North America's Leading Siemens PLM Partner

Designfusion Blog

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, or attend one of our upcoming “What’s new in ST7” courses.

Using the Improved Drawing View Wizard in ST6

John Pearson - Thursday, December 26, 2013
As more and more users migrate to Solid Edge ST6, I am receiving more calls asking about the Drawing View Wizard. There was a major overhaul in ST6, but do not panic, for you can reset it to behave as it did in previous versions. The new method utilizes the toolbar approach which is found in most Solid Edge commands, where the old way uses the wizard approach.

How to set the drawing view command to the wizard method

A new tab has been added to the Solid Edge options in the Draft environment. The tab is entitled Drawing View Wizard, and allows you to define some default settings.



To learn about the other settings, click on the Help button. The help documents have a complete breakdown of all the other settings.

Using the new Drawing View Wizard method

If you leave the previously mentioned option checked, you will use the new simplified workflow for placing a drawing view. The simplified mode reduces the number of steps required to generate drawing views. It omits the wizard dialog boxes and instead displays the View Wizard command bar at the drawing view placement step. This is the default mode for the View Wizard command.


In the image above you can see that after I selected the part file and I am given a Front view of the part, attached to my cursor, along with a command bar. In this example I am using the horizontal command bar. I could also use the vertical command bar as shown in the following image.

Note: You can choose whether you want to use vertical or horizontal command bars in the Solid Edge options, under the Helpers tab.



I can place this view on my draft sheet and I am immediately put into the principal view command. This allows me to place alternate companion views based on the position of my cursor. For example, if I want a Top and Right view, along with the Front view, I simply move my cursor up and click for the Top view.




I can then move my cursor to the right and click for the Right view.





To exit the command I hit the Esc key, on the keyboard.

Preselecting layouts and presetting options

Before I place any views I can preselect layouts or preset some options. All these options are on the command bar. The image below is that of the vertical command bar. I use this for training because it shows the option names.


As you can see there are over a dozen options here. I will focus on the 6 most common, but a description of all the options can be found in the Solid Edge Help section.

Drawing View Wizard Options   

This option allows you to specify content and display options based on whether the drawing view is an assembly, part, or a sheet metal model. When you select it the following dialog appears:

•    For Part or Sheet metal files.



•    For an Assembly file.



For those of you familiar with the old Drawing View Wizard, you will recognize these dialogs as the first dialogs that appear. All the options that you are used to are still here.

Drawing View Layout  

This option allows you to select additional views to place along with the primary view. You also can change the orientation of the primary view. When you select it the following dialog appears:



Once again this dialog should be familiar to existing Solid Edge users. It is a combination of the 2nd and 3rd dialogs of the old Drawing View Wizard. Here you pick your primary view and the companion views. Note that the primary view can be a preset view or a custom view.

View Orientation

This option allows you to change the view orientation before you place it. For example, if you just wish to place a single view, you can control the orientation by selecting this option and choosing from the following drop down list:



You can use this option if you don’t plan to add companion views.

Best Fit, Set View Scale, Scale List and Scale value



These options allow you to control the size of the view that you are placing. They are identcal options that you would find in the previous Drawing View Wizard command, and are used the same way.

Saved Settings

This is a new and very useful option to ST6. It allows you to save your layouts for reuse in other draft files. For example, if I always place a flat pattern of my sheet metal parts, I can place my first layout and save it. To do this I do the following steps:

1.    Start the Drawing View Wizard command and select the file that I want to place onto the draft sheet




2.    Set the Flat pattern option.




3.    Select the scale that I want to use. But do not click to place the view yet.



4.    In the Saved Settings dialog I name this layout as Flat and hit the save icon.




5.    Place your view.



The next time I run the Drawing View Wizard, with a Sheet Metal part that contains a flat pattern, I just have to select “Flat” from my saved settings.




Following the same steps I could save another layout showing the Front, Top, and Right view for the same model, and save it as “FTR_view”. The next time I run the Drawing View Wizard on a Sheet Metal part, I could select from either layout.




Note: I find saving layouts easier if you always start with a new draft file, per layout.
There are a couple of things to note here.
•    To use a saved setting, that setting has to be selected before the drawing view is placed on the drawing sheet.

