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How to create an adjustable coil spring

John Pearson - Wednesday, September 18, 2013
How to create an adjustable coil spring

If you wish to create an adjustable part, you must build a part that is adjustable. Sounds obvious, but sometimes what seems adjustable to the eye is not adjustable in the CAD system. For example, let’s look at this coiled spring.

New users may look at the part and model it using the helical protrusion command to make the coil. Then use protrusion and/or swept protrusion to complete the part. This will look good but will not be adjustable. Why? Let’s look at the part in an adjusted or deformed state.

Notice that the coil deforms as the part adjusts. If you model this with a helical protrusion, the rules of the helix will prevent you from deforming the coil. So how do you model this to get the adjustable results?

There may be other ways to model this part, but I find this method fairly easy to create while giving me the control I need. I start by creating a flat sketch of my part, on the Top reference plane.

Notice the 2 lines labeled A. These lines represent my wrapped coil center lines. My wire will be 7.5 mm in diameter, so I’ve made the opposite ends 8 mm wider, to avoid any body intersection. The 157.1 mm length of these lines is equal to the perimeter of the initial coil size. I‘ve used two tangential arcs to create the lines, because it generates a nice smooth flowing coil.

I then create a second sketch on the Right reference plane to represent the initial coil position.

The top quadrant is connected to the (0,0,0) point with the center of the circle horizontally aligned beneath it.

I then create an extruded surface, which I will use to wrap the coil around. The Extruded Surface command is found on the Surfacing Tab, in the Sufaces group.

Next, I use the Wrap Sketch command to wrap the arcs around the extruded surface. This command is found under the Surfacing tab, in the Curves group.

I am first prompted to select the face that you will wrap around. I select and accept the extruded surface.

I am then prompted to select the sketch that I wish to wrap. I set the selection filter to single and pick the four arcs from the sketch.

Once I accept the selection, the arcs wrap around the extruded surface.

To make it easier to visualize the next steps, I hide the extruded surface. I then create a sketch, to represent the diameter of my wire, centered on the top of the flat wire, on the Front reference plane.

I then use the Swept protrusion command to create 3 features. Note: I use the following options when creating all 3 features.

The first swept feature looks like this:

The second swept feature looks like this:

The third swept feature looks like this:

Finally, I hide all sketches and curves, and then I create the last two wire sections. I could use several different methods to create these sections, but for simplicity I used the Thicken command, and simply thicken the end faces the distance that I need.

I now have the modeled part which I can make adjustable.

In this model we want to adjust the tilt angle of the legs, which is actually controlled by adjusting the diameter of the coil.

To simplify the process I open the Variable Table and rename the variable that controls the diameter of the coil, to Coil_diam.

I then create an associative sketch, on the Right reference plane, to allow me an easy way to monitor the tilt angle of the legs.

Note: I used the Include command to create this associative line.
In the Variable table, I located  the 90 degree variable and renamed it to Tilt_angle.

If I change the Coil_Diam  value, I will notice that the Tilt_angle  value changes because of the associativity between the Sketch and the model.

For example, if I change the Coil_Diam to 55 mm the Tilt_angle changes to 57.27 degrees.

Now that I have this relationship, I can use the Goal Seek command to get the exact Tilt_angle  value, that I need. 

I select the Goal Seek command from the Evaluate group, under the Inspect tab.

On the command bar I input the following information;

Goal: Tilt_angle
Target: My desired Tilt_angle (e.g. 45 degrees)
Variable: Coil_diam

When I accept this input, the Goal Seek will run through a series of iterations, until it finds the exact Coil_Diam value, to give me the desired Tilt_angle value. 

In the example, the results are as follows:

I now have a part that can easily be adjusted, without having to create any complicated formulas.

Note:  Clearly the deformation of the coil has it limits. If you enter in too large of a Tilt_angle, the model may fail. I have also kept this example simple; therefore if you try too many different angles, without resetting back to the original angle, the model may fail.

It is important to note that this example could be created in several different ways and still provide you with similar results. The main thing here is that the model must have the flexibility to adjust. If I had used the Helix command instead of the Wrap Sketch command, I would not be able to adjust the coil. I can also obtain the desired results using the Goal Seek command. This saves me from having to derive complicated mathematical formulas. 

How to copy styles from an existing document to an active document

John Pearson - Thursday, August 29, 2013
I recently had a technical support call, in which a customer wanted to add her own styles to the company template. She did not have access to the company templates, to change the styles, but needed to add specific styles for her current project. She wanted to know if there was a way to achieve this task without having to recreate the styles in every new document.  Fortunately the answer is yes. There is an often overlooked tool in the styles dialog called the Style Organizer. The Style Organizer tool is found on the Style dialog box.

