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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.


ST9 Assembly In context Contour Flange

Manny Marquez - Thursday, October 13, 2016


Check out our other videos here

Common Mistakes made by novice, or self-taught users – Part 2 of 3

Manny Marquez - Wednesday, June 25, 2014
When talking to customers and looking over their models for unrelated issues, I occasionally recognize simple mistakes made on the part, that normally consist on how the part was initially created. Typically, I will explain to them why the part should be modeled in a specific way, or (best practices).

The way a part is modeled plays a big role on the downstream process, usually when trying to modify the model in “ordered”.


Here are the focus areas for today’s post.

Part modeling 101

  •     • Planes
  •     • Sketching
  •     • Base feature
  •     • Treatment Features

Correct plane selection.

1. A reference plane is a flat surface that is typically used for drawing 2D profiles in 3D space; this will be your foundation for your model.


2. It is always a good practice to have the part center to all base plane on X,Y,Z. in this instance (B) would be the correct method.

Choose the correct reference plane.
The following example illustrates the results of using different reference planes to draw the first profile. For this sample,
using the “xy top” plane (A) the result is a part which is easiest to visualize in the isometric view (ctrl + I). 

4. You can also think of consumer products, how you can better visualize the product, again the example (A) is the best to comprehend it in your mind. 

Correct sketching method

5. Sketching to a correct scale.
Below is a shape of a profile, I have placed a green dotted (reference) line on (X) 7.5 and(Y) 3.5 to indicate overall length and to visualize the scale. When you start placing dimensions, that’s when you realized how small or big your sketch is.

6. It is always a good practice to draw a line to actual length or approximate of the base profile. So as you start to sketch your profile, it will not deviate when you are entering true values.

Below is the same sketch out of scale, placed dimensions, enter true values. See how your sketch starts to look more like a maze. Not a good practice!

Below is a sketch scaled properly with correct dimensions.


Base features

7. Consider these questions when starting a new model:

What is the best profile for the first feature on the part?
Which reference plane should it be drawn on?
Are there symmetric features on the part? 

When constructing a 3D model, it is helpful to evaluate the basic shape of the part, and develop a plan as to how you want to construct the model. 
The first feature created for a part or sheet metal model is called the base feature.

Choose the best profile for the base feature.


8. Profile C would be the best choice. It defines the basic length and width of the model and includes the tapered end. Two additional protrusion features complete the basic shape of the part. A hole feature, a cutout feature, and a round feature complete the part. 

Treatment Features

9. A treatment feature is a feature applied to faces and edges of a solid body. The most commonly used treatment features include rounding an edge(s), chamfering an edge(s), adding draft and thin walling a part.
 For best results, add treatment features to your model as late as possible in the design process. 


I hope these simple examples can serve as a quick guide on basic part modeling.

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.


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.


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.


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.


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

Until next time!