•    Your saved settings are based on model type and model size. For example if I place a part file, I will not see the Flat or FTR_view saved setting, because I created them using a Sheet metal part.

•    Your saved settings can be predefined per model type and model size (for assemblies) on the Drawing View Wizard tab (Solid Edge Options dialog box).




    Items stored in the saved settings:
o    All properties from the properties tab.
o    View orientations
o    Custom orientations
o    Best Fit
o    Set View Scale
o    Shading Options
o    Edge Colors

•    Saved Settings file will be created in the reports directory called DraftWizard.txt.

Once you’ve created a list of saved settings, I believe that you’ll find the new approach more efficient and easier to use. But if you still prefer the old method, you can still use it. As always, if you have any questions, and are a customer of ours, please call us on the toll free tech line at 1-877-215-1883 or email us at If you are not a customer of ours, please contact your reseller for further support.

Ordered vs. Synchronous – Which should I use? – Part 1

John Pearson - Thursday, October 10, 2013
  1. I’ve been approached by many Solid Edge users who ask me if they should be using the synchronous or the ordered method for the designs. I always answer yes. To which they smile and usually ask “No, really, which is better?” To which I respond, why choose? Use both. This may seem like a political answer, but it’s not. The true power behind Solid Edge is the hybrid approach utilized through integrated modeling. To understand the benefits, we first have to look at the pros and cons of each paradigm.

Pros and Cons of the ordered paradigm

Ordered modeling has been in Solid Edge since day one. It is like an old friend that many long time users are comfortable with, and experienced in. Many of the users I talk to claim that they like the control that ordered modeling gives them. Ordered modeling forces the user to build the model in a certain order of steps, which are predefined by the intent of the designer.

For example, the designer starts with the sketch or profile for his/her base feature. He/she draws the profile and constrains it with 2D geometric and dimensional constraints. By doing this he/she is controlling how the sketch can change. This involves some thinking ahead and predictions of potential future edits. 

Once the sketch is complete, it becomes the parent of the base feature. In other words the sketch drives the base feature. Additional profile base features are then added to the base feature in a similar manner. Each becoming a child of the base feature, thus creating an ordered structure that is shown in the Pathfinder. Treatment features are then added, creating more parent child relationships, until you have a completed model.

The ordered structure appeals to a lot of designers. Especially, if the design lends itself to a master model approach, where you create a master model and then generate many variations off that model by simply changing a few parameters. This does require intelligent set up of the master model and a good understanding of how the model was constructed.

So when I ask my customers what they like most about ordered? I get the following list of Pros:

Very structured approach to modeling.
Predictability to the designer who created the model.
Ability to lock down how the model behaves.
Other users can’t accidentally change my design.
Easy to set up family of parts or family of assemblies with a master model approach.
Long accepted method of modeling with a proven track record.  
Creating the initial model is just as fast in ordered as it is in synchronous method.
I am use to ordered design and have lots of ordered legacy data.

From a designer’s point of view, all these are good reasons to stay in the ordered paradigm. However when I look at the list, I get a feeling of déjà vu. It looks very similar to the list of reasons that designers use to give for staying in 2D. But we all know that many companies have switched to 3D. Why? Because the industry recognized that switching to 3D design provided many advantages. In other words there were a lot of Cons in 2D design. So what are the Cons of the ordered method?

It should be noted that some of the Cons or disadvantages that I am about to list come from working with the synchronous technology for almost 6 years now. Many designers will disagree with some of these because they do not have a true understanding of how synchronous modeling works. So with that in mind let me list some of the main problems with ordered designs.

Forced structured approach to modeling.
Modeling requires the designer to predict how the model could change in the future.
Editing the model is slow and cumbersome if the designer incorrectly predicted the

        future changes, or uses the part as a reference part to initiate a new model.
Making changes requires an in-depth understanding of how model was originally  

        created.In some situations it has proven faster to re-model the part then to try

        and understand all the parent-child relationships.
On large models, re-compute times can be lengthy due to the structured approach.
Models are heavy because of all the history saved in the part files. This makes opening and saving times lengthy.
Working with foreign data can be a challenge without the history/feature tree.

