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How to Model an Airfoil

Manny Marquez - Wednesday, March 12, 2014
Last week, on my flight back to Chicago, I always find it more enjoyable for long flights especially to have the window seat for a few reasons. Of the few things that I enjoy, one is watching how thrust is pushed in between the turbine blades of the engines and how the wing flaps pivot when used for breaking as the plane lands.

When I had landed, a thought came to me; and that was that I have never seen a turbine engine airfoil blade or wing model in Solid Edge. So I took it upon myself to do some research on how I would model airfoils. I came across some interesting web sites that explain the whole explicit mathematical functions used for 2D curve definition for airfoil design; very fascinating however, I just wanted the basics.




Here is the basic anatomy of a blade; you have root type, root width, root height, and airfoil height.

For many years, research and studies have been conducted on airfoil blades and also on the performance of wing design aerodynamics. Shown below is an airfoil generator for blades that I found online.

As you can see by entering the appropriate values you should be able to generate an airfoil based on you requirements.

Geometry Airfoil Generator Example: 



After generating the foil you have two options, either to create a DAT file or simply copy and paste the X,Y,Z coordinates to your excel.

I chose to just simply copy and paste directly to Excel. Notice A=X B=Y C=Z, in some cases if you are creating a simple airfoil you may only get XZ coordinate values. If that is the case you need to insert a cell and enter zero for Y as shown in this case.



 1. Before you start anything you will need to model up the root type, make this part in ordered. Surface modeling works best on the ordered mode. I downloaded a CAD model from GrabCAD website. If you have the time to model, a basic shape like shown below, make sure the XYZ origin is setup correctly. Therefore, when creating the airfoil via the Solid Edge curve by table option, it is placed correctly on the root top surface.



2. Next click on the curve by table option. It is located in the surfacing tab on the curves group.



3. Click on browse, then find the excel files.


4. Select finish. Notice the 2D airfoil automatically sets on the origin.



5. By clicking on the edit points data step, the Excel sheet will open. If there should be a need to modify the XYZ points manually you will be able to do so at this step. Click finish when you are satisfied.



6. Another option is to set the curve fit and curve end conditions.


7. On the next step, we are going to create two User coordinates systems.
Under the surface tab, find coordinates system on the planes group. This will allow us to place new airfoils at any point in space.

Select (key-in (relative to another Coordinates system)


8. Enter 3 on the (Y), next then preview and then finish. Repeat the same step for the second UCS, except enter 6 for (Y).


You model should look like this.



Now, we can continue since we have created the UCS to place the airfoils.

9. Repeat the same steps for the second airfoil. You may have as many airfoils as you wish- usually that varies on how
complex your blade may be. For this example, I will only be using three airfoils.


10. This time before clicking on finish, select the second coordinate system (the names may vary).



Repeat for last Airfoil.



Your model should look like this: Root with all three USC in place.

11. We are now going to create a BueSurf. This will create the outer shell for each airfoil, thus creating the turbine blade.

12. Click on the BlueSurf command, located on the surfaces group.

13. Select the first airfoil sketch.




Make sure the cross section vectors are consistent with the other geometery.

14. Select on the second airfoil sketch, notice again the vectors are consistent with the first selection.



15. You model should look like this.



16. Continue on with the selection



The overall blade has been constructed, we will now add rotation to the blade. Some blades have more complex geometry, I’m only using three airfoils to crreate a simple blade

17. Select the origin, and then click on edit definition.




18. Click on the orientation step.



19. Enter 25˚ for the Y direction.



Notice the foil is now 25˚ about the Y

20. Repeat the same step for the last coordinate system. Enter 30˚



21. You have completed this turbine blade using a geometry generator with BlueSurf. I hope you enjoyed it.

Did you know that you can do this in Solid Edge . . .

John Pearson - Tuesday, February 11, 2014

Did you know that you can do this in Solid Edge . . .

As a support team member, and technical trainer, part of my job is to learn the technology inside Solid Edge. Therefore, I’m allotted time to learn, test and research the latest technology. But as I’m sure many of you will agree, this is a privilege most users don’t have. Users are under the gun to meet deadlines and therefore often stick to what they know, even if it’s not the most efficient approach.  As a result many users are unaware of the full potential of Solid Edge. 

