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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.

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.

Integrated Modeling in Solid Edge

John Pearson - Monday, November 19, 2012

With any new technology, you have your early adopters. This is followed by a general acceptance of the new technology, and of course, you always have your hold outs or late adopters.  Solid Edge ST and ST2 appealed to the earlier adopters for synchronous technology. With ST3, ST4 and now ST5, we are seeing most of our customers starting to use synchronous modeling. This of course has led to many questions. The most asked question is; “Should I use synchronous or ordered modeling?” The answer to this is yes.

One of the unique qualities of Solid Edge is that you are not locked into using synchronous or ordered modeling. Integrated modeling allows you to use both synchronous features and ordered features within the same part or sheet metal model. As a rule of thumb, I encourage users to start with synchronous modeling. If they run into some issues that can’t be addressed with synchronous features, they can switch to the ordered paradigm to complete the model. Let me illustrate this with the following example:

I wish to model the sheet metal cover shown in the following image.

I start in the synchronous paradigm and create a tab, for the top of the cover.

I then add 2 synchronous flanges, in one step, to create the back and left side of the cover.

One of the current limitations, in synchronous sheet metal modeling, is that you cannot drive a flange along a circular edge. Realizing this I will hold off creating the front and right sides until the end, when I will use an ordered feature.

I next use 2 bead synchronous features to create the slots at the top of the part.

I then transition to the ordered paradigm to complete the model.

I use the ordered Contour Flange command to create the front and right face of the cover.

The nice thing about this approach is that it still allows me to modify the model using the synchronous Move/Rotate command.

Live Rules and all the other synchronous editing tools still apply to the model.

As I modify the model, synchronous features update instantly, followed by the re-computing of any ordered features.

For those of you who attended our productivity seminars, you saw this demonstrated live. Other users have learned this process in one of our many synchronous modeling courses, offered over the last year.

This is just one of many examples where Integrated Modeling allows you to benefit from the new synchronous technology, while still utilizing some of the tried and true methods of the ordered technology.  As Solid Edge continues to develop the synchronous features, you may find that you’ll use less integrated modeling. But for now this provides you with a reliable and safe platform to further advance your adoption of this amazing new modeling paradigm we call synchronous technology.

If you’d like to learn more about integrated modeling, you can attend one of our synchronous modeling courses

Editing Part/SM Operations in Assembly

Cory Goulden - Monday, November 05, 2012
In ST5 you can now perform edit operations, from the assembly environment, without first in-place-activating to enter the model directly.  Things you can do:

• Locate, select and edit of ordered features
• Edit synchronous procedural features
• Delete synchronous face-sets and ordered features
• Move face-sets (sync feature) in synchronous parts

Let’s take a look!

Firstly, ordered features are now selectable via the Face Priority select option. (remember hotkey combo is CTL + Spacebar)

Notice in the example below that “Protrusion 1” is available from the Quickpick options in assembly now.

Once selected, “Protrusion 1” has its options displayed for going directly into the features parameters.

Select whatever you would like to edit and SE will take you directly there.  Once complete, just close and return.  This will take you back to where you were in the assembly.

This saves time from previous versions by allowing you to go directly to what you want to modify and brings you back to the assembly reducing the number of mouse clicks.

Editing synchronous procedural features from the assembly level does not in-place-activate the user into the part.  Procedural features are things such as Patterns, Thin wall, Helix, Hem, Dimple, Louver, Drawn cutout, Bead, Gusset, and Etch.  These are editable directly in the assembly.

Using Face Select again, “Louver 1” is selected.
The handle for the procedural features shows up.  If selected we are presented with the following options.

Also, if we were to select the adjacent lover we would be presented with the following options:

Notice that the option to edit the pattern is there.  I know what the usual next question would be “How would I know how to edit the parent of the pattern?”.  Notice the option for “Louver 14”.  If you were to select it, you would be presented with the same options as previously mentioned.

We select “Pattern 1” and now we can modify the parameters that define the pattern.

Once selected, click on the PMI callout “Pattern 2 x 4” and we will get the following options:

Notice we have not left the Assembly environment.
One thing to note about this type of editing: Procedural Feature profile editing requires in-place-activating first.  Also, there is no access to the profile handle from within the assembly.
Happy Edging!

If you would like to learn more about “What’s New in ST5”, stay tuned for our new Update Training course.