Using a Quick Query in Assembly

October 16th, 2012blog by Cory Goulden

Over the years I have noticed some gems in Solid Edge that I would like to share.  Quick Query I feel is a small but powerful little nugget.   I will list the steps below to perform a quick query in assembly and also try to state some benefits to this.  Trust me it takes longer to explain than to do.

Firstly it is important to note that parts and assemblies have properties embedded in them.  These fields should be used for a multitude of reasons from parts lists to searches.  It would be important for all to understand this before moving on.  Obviously these fields must have information in them in order for Solid Edge to report back anything.

Below I have an example part that exists in the example assembly I will use.

To check the properties

We can check what has been entered by going to the part properties.  Select the Solid Edge application button and go to Properties>File Properties.

You can also look at the property manager, which will be discussed at a later date, or perhaps through automation if you have a custom program to assist in entering this data.


As you can see below we have an entry of “hardware” in the “Category” field.  This is what we will perform a quick query on later.

We now return to the assembly.


Click on the “Select Tools” tab. 

Perform a quick query

RMB in the blank area just below the words in the title bar that say “Select Tools” and the following menu appears.  Note that these options correspond to those fields we had seen in the part properties.  You can set up a search to find these items based on these same categories.


You can see the many choices presented to you for searching.  Any one of them can be used.  For this example we will search the “Category” field.

Let’s set up a Quick Query to find and part in the assembly with the word “hardware” in the “Category” field.  We RMB in the blank area, and select “Category”.  This sets the Quick Query option to search the “Category” field in all parts and select and highlight all that contain the word “hardware”.

Once the text has been entered, press the enter key and you should have all the parts highlighted and selected like below:

Note that the highlighted parts are any that contain the word “hardware” in the “Category” field.  This search went into sub assemblies and patterns to select items.  It would also select different items as long as the field had the word hardware in it.   You could do a “Show Only” or other options for the selected set of parts.

There are many applications for this tool (another time we will discuss a full Query).  Quick Query is very useful.  It can select a set of items so you can do things like double check quantities or locations.  Also, because it shows only items matching the query, it can help determine if an item might also be missing properties.  This is good to know especially if those fields are required for a parts list in draft for example.



Accelerate tool design with a few simple surfacing commands

September 14th, 2012e-mail by John Pearson

After completing a 3D model of your design, it may be necessary to design some custom tooling for manufacturing. Solid Edge provides some very simple surfacing commands to aid in the rapid generation of tool design. For example, you may have to design a custom dimple punch or a dimple punch and die set. Let’s assume that you have to design a tool to create the dimple shown here.

For this example, I will just illustrate how you can quickly design the face of the dimple tool. In a new part template, I use the Part-Copy command to insert the sheet metal part containing the dimple.

I will insert this as a construction body.

Notice that I have several other options available to me, if needed, in the Part Copy Parameters dialog.

From the inserted construction body, I can copy the inside faces of the dimple. I select the Copy Faces command from the Surfacing tab > Surfaces group.

I select all the inner faces of the dimple.

I then hide the construction body and I am left with the inside surface.

Next I create a symmetric protrusion which encompasses the surface.

I then select the Boolean command.

With the default subtract option selected; I select the surface as my tool.

I then select the direction that I wish to subtract, or remove the material, from the protrusion.

The protrusion is trimmed from the surface, as shown.

I now have a perfectly matched solid to the inner dimple face. I can now model the rest of the tool.

Using the same procedure I could create a matching die if necessary.

Many users are unaware of the powerful surfacing commands in Solid Edge. As shown above, these simple yet powerful commands can significantly accelerate your design process. If you would like to learn more about surfacing, we offer training in our advanced modeling class ( or you could try the self-paced training course online at

Using Goal Seek to aid in model design

July 19th, 2012terms by John Pearson

The Goal Seek command is one of the calculation tools available for engineering problem solving. It is available in the 3D environments and while drawing 2D geometry in a 2D Model sheet, a drawing sheet, a profile, or a sketch.