The following steps are used to copy a style from an existing document to your active document:

Step 1. From the active document choose View > Style > Styles. 

Note: This example uses images from the part environment. The steps are the same in the draft environment, but the ribbon bar looks different.

Step 2. On the Style dialog box, set the Style Type box to the type of style you want to copy.

For example, you may want to copy an existing Face Style that you previously created in an older document.  In this case you would highlight the Faces Styles, as shown below.

Step 3. On the Style dialog box, click the Organizer button.

Step 4. Browse to locate the existing file that has the styles that you want to copy.

Note: In this example, I browsed for an existing file called Head Board.prt. Notice that all the Face Styles for Head Board.par are listed in the left side window and all the Face Styles of my active part are listed in the right side window

Step 5. Locate and select the Face Style that you want to copy and click Copy.

In this example I want to copy a “Wood, Cherry” face style, from the Head Board.par. I scroll down to locate the Face Style, highlight it, and then click Copy.

Notice that the “Wood, Cherry” face style now exists in my active part file.

Step 6. Close out of the command and use the style as you see fit.
Remember, you can copy any style, such as Dimension Styles, Drawing View Styles, Hatch styles, etc. into your active document. You may have noticed that you can also delete unwanted styles, using the command.

This is also a great tool for updating templates. If a user has created a style that he/she uses all the time, the CAD administrator can use this command to copy it into the company template. This is much easier than trying to recreate the style and also ensures accurate results. I hope you find this tool as useful as I do.

ST6 Released!

Cory Goulden - Saturday, July 27, 2013

Hot off the Press….ST6 RELEASED!!!

It is with great anticipation and excitement that I can say Solid Edge ST6 has once again been produced as a top quality product that has TONS of new functionality and features.  The latest version of Solid Edge has been released…officially. 

You may have received a new license file via email earlier.  As this is (once again) an exciting release I wanted to mention a few very high level notes about installing.*

*Of course you will always read and follow the install notes.

Prior versions of Solid Edge required you to turn off User Account Control (UAC) before installing.  This is part of Microsoft’s attempt to make the software more secure.  There are certain areas in programs that require read access and other components that require read and write access.  Microsoft requires programs to have the areas that require write access to be set aside in a designated folder.  This folder, in ST6, is called the “Preferences” folder.

The preferences folder is here:

C:\Program Files\Solid Edge ST6\Preferences

 Things like your license file (SELicense.dat by default), options.xml file, material.mtl file are located here now.  Things a user may need to have modified.  For those of you who attended my presentation on the SEAdmin functionality of SE the preferences folder location itself cannot be changed.   See below for an image of what the contents of this file are.

Happy Edging! 

Solid Edge ST6 introduced at SEU2013 – Part 2

John Pearson - Thursday, July 25, 2013

In last week’s blog I had started to discuss what was new in Solid Edge ST6, as introduced to us at Solid Edge University 2013 (SEU2013). I had left off with mentioning the new enhancements in surface modeling. So let’s continue with what’s new in Part and Sheet Metal modeling.

ST6 Part and Sheet Metal Design

Improved Steering Wheel – now has 3 directional axes to eliminate the annoying need to always flip the steering wheel.

Improved solution manager – including color control, something I had requested for some of our color blind users.

Faster revisions with synchronous technology - Include or exclude edges of peer parts during creation. Added exclude interior loops or use only interior loops, to the Extrude planar face option from ST5.

Better reuse with synchronous technology

  • ·         More robust rectangular and circular patterning.
  • ·         Pattern recognition allows count and instance editing of imported patterns.
  • ·         Partial round delete with end capping.
  • ·         Dimensioning chamfered edges uses virtual vertices.


Create stamped sheet metal parts with a single command – emboss a tool or punch into a sheet metal part.

Stiffen parts by adding features across bends - add beads, dimples, louvers, emboss features across bends

Sheet Metal Features on Parts - sheet metal features can be placed on regular ordered parts of uniform thickness without having to transform the part to sheet metal. This provides an especially efficient method in stamped metal design.

Again, there are many other enhancements in Part modeling which will benefit all users.


ST6 Assembly Design

Solid Edge continues their dominance in working with large assemblies. Along with some nice enhancements to PathFinder Indicators and Physical Properties, here are my favorite improvements:

Assembly occurrences can now be used for inputs to Boolean operations - No inter-part copy of the geometry is needed and multiple tool body components can be selected (see previous blog article).

