Posts Tagged ‘Solid Edge with Synchronous Technology’

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New Parts List Architecture

Tuesday, January 17th, 2012

In Solid Edge ST2, Parts Lists were redesigned to take advantage of the user table architecture. The new architecture was needed to meet the demands of our customers. In this first release of this new Parts List command, just under 250 customer requests were implemented, and many more have been added in ST3 and ST4. Below is a list of highlights followed by some example of the new capabilities.


 The new Parts List architecture allows you to:

  • - Edit Item Numbers from Parts List, not just from balloons
  • - Combine Multiple Properties in Single Column
  • - Comments Columns – User defined text
  • - Split Parts List among Multiple Sheets
  • - Sort on Hidden Columns
  • - Manual Reorder Columns and Rows
  • - Resize Columns in Graphic Display
  • - Placement via cursor
  • - Title/Footer
  • - Display an exploded list of the BOM
  • - Display level based item numbers with the exploded list
  • - Indent any column to aid in the showing of sub-assemblies
  • - Derive item number from the assembly
  • - Display Mass property as Mass of single item, and Mass of total occurrences of the item
  • - Frame data display enhanced to allow for distinction of frames based on cut length, mass, and miter
  • - Align and control style of table titles
  • - Control column headers
  • - Merge column headers
  • - Rotate column headers
  • - Turn on Cell Aspect Ratio adjustment
  • - Format the font for any cell
  • - Override disabled cells
  • - Insert user defined rows
  • - Merge vertical cells with same value
  • - Plus more ….



The following are just a few examples of some of the new capabilities in the new Parts List architecture.



Example 1: How to add a title to the Parts List

 To add a title to your Parts List you must first go to the “Title” tab and click on the Add Title icon.

In the Title text field, type the title that you wish to use – for example Solid Edge Parts List.

 You can also control how the title is formatted by adjusting the following settings:

Position – Specifies the position for the title within the table. You can place a title at the top of the table (Header option), at the bottom (Footer option), and in ‘Both’ locations.  Select ‘Neither’ from the list if you do not want to use the title in the table.

Font – Specifies the font to apply to the currently selected table title. All installed fonts are available.

 Font style – Specifies the font style to apply to the currently selected table title. The options are Regular, Bold, Italic, and Bold Italic.

 Font size – Specifies the text size of the currently selected table title.

 Alignment – Adjusts the horizontal alignment of the currently selected table title text. The options are Left, Center, and Right. The default is for text to be centered.

 Underline – Applies underline to the currently selected table title text.

 Adjust text to title width – When checked, automatically adjusts the aspect ratio of the title text when the length of the text exceeds the cell width. Changing the aspect ratio only changes the text width, not its height. The effect of selecting this check box is to shorten the text string to fit the column width; text is never lengthened to fit the column width.

Use this option to prevent text from wrapping within a cell in a title block.

For this example I set the following settings:

  • - Font = Arial Black
  • - Font size = 7.00mm
  • - Toggle on Underline


Below is how this would appear on my Parts List.



Example 2: How to modify individual columns

In this example I wish to rotate the header of the ‘Quantity’ column and merge any cells that have the same quantity, while maintaining my item number order. To do this I first go to the Columns tab, and select the Column that I wish to modify – for example ‘Quantity’.

To rotate the header, select the ‘Format Cells’ button, beneath the header ‘Text:’ field, and change the Orientation to Rotated

I then toggle on ‘Adjust text to column width’ and hit OK.

Notice that when this is applied, the header is rotated and column width is adjusted appropriately.

To merge like cells, toggle on “Merge vertical cells with same value”

If you wish to center the cell’s data, click the adjacent “Format Cells”  button and set both Horizontal and Vertical alignment to ‘Center’ and click OK.

Below is an example of how these changes would appear when applied.



Example 3: Creating indented item numbers

In this example I wish to create an exploded BOM and have the Item Numbers indented to illustrate the parts belonging to the sub-assemblies. To do this I select the Columns tab. Next I select the Item Number, from the Columns list, and click on the ‘Format Cells’ button. Under the Horizontal alignment I select Indent. 


Next I go to the List Control tab.


Here you will select the type of list you want, in this case an ‘Exploded list’. Under the Global settings, change the settings to match those shown below.

You can preview the results on the Data tab. Notice the indent item numbers for assembly number 1.




The new Parts List architecture has allowed the Solid Edge development team the ability to add a tremendous amount of user control to Parts List creation. For more information view the ‘Parts List’ section found in the Solid Edge Help documents.

