The final sensor to trigger is weight, Select the (contour flange 1), then click on dynamic edit. Select value 250, and then enter 400.

22.


I hope this simple example on sensors gave you an insight on the usefulness of sensors during design.

Until next time!

Constraints and how they work in ordered and synchronous modelling

John Pearson - Thursday, April 03, 2014
There seems to be some confusion amongst some users regarding the ability to constrain synchronous parts. The confusion has even lead to inaccurate information being perpetrated as truths, by some competitive product’s resellers. So I’d like to set the record straight and clear up several misconceptions. First and foremost, you can constrain synchronous models. Secondly you can use the variable table to drive synchronous models. And last, but not least, you can automate synchronous models through custom programming or a configurator.

Ordered constraints


To understand how this works, let’s fist look at an ordered part. Below is a sketch for a part that I wish to model. Notice that I have fully constrained the sketch.

 

 


The sketch has zero degrees of freedom, so I can predict what will happen when I make a dimensional change to any of the 3 values. I control part of the sketch with geometric constraints, which include the following 2D relationships:

 

 


When I use the sketch to create a model, the sketch becomes the parent of the solid model, as shown below:

 


This model is considered constrained because it is controlled by the fully constrained sketch and the depth dimension, added during the extrusion command. Notice that we can go into the variable table and apply specific names to each dimensional variable.

 

 

 

I can now drive predictable model changes using the variable table. Furthermore I can link the variable table to an Excel spread sheet, a custom program, or a configurator to drive model changes.

When a variable is changed, the system first re-calculates the sketch and ensures that the sketch is still a valid profile. It then moves on to the child of the sketch, in this case the model, and re-computes the model to ensure that we still have a valid model. If additional features were added to the model (like a round or chamfer) it would continue to re-compute the next feature(s) until it has completed the feature tree list. For small models with few features, this is a rapid process. However, the more features an ordered model has in it, the longer the re-compute time will take.

Synchronous constraints

Now let’s make the same part in the synchronous mode. We start by making a sketch, as shown below:

  


Notice that I can fully constrain the sketch in synchronous mode. The difference here is that when I create the solid, only the dimensions are migrated to the 3D model. The 2D geometry and 2D geometric constraints are left in the Used Sketch header on the PathFinder. In other words, no parent child relationship is created between the sketch and solid, and the 2D dimensions are converted to 3D driving dimensions on the model, shown below:

 

 


Notice that 3 of the 4 dimensions are red in colour, while the depth dimension is blue. A red colour means that the dimension is locked and can only be modified by a direct edit of that dimension. Let’s make the fourth dimension locked as well.

 

 


So now we have the dimensions fully constrained or locked. What about the geometric constraints? Since the 2D geometric relationships have not been transferred to the model, a lot of users become concerned that the model is no longer fully constrained. They are partially correct. Let’s take a closer look at the model.

By the nature of the solid, we can make a few assumptions.

1. The connect relationships will be maintained at the model level. Why? Because if they are not we no longer have a solid.

2. Synchronous edits use Live Rules, and Live Rules will maintain most of the pre-existing geometric situations. For example, if you attempt to change the values in the part, default Live Rules will keep the walls in their current horizontal/vertical position.

3. Synchronous will only analyze the effected faces in any move. Therefore it only has to re-compute faces affected by an edit.

Even with these assumptions, there admittedly could be some un-expected results if you are using this model in a custom program or configurator. So how do we eliminate potential un-expected results? We use 3D geometric relationships.

Persistent (3D) relationships

 

Looking at the original sketch of our model, you’ll notice that the sketch was centered on the base coordinate system. I can do the same with the model by using the horizontal/vertical persistent relationship command. I’ve placed these relationships in the model, shown below. Notice that they also are listed under a Relationship header in the PathFinder.

 

 


Simply by placing these two relationships, I now have predictability in any dimensional edit. I can now set this synchronous model up in the Variable Table.

 

 

 

I can now drive predictable model changes using the variable table. Furthermore I can link the variable table to an Excel spread sheet, a custom program, or a configurator to drive model changes.

For more complex models, synchronous offers even more 3D geometric relationships.

 

 


Notice the striking similarity between our 3D geometric relationships and our 2D geometric relationships. There is however one big difference. I only have to use the relationships that I need to control my model. Because synchronous technology only re-computes faces that are affected by an edit, I may not have to fully constrain a model.

Some will argue the fact, but the truth is the majority of ordered models that I see from customers are under-constrained. Because of the parent child nature of ordered modelling, this could be, and often is a problem when editing ordered part models. If you doubt this statement, go back to your database and open some of your existing models. Under the Solid Edge options > General tab, turn on the ‘Indicate under-constrained profiles in PathFinder.

 

 

 

If a red pencil icon appears anywhere in the PathFinder, you have under-constrained features.

 

 


This is a real concern in ordered modelling, but not in synchronous modelling. As you’ve seen, the nature of synchronous modelling puts the focus on only what’s being edited. As you have also seen, a synchronous model can be fully constrained if necessary. Either way you can have complete predictability of the model and use it in configurators or custom programs.

So, as I stated at the start of the blog article, you can constrain synchronous models. You can use the variable table to drive synchronous models. And you can automate synchronous models through custom programming or a configurator. Anyone who tells you different has not been properly trained in synchronous modelling or works for a competitive software package.

If you would like more information on synchronous technology or would like to attend one of our synchronous training sessions, please contact us at sales@designfusion.com or visit our training web page at http://www.designfusion.ca//technical-training.html.