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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.

Solid Edge ST6 introduced at SEU2013 – Part 1

John Pearson - Friday, July 12, 2013

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

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

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

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

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

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

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

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

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


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

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

ST6 Surface Modeling

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

Major overhaul of the Surfacing environment

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

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

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

John Pearson - Thursday, July 11, 2013

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

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

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

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

Click on the New button in the Style dialog.

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

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

In this example I selected Dk Gray. Click OK.

Click Apply to accept the new Fill Style.

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

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

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

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

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

Synchronous Assembly Modeling Boolean Commands in ST6

John Pearson - Wednesday, July 03, 2013

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

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


Let’s have a look at the following example:

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

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

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

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

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

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

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

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

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

Solid Edge ST6 Offers Multiple Version Installation

John Pearson - Thursday, June 27, 2013


Solid Edge ST6 Offers Multiple Version Installation


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


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


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






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


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


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

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


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



Solid Edge Silent Install


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


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


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


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

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

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

/l*v “K:\temp\mysilentsetup.log”


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


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





















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


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


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


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


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


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


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


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

Set Active Solid Edge Version


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



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


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

Uninstalling Multiple Versions


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