On more than one occasion I have received requests for custom programming for capabilities that already exist in Solid Edge. I often find myself saying “Did you know that you can do this in Solid Edge already”. With this in mind I thought it might be a good idea to start recording some of these moments and share them in our blog. So below are some of the questions I get from our customers along with how to do it in Solid Edge.

I have to delete a part list from my draft file, is there a quick way to delete all my balloons, or do I have to pick them individually?

Did you know that you can do this in Solid Edge using the SmartSelect command? To select all the balloons at once do the following steps.

- Pick the Select tool to launch the Select tool command bar.




  • - Select the SmartSelect icon from the Select tool command bar.



  • - Select one of the balloons from your view.

  • - The SmartSelect Options dialog box appears.  Check Element type and click OK.






  1. - Notice that all the balloons highlight.
  2. - Hit the Delete key and they are all deleted.
  3. The SmartSelect command searches the active sheet for other elements with similar attributes, such as element type, color or line width. All matching elements are automatically added to the selection set. Now you can make changes to the selected elements all at once. This is ideal to make changes or delete dimensions, lines, callouts, etc. in the Draft environment.
  4. I have a large assembly and when I’m zoomed in and try to rotate the part, it flies off the screen. Is there a better way to control the rotation? 
  5. Did you know that you can do this in Solid Edge using the middle mouse button? The problem here is that the default center of rotation is (0,0,0). So if you are zoomed in, away from the origin, any rotation appears to rotate out of view. What you need to do is change the center of rotation by following these steps:
  6. - Zoom into the area you want to view.


  9. - Click your Select tool. Notice that the cursor has a small gold box beside it.
  10. - Click the middle mouse button, in an empty space, and the gold box will disappear.
  11. - When the gold box disappears, move the cursor over the model. Notice the bright pink dot attached to the cursor.
  12. - This bright pink dot represents the center of your next rotation. Move it to where you want the center of rotation to be, and then hold down your middle mouse button to rotate.



  2. - Notice the rotation symbol on the cursor, and that you are rotating around the pink dot.


  1. When you release the middle mouse button you are placed back into selection mode. You can also use this in the part or sheet metal environments. For more information, and additional mouse tips, read the Solid Edge Help docs under the “Using the mouse” heading.
  3. I want to place a dimension between two points that are not horizontally or vertically aligned.
  4. Did you know that you can do this in Solid Edge using the Distance Between command? All you have to do is follow these few steps:
  5. - Select the Distance Between command.
  7. - On the command bar, change the Horizontal/Vertical option to By 2 Points
  9. - Select the 2 keypoints and place the dimension.
  10. For more information, and additional options, read the Solid Edge Help docs under the “Dimensioning overview” heading.


These are actual questions that I have received many times from our user base. It just goes to illustrate that Solid Edge is not always being used to its full potential and that there is always room for improvement. The more you understand about the software the more efficient you will become. I plan to continue sharing the more popular questions, from our tech line, in future blogs. If you are a customer of Designfusion’s, and have a question, please don’t hesitate to call our tech line at 1-877-215-1883 or email us at

  • HELP !!!!!!!

    Cory Goulden - Thursday, February 06, 2014



    Need help with something?? Having trouble with a difficult question?




    Many users try their best to stay current and up-to-date with information regarding Solid Edge – especially nowadays in this tech-savvy environment.  There are many ways where you can get help in resolving different problems, questions, concerns and even ways to request changes to the software by logging an enhancement request or two.


    First and foremost, your first option being our amazing DF technical support can be reached from:


    •    Calling our tech support line at 1-877-215-1883 or
    •    Zendesk (on-line help ticketing system) at
    •    And of course, because you are reading this, our blog page at


    In addition to these resources, information and technical assistance can be found from some other places.  I will list some below. 


    Many people have asked me how to acquire certain information about the different software packages from Siemens.  The most typical question being;


    1)    How can I be kept in the loop for any notifications about maintenance packages for Solid Edge?  

