January 26, 2009
NX 6 – Synchronous Modeling Promotes Design Freedom
Please note that contributed articles, blog entries, and comments posted on MCADcafe.com are the views and opinion of the author and do not necessarily represent the views and opinions of the management and staff of Internet Business Systems and its subsidiary web-sites.
| by Jeff Rowe - Contributing Editor
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As a long-time product designer I’ve been a member of the CAD community since the late 1980s and have followed developments (good and bad) closely since then. In the early days, it seemed like just about every release of software contained a bunch of new features and capabilities – some useful, some not so useful. “Feature bloat” became a real problem with a lot of MCAD products at the expense of real utility and stability. Recently, however, most MCAD vendors have become more concerned with product quality and reliability than just continuing to pile on more “stuff,” that few customers understand or actually use.
In the spring of 2008 Siemens PLM Software announced not just a new feature or capability set, but a new CAD methodology that it claimed to be the biggest MCAD breakthrough in a decade called Synchronous Technology. At the time, the announcement was actually more speculative than a true demonstration, but nonetheless, from the beginning, the concept and its implications were pretty intriguing. Synchronous Technology that forms the basis for synchronous modeling were integrated into the newest versions of Siemens’ MCAD products – NX 6 and Solid Edge ST. Using NX and Solid Edge as vehicles, Siemens PLM Software became the latest MCAD company to tout the advantages of
non-history-based design methods. However, NX 6 has a notable difference with the way synchronous technology is implemented in what the company calls Design Freedom that I’ll discuss later. Also, NX 6 differentiates itself with the fact that synchronous technology can be used in both history and history-free modes.
Before we jump into synchronous technology and synchronous modeling, I think it’s worthwhile to briefly cover the three underlying technologies that form the basis for the geometry component of synchronous technology and synchronous modeling:
Siemens PLM Software collectively refers to these core geometry technologies as its “geometry triangle.”
The “change” technology is used to modify the faces of a model. This technology is the basis for several synchronous modeling commands, such Move Face, Offset Region, Resize Face, and Make Coplanar. Within the Move Face command the change technology moves selected faces and adapts neighboring faces to accommodate the change.
The “delete” technology is employed to remove faces from a model. This technology is the foundation of the Delete Face and Cut Face commands. The delete technology deletes selected faces and heals neighboring faces to close the open area left where faces are deleted. Delete has enhanced support for merged faces and dependent blends.
The healing function is the emphasis for delete technology. Limitations are being addressed but there will be cases where neighbor faces cannot heal an open area. In this case you can incrementally delete smaller sets of faces with multiple uses of the Delete Face command. The Replace Face command can also serve as alternative to Delete Face.
The “re-blend” technology is a companion to “change.” It is employed to adapt blend faces when selected faces change (move and offset), and also applies to constant radius rolling-ball blends.
So, with this little bit of background, let’s take a look at what NX 6 is about and what it can do.
Getting Started With NX 6
For the purposes of this review, I received the core NX 6 application pre-loaded and configured on an HP Compaq nw9440 mobile workstation. It had an Intel Core 2 CPU running at 2.16 GHz, 4GB RAM, nVIDIA Quadro FX 1500M video card, and Microsoft Windows XP Pro SP2. This set up was more than adequate for the part and assembly solids and surfaces that I modeled with NX 6 (188.8.131.52).
It wasn’t all that long ago that NX’s interface was known as being quite intimidating. However, with NX 5, a lot of that changed as the UI became much more Windows-compliant, and, therefore, more user friendly. A big part of the movement toward ease of use are NX’s Roles that let you customize and limit the UI by hiding tools that you are unlikely to use. This is especially important to new NX users, or so-called casual users who can use the default Essentials role. In this default role, the command buttons display both icons and the command name. If you want a more comprehensive set of tools, click the roles tab in the resource bar and select a more advanced role.
It you have used an earlier version of NX, you can reinstate your previous UI layout from the Last Release folder in the roles palette.
The UI, roles, and customization combined are what help give NX 6 the ability to accommodate a wide variety of users and workflows.
