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How to Create a Rod That Has Bends in Two Directions

Cory Goulden - Monday, March 31, 2014

I have received a few calls lately regarding this subject so I thought I would provide a walk-through on how to make something like the drawing below. This will be one of the rare times I prefer to model in Ordered.




The first step is to understand that we will have to let the 3D system do most of the work for us. We will, like all good trouble-shooters, work out what we know. On one plane create a sketch of the top profile. Then on the corresponding plane create a sketch of the side profile.

Once this is complete we will use some surfacing tools for the second step. Go to the “Surfacing” tab and select the “Extruded” command in the “Surfaces” group.

Once the command is selected ensure the option to “Select from sketch” is selected. We then will need to select one of the earlier selected sketches. Once selected we will ten need to extrude the surface. The extend distance need to be further than the entire profile for the other sketch.


Do the same procedure for an extruded surface from the second sketch. Be sure both surfaces overlap each other after they are completed. You can always go back and adjust any extents after.
Once complete you should have the result similar to what is illustrated below. (I have hidden the sketches for clarity)



From here we will go back to the Surfacing tab and use the “Intersection” command under the “Curves” group.



This command asks us to select the 2 elements. Firstly select one of the surfaces and accept. Next step is to select the second surface and accept.



You will now have a 3D path that you can use for a lofted protrusion.

You can use another command called “Cross Curve” to accomplish the same thing but to understand the concept and break it down a bit I chose to illustrate this methodology. Feel free to use the Command finder for further information.

Once you have created a Lofted Protrusion using this curve as a path you will end up with this;



We have created 2 extruded surfaces, used Solid Edge to create an intersection curve, and then used that curve for a lofted protrusion.

 

I hope this has been useful and Happy Edging!

There’s a CAMWorks for Solid Edge?

John Pearson - Tuesday, March 25, 2014

Last year at Solid Edge University (SEU2013) I was introduced to CAMWorks from Geometric. What I had always considered a competitive product was now being offered as an add-on to Solid Edge. Being a long time NX CAM user, I was a little surprised that Solid Edge would partner with another CAM package, especially one so closely linked to another CAD package. At my company’s request, I put aside my skepticism and started to find out what I could about this new offering.

The first release of CAMWorks for Solid Edge was limited to 2.5 and 3 Axis Milling and Turning. Since most CAM packages can easily handle this type of manufacturing, I focused on what made CAMWorks unique, and how it worked with Solid Edge. Three distinct factors stood out for me during my initial analysis of the product:

    1. CAMWorks for Solid Edge is embedded and fully integrated into Solid Edge.

 

When you install CAMWorks for Solid Edge, it becomes part of Solid Edge. A CAMWorks ribbon is created, and a CAMWorks edge bar is added to the PathFinder.

 

 

This eliminates wasted time and potential errors in loading your Solid Edge model into external CAM packages. Plus you can easily switch back and forth between the CAD and CAM ribbons, to make associative edits or revisions.

     2. CAMWorks for Solid Edge utilizes feature-based machining to allow for rapid tool path generation.

CAMWorks for Solid edge utilizes automatic feature recognition and an advanced database to create some truly impressive knowledge based machining. Once setup the basic workflow is as follows:

 

    - Identify the parts for machining

 

     

     

 

    - Extract features to be machined

 

 

 

    - Generate the Operation Plan (utilize the database to determine how the features are to be machined)

    - Generate the toolpath

 

  

 

 

 

    - Simulate/Verify the toolpath

 

 

 

 

 

    - Post process to create the G-code

 

 

 

If the database is setup correctly, each process is automatic. I’ve seen situations where you can go from CAD model to G-code in 5 button clicks, if you skip the simulation step.

 

    1.      3. CAMWorks for Solid Edge can be customized to meet the individual needs of each company.  

 

The database (TechDB) used in CAMWorks for Solid Edge, can be set up differently for each company and even each user. This allows companies to capture and reuse their best machining practices, saving time and eliminating repetition. It should be noted that you can create operations on the fly and save them to the database, allowing you to continually expand and improve your knowledge base for future machining.  The potential exists to reduce programming time from hours to minutes, but it does require some up front effort to realize this kind of result.

Despite these impressive points, I wanted to learn more about future plans for the product. Two weeks ago, I was invited, by Geometric, to attend a training session for VAR’s in Scottsdale, Arizona. I eagerly accepted the invitation, mainly to escape the brutal winter we’ve been having, but it also gave me an opportunity to get answers right from the source.

I was not disappointed; the temperature ranged between a balmy 25-28 degrees Celsius, and the capabilities of CAMWorks exceeded my initial expectations. They have recently added Multi-Axis milling, Mill-Turn, and Wire EDM capabilities and continue to work with Solid Edge to improve the product.

As a combined result of my investigation, and the work of our management team, we will be adding CAMWorks for Solid Edge to our product line. We believe this will complement our existing products, and provide more choice to our customers. We will be adding more information to our website, as it becomes available, and have plans to offer training in the future. In the meantime, if you’d like to learn more about CAMWorks for Solid Edge, please contact your account manager or contact us directly at sales@designfusion.com.     

        

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.
  7.  
  8.  

     

  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.

 

 

  1.  
  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.
  2.  
  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.
  6.  
  7. - On the command bar, change the Horizontal/Vertical option to By 2 Points
  8.  
  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 support@designfusion.com.

  • 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 http://www.solidedgeu.com/.

    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

         word.

     

     

     

         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

         unchecked).

     

     

     

    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

        Shillingford.



    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 support@designfusion.com. If you are not a customer of ours, please contact your reseller for further support.

    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.
      (ctrl+H)

    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.)


      Results



    Note: 
    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 sales@designfusion.com 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.







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

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


    Pros and Cons of the ordered paradigm


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

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

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

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


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

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

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

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

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

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

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

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

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

     


    Pros and Cons of the Synchronous paradigm


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

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


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

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

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

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


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

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

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


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


    Pros and Cons of the integrated modeling approach


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


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

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