    •    Below is an example of what you will receive.  This is the actual notification for ST6 MP4


    To subscribe to this service or any other you may find of interest please go to the following link:
    The following link provides a great tool to service this exact need mentioned.  The many features of this link include:


    •    A function that allows you to subscribe to mailing lists and be sent the information as it becomes available.
    •     A feature that allows you to subscribe to “Software Field Bulletins” or SFB’s and to receive notifications regarding whatever topics you select.  
    •    There is a filtering option to ensure you are getting only the subjects that are pertinent.  
    •    You can subscribe to a summary that will list those as a weekly summary if preferred.  
    •    There is also a newsletter that contains articles written by the global support staff that you can subscribe to.


    One other nice thing is that if you no longer wish to receive these messages there are very clear instructions about unsubscribing.


    From there you have links on the side of the page as well for information regarding questions that may have already been asked to GTAC called “Solution Center”, license management, documentation, download link (for Maintenance Packs and full product releases), and link to help with WebKeys (create new, forgot passwords, or to update information.



    Of course we, at Designfusion, are always happy to help and are here for you when you need us.
    Happy Edging!


    Join us at Solid Edge University 2014

    John Pearson - Friday, January 31, 2014


    Siemens PLM Software has announced that this year’s Solid Edge University will be held in Atlanta, Georgia on May 12-14, 2014.  For those of you who have not attended this conference, you are truly missing a great opportunity. Not only do you get a preview of the next release of Solid Edge, but you get to connect with the Solid Edge developers and provide input to the direction of future development. You can also participate in hands-on learning, attend presentations given by CAD users and meet with experts from all aspects of the design continuum. Focus areas will include CAD, design data management, simulation, manufacturing and a host of complementary applications to help you design better. Some of us at Designfusion will be presenting again at this year’s conference.



    This is also a great opportunity to visit with our sponsors and technology partners and learn new ways to enhance the power of Solid Edge. Many partners are set up at the conference, ready to answer any questions you may have. Plus there is no better place to network with other Solid Edge users who make up this vibrant user community.  I personally spoke with the Designfusion customers who attended last year event and everyone said that the learning experience was well worth the cost of the conference.


    I hope you can join me and my colleagues at the Solid Edge University 2014. For more information, and to take advantage of the early bird registration, go to the Solid Edge University website at

    Working With Revision Manager

    Manny Marquez - Thursday, January 09, 2014

    In the past few days, customers have called about revision manager and have asked several questions on how  they can move or copy assemblies to new locations.

    There were a few main issues custumers have had in regards to Revision Manager, and what I have done is created multiple scenarios to tackle these issues .  


    Scenario 1: Copy all assemly with all parts to new location.  

    Scenario 2: Copy all parts associated to assembly and folder structure to new location folder.

    Scenario 3: If a folder with parts related to an assembly gets nenamed  and links get broken, how to redifine links.  


    Sample Folder structure (this can be any combination of folder locations) the point is that, we need to move or copy files to a new location.    



              Scenerio 1: copy all assembly with all parts to new location, this is ideal when you need to clone

              the whole asssembly to send to a customer.  


    1. 1. Open TOP level assembly with Revision Manager.


    1. 2. Expand then select all, this option makes sure that all files will be copied. Notice action is unchanaged.


    3. Copy; this indicates the coping process.

    4.The next step is to set the path for the new location to copy the whole assembly.




    5. Final step is to perform actions. At this point the assembly is copied to the (new) folder location.
        However notice the subfolders are NOT copied.  This completes this scenerio.




              Scenerio 2:  Move the whole assembly with subfolder structure and related files only.

              Another method is just to copy all folders to the new location, but note that there may be

              files that do not relate to the assembly.

              In cases where you only need to move  files that relate to that top level assembly and keep the 

              same folder structure, files not related will not copy or move.  


    6. Open selected assembly with revision manager.




    7. We are going to move to (new location) and copy the same folder structure. By selecting the (rename)

        you are moving the files from the (original) folder.




    8. Notice action is to rename document.




    9. Now click on replace old folder (Original) with new folder (New). Then select replace all then cancel.





    10.Once replaced, see new folder with new location.




    11.Click on Yes and close Revision Manger.