Faster display - New display capabilities speed pan/zoom/fit by up to 2 times.

Complete overhaul of simplify assemblies

         New environment for creating user defined simplified representations.

         Enclose component automatically encloses components with rectangular or cylindrical solids.

         Duplicate body speeds simplification of copied or patterned components.

         Goal is to simplify models for effective design of 1 Million+ parts.


Create In-Place Enhancements – moved to optional QuickBar with better control over placing the origin.


Synchronous Assembly Modeling Peer Edge Locate – allows for improved key-point selection when modeling in the Assembly.

Plus several new enhancements to synchronous commands have been made while a user is in-place activated into a part or sheet metal file from an assembly.

ST6 Drafting

Two of the most exciting enhancements in Solid Edge ST6 appear in the Draft environment. When the following was demonstrated they received an enthusiastic round of applause from the audience at SEU2013.

Alignment control

         Align annotations with a linear, rectangular or fitted shape.

         Reposition the annotations by dragging the alignment shape.


Dimension auto-arrange

         Clean up messy dimensions with a single mouse click.

         Select dimensions by fence or by drawing view.

         Creates and aligns dimension grouping.


Some other notable changes in drawing production are:


         Faster zoom/pan, and hatch display with large 2D drawings.

         Auto-constrain 2D elements during drag-modify.

         Retrieve slot feature centerlines.

         Partial bolt hole circles.

         Simplified drawing view wizard.

         Shortcuts and easier sheet tab creation.

         Edit tables in place.

         Better editing of embedded documents.

         Drawing views are now displayed before placement.

         Derived break lines from one view to another.

         Align any drawing view with key-points or drawing view centers.

         2D directional fence select: left for overlapping, right for inside locate to.

         Create tables from placed blocks on schematic drawings.


These enhancements, and more, continue to make Solid Edge’s drawing capabilities the best on the market.

Help for SolidWorks refugees

One other noteworthy feature, added to Solid Edge ST6, is the new SolidWorks migration tool. Siemens is going after the SolidWorks customers who are concerned about the kernel change and loss of legacy data. This tool, combined with some other enhancements, will allow the SolidWorks user to:

  • ·        Protect their investment in design.
  • ·        Get the power of synchronous technology.
  • ·        Maintain speed and reliability with Parasolid.

  • If you are a SolidWorks customer and are concerned about the ongoing changes and mixed messages from Dassault Systemes, Siemens is willing to help you transition to Solid Edge, while protecting and reusing your legacy data.


Solid Edge ST6

As mentioned at the beginning of the article, I have only scratched the surface of what’s new in Solid Edge ST6. I did not even mention the enhancements in the simulation package, standard parts, framing, or data management. I will attempt to expand on the improvements in future blog articles. But I felt it important to give an overall account of Solid Edge ST6, as presented at SEU2013. I have worked with Solid Edge for over 10 years now and I am truly impressed with how the development team continues to listen to the actual customers. Solid Edge ST6 enhancements have truly been driven by the customers. The 3 core values for this release were to:

  1. 1.    Accelerate design for faster time to market.
  2. 2.    Faster revisions for higher repeat business.
  3. 3.    Better reuse for lower development costs.

Siemens has done a great job at meeting these core values with Solid Edge ST6. Judging by the excitement at SEU2013, this looks to be a great release with customers eagerly awaiting the arrival of Solid Edge ST6. The release date has not been finalized yet, but the general consensus is that customers can expect to receive their copy sometime in August 2013.

Solid Edge ST6 introduced at SEU2013 – Part 1

John Pearson - Friday, July 12, 2013

In the last few blog articles I have highlighted a couple of enhancements coming in Solid Edge ST6. Having just returned from Solid Edge University 2013 (SEU2013), where customers were introduced to Solid Edge ST6, I thought I should try and list some of the more than 1300 enhancements. Clearly, with over 1300 enhancements, it would be a major job to list and discuss all the changes, so I will only highlight some of the major improvements.

Before looking at some of the new features in Solid Edge ST6, I think it’s worth mentioning that in Q2, Solid Edge license business in the US has seen a 25% year over year growth. Combine this with the growing number of packages that work with Solid Edge; it is clear the Siemens is fully committed to the continued growth and success of Solid Edge.

Some of the new partners introduced at SEU 2013 include CAMWorks for Solid Edge, KeyShot and CRABCAD, just to name a few. I found the CAMWorks for Solid Edge to be the most intriguing new partner. It allows for machining of your Solid Edge model directly in the Solid Edge package. I will discuss this in future blog articles once I have been fully trained on this new package.