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New training schedule announced for the first half of 2012

Thursday, January 5th, 2012

If your New Year’s resolution is to improve your Solid Edge skills, then this is the article for you. We have released our new training schedule for the first half of 2012. The schedule includes some new course offerings, along with our traditional courses. Below is a brief description of each Solid Edge course along with a link to a more detailed outline.

Solid Edge Fundamentals (4 days) or Solid Edge Fundamentals Plus (5 days)

This is our introductory course for any novice user. The first four days cover both ordered and synchronous part modeling, assemblies, and drafting. The 5th day is optional and covers sheet metal modeling. For more information follow this link

Solid Edge ST4 Update Course (2 days)

This is our “What’s New in ST4 course”. It focuses on introducing the experienced user to the popular enhancements in our latest release of Solid Edge. For more information follow this link

Advanced Solid Edge Modeling (3 days)

This is one of our newer courses. It’s designed to improve the users’ modeling skills by introducing them to surface modeling, along with advanced modeling tools. Many of the techniques taught in this course have been included based upon queries we have received from our technical support line. For more information follow this link

Advanced Solid Edge Assembly (3 days)

This course is for the more experienced user, who wants to improve his knowledge in working with assemblies. It focuses on improving the user’s assembly design skills and introduces many advanced assembly design tools. For more information follow this link

Solid Edge Synchronous Technology Course (4 days)

This is our newest course, and is designed for our traditional users who have yet to learn the new synchronous paradigm. Its focus will be on showing the difference between ordered and synchronous modeling and how to use both paradigms to improve your design productivity. For more information follow this link

All of our courses are designed in house, by a certified trainer of adults, and are unique to Designfusion.

All of our instructors are SETA certified and come from a CAD/CAM industry background with many years of experience.

For our course schedule, please visit the following web sites:

English courses in Canada:

French courses in Canada:

Courses in the USA:

For further inquires, including requests for quotes, please contact your local Account Manager. You can also contact the appropriate inside sales representative listed below:

English Canada:      Rose Francella at

French Canada:       Lily Brault at

USA:                           Sarah Pritsch at

Remember, it is estimated that 1 hour of an instructor led course is equivalent to 16 hours of teaching yourself. Students, who have attended our courses, see immediate benefits for themselves and their companies.

Editing with Live Sections

Tuesday, December 13th, 2011participate

In the Solid Edge synchronous modeling paradigm, you can use the Live Section command to create a 2D cross-section on a plane through a 3D part.

Live sections can make it easier to visualize and edit certain types of parts, such as parts that contain revolved features. You can then edit the 2D elements of the live section to modify 3D model geometry.

Recently we have received some questions from customers who have received synchronous models, which they need to edit. They are still working in the ordered paradigm and have not taken any synchronous training. They want to know how they can accurately edit a synchronous part. For these customers, we often show them how to use the Live Section command. It is similar to working with dimensional sketches and is often easier to visualize than some of the other approaches. Below is such an example:

Scenario: The user has a synchronous roller part for a conveyor mechanism, as shown below.


The user wishes to edit the part to look like the following part.

First, it should be noted that there are several ways to edit this part. But we will illustrate a method using the Live Section command. To create a live section you follow these simple steps:

          1.  Choose Home tab→Section group→Live Section.

          2.  Select an existing planar face, reference plane, or principal plane on a coordinate system.


          The live section is created.


  • - You can use the Live Section Colors section on the Colors page of the Solid Edge Options dialog box to specify the colors you want to use for the edges, center lines, and regions for live sections.
  • - You can use PathFinder to display and hide live sections.
  • - The live section automatically updates when you add or remove features, or modify the 3D model.
  • - Move the live section plane and the section updates as the plane intersects the model.


To get a better view of the live section, hide the design body using a RMB click over the display screen, to access the following menu:

Align the view to give you a top down view of the live section. Below is a list of keyboard shortcuts to help you orient your view.

In this case I used a Ctrl+R to get the top down view of the live section.

I then used the Distance Between command to place the following dimensions.

In this scenario, I have to modify the 1.000” to 0.500” and the 0.875” to 0.375”. I first select the 1.000 dimension. I ensure that the directional (red) arrow is pointing to the side that will move. I then type in the 0.500 value.

Before hitting enter, I lock the dimension by clicking on the little lock icon. This will prevent the edit to the 0.875 dimension from altering this edit.

I click enter to accept the dimensional change. Notice that the new value is in red, indicating a locked state.