    12.Notice the new folder structure in new location, notice the subfolders are copied as well.




    13.Review new folders using window explorer to take a look at the previous folder location; notice only

         files that were not associated to the assembly did not copy (This is also a good way to isolate

         assemblies) with the folder structure. This complete this scenerio.



              Scenario 3: Cases when a folder gets renamed and then you open the assembly and notice that

              all links are broken. This is very common in networks with many users.


    14.So let’s go ahead and rename each folder as shown below, just by adding “1” at the end of each





         If you try to open the assembly now with RM or Solid Edge, the files will not open; you will get a notice

         that files are missing.




    15.Click on the redefine links then select top level folder then ADD (make sure that the subfolder is





    16.The easiest way to get the folder address correctly is by going to the window explorer, and then copy      and paste.

         -(ManufacturedParts) is the original folder

         -(ManufacturedParts1) is renamed folder

         -click next twice




    17. Click on Back twice  




    18. Repeat for other folders


    19.Next twice


        Close Revision Manager, and then reopen with top level assembly. This completes this scenario.


        This was also presented at one of our Solid Edge Productivity summits by Barry


    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.

    Helpful Solid Edge Tips and Tricks

    John Pearson - Wednesday, November 13, 2013


    I just heard my first Christmas carol this year. It was “These are a few of my favourite things”, sung by Julie Andrews. It got me thinking two things. First; it’s still too early for Christmas and second; this would be a good idea for our blog. When I teach advanced classes, I am often amazed how many basic tips and tricks, that I take for granted, are not known by the average user. So here are few of my favourite, yet often overlooked, useful tips and tricks in Solid Edge.

    Sketching Tips and Tricks

    The A key in the line command 

    This line command draws a continuous series of lines and arcs that can be perpendicular or tangent to each other. Note that it says lines and arcs. Many users are not aware of the arc capability in the line command.

    This command starts in line mode by default. If you want to start by drawing an arc, press the A key on the keyboard, or click the Arc button on the command bar. Once the arc is drawn the command defaults back to line mode.

    Snap-to-point shortcut keys 

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

    Midpoint - press M
    Intersection point - press I
    Center point - press C
    Endpoint - press E.

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

    Ctrl key to focus scroll wheel control

    If you hold your cursor over a dimension field, you can scroll the value up and down.

    However, if you move the cursor off the dimension field, the focus of the scroll wheel changes to zoom in and out. To avoid this hold down the Ctrl key and the focus of the scroll wheel remains on the dimension field. 

    Note: You can have the scroll wheel set to always focus on the dimension field, by toggling on the options in Solid Edge Options>General tab.

    Keyboard options for the Smart Dimension Command  

    Before you click to place the smart dimension, you can use the following keys to affect the dimension that is created. The options that are available depend upon what, and how many, elements you select. Refer to the specific prompts displayed on PromptBar as you select elements.

    Part Modeling Tips and Tricks

    Replace Face command 

    This command replaces selected faces on a part. The replacement face can be a construction surface, a reference plane, or another face on the part. When replacing more than one face, the faces being replaced cannot touch each other.

    When you replace a face using a construction surface, the construction surface is hidden automatically when you finish the feature.

    If edges on the face you are replacing have rounds applied, the rounds are reapplied after you complete the replace face operation.

    Steps to replace a face

    1. Choose Surfacing tab→Surfaces group→Replace Face   . 
    2. Click the face you want to replace and then click the Accept (check mark) button on the command             bar.
    3. Click the surface you want to replace the face with.
    4. Finish the feature.

    Subtract command (boolean) 

    With this command you can remove the tool body volume from selected target bodies. You can select multiple target bodies and multiple tool bodies. The tool body can be a design body or construction body.

    You can also use a reference plane or a surface as the tool. These tools have no volume. You choose a direction to subtract volume from the target body.

    You can preset the type of output body to create if the resulting body is a non-manifold by using one of the following options on the Boolean Options dialog box.

    Create multiple bodies
    Fail (no output)

    Lock and Unlock PMI dimension form the PathFinder

    By clicking on the lock icon in the Pathfinder, users can lock or unlock PMI dimensions in the synchronous paradigm.

