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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.

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.


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.

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. 

How to create an adjustable coil spring

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

The first swept feature looks like this:

The second swept feature looks like this:

The third swept feature looks like this:

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

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

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

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

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

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

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

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

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

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

On the command bar I input the following information;

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

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

In the example, the results are as follows:

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

ST6 Released!

Cory Goulden - Saturday, July 27, 2013

Hot off the Press….ST6 RELEASED!!!

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

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

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

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

The preferences folder is here:

C:\Program Files\Solid Edge ST6\Preferences

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

Happy Edging!