It was also clear, to the over 500 users that attended SEU2013, that Siemens is listening to their customers. As I mentioned earlier, Solid Edge ST6 satisfies over 1300 customer requests. This is the breakdown as presented to us at SEU2013:

So what did I find to be the most intriguing new features? First, I really like the new ability to install multiple versions on the same computer (see earlier blog article on how to set this up). Although this is for test purposes only, it will go a long way to allowing smoother upgrades, especially for smaller companies. Solid Edge ST6 also adds some new user experience tools, such as:

New user persona environments - to customize the user environment based on his level of expertise with the software.

YouTube in Solid Edge - The YouTube search and upload feature within Solid Edge ST6 allows you to upload pre-recorded videos, or record your own video within the UI and upload it directly through the Solid Edge application.

Record Videos in Solid Edge - Solid Edge ST6 provides the ability to record design workflows within the application.

Command Finder Updates - Enhancements have been made to the Command Finder to provide the user with additional information for searched items that are not considered Solid Edge commands.


Android Tablet Viewer - Solid Edge now has an App available to view part, sheet metal, and assembly files on an android powered tablet. Similar to the iPad App introduced in ST5.

Combine these new tools with enhanced learning tools and the expanded Solid Edge community, and you will find the overall user experience is greatly improved.

ST6 Surface Modeling

Some major improvements in Part modeling also impressed me and many of the other users at SEU2013. My favorite enhancements include the following:

Major overhaul of the Surfacing environment

  • ·         New easy-to-use 3D surface control handles for on screen edits of curvature with graphical            magnitude handles and numeric values.
  • ·         Key-point curves now with C2 support.
  • ·         Robust bounded surfaces also with C2 support.
  • ·         Blue surface command now has C2 handles and optional curvature combs.
  • ·         Trim and extend is now a single super command.
  • ·         Ruled Surface command added - allows the user to pick a curve and
  •        generate a sweep of linear cross section along a curve or edge.
  • ·         Redefine Surface command added - that allows a surface or group of adjacent surfaces to            be replaced with a single editable BlueSurf.
  • ·         Model Reflective Display - a new display mode has been introduced specifically designed            for studying curvature and volumes of surface models of symmetric parts.
  • ·         Plus so much more to allow users to model highly aesthetic consumer products.

There are many more improvements to mention, and I will continue to do so in next week’s blog.

How to show/paint individual parts/components in a draft file

John Pearson - Thursday, July 11, 2013

In the following example I wish to show only the weld bead as a solid in the draft view.

To do this, I first create a Fill Style by doing the following:

On the Home tab > Dimension group select the Styles command.

Select Fill from the Style types: list, in the Style dialog.

Click on the New button in the Style dialog.

In the Name: field type in a new name, for the style. In this example I used Weld.

Move to the Properties tab and select a desired fill color from the Solid color: pull-down list.

In this example I selected Dk Gray. Click OK.

Click Apply to accept the new Fill Style.

Now I can paint the sections in the draft view by doing the following:

From the Sketching tab > Draw group, select the Fill command.

Select the Weld fill type, from the list in the command bar.

Now select the enclosed areas that you wish to paint on the draft views.

I now have a solid looking weld bead, while maintaining the wireframe look to the rest of the parts in the drawing view.

Synchronous Assembly Modeling Boolean Commands in ST6

John Pearson - Wednesday, July 03, 2013

The user can now use faces and bodies from other assembly occurrences directly when executing Boolean operations for the “Tool” step such as Union, Subtract, Intersect, and Split.

This enhancement is intended to remove the Inter-Part Copy step during a synchronous in-place activated modeling operation. Not having to create Inter-Part copies accelerates the design process and avoids the necessity of having to save the Inter-Part copies in the PathFinder.


Let’s have a look at the following example:

In this example, I have raised the motor up to show that we need to place some cutouts and holes in the underlying plate.

First, I will edit into the Base Plate part from within the assembly. Make sure that the Hide Previous Level command is turned off in the Part environment. 

Next, I select the Boolean Subtract command from the Solids group in the Home tab.

You are prompted to select the target bodies for the Boolean. In this example, I select the base plate part. 

You are then prompted to identify the tool bodies. In this example, I select the motor and the four mounting bolts, and accept the selection. 

If we hide the tool bodies, you can see the result of the Boolean operation.

Remember, this is a synchronous part, so we can easily add a dimension to the inner cutout and increase the size for clearance.