    Assembly Tips and Tricks


    The FlashFit option reduces the steps required to position parts using mate, planar align, and axial align relationships when compared to the traditional workflow. Because many parts are positioned using these relationships, FlashFit is appropriate in most situations.

    When you position a part using FlashFit, you first select a face or edge on the placement part. You then select a face or edge you want on the target part and let the inference logic built into Solid Edge determine the most likely relationship, based on the target part element. 

    For example, if you choose a planar face on the placement and target parts, the software assumes that you want to establish a mate or planar align relationship. When you select the target part element, the placement part is positioned in the assembly using the closest solution.

    If the two faces you select are closer to a mate solution, a mate relationship is applied.

    If the two faces you select are closer to a planar align solution, a planar align relationship is applied.

    A Flip button on the command bar allows you to select the alternate solution. You can also use the Tab key to select an alternate solution.

    FlashFit also allows more flexibility to use edges, in addition to faces, when positioning a part using mate, axial align, and planar align relationships.

    This can be especially useful when positioning a fastener, such as a bolt into hole. For example, when positioning a part using an axial align relationship, you cannot use a circular edge to position a part. With FlashFit, you can use a circular edge on both the placement part and target part to completely position the part in two steps.

    Note:  The Flip option or the Tab key selects an alternate solution if desired.

    Capture Fit command 

    Use the Capture Fit command to capture the assembly relationships and faces used to position a part or subassembly already placed in the assembly. You can then place the part or subassembly again later using fewer steps. This command is ideal for hardware and commonly used parts. When you drop the part into the assembly document, the faces of the placement part highlight and you are prompted to select the corresponding faces on the target part. With capture fit parts, you can fully place a part in 3 clicks.

    You can use the Capture Fit dialog box to specify which relationships you want to capture.

    Steps to capture the assembly relationships for a part

    1. In the assembly window, select a part for which you want to capture relationships. Note: the                       assembly relationships must already exist on this part.

    2. Choose Home tab→Relate group→Capture Fit. 

    3. In the Capture Fit dialog box, use the Add and Remove buttons to specify which relationships you             want to capture, and then click OK.


    You can also select the part you want to use in PathFinder.

    When you use the Capture Fit command, the relationships and faces used to position the part or             subassembly the first time are stored so you can place the part using fewer steps later.

    If you used the Insert option to position a part, the Capture Fit command will capture a mate and an           axial align relationship, since these are the relationships that the Insert option actually places.

    The Capture Fit command cannot capture angular, cam or center-plane relationships.

    Drafting Tips and Tricks

    Creating drawing views from a model dragged onto a sheet
    Another way to create drawing views is to drag a model onto a drawing sheet. When you do this, the View Wizard command runs automatically to create the drawing views. This produces a 

    standard drawing view based on the type of model. The view orientation of the first view placed is shown in the following table. 

    Example:  If you drag a part or sheet metal model onto the sheet, a standard set of views is generated and placed.

    Example:  The first view placed in an assembly model is an isometric view. After placing the first view, you can create additional views from the primary view by moving the cursor and clicking to place each one.

    Updating Views tips

    To update a single drawing view, select the drawing view and click the Update View command on the shortcut menu.

    Force Drawing Views to Update--If you hold Ctrl+Shift when you click Update View, Solid Edge         performs a full update, just as it would on initial view creation. That is, it rereads all of the model               data to regenerate the view, rather than only the model data thought to have changed.

    Now obviously there are many more tips and tricks available, but these are some of my favourite ones, which I feel should be basic knowledge. More information can be found on these commands in the Solid Edge Help docs. If you are a Designfusion customer, you can always get more detail by contacting our support desk at 1-877-215-1883 or email us at  

    Setting up your CAM Express role in NX9

    John Pearson - Thursday, November 07, 2013
    Due to the increasing popularity of CAM Express, we are receiving more calls on our support line. The most recent calls have been requesting help in setting up the new NX9 CAM Express role and setup pallets. So to help those of you who will be making the switch soon, I thought I’d be pro-active and add these answers to our blog site.

    How do I set the CAM Express role in NX9?