Live sections are subject to the same live rules as 3D editing. Therefore, since this part is symmetrical about a base plane, I only have to edit the one side and the other side automatically updates.

Next I modify the 0.875 dimension to 0.375, again making sure that the directional (red) arrow is pointing to the side that will move.

Since this is the last dimension I will edit here, I choose not to lock it.

Once again the symmetric live rule updates the other side for me.

Next I have to place some cutouts into the roller. Although I will do this on the 3D model, I can use the live section to help me accurately place the initial cutout sketch, as shown below:

I then show the Design Body and hide the Live Section

Using the Revolve command, I set the selection type to Face and select the sketch region, created by my sketch and the edge of the cylinder.

I RMB click to accept this selection. Notice the Axis icon activates and you will be prompted to select the axis of revolution.

I move the cursor over the large cylinder and the axis of the cylinder highlights for selection. I select this axis.

I then ensure that this will be a revolved cutout by selecting the remove option.

Next, I select a full 360 degree revolution.

And I have created my first groove, accurately positioned and dimensioned.

To complete the model I use the Rectangular Pattern command. I first select the newly created Revolved Cutout from the PathFinder.

Then I select the Rectangular Pattern command.

I select the Right(zy) reference plane to place the preview of the pattern.

Note: The synchronous pattern command automatically generates a preview of a default pattern and provides on screen dynamic input boxes for you to enter your desired parameters.

In this scenario, I entered the following values.

  • - X Count: 14
  • - Y Count: 1
  • - X distance of 14”
  • - Because the Y Count is 1, I don’t have to enter a Y distance.


I RMB click to accept the pattern and model is complete.

Notice that if I hide the PMI dimensions and turn on the Live Sections, my live section has updated to include the grooves.

Notice that in this scenario we could have modified this part using just the 3D model and steering wheel to adjust the ends. We could have also just used 3D dimensions directly on the model. However, using the live section provides some users with a comfort level and easier visualization, similar to working in the ordered environment.

I think it’s also worth mentioning that if this model had been designed in another CAD package, the exact same steps would be used to make the exact same edits. With synchronous technology, the user can take any CAD model and work with it as if it was modeled in Solid Edge.

For additional information, please see the topic Live Section command in Solid Edge Help. A training activity for this command is located in the self paced training section. Follow this link, and then click on the Working with Live Sections chapter.


Benefits of switching to ST4 for Traditional/Ordered Users

Thursday, November 3rd, 2011

Some Solid Edge Users have questioned the benefit of switching to the newer versions of Solid Edge. They do not wish to use the new Synchronous Technology, therefore feel that there is no benefit to upgrading. Admittedly, in the last few releases, Siemens marketing has focused on the introduction of their new, and industry changing, Synchronous technology, primarily because it is revolutionary technology, which our competition simply doesn’t have. However, they have not forgotten or ignored the Solid Edge Users, who still need or prefer the traditional parametric approach to modeling. Below is a list of just the highlights of enhancements made to the ordered paradigm: 

