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How to Calculate the Surface Area of an Assembly

John Pearson - Thursday, March 19, 2015

Calculating the surface area of an assembly can be useful for your manufacturing and other downstream applications. For example, knowing the surface area can allow you to predict how much paint you will need. This knowledge will allow your purchasing department to procure the exact amount of paint in advance, while also helping your company determine production costs.

Here is the method for calculating surface area:


  • Step 1. In assembly environment go to Tools tab and toggle on Simplify and then select the Button 'Visible Faces'.
  • Step 2. Ensure the option 'Analyze Assembly' is active and click on 'Process'.
  • Step 3. In the next ribbon select the option 'Copy Body' and then click on Preview and Finish. A simplified assembly model can now be found in the       Pathfinder.
  • Step 4. Select the Simplified Assembly with the right mouse button and save it as a part.
  • Step 5. Close the assembly and open the just saved Part.
  • Step 6. You should now see the Construction body and also a Toggle to Design Body, i.e. you will now have a closed Body, currently without any assigned material.
  • Step 7Assign any material to the body via the Application Button --> Properties --> Material Table, otherwise you will not be able to calculate the mass, volume and desired surface of the part.
  • Step 8. Go to Inspect --> Physical Properties and in the sub-menu simply click on the Update Button for a fresh calculation of the model.


The system calculates the mass (dependent on the material), the volume and the required surface area.

​How to repair the parametric links in an assembly (Assembly environment and V&M)

Frederic Menage - Thursday, January 29, 2015



A parametric assembly contains links that can transfer data (number, geometric references) between components so that they can share common characteristics. Such a link can be updated if the communicating components are activated and if the active context wasn’t modified since the link was created.


The context

One way to alter the context is to use the ‘save as’ command when in the assembly environment. Solid Edge warns the user about the danger of such an operation:



Analyzing a “broken” model

If you have a parametric assembly that is unresponsive, select a part with a chain beside it and edit it. At the top of the modelling tree for that part, you will see a ‘Links’ collector. If you expand it, you will see the context (the complete path is in the tool tip as shown below) in which parametric features of that part can receive data from other components.



How to fix it with ‘Redefine links’

Open the View & Markup application (Start/Programs/Solid Edge...). In the ‘Tools’ tab of the ribbon, start the command called ‘redefine links’.

Select folder(s) in which all components of the “broken” assembly as well as the assembly itself reside. Note: for a complex assembly with many components distributed across multiple folders, it is possible to use a result log (txt file) of the V&M ‘search broken links’ command.

Enter the path including the filename to the original (old) context (the one listed in Solid Edge as shown in the previous image) and then the path to the current “broken” assembly (also with the file name).



Altering the context of a parametric model can occur in different ways. It is always recommended to use the revision manager and its ‘where used’ command when moving or copying projects or libraries in order to prevent this kind of damage. Nevertheless, mistakes happen and it is nice to have an easy tool to repair parametric links.

How to: 3D Sketching

Manny Marquez - Thursday, October 23, 2014

Check out our newest youtube video on 3D sketching.


View our collection of youtube tutorials and other videos here .



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.

Join us at the annual New York State Regional Users Group meeting

John Pearson - Wednesday, September 24, 2014

Designfusion is proud to be a sponsor and major contributor to this year’s New York State RUG meeting. This year’s meeting will be held at the RIT Inn & Conference Center in Rochester NY, on October 7, 2014. All users are invited, even those who live outside of New York State. Designfusion will be presenting at 8 of the 35 planned seminars.  Our focus this year is Solid Edge and Teamcenter Administration, however there are plenty of other presentations for all attending, as you can see from the agenda below.




Not only is this a great learning opportunity, but it’s also a chance to meet and network with other users and some of the people who support your Siemens’ PLM software.

There is a small fee to attend this event, and you must register in advance. You can do this online at  This site will provide you with all the details of the conference and directions to RIT Inn &

Conference Center. We hope to see you there, and don’t forget to drop by the Designfusion booth in the sponsor’s area.

How to video: Frame Design

Manny Marquez - Tuesday, September 02, 2014
Check out our latest Solid Edge tutorial by Manny Marquez.

For more videos take a look at the Designfusion youtube channel here

How-to create a reference in draft from the assembly

Charles-Etienne Lavoie - Tuesday, August 12, 2014

How-to create a reference view in draft and keeping associativity to your assembly.


1) Place the assembly has you would normally do in a MASTER MODEL draft,




2) To create the individual views, return to the MODELING environment.




3) Open the exploded view menu

4) Orient the view to the desire position and save as





5) From the exploded view menu, select hide component to hide the unwanted part

6) Hide the component




7) You can use the show component in view to show component





8) Save the work view when done




9) To change the work view to a canned view, RMB in the work environment and select replace view, from there select any view or use custom for a more specific view.