    1. Open up the NX9 gateway, and click on the Roles tab.

    2. From the Roles pallet, select the CAM Express role.

    3. Click OK to the Load Role message.

    4. Open a Solid Edge part file or NX part file.

    5. Click on the Web Browser tab.

    6. Start your first setup from the Web Browser pallet, by clicking on the “Create a new setup for this model” shortcut, near the bottom of the pallet.

    7. Select the desired Units and then select the desired Setup, from the Create New Setup dialog. For example, below I selected Millimeters and the Machinery (Express) Setup.

    8. Click OK, to launch the selected setup.

    How do I turn on the Express Setup pallet?

    Once you have entered into manufacturing, using the previous steps, you can turn on your manufacturing pallets. 

    Notice the Manufacturing – Express tab is missing.

    1. Go to File > Preferences > Manufacturing.

    2. Select the Add Setup Pallet icon, under the User Interface tab.

    3. From the pallet list, select Express and click OK.

    4. Click OK to dismiss the Manufacturing Preferences dialog

    Notice that the Manufacturing – Express tab is now present.

    5. Click on the Manufacturing – Express tab and you now have access to all your Express Setups for future jobs.

    If you would like to learn more about NX CAM Express, feel free to contact us at If you are a Designfusion customer, you can contact us at or call our support line at 1-877-215-1883.

    How to create an adjustable coil spring in synchronous

    Manny Marquez - Wednesday, October 30, 2013
    In the September 18th  blog, we showed you how to create an adjustable coil spring using the Ordered/History modeling techniques. We can take different approches as to how to model this spring. We can use helix or wrap sketch techniques, but that doesn’t mean we can make the spring adjust using ST. In the following steps, we will take a look at how to model the coil spring using  ST modeling.

    1. Create all sketches as needed. We will start with sketching path for all features.

    2. Select sweep. We are going to use the Twist option

    3. At this point the twist option is not selectable.

    4. Select the path then accept.

    5. Then pick on the cross section.

    6. After selecting the cross section, you will get this message. It’s Ok, just click on EDIT, and then edit definition.

    7. Notice that the Twist option is now available. For the first feature select number of turns of (-1.0)

    8. This is the result.

    9. Next, repeat the same step for the opposite side, using (1.0) for the number of turns.

    10. Click on sweep protrusion.

    11. We will now create the extended protrusion out from the twist using a single path.  Select options as shown click ok. Then select path and accept.

    12. At this point select the cross section.

    13. Repeat step for opposite side.

    14. The next step is to create a revolve protrusion about an axis; we need to draw a line offset from the center of circle. Lock plane then (ctrl+H) this will allow viewing normal to surface

    15. Draw a line .032 from the center of the circle and add a perpendicular relationship from the 33˚ line.

    16. Select the end surface; then drag the steering wheel to the line created from the last step. Snap into the line so the torus is perpendicular to the line.

    17. By selecting the torus then selecting the (lift) option on the ribbon, this will allow the surface to rotate about the center line. Enter 70˚ or appropriate value.

    18.  In this step there are two options. (I used option 2)
    1. Click on the protrusion command select surface as indicated, enter value.
    2. Select the surface as shown, use the lift option and drag .300 distances.

    19. Mirror features for opposite side.

    20. This portion is a very crucial step in order to make this Synchronous part coil deform   
     as the part adjusts.

    I’m going to show you two options to adjust the coil spring.

    OPTION 1
    Select every surface/ feature, except the two as indicated with red arrows; drag the steering wheel to the coordinate system. The torus must be parallel to the direction in which to rotate the part. (See image)
                     (Do not include any of the sketches to rotate along with the part.)

    21.  Select the steering wheel torus, then dynamically rotate the part or enter a value.
       (Notice the two surfaces that were not selected stay stationary.)
    You can repeat these steps at any time if you wish to adjust the coil.

    Remember what value you use. This will be helpful, if you need to change it back to original state.

    FYI:   If you decide to finish the model, then try to rotate to adjust coil spring angle,   this will not work. ST will not allow you to dynamically drag angle from both ends, only   one at either end.

