Posts Tagged ‘Solid Edge ST3’

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Tuesday, November 20th, 2012home

A “Quicksheet” is a template of drawing views that are not linked to a model. You can then drag a model from the Library tab or from Windows Explorer onto the template, and the views populate with the model.  If you have standard views on a particular size of drawing, for example, you can have the Draft preconfigured to populate itself based on the model you place on the sheet.

You will to need to set up a Draft sheet (but do not use production drawing as the drafting information will be removed upon save) with your views and other items such as Parts Lists.

1. Go to the SE Application button

2. From the Application menu, choose the “Create Quicksheet Template” command.

3. Save the file to a location and give it a name that easily identifies it.  It is best to place this on a network area other users can get to if it is useful to share the Quicksheet.   It is also best to locate it in a similar area to where the company templates for SE reside.

* Almost all view properties, including general properties, text and color properties, and annotation properties, are maintained. However, some display properties, such as selected parts display, Show Fill Style, and Hidden Edge Style, are not maintained.

Now a Quicksheet template has been created, but how do we use it?

1. Open your Quicksheet template (either through Windows Explorer or if you set up your User Templates and placed the Quicksheets in that location hit New>Quicksheet> and select your Quicksheet).

2. Drag and drop your desired Part or Assy onto the sheet from Windows Explorer or through the Library tab in Solid Edge.

3. Solid Edge will place the geometry and will be ready for the next steps.

Integrated Modeling in Solid Edge

Monday, November 19th, 2012

With any new technology, you have your early adopters. This is followed by a general acceptance of the new technology, and of course, you always have your hold outs or late adopters.  Solid Edge ST and ST2 appealed to the earlier adopters for synchronous technology. With ST3, ST4 and now ST5, we are seeing most of our customers starting to use synchronous modeling. This of course has led to many questions. The most asked question is; “Should I use synchronous or ordered modeling?” The answer to this is yes.

One of the unique qualities of Solid Edge is that you are not locked into using synchronous or ordered modeling. Integrated modeling allows you to use both synchronous features and ordered features within the same part or sheet metal model. As a rule of thumb, I encourage users to start with synchronous modeling. If they run into some issues that can’t be addressed with synchronous features, they can switch to the ordered paradigm to complete
the model. Let me illustrate this with the following example:

I wish to model the sheet metal cover shown in the following image.

I start in the synchronous paradigm and create a tab, for the top of the cover.

I then add 2 synchronous flanges, in one step, to create the back and left side of the cover.

One of the current limitations, in synchronous sheet metal modeling, is that you cannot drive a flange along a circular edge. Realizing this I will hold off creating the front and right sides until the end, when I will use an ordered feature.

I next use 2 bead synchronous features to create the slots at the top of the part.

I then transition to the ordered paradigm to complete the model.

I use the ordered Contour Flange command to create the front and right face of the cover.

The nice thing about this approach is that it still allows me to modify the model using the synchronous Move/Rotate command.

Live Rules and all the other synchronous editing tools still apply to the model.

As I modify the model, synchronous features update instantly, followed by the re-computing of any ordered features.

For those of you who attended our productivity seminars, you saw this demonstrated live. Other users have learned this process in one of our many synchronous modeling courses, offered over the last year.

This is just one of many examples where Integrated Modeling allows you to benefit from the new synchronous technology, while still utilizing some of the tried and true methods of the ordered technology.  As Solid Edge continues to develop the synchronous features, you may find that you’ll use less integrated modeling. But for now this provides you with a reliable and safe platform to further advance your adoption of this amazing new modeling paradigm we call synchronous technology.

If you’d like to learn more about integrated modeling, you can attend one of our synchronous modeling courses. For more information visit our website at New 2013 courses will be added to our schedule soon.


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, 2012home

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.

MICE hotkeys assist in snapping to points.

Thursday, July 21st, 2011

When working wth Solid Edge sketching, situations can arise where more than one keypoint resides in the same location. You can use the quick pick to filter through the multiple points and select the point you want, or you can use the MICE hotkeys. The hotkeys only require you to locate the element and hit the hotkey to snap to the point.

 Snap-to-point shortcut keys

Once you have located an element with the cursor, you can use the following shortcut keys to snap to keypoints and intersection points.

  • Midpoint – press M.
  • Intersection point – press I.
  • Center point – press C.
  • Endpoint – press E.

Tip: To help you remember what the shortcut keys are, note that the letters can be arranged to spell the word mice.

Shortcut keys are not case sensitive.

You can use the snap-to-point shortcut keys to select and apply the coordinates of a center point, midpoint, endpoint, or intersection point to a command in progress.

You can use the shortcut keys when creating 2D drawing or sketch elements, dimensioning the distance or angle between elements, adding many types of annotations, and defining patterns. You also can use the shortcut keys with commands that manipulate 2D elements, such as move, rotate, mirror, scale, connect, and stretch.

Snap to a center point

  • Start the command you want to use.

For example, to draw a line that snaps to another element, choose Line.

  • At the prompt to click a point, in the graphic window, move the cursor over the arc, circle, or ellipse element you want to snap to.
  • On the keyboard, press C to select the center point of the located element and apply its coordinates to the current command.


Snap to a midpoint

  •  Start the command you want to use.

For example, to draw a line that snaps to another element, choose Line.

  •  At the prompt to click a point, in the graphics window, move the cursor over the element you want to snap to.
  •  On the keyboard, press M to select the midpoint and apply its coordinates to the current command.


 Snap to an endpoint

  • Start the command you want to use.

For example, to draw a line that snaps to another element, choose Line.

  •  At the prompt to click a point, in the graphics window, move the cursor over the end of the line element that you want to snap to.
  •  On the keyboard, press E to select the endpoint and apply its coordinates to the command. The cursor location determines which endpoint is selected.


 Snap to an intersection point

  •  Start the command you want to use.

For example, to draw a line that snaps to an intersection point, choose Line.

  •  At the prompt to click a point, use the cursor to briefly touch each element for which you want to find the intersection point.

 Pause the cursor on the last element, so that it remains highlighted.

  •  On the keyboard, press I.
  •  Do one of the following:
    •  If there is only one eligible intersection point, then the point coordinates are applied automatically to the command in progress.
    •  If there are multiple eligible intersection points, select the one you want to snap to Element and object selection.

 Example—Touch each of three lines with the cursor, moving from left to right. Pause with the right-most line highlighted, and then press I. QuickPick opens automatically. The most recently located intersection point is listed first, and the intersection point for the first two lines you touched is listed second.


In the QuickPick list, click to select the intersection point you want.


  •  The shortcut keys are not case sensitive.
  •  If you cannot snap to a point when you press the appropriate shortcut key, choose IntelliSketch, and then verify that the point type has not been deselected on the Relationships page of the IntelliSketch dialog box.

Clipping Planes in Solid Edge

Monday, June 20th, 2011

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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