The Goal Seek command automates engineering calculations, which can be based on dimensioned geometry, to achieve a specific design goal. Goal seeking finds a specific value for a dependent variable (dependent by formula, for example) by adjusting the value of another variable, until it returns the result you want. Goal seeking shows you the effect on the geometry and it will also update the Variable Table with the new value.

The following is just one example of how to use the Goal Seek command to aid in model creation. This example illustrates how to use the Goal Seek command to help design a sheet metal cover.

Note:  For this example, we have to create a hole pattern, on the top of the cover, to allow for air flow. From previous analysis it’s been determined that we need a minimum open area of 6000 mm². To achieve this we will start by creating a circular cutout and rectangular pattern.

I first create and position a 10 mm radius circle, as shown below, to create our initial cutout.

While still in the sketch environment, I select the Area command, from the Inspect tab > Evaluate group.

I then click in the area of the circle.

I accept the Area by selecting the green checkmark on the command bar.

Next I open the Variable table and locate the Area variable and rename it to Cutout_Area.


I also locate the 10 mm variable for the circle radius and rename it to Cutout_Rad.

I then close the Variable table and complete the cutout using the Through All extent option.

Next I create a Rectangular Pattern, as shown below, using the Fit option with the following values:

  • X: = 10
  • Y: = 5
  • Width: = 170 mm
  • Height: = 65 mm


The completed pattern should look like the image below.

To prepare to use Goal Seeking I need to create some User Variables. First, I find the X and Y occurrence variables and rename them to X_count and Y_count.

Next I create a Total_Area variable by clicking in an empty row and selecting the area type, from the pull down scroll, as shown below.

I then type in the name Total_Area and tab over to the Formula column. In the Formula column enter the following formula:



Note:  I have now created a variable to calculate the total open area created by the pattern. I can now use this variable to help adjust the cutout radius to obtain the desired area of 6000 mm².

To do this I select Goal Seek from the Inspect tab > Evaluate group.

The Goal Seek command bar will appear.

I select the Goal Variable, which is the Total_Area.

I then select the variable that I will allow to change to obtain the Goal variable, which is the Cutout_Rad.

Now I enter in my target value of 6000 mm². (I just have to enter in 6000)

Note:  Goal Seek will now run through a series of iterations, where it will adjust the cutout radius, until it obtains the target value. When it is complete, it will show you the finished model, and post the number of iterations it used and the total elapsed time it took, in the bottom on the Status bar.

If I open the Variable table and view the User Variables, I can see that the radius of the cutout is changed from 10 mm to 12.36 mm, and our total area is now 6000 mm².

Using the Goal Seek command allowed me to determine the optimal radius for my holes without having to do any advanced calculations.

For more practice, try the Solid Edge tutorial on ‘Using Engineering Calculation Tools in Solid Edge.


NX – Create a family of standard parts (Excel)

July 4th, 2012blog by Charles-Etienne Lavoie

Design Intent:  The most common use of Part Families is to define a standard library part that has many variations.

     1.  Create an hexbolt  

     2.  Rename the expression that you want to keep

             a: Width = the radius of the cap

             b: Length = length of screw

     3.  Define the columns for the Family Table.

 >Choose Tools→Part Families from the main menu bar.

 >Make sure the Importable Part Family Template option is  cleared.

 >Click OK on the Warning dialog box.

 >Select the width expression from the top window of the Part Families dialog box.

 >Click the Add Column button.

 >Select the lenght expression from the top window of the Part Families dialog box.

 >Click the Add Column button.

Note:  Instead of choosing, Add Column, you could just double-click on the expression name in the Available Columns list, i.e. head_dia.

> Change the option menu at the top of the dialog box from Expressions to Features.

> Double-click chamfer from the top list of the Part Families dialog box.

Note:  The order in which you select the attributes determines the order of columns in the spreadsheet.

Tip:  In production, you would specify a writable folder for the Family Save Directory, but it is not necessary for this activity since you are not creating Part Family Member files.

     4.  Create the family table.

  > Click the Create button from the bottom portion of the Part Families dialog box.


 > Type in a few values

    5.  Verify a family member

 > Select a cell in row 3.

 > From the spreadsheet ADD-INS menu bar, choose PartFamily→Verify Part.