    OPTION 2

    22.  Select the circle command and lock to Base plane to create a circular cutout.

    The idea behind this is to have live rules recognize the concentric cutout; this will    prevent the coil from moving about the center when we later add an angular   dimension.

    (The Diameter size should be minimum size possible as long as it cuts into coil without making an impact on your design intent.)

    23.  Select the symmetric extrude and remove options from the smart ribbon bar.
     (You can use the space bar to toggle between add or remove)

    24. Add an angle between dimension, select the (y) axis vector from the (UCS) then place dimension.   ( See images)

    25.  At this point select all surfaces except two as indicated with red arrows.
    RMB click to create a user-defined set.

    26. The next step is to select the (a) user-defined set. 
    Then click on (b) angular dimension to start modifying the angle.

    27. As you can see, by dynamically changing the value, the coil is changing and adjusting. Notice the center cutout stays concentric to the center of the UCS origin. That was the only reason to create that cut out, so that live rules recognizes this predictable behavior.

    You can repeat these steps at any time if you wish to adjust the coil.
    Remember what value you use. This will be helpful, if you need to change back to original state

    28. You will create the last feature using the sweep command.

    Select path then cross section.

            (This feature will not rotate or adjust like previous modification.)


    For future modifications you may need to restore sketches, to use when deleting the feature to reuse after modification is made. In other words, if you need to change the angle, you have to: 
       a. Delete feature.
       b. Restore sketch.
       c. Rotate, modified angle.
       d. Add feature again.

    29. Fence select all parts (except sketches), hit (Ctrl +R). This will allow viewing from right view.

    30. Drag steering wheel to coordinate, snap so that torus is parallel to rotating angle.
    Dynamically rotate or enter a value.

    31. Keep in mind, if you need to modify like in step 19 or 21, delete feature.

    Ordered vs. Synchronous – Which should I use? – Part 2

    John Pearson - Thursday, October 17, 2013
    If you read Part 1 of this article, you’ll recall that I discussed the Pros and Cons of ordered and synchronous modeling. I also suggested that you should use both paradigms in an integrated approach to get the best of both methods. In this article I want to take a closer look at why some users claim that they can’t use synchronous modeling. There are some myths that are cropping up about synchronous which are simply not true.  Of these myths, the most prominent one is the following:

    I have complete control of my design in ordered, but not in synchronous.”

    This is simply not true. First let’s look at the first part of the statement. The designer only has complete control of the sketch if it is fully constrained. Plus that control is per sketch, there is no guarantee that changing that sketch will not negatively impact other sketches in the model. It takes a lot of work to constrain and relate all your sketches to get models to always behave in a set manner. For this reason many users don’t bother to put in the effort. Plus, if your company follows standard PLM practices, once you complete and review the model, it is released. A released model should never be changed anyway. You should create a revision of a released model to be able to update or modify it. If you don’t use released models, your perceived control of the model is only good assuming no one goes into your sketch and starts deleting your constraints.

    The second part of this statement is also false. Not only can you control a synchronous model, but you actually have more tools to do so. The main reason users go into the sketch is to change the dimensions. In synchronous modeling, driving dimensions are placed directly on the model, allowing the user easy access with the same dimensional edit control as ordered. Geometric relationships can be maintained by using the Live Rules, without first having to place any geometric constraints, or by locking down 3D geometric relationships. If you compare the 2D geometric sketch relationship to the 3D face relationships, you will note that they are almost identical.

    So the reality is that you can have complete control of your models in the synchronous paradigm. In fact you have complete control without having to fully constrain your sketches. Remember, the sketch is merely a launch point for the model; it does not drive the model. For those of you who have struggled to fully constrain sketches, you can appreciate how much time this will save.

    This statement brings up another issue with ordered modeling. Many users lock there models down to try and ensure easy edits in the future. The problem here is that you have to try and predict what kind of changes can occur, if any, in the future. So the user invests a lot of time locking down or constraining a model, that may never change, or may change in a completely different way than the user predicted. If the model does change in the predicted manner, the designer still has to remember how it was originally constrained, in order to make predictable edits. The reality is that some parts never get changed, and those that do, are often changed in an unpredicted manner or, by a different designer. Even if it’s the same designer, he/she may not remember how it was originally constrained. Thus you spend more time trying to understand how the model behaves, even before you can attempt any edits.

