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How to video: Frame Design

Manny Marquez - Tuesday, September 02, 2014
Check out our latest Solid Edge tutorial by Manny Marquez.


For more videos take a look at the Designfusion youtube channel here

Constraints and how they work in ordered and synchronous modelling

John Pearson - Thursday, April 03, 2014
There seems to be some confusion amongst some users regarding the ability to constrain synchronous parts. The confusion has even lead to inaccurate information being perpetrated as truths, by some competitive product’s resellers. So I’d like to set the record straight and clear up several misconceptions. First and foremost, you can constrain synchronous models. Secondly you can use the variable table to drive synchronous models. And last, but not least, you can automate synchronous models through custom programming or a configurator.

Ordered constraints


To understand how this works, let’s fist look at an ordered part. Below is a sketch for a part that I wish to model. Notice that I have fully constrained the sketch.

 

 


The sketch has zero degrees of freedom, so I can predict what will happen when I make a dimensional change to any of the 3 values. I control part of the sketch with geometric constraints, which include the following 2D relationships:

 

 


When I use the sketch to create a model, the sketch becomes the parent of the solid model, as shown below:

 


This model is considered constrained because it is controlled by the fully constrained sketch and the depth dimension, added during the extrusion command. Notice that we can go into the variable table and apply specific names to each dimensional variable.

 

 

 

I can now drive predictable model changes using the variable table. Furthermore I can link the variable table to an Excel spread sheet, a custom program, or a configurator to drive model changes.

When a variable is changed, the system first re-calculates the sketch and ensures that the sketch is still a valid profile. It then moves on to the child of the sketch, in this case the model, and re-computes the model to ensure that we still have a valid model. If additional features were added to the model (like a round or chamfer) it would continue to re-compute the next feature(s) until it has completed the feature tree list. For small models with few features, this is a rapid process. However, the more features an ordered model has in it, the longer the re-compute time will take.

Synchronous constraints

Now let’s make the same part in the synchronous mode. We start by making a sketch, as shown below:

  


Notice that I can fully constrain the sketch in synchronous mode. The difference here is that when I create the solid, only the dimensions are migrated to the 3D model. The 2D geometry and 2D geometric constraints are left in the Used Sketch header on the PathFinder. In other words, no parent child relationship is created between the sketch and solid, and the 2D dimensions are converted to 3D driving dimensions on the model, shown below:

 

 


Notice that 3 of the 4 dimensions are red in colour, while the depth dimension is blue. A red colour means that the dimension is locked and can only be modified by a direct edit of that dimension. Let’s make the fourth dimension locked as well.

 

 


So now we have the dimensions fully constrained or locked. What about the geometric constraints? Since the 2D geometric relationships have not been transferred to the model, a lot of users become concerned that the model is no longer fully constrained. They are partially correct. Let’s take a closer look at the model.

By the nature of the solid, we can make a few assumptions.

1. The connect relationships will be maintained at the model level. Why? Because if they are not we no longer have a solid.

2. Synchronous edits use Live Rules, and Live Rules will maintain most of the pre-existing geometric situations. For example, if you attempt to change the values in the part, default Live Rules will keep the walls in their current horizontal/vertical position.

3. Synchronous will only analyze the effected faces in any move. Therefore it only has to re-compute faces affected by an edit.

Even with these assumptions, there admittedly could be some un-expected results if you are using this model in a custom program or configurator. So how do we eliminate potential un-expected results? We use 3D geometric relationships.

Persistent (3D) relationships

 

Looking at the original sketch of our model, you’ll notice that the sketch was centered on the base coordinate system. I can do the same with the model by using the horizontal/vertical persistent relationship command. I’ve placed these relationships in the model, shown below. Notice that they also are listed under a Relationship header in the PathFinder.

 

 


Simply by placing these two relationships, I now have predictability in any dimensional edit. I can now set this synchronous model up in the Variable Table.

 

 

 

I can now drive predictable model changes using the variable table. Furthermore I can link the variable table to an Excel spread sheet, a custom program, or a configurator to drive model changes.

For more complex models, synchronous offers even more 3D geometric relationships.

 

 


Notice the striking similarity between our 3D geometric relationships and our 2D geometric relationships. There is however one big difference. I only have to use the relationships that I need to control my model. Because synchronous technology only re-computes faces that are affected by an edit, I may not have to fully constrain a model.