The NX session becomes active and the family member is displayed in the graphics window.

 > Click Resume in the Part Families dialog box.

Warning:  The Part Families dialog box may be obscured, if so, click anywhere in the NX window.

     6.  Save the Part Family and the template part.

 > From the spreadsheet menu bar, choose PartFamily→Save Family.

Note:  The Save Family option internally stores the spreadsheet data within the template part file. It does not save the template part file itself.

Note:  In order to save the template part containing this newly created Part Family Spreadsheet, you would also choose File→Save.

Since we do not use this part anywhere else we are not going to do that.

     7.  Close all parts.


Using the mouse to manipulate the model view in Solid Edge

June 21st, 2012e-mail by John Pearson

The middle mouse button, or scroll wheel, provides improved model rotation in ST4. You can now select a vertex, edge, or face as the model rotation center. To do this, simply following the steps below:

First you must let the system know that you want to enter the rotation mode. This is achieved by a single click to the middle mouse button (MMB), on an empty space. You will notice the cursor changes appearance. Before you click the MMB your cursor looks like this:


After you click the MMB you cursor will look like this:


Notice that the little blue face, indicating selection mode, has disappeared.

You now have three options available to you: 


1. Rotate using a position on a face.

  •  - You can now move the cursor over the face shown below. Notice the dark pink dot, indicating that you are in the rotate mode.


  • - If you now hold the MMB down, the part will rotate about the dark pink dot. In other words, the dark pink dot becomes your center of rotation.


2. Rotate using a position on an edge.

  • - You can move the cursor over any edge. Notice the entire edge highlights.


  • - Holding the MMB down allows you to rotate about the edge. In other words, the edge becomes the axis of rotation.


3. Rotate using a position on a vertex.

  • - You can move the cursor over any circular edge. Notice the entire edge highlights.


  • - Holding the MMB down to rotate allows you to rotate about the vertex of the circular edge. In other words, the vertex of the circular edge becomes the axis of rotation.


Note:  Once you have completed the rotation, you are returned to selection mode. You will have to single click to the middle mouse button (MMB), on an empty space, if you wish to perform another controlled rotation.


Other handy mouse controls in Solid Edge

 - Pan the view. Press the Shift key while you drag the MMB to pan the view.


- Zoom. Scroll the mouse wheel to zoom in and out.


Note: The setting for this scroll behavior is found in Solid Edge options_Helpers page. Enable Value Changes Using the Mouse Wheel. If this option is on, the mouse wheel changes the value in a value edit field. Use Ctrl+mouse wheel to zoom in or out.

- Zoom Area. Press the Alt key while you drag the MMB to zoom into an area.

- Double–click the MMB: Fits the view.


Solid Edge University 2012 spotlights ST5

June 14th, 2012terms by John Pearson

Nashville, Tennessee, was the site of this year’s Solid Edge University convention. User’s got their first real look at ST5, which will be released next month. Dan Staples, Director of Solid Edge Product Development, introduced ST5 to a large and enthusiastic crowd. Now that the synchronous paradigm has been implemented, the focus seems to be on implementing as many user requests as possible.


The new functionality in ST5 benefits all users, whether they work in the ordered or synchronous paradigms. To see what’s new in ST5 visit the Solid Edge ST5 web page.

 After Dan’s presentation, users had a selection of breakout sessions that they could attend. These sessions included closer looks at what was new in ST5, sessions on how customers use Solid Edge, knowledge enhancements sessions, and round table sessions. The round table sessions allowed users to tell the planners and developers what improvements they liked and what else they’d like to see added to the software.

Our own John Pearson presented a session on the Draft environment and improving the speed of drawing creation in Solid Edge. John was amazed at how many users attended his session and extremely pleased at the number of users that approached him afterwards to thank him, and mention how much they had learned.


For those of you who were unable to attend John’s presentation, you can click here to download the PowerPoint and accompanying help documentation.

 John and Manny Marquez, from our Chicago office, were able to meet with many of our customers at the conference. The overall feeling around ST5 was very positive and users seemed genuinely excited about this release. We’d like to thank those users who attended the conference and we hope to see many more of our users at next year’s event.