10) Return back to the drafting environment and add the newly create view to your sheet







How to reattach a bolt circle and its dependent dimensions (Draft environment)

Frederic Menage - Thursday, July 31, 2014


Draft annotations and dimensions rely heavily on their support geometry. Since it is possible with Solid Edge to attach dimensions to center marks, center lines and bolt circles; you have to know how to reattach those elements when the support geometry is replaced by another one.


So, as usual, you have modified your 3D model and the draft file needs to be updated. After updating the view, a dialog called the ‘dimension tracker’ automatically opens (default setting).

First, you can classify the changes by clicking on the ‘reason’ column header. The changes and auto-reattachments can be validated and cleared (‘Clear Selected’ button) and you can then focus on the detached elements.

The Bolt Circle Example

The first thing you need to do is select the bolt circle itself (not the dependent center marks). It should highlight as shown in the image below and a quickbar should appear.

The two circles shown in red are still used as a reference (Note: the bolt circle was created using the 3 points technique). One of the three gray dots doesn't have a red circle attached to it. You need to reattach that third grey dot (beside #4) to the circle with the detached center mark.

By left-clicking on that grey dot (handle) and dragging to the circle (hole beside #4), you can “fix” the bolt circle. You can see (on the image below) how all the holes on the bolt circle are now shown in red when it is selected.

Notice how the dimension tracker is now showing only one detached element.

It is also necessary to reattach the center mark itself. Start by selecting the detached center mark as shown in the image below.

You can see that the bolt circle doesn't highlight (it is different from center marks that are correctly attached). Select the grey dot at the center of the bolt circle and drag it on the bolt circle itself (avoid other center marks and other keypoints). Selecting the detached centermark should now give you this result (bolt circle shown in red).

The second step is to reattach the center mark itself to the hole. Simply drag it (left click on gray dot at center) on top of the circle with no centermark.


What is important here is that we did not have to delete and recreate any object. We updated our drawing by simply reattaching the handles to the appropriate references.

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

Cory Goulden - Wednesday, July 09, 2014

The area of major concern I see (and coincidentally usually by users that are self-taught) is that the user will rely on the tutorials to learn how to create models and drawings. There is more to 3D models though as models interact with each other.


A model is not just a shape. There are inter-dependencies that exist between the drawing and the model, that model and any assembly that may contain this model, and more advanced methods of creating links associatively.


Once this is understood ask yourself “What would happen if I used Windows Explorer and dragged something to a different folder?” Well, the part would be relocated. If that is what you wanted to do congratulations…or is it? I thought we were also concerned with these interdependencies? New users need to know how to properly accomplish common tasks so I will discuss this in this segment.


Also we have a 3D model. A picture is worth a thousand words right? Well maybe sharing a drawing is worth a thousand words but what is a 3D model worth? Maybe we can also share this information a lot easier than you might have thought.


There is an App for That

Solid Edge comes with an application called Revision Manager. This program is located under All Programs>Solid Edge ST6> and it is a component of a program called “View and Markup”. Under this program you can open files in two ways. We will look at Revision manager.


Revision Manager will open a file so you can see the tree structure that any model file has. This is the preferred method to relocate files, repair links, rename file, and so on. Below is an example of what you might see. From there you can RMB on a part and select the action you would like to perform. This tool can not only do simple tasks but it has some advanced functions as well.




First point covered. Please use Revision Manager and save yourself the anguish of breaking links all the time and becoming frustrated, relocating files and getting errors about “File cannot be found” and so on. This subject is an imperative one that is covered in Fundamentals training. If you missed it or forgot about it now might be a good time for review.


All In One

So we have made a change to the file using Revision Manager, now you would like to open it up in Solid Edge. Sometimes, I see even experienced users make this mistake, they will close Revision Manager and open SE and then re-open the file. No Need. In the image above you will notice an icon that has the name “Editor”. If you were to hit this button the model you have open in Revision Manager will open in SE. Pretty handy command.




Now you save the time and clicks of closing and opening another application, browsing to the file and waiting for it to reload.


It Is Always Polite To Share

Another thing you can do is send a lightweight version of this file to someone to view who does not have Solid Edge. How you say? The icon next to “Editor” states “View and Markup”. I will give you one guess what it does. When you hit this button, the View and Markup environment opens. I am only going to cover a very brief overview. If you would like to know more try to attend one of Designfusion’s Productivity Summits.




Here you will get a view of your model. Markups, notes, and even the ability to email to another person can be done. If an email is sent, using “Send to Mail Recipient” the link to download the Xpresreview program for free will be included in the body of the email. Yup I said FREE! It will also be a unique file format that should be allowed through most email filters. The file size is also reduced.




So in summary there might be a few items you may want to review. Mind you these subjects are covered in our Fundamentals course. A few snags you may commonly run into if you are trying to learn on your own that cost time and energy. Hopefully I have offered something of value.


Happy Edging!

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.