Some will argue the fact, but the truth is the majority of ordered models that I see from customers are under-constrained. Because of the parent child nature of ordered modelling, this could be, and often is a problem when editing ordered part models. If you doubt this statement, go back to your database and open some of your existing models. Under the Solid Edge options > General tab, turn on the ‘Indicate under-constrained profiles in PathFinder.

 

 

 

If a red pencil icon appears anywhere in the PathFinder, you have under-constrained features.

 

 


This is a real concern in ordered modelling, but not in synchronous modelling. As you’ve seen, the nature of synchronous modelling puts the focus on only what’s being edited. As you have also seen, a synchronous model can be fully constrained if necessary. Either way you can have complete predictability of the model and use it in configurators or custom programs.

So, as I stated at the start of the blog article, you can constrain synchronous models. You can use the variable table to drive synchronous models. And you can automate synchronous models through custom programming or a configurator. Anyone who tells you different has not been properly trained in synchronous modelling or works for a competitive software package.

If you would like more information on synchronous technology or would like to attend one of our synchronous training sessions, please contact us at sales@designfusion.com or visit our training web page at http://www.designfusion.ca//technical-training.html.

Join us at Solid Edge University 2014

John Pearson - Friday, January 31, 2014

 

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

 

 

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

 

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

How to create an adjustable coil spring in synchronous

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

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



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


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



4. Select the path then accept.


5. Then pick on the cross section.


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


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


8. This is the result.


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


10. Click on sweep protrusion.


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


12. At this point select the cross section.

13. Repeat step for opposite side.

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


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


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


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

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

19. Mirror features for opposite side.



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

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

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

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

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

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

OPTION 2

22.  Select the circle command and lock to Base plane to create a circular cutout.
  (ctrl+H)

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

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


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

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

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

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

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

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

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



Select path then cross section.

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


  Results



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

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

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

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









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

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

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

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

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


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

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

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

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

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


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

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


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



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

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

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


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

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



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

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






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

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

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



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



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

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

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

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







Solid Edge ST6 introduced at SEU2013 – Part 2

John Pearson - Thursday, July 25, 2013

In last week’s blog I had started to discuss what was new in Solid Edge ST6, as introduced to us at Solid Edge University 2013 (SEU2013). I had left off with mentioning the new enhancements in surface modeling. So let’s continue with what’s new in Part and Sheet Metal modeling.


ST6 Part and Sheet Metal Design


Improved Steering Wheel – now has 3 directional axes to eliminate the annoying need to always flip the steering wheel.




Improved solution manager – including color control, something I had requested for some of our color blind users.


Faster revisions with synchronous technology - Include or exclude edges of peer parts during creation. Added exclude interior loops or use only interior loops, to the Extrude planar face option from ST5.


Better reuse with synchronous technology


  • ·         More robust rectangular and circular patterning.
  • ·         Pattern recognition allows count and instance editing of imported patterns.
  • ·         Partial round delete with end capping.
  • ·         Dimensioning chamfered edges uses virtual vertices.

 

Create stamped sheet metal parts with a single command – emboss a tool or punch into a sheet metal part.


Stiffen parts by adding features across bends - add beads, dimples, louvers, emboss features across bends


Sheet Metal Features on Parts - sheet metal features can be placed on regular ordered parts of uniform thickness without having to transform the part to sheet metal. This provides an especially efficient method in stamped metal design.

Again, there are many other enhancements in Part modeling which will benefit all users.

 

ST6 Assembly Design


Solid Edge continues their dominance in working with large assemblies. Along with some nice enhancements to PathFinder Indicators and Physical Properties, here are my favorite improvements:


Assembly occurrences can now be used for inputs to Boolean operations - No inter-part copy of the geometry is needed and multiple tool body components can be selected (see previous blog article).


Faster display - New display capabilities speed pan/zoom/fit by up to 2 times.


Complete overhaul of simplify assemblies


         New environment for creating user defined simplified representations.

         Enclose component automatically encloses components with rectangular or cylindrical solids.

         Duplicate body speeds simplification of copied or patterned components.

         Goal is to simplify models for effective design of 1 Million+ parts.

 

Create In-Place Enhancements – moved to optional QuickBar with better control over placing the origin.

 

Synchronous Assembly Modeling Peer Edge Locate – allows for improved key-point selection when modeling in the Assembly.