I’m sure my colleagues, could list a few others, but I think that these are the main ones. The next question then becomes how can synchronous eliminate or minimize the problems we face in ordered, and is it enough of an improvement to start using synchronous modeling? To answer this question, let’s look at the Pros and Cons of the synchronous paradigm.


Pros and Cons of the Synchronous paradigm

If you believe the marketing from Siemens, they claim the following:

“Synchronous technology provides the first history-free, feature-based modeling technology that enables up to 100 times faster design experience.”

Let me clarify this statement. It is not saying that all your designs can be done 100 times faster. In fact, if you start a design from scratch, the initial design process may only be slightly faster in the synchronous paradigm. However, there are aspects of the design process, which are up to 100 times faster if not more. Synchronous takes advantage of today’s powerful computer processers, and the elimination of Parent-Child relationships, to allow fast flexible modeling. Yet, with tools such as Live Rules, Procedural Features, 3D driving dimensions (PMI), it still provides the designer with control over the design when needed. So let me give you my list of synchronous Pros:

Rapid, flexible design tools.
The designer does not have to predict how the model will change in the future. 
History free approach allows for instantaneous model changes while editing the model.
The sketch does not drive the model. The dimensions are migrated to the model and directly drive the model at the 3D level.
Rapid edit tools and handles allow the designer to edit the model without having to understand how it was originally modeled.
Can edit a part file or group of parts from the assembly level, without having to edit into each part.
Can edit models from any CAD system as easily as editing solid edge models.
Model can be constrained at the 3D level, but not really necessary.
Models are lighter therefore open and save faster than in the ordered paradigm.
Can convert legacy ordered models into synchronous models.  
Although a different approach to modeling, it shares many similarities with the ordered paradigm. Thus easier to learn for existing Solid Edge users. 

Given all the Pros, you may be asking why everyone hasn’t changed to synchronous modeling. I believe that there are a few reasons for the hesitance to change. The first is the way Siemens introduced synchronous technology. It was first launched in the fall of 2007 in Solid Edge ST. It was new, and limited to part modeling with no real tie in to the ordered parts. Many users tried it then, but were left unsatisfied due to the limitations. The following year Solid Edge ST2 was released and introduced synchronous sheet metal modeling.  But again there seemed to be two separate paradigms with limited connection between the two. This all changed with the release of ST3 which introduced integrated modeling, allowing users to combine both paradigms within the same part. Unfortunately, many users had already made up their minds based on their less than successful attempts with ST and ST2.

Another reason for resistance is lack of training. Too many companies fail to see the benefit in properly training their users in the synchronous paradigm. They expect the user to pick it up on their own, while maintaining the same level of output.  It has been my experience that this approach fails most of the time. Designers may attempt to learn it, but will often revert back to the way they know, in order to meet company deadlines. The user will often resist the change for no other reason than lack of time to properly learn it.

The third reason is that there are some definite limitations in synchronous modeling. Certain features or techniques behave better in ordered because of the nature of synchronous modeling. I list the main Cons of synchronous modeling as follows:

Certain features have limited editing capabilities and are handled better in the ordered paradigm. Some examples include:
o Swept and lofted features 
o Certain rounds and blends
o Surfacing
Dangling bends are not currently supported in synchronous sheet metal. This limits

certain functionality.
Training – users need proper training to understand the synchronous paradigm. 

Some users may believe that they have more control in ordered, but that is a myth, based on lack of knowledge of the synchronous modeling tools. I will explain this more in my next blog article. But let me finish this article by discussing the integrated modeling approach.

Pros and Cons of the integrated modeling approach

Solid Edge allows the user to start the design in the synchronous paradigm and add ordered features if necessary. This approach allows the user to utilize the best of both paradigms. The synchronous portion of the model becomes the parent of the ordered features. This allows the user to change the synchronous parent which triggers an automatic update of the ordered dependent features. Furthermore the assembly can be populated with ordered parts, synchronous parts, and integrated parts. 

The only Con for this approach is that the designer has to be trained properly.

In my next blog article I will continue this article and further discuss the reasons why  customers are resistant to changing to synchronous technology. I will show how these perceived reasons are based on myth or inaccurate information. It is my hope that after reading both these articles you will have a better understanding of synchronous technology and be willing to take a second look at how it can be integrated into your design process, saving you time and money. 