    This doesn’t even take into account the parts that are often grabbed to use as reference parts. It’s been my experience that most designers prefer not to start from scratch unless forced to. They will often look for similar designs from their legacy data, copy and rename the model, and then edit the model to meet the new criteria. This can sometimes prove to be a frustrating experience if the reference model is constrained differently than your new model should be.

    This is the beauty of synchronous technology. You do not have to predict the design intent at the time of creation. It enables you to determine the design intent each time you make a change or edit to the model. Let me give you a simple example of this:

    Below is a fully constrained sketch that I use in my fundamentals course.

    Notice that this has been constrained such that the circles for the holes are centered on the rounded top corners and will move outward symmetrically, if I increase the value of 3.000. Likewise the holes and rounds will move upwards if I increase the value of 2.000. All the walls are locked to either vertical or horizontal positions, and the center half circle’s radius is controlled independently.

    This sketch is used to create the base feature of the following model.

    Based on my design intent, I have predicted that the model could change in one of the following ways:

    I could also change the diameters of the holes and the radii of the rounds or center cutout.

    However, what happens if I need to make different changes that were not predicted or I use the model for a reference part to make the following models:

    All three changes above would require some editing of the sketch beyound simple dimensional edits. Making the same model in synchronous, I create the following sketch:

    Notice that I don’t show any geometric handles. I can use them, if they speed up the creation of the sketch, but I don’t need to pit them in. I generate the model using similar commands that I used in the ordered paradigm.

    Editing the model is easily done in one step, using the steering wheel and Live Rules. Not only can I make the predicted changes to the model:

    Note: Live Rules automatically maintains the concentric relationships between the holes and the rounds.

    But I can just as easily make the unpredicted changes to the model, by turning off the concentric Live Rule.

    Plus I could make many more modifications directly to the model. I could lock down the 3D relationships thus restricting my model as I did in the ordered paradigm, but despite protests from ordered users, this isn’t absolutely necessary. If you choose to lock all your geometric relationships, they will appear in the Pathfinder, under a relationship header.

    Even if I lock the model down, these locked relationships can be deleted from the Pathfinder, keeping it easy to edit. But keep in mind that you do not have to do this, because Live Rules will maintain those relationships without having to previously define them.

    Another big reason for not using synchronous is, as I noted in the Part 1 of this article, there are some limitations to certain features. Some users believe that any limitations justifies not using the synchronous paradigm. Again these users have not been fully trained and do not understand the power of integrated modeling. For example, synchronous modeling does not support dangling bends in sheet metal. This prevents user from creating contoured flanges along a curved edge. In the model below I created this using an integrated approach.

    Notice that the model was started in the synchronous paradigm and the contour flange was added in the ordered paradigm. If I edit the synchronous features, the ordered features are automatically updated. For example, if I move the one side of the part, effectively changing the overall width, the ordered contour flange updates with the symmetrical move.

    So I still have the benefits of synchronous editing, yet the ordered feature provides me with the feature currently lacking in the synchronous paradigm. In other words, I get the best of both paradigms. Any limitations in synchronous are easily overcome by using the integrated approach.

    Finally, and I know you’ve already heard this from me in several posts, make sure you attend training. Synchronous technology requires a good basic understanding before you see the true benefits. It has been described as a mind shift similar to that of transitioning from 2D to 3D. Most resellers offer synchronous training for experienced Solid Edge users. At Designfusion we have a 3 day synchronous course with an optional 4TH day for sheet metal.

    Another way of looking at this would be to ask yourself what you would pay for a new CAD system that will significantly improve your efficiency, thus saving you time and money. Now, if you are a current user of Solid Edge, consider that you already own this and the only thing stopping you from reaping all the benefits is 3 or 4 days of training.

    If you are interested in seeing how synchronous can benefit your company, contact your local reseller for a demonstration. If you are already a Designfusion customer, or would like to be, contact us directly at or contact your local account manager. Synchronous technology is here to stay and will continue to get better. The sooner you learn how to use it, the sooner your will reap the benefits.