Plus several new enhancements to synchronous commands have been made while a user is in-place activated into a part or sheet metal file from an assembly.




ST6 Drafting


Two of the most exciting enhancements in Solid Edge ST6 appear in the Draft environment. When the following was demonstrated they received an enthusiastic round of applause from the audience at SEU2013.


Alignment control


         Align annotations with a linear, rectangular or fitted shape.

         Reposition the annotations by dragging the alignment shape.

 

Dimension auto-arrange


         Clean up messy dimensions with a single mouse click.

         Select dimensions by fence or by drawing view.

         Creates and aligns dimension grouping.

 

Some other notable changes in drawing production are:

 

         Faster zoom/pan, and hatch display with large 2D drawings.

         Auto-constrain 2D elements during drag-modify.

         Retrieve slot feature centerlines.

         Partial bolt hole circles.

         Simplified drawing view wizard.

         Shortcuts and easier sheet tab creation.

         Edit tables in place.

         Better editing of embedded documents.

         Drawing views are now displayed before placement.

         Derived break lines from one view to another.

         Align any drawing view with key-points or drawing view centers.

         2D directional fence select: left for overlapping, right for inside locate to.

         Create tables from placed blocks on schematic drawings.

 

These enhancements, and more, continue to make Solid Edge’s drawing capabilities the best on the market.




Help for SolidWorks refugees


One other noteworthy feature, added to Solid Edge ST6, is the new SolidWorks migration tool. Siemens is going after the SolidWorks customers who are concerned about the kernel change and loss of legacy data. This tool, combined with some other enhancements, will allow the SolidWorks user to:


  • ·        Protect their investment in design.
  • ·        Get the power of synchronous technology.
  • ·        Maintain speed and reliability with Parasolid.

  • If you are a SolidWorks customer and are concerned about the ongoing changes and mixed messages from Dassault Systemes, Siemens is willing to help you transition to Solid Edge, while protecting and reusing your legacy data.


 

Solid Edge ST6


As mentioned at the beginning of the article, I have only scratched the surface of what’s new in Solid Edge ST6. I did not even mention the enhancements in the simulation package, standard parts, framing, or data management. I will attempt to expand on the improvements in future blog articles. But I felt it important to give an overall account of Solid Edge ST6, as presented at SEU2013. I have worked with Solid Edge for over 10 years now and I am truly impressed with how the development team continues to listen to the actual customers. Solid Edge ST6 enhancements have truly been driven by the customers. The 3 core values for this release were to:


  1. 1.    Accelerate design for faster time to market.
  2. 2.    Faster revisions for higher repeat business.
  3. 3.    Better reuse for lower development costs.


Siemens has done a great job at meeting these core values with Solid Edge ST6. Judging by the excitement at SEU2013, this looks to be a great release with customers eagerly awaiting the arrival of Solid Edge ST6. The release date has not been finalized yet, but the general consensus is that customers can expect to receive their copy sometime in August 2013.

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.



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. 


Synchronous Hole Recognition

John Pearson - Thursday, June 20, 2013

If you are using the synchronous modeling in Solid Edge ST5 you may have noticed the new Recognize Hole command found under the Hole Command flyout.




This command, specifically designed for imported models with no history, enables cylindrical cutouts to be automatically identified and re-defined as synchronous procedural hole features. It is available in the Part, Sheet Metal and Assembly environment. The user simply has to select the command and select the model. Holes are automatically recognized and displayed in the Hole Recognition dialog.


 




Hole types and sizes are grouped together automatically.


 


A user can choose not to recognize a cylindrical feature as a hole by toggling off the check mark for the feature.



Within the dialog, you can rename the hole features, by double clicking on the default feature name. You can also redefine the hole feature, by applying saved settings or by using the hole options dialog.




Once the user selects OK, to accept the hole options change, a preview of the new hole parameters is shown on the model. The user then selects OK, in the Hole Recognition dialog, to accept the change.



The user can use the Face Selection option to recognize holes only on selected faces.




Pre-selection of a face, or faces, is also supported. You can select a face, or faces, and then run the Recognize Holes command, to perform recognition on only the selected face(s).



The Hole Recognition command allows users to add intelligent synchronous procedural hole features to imported models. Because it’s a hole feature, it also recognizes the user defined pattern created in all hole features, which can be used for rapid placement of bolts or screws in the assembly.


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