We can also use the Recognize Hole command and easily convert the holes to threaded holes.

This is just one of the many new features in Solid Edge ST6 geared to accelerate your design process, allowing for faster time to market. 

Solid Edge ST6 Offers Multiple Version Installation

John Pearson - Thursday, June 27, 2013


Solid Edge ST6 Offers Multiple Version Installation


Solid Edge ST6 now provides the user with the ability to run multiple release versions at the same time. This will allow easier testing of new releases prior to putting them into production. The earliest supported version of Solid Edge for multiple install with ST6 is Solid Edge ST4.


Solid Edge Multiple Install will not allow certain combinations of the software to be installed together. For example, users will not be able to have multiple versions of MP’s (maintenance packs) installed from the same release version.


Users should also not install different 32/64 Bit versions of Solid Edge on the same system.






Since this new feature is designed for testing purposes, secondary applications are not fully supported with multiple installs. For example, Solid Edge Embedded Client, Standard Parts, Automated Executions, are not supported.


In order to successfully install multiple versions of Solid Edge, the user must run a silent install on the latest version. Before running the silent install, a few steps must be followed:


1.    When installing multiple versions of Solid Edge, it is recommended that users install the oldest version first, followed by the latest.

2.    Ensure that you install the associated MP for the oldest version prior to installing the second version on your system.


3.    Ensure that the user attempting the silent install has administrator privileges.



Solid Edge Silent Install


You can silently install Solid Edge ST6 using the following command. Be sure to enclose path names in quotes if they contain spaces.


Note: Do not silently install Solid Edge if you use Standard Parts or Web Parts. These components require the .NET framework, and the .NET framework is installed only when you run setup.exe.


C:\>msiexec /i “D:\CM_SETUP\DISK1\Solid Edge ST6.msi”


USERFILESPECXML=”K:\temp\My Docs\Options.xml”

USERFILESPEC=”K:\temp\My Docs\selicense.dat”

INSTALLDIR=”C:\Program Files\Silent Solid Edge\” /qn+

/l*v “K:\temp\mysilentsetup.log”


·         The string D:\CM_SETUP\DISK1\Solid Edge ST6.msi represents the fully qualified path to the Solid Edge MSI file. The drive letter D is only an example of the drive letter for the DVD ROM. Your drive letter may be different.


·         The MSI property MYTEMPLATE indicates which type template files are to be installed. Ignoring this property defaults the installation to ISO template files.





















·         The MSI Property INSTALLDIR is used to specify the installation folder for the application.


·         The MSI Property USERFILESPECXML provides the optional installation of a SE Admin file. You should supply a fully qualified path and filename. This file is copied to the Solid Edge Program folder and processed at the end of the setup.


·         The MSI Property USERFILESPEC optionally provides a license file that setup copies to the Solid Edge Program folder at the end of the setup.


·         The argument "/qn+" instructs the Windows installer to provide NO user interface and alert you at the completion of the setup using a dialog box. Refer to the Windows help system for further information about Windows Installer arguments. Leaving this argument off the command line will display the setup user interface with selections made and fields provided.


Note:  If you are using this option, some installations that require user interaction could fail.


·         The argument "/l*v" tells the Windows installer to create a log file of important messages, warnings and errors and write it to the location provided, in this example, K:\temp\mysilentsetup.log. Additional information regarding logging options can be found in the Solid Edge readme.txt file.


Note:  Solid Edge requires Microsoft SQL Server 2008 Express. Solid Edge setup.exe automatically installs SQL Server 2008 Express, if it does not exist on the machine. The msiexec utility, commonly used for silent install, will not install the SQL Server 2008 Express software. This must be done manually.


Note: After you complete the commands on the command prompt and press “Enter” there will be no indication that the install is running. The install will run in the background until complete, in which case it will inform you whether it was successful or not.

Set Active Solid Edge Version


When running multiple versions of Solid Edge on a single machine, users will have to decide which version they will want to be active.



Users will be provided with a SESetActiveVersion.exe tool in order to switch between active versions of Solid Edge.


This will be located within the “DVD\Solid Edge\SptTools\SESetActiveVersion” directory on the installation disk. The User Interface provided with the tool will show which major release versions of Solid Edge are present on the system. To activate a different version, select the desired option from the drop down list and click “Activate”.

Uninstalling Multiple Versions


Upon completion of your testing of Solid Edge ST6, it is recommended that you uninstall all versions and reinstall the production version from scratch. The possibility of corruption of the remaining versions exists following the uninstalling of only one version of Solid Edge.

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.