  • New standard based templates
  • New interface base on Microsoft office 2007 interface
  • Show/Hide check box added to PathFinder.
  • Command Defaults Improvements
  • Command Finder Updates
  • Mouse Wheel Improved Input
  • Enhanced Middle Mouse Button Rotate
  • Fastener System Improvements
  • Frames Live Update on Drag (Global Undo)
  • Standard Parts Enhancements
  • An option was added to the curve Quickbar to create a closed Bspline curve
  • A new Hatch Style has been added called Radial
  • Unique behavior for TAB and ENTER within the same cell of the variable table. Made to work similarly to Excel
  • A Gage Table option, “Use Excel File”, has been added to the Material Table dialog
  • New sweep option added. Can now twist and scale a swept protrusion.
  • New suppress region control when patterning.
  • Improved cursor feedback – better graphic indicators
  • New sketch display option to deal with large sketches
  • New Polygon by Center command
  • New Rectangle by Center command
  • New Flat Pattern option for viewing deformed features
  • Enhanced flat pattern algorithm to flatten ruled surfaces from lofted flanges
  • New transparent option for PathFinder (Vista, Windows 7)
  • New Radial Mouse Menu made up of 16 customizable sections.
  • Added to ability to customize Command Ribbons
  • Overall customization improvements
  • Enhanced Solid Edge switch windows command to include previews
  • Solid Edge now has UI to control the application color scheme through the Solid Edge Options…Helpers tab
  •  Standard Parts has been moved to SQL Express 2008 allowing for improved performance and more options.
  • Closed Corner command now supports new corner treatment types
    • - New options include: 
    • - Circular with Offset – modification to existing treatment
    • - U-Shaped Cutout
    • - V-Shaped Cutout
    • - Square Cutout
    • - Miter
  • The ability to add tabs to the flattened model has been added.
  • New Etch Command has been added.
  • Parts that are currently open in Solid Edge can be easily added to an open assembly
  • Weld bead enhancements allowing for more successful results
  • Redesigned the display configurations. Allows for multiple configuration to be turned on simultaneously.
  • Item numbers for the Solid Edge BOM can now be defined in the assembly
  • Selection Performance Improvements
  • Improved selection filters
  • Assembly Relationship Enhancements
    • - Grounded Component Indicator
    • - Ground Relationship
    • - Tangent Relationship Flip option
    • - Edit Relationship Flip Option
    • - Relationship Command Processing
    • - Relationship Dimension Color
    • - Center Plane Relationship
    • - Range (Value Limits)
  • Key-point Processing Improvements
  • The “Round” feature has been added to the “Assembly Features” group
  • ERA – Flow Line Enhancements
  • Replace Part uses “Select Configuration” option
  • Auto scroll in PathFinder
  • Replace part can now use part with same name
  • Mass computation in Assembly (Qty Overrides)
  • IPA Shift+Click uses Assembly Coordsys planes as input
  • Simplified Assembly command processing
  • Assembly Pattern support pattern adjustable sub-assemblies
  • Weldment Assembly Icons
  • New dimension prefix on/off command
  • New ability to place dimension between draft views
  • New ability to add custom scale factors to the View Scale pulldown in Command Bar
  • New ability to see and change the scale of a block after it has been placed.
  •  Added to ability to control annotation break lines via a font scale
  • Added the Russian Standard (GOST) weld symbols
  • Added PMI Annotations option to the Drawing View Wizard when placing a PMI Model View
  • Detail views have been enhanced to give users more control over the detail envelope
  • Enhanced the Surface Finish Symbols not only to adhere to the ESKD standards, but also addresses other customer requests
  • Dimension enhancement allows you to specify a tolerance class for a dimension. When the dimension is placed on the geometry, it will automatically look up the tolerance values in the appropriate table for the size and measured class specified.
  • The edge condition symbol and UI has been updated to allow the selection of the direction of the edge (i.e. burr/undercut)
  • The Create 3D Tool has been enhanced to create PMI dimensions in the 3D Model from selected dimensions in the Draft file
  • Parts List – Just Under 250 Customer Requests Implemented
    • - Edit Item Numbers from Parts List, not just from balloons
    • - Combine Multiple Properties in Single Column
    • - Comments Columns – User defined text
    • - Split Parts List among Multiple Sheets
    • - Sort on Hidden Columns
    • - Manual Reorder Columns and Rows
    • - Resize Columns in Graphic Display
    • - Placement via cursor
    • - Title/Footer
    • - Assembly Structure – Exploded List
    • - Level Numbering – Also in Balloons
    • - Indent Each Level
    • - Deriving Item Number from Assembly
    • - Sort by Assembly Order
    • - Column Totals
    • - Frame Data
    • - Auto Balloon
    • - Table Titles
    • - Column Headers
    • - Headers Merging
    • - Header Rotate
    • - Cell Aspect Ratio
    • - Cell Formatting
    • - Overriding Disabled Cells
    • - Inserting User Defined Rows
    • - Convert Deleted Parts/Assemblies to User Defined Rows
    • - Display Control through Configuration
    • - Merge Vertical Cells with Same Value
    • - More…..
  •  When using the Drawing View Creation Wizard, use the “Custom” button to get to the Perspective Options
  • Added Model Edge Colors display options for drawing views
  • The Drawing View Creation Wizard now supports the placement of views based on an Assembly Zone
  • Bend Table/Callout enhancements
  • Improved Callout formatting
  • New Smart Measure command
  • The retrieve dimensions command now retrieves sketch dimensions and annotations from any assembly sketches (including PMI)
  • New Printing/Plotting process for printing multi-sheets
  • Angular Dimension to Center Marks
  • Enhanced Drawing View Caption control
  • Undo button is available if deleting the following:
    • - Drawing Views
    • - Parts Lists
    • - Bend Tables
  • Added a lock drawing view position command
  • Added support for both horizontal and vertical breaks in the same view
  • New ANSI ASME symbols and ISO equivalent symbols have been added to bring the standards up to date.
  • New JIS Weld Symbols
  • Overall improvements to Annotations
    • - Auto balloon – Fastener Systems –Stacked balloons
    • - Callout – Aspect Ratio
    • - Feature Control Frame enhancements
    • - Text Box enhancements
    • - Reattach Centerline and Center marks
  • Dimension control enhancements
  • Added Hole Callout to dimensioning
  • Added a 3D PDF Translator
  • Added Inventor Direct Translator
  • More…

These enhancements do not include all the improvements to the graphic display, or memory handling, for overall performance improvement. There have also been enhancements to the translators, and other add-on modules such as our Rendering and Xpresroute modules.