Synchronous Hole Recognition

John Pearson - Thursday, June 20, 2013

If you are using the synchronous modeling in Solid Edge ST5 you may have noticed the new Recognize Hole command found under the Hole Command flyout.

This command, specifically designed for imported models with no history, enables cylindrical cutouts to be automatically identified and re-defined as synchronous procedural hole features. It is available in the Part, Sheet Metal and Assembly environment. The user simply has to select the command and select the model. Holes are automatically recognized and displayed in the Hole Recognition dialog.


Hole types and sizes are grouped together automatically.


A user can choose not to recognize a cylindrical feature as a hole by toggling off the check mark for the feature.

Within the dialog, you can rename the hole features, by double clicking on the default feature name. You can also redefine the hole feature, by applying saved settings or by using the hole options dialog.

Once the user selects OK, to accept the hole options change, a preview of the new hole parameters is shown on the model. The user then selects OK, in the Hole Recognition dialog, to accept the change.

The user can use the Face Selection option to recognize holes only on selected faces.

Pre-selection of a face, or faces, is also supported. You can select a face, or faces, and then run the Recognize Holes command, to perform recognition on only the selected face(s).

The Hole Recognition command allows users to add intelligent synchronous procedural hole features to imported models. Because it’s a hole feature, it also recognizes the user defined pattern created in all hole features, which can be used for rapid placement of bolts or screws in the assembly.

Customizations and Upgrading Solid Edge

Cory Goulden - Tuesday, April 30, 2013
With the ST6 coming one thing is certain…changes are coming.  This next topic will discuss how to transition from ST4 to ST5 (and as well can be used for ST6 upgrades) in relation to the customizations in Solid Edge.
There are certain things that a CAD Administrator can set up for you and share amongst the masses.  If you do not have the luxury of a CAD Administrator, it is very worthwhile to have users share setups.  It would be best if there was only one person setting things up as this keeps everything to a standard.
Solid Edge can, quite easily, bring toolbar settings from version to version.  The toolbars can be re-used as it were.  Also to note is the fact that these customized toolbars can be deployed on a user specific basis as well as a base company template type setting.  For instance, a company standard toolbar customization could be deployed and the user would then be allowed to take it from there.  Every company has certain functions that vary from what SE sets up out of the box.  Companies vary as well.  Users vary even further.  It would be worthwhile to invest the time once to set up company templates and environment settings.  If you do it once, there would be years of savings moving forward.
The image below illustrates the settings you can set up and take with you from version to version.  Keyboard, Quick access, Ribbon, and Radial Menu options can all be set up.

Screenshot of "Customize" Menu


The next sessions we will discuss how to set up everything.  I always like to have the “Previous Window” (in Draft for this example).  These are the steps I would go through.  Open a draft file, although you can do this without opening a file.  Select the down arrow beside the QAT and go to “Customize the Ribbon”.

The following dialogue box opens:

Expand the “View” tab on the left and expand the “Home” tab on the right to look like the image below.

Have “Previous View” selected on the left and select “Window” from under the home tab on the right and then hit the “Add” button.  It should look like this:

Close the dialogue box and you should notice on your Home toolbar that the Previous View icon has been added.  You may be asked if you want to save this if you need to create a new theme or you could save it to an existing customization.

You can also right click and the following menu shows up allowing you to set the options for the new icon:


These settings are saved in the following locations in ST5:

Vista/Win 7:

C:\Users\”username”\AppData\Roaming\Unigraphics Solutions\Solid Edge\Version 105\Customization\


C:\Documents and Settings\”username”\Application Data\UnigraphicsSolutions\Solid Edge\Version 105\Customization\

Windows 7 shown below for reference:

These settings can be shared between different users and computers.  As you can see, each theme is in a different folder and each type of customization (QAT, Radial Menus, Ribbon, ect) is in a separate file.  Because it is external to the install directory of Solid Edge and is not in the registry these customizations traverse updates to the software version.

Solid Edge Quicksheets

Cory Goulden - Tuesday, November 20, 2012

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.