With all these improvements in the traditional parametric modeling paradigm, it should be obvious that Siemens continues to support and develop the “Ordered” modeling paradigm. For those Users who feel there is no benefit to upgrade, please feel free to contact us, so we can enlighten you on all the enhancements in the ordered paradigm. Our goal is to give you a powerful, easy to use, and reliable modeling experience, regardless of whether you model in the “Ordered” or “Synchronous” paradigm. We will continue to add enhancements to both paradigms in future releases.

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How to Wrap or Project a Sketch

Friday, October 21st, 2011

Last month’s blog prompted several calls asking if the sketched text could be placed on non-planar surfaces. The answer is yes. There are two methods to achieve this:

1)    Wrap Sketch command

2)    Project Curve command

Wrap Sketch command

 The Wrap Sketch command can be used to wrap a sketch around any analytic surface, such as a cylinder or cone. Before using the command, you must create a sketch on a plane which is tangent to the surface. For example, proper reference plane tangency to a cylinder (A) or cone (B) is as shown.

Once the sketch is created you  can select the Surfacing tab→Curves group→Wrap Sketch command.


Next you select the analytic surface (A) that you want to wrap the sketch around.

Then select one or more sketch elements (B), that you want to wrap.

After you wrap a sketch onto a surface, you can use the Normal Protrusion or Normal Cutout commands to construct a protrusion or cutout feature using the wrapped elements.


  • - When selecting more than one surface, the set of surfaces must be connected.
  • - The sketch plane must be tangent to one of the input surfaces.
  • - You can select individual sketch elements, a chain of sketch elements, or the entire sketch using the Select options on the command bar.


Project Curve command

The Project Curve command projects 2D or 3D curves onto any surface or set of surfaces.

First you must have a sketch or curve created. You then select the Surfacing tab→Surfaces group→Project Curve command.


You can set the options to project along a vector or to project normal to the selected surface.

For the ‘Along vector’ options, do the following steps:

Click the curve or point you want to project onto a surface and then click the Accept (check mark) button.

Click the surface onto which you want to project the curve and then click the Accept (check mark) button.

Click to specify the direction you want project the curve.

Finish the feature.


  • - When you are projecting a planar curve along a vector, the Projection Plane Step is skipped, and the plane the curve is on is used to define the normal direction in which to project the curve. If you want to project along a different normal, you can click the Projection Plane Step button and define the plane you want.
  • - You can also use the Project Curve command to project a point onto a surface.
  • - You can use the command bar to specify that you want to project a single element, a chain of elements, a point, or an entire sketch.


For the ‘Normal to selected surface’ options, do the following steps:

Click the curve or point you want to project onto a surface and then click the Accept (check mark) button.

Click the surface onto which you want to project the curve and then click the Accept (check mark) button.

Finish the feature.


  • - You can also use the Project Curve command to project a point onto a surface.
  • - You can use the command bar to specify that you want to project a single element, a chain of elements, a point, or an entire sketch.

 After you wrap a sketch onto a surface, you can use the Normal Protrusion or Normal Cutout commands to construct a protrusion or cutout feature using the wrapped elements.

Clipping Planes in Solid Edge

Monday, June 20th, 2011participate

You can set clipping planes, in Solid Edge, to control the display depth in a 3D window. This is often referred to as sectioning the model. This can be achieved by following these simple steps.

Step 1: Choose View tab→Clip group→Set Planes.

Step 2: Select a planar face or reference plane, position the cursor to define the first clipping plane (A), and then click.

Step 3: Position the cursor to define the second clipping plane (B), and then click.

Step 4: Click Finish.

Note: You can turn the clipped display on and off using the ‘Clipping On’ command, located below the Set Planes command, or use the Hot Keys (Ctrl + D).

Note: This command is designed for simple section/3D depth views. For more elaborate section views use the Section command on the PMI tab>Model Views group.

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