As far as command flow is concerned, and to further illustrate how the UI continues to improve, commands are displayed in dialog boxes that are organized by workflow that let you logically work from top to bottom to perform a command. A red asterisk marks steps that require some selection, and a green check mark replaces the red asterisk after a suitable object is selected. An orange highlight indicates that the current selection is active, while a green highlight indicates the next recommended step. When all required inputs are completed, the OK or Apply buttons are highlighted in green. To keep things relatively simple, some commands, such as Dimension Creation, are optimized to
complete automatically and loop after you make the required selections, and only have a Close button.
Models, assemblies, drawings, and most other objects created in native NX 6 are saved as parts with a .prt extension, and you can open as many parts as you want or need to at any time. If you have Teamcenter integrated with NX, parts are stored as datasets and identified by part numbers. Specifically for drawings, to make things more efficient with a more direct workflow, I’d recommend that you use a “master model” approach that separates the drawing part from the model part by using a drawing template that automates this method.
Like virtually all MCAD packages, parts in NX 6 often begin with sketches as one of its several available design approaches. The sketcher is an NX tool for creating 2D geometry within a part, and each sketch is a named collection of 2D curves and points on a specified plane.
The strategy you use to create and edit your model to form the desired object depends on the form and complexity of the object. In reality, you will probably use several different methods during a design session.
NX sketcher tools let you capture design intent through geometric and dimensional relationships, collectively referred to as constraints, to create parameter-driven designs that can be updated later. Sketcher continuously evaluates constraints to ensure that they are complete and do not conflict. Sketcher also lets you create as many, or as few, constraints as required.
You use NX’s sketcher to freehand a sketch, and dimension an outline of curves. You can then transform the 2D sketch into 3D using tools such as Extrude or Revolved Body to create a solid or sheet body. You can later refine the sketch to precisely represent an object by editing the dimensions and by creating relationships between geometric entities. Editing a sketch dimension modifies the geometry of the sketch, as well as the body created from that sketch.
You can position a feature, such as a hole or groove, relative to the geometry on a model by using positioning dimensions. The feature is then associated with that geometry and will maintain those associations whenever you edit the model. You can also edit the position of the feature by changing the values of the positioning dimensions. If the model is edited later, the associated drawing and dimensions are updated automatically.
Although it can produce some outstanding surfaces, getting to a final solution can be somewhat challenging because some of the curve creation tools can take some trial and error to arrive at the precise shape and form you are looking for.
Overall, though, once you get beyond some NX nuances, creating sketches and parts is about on par with other MCAD packages – not really any easier, but definitely not as difficult as many have been mistakenly led to believe.
NX uses the concept of associativity to link separate pieces of information together that helps automate part design.
Associativity is used to indicate geometric relationships between portions of a model. Associativity is used when creating geometry. For example, an object may be part of the model (in Modeling) or specifically linked to a single view (in Drafting). These relationships are established as you create a model. In an associative model, constraints and relationships are captured automatically as the model is developed. For example, in an associative model, a through hole is associated with the faces that the hole penetrates. If the model is later changed so that one or both of those faces moves, the hole updates automatically because it is associated with the faces.
In NX all drafting objects are associative. Some drafting objects, like dimensions, are linked directly to geometry so that they automatically update when changes occur. Other drafting objects, such as notes, are associated to a position rather than specific geometry. Some drafting objects, such as labels, ID symbols, forms and positional tolerances, can be associated to either the geometry or to a position.
You can associate non-geometric information with objects and parts. You can link attributes to objects in order to record special characteristics of the objects.
There are two types of attributes – system and user-defined. System attributes are recognized by the system and assigned by a user, such as when you assign a name to an object or a group to aid in the selection process, the system will recognize that name until you explicitly change it. User-defined attributes are those that you create, but have no meaning to the system. For example, you may associate attribute information to a group of geometric objects so they appear correctly in the bill of material for the product.
You can position a feature relative to the geometry on a model by using positioning dimensions. The feature is then associated with that geometry and will maintain those associations whenever you edit the model. You can also edit the position of the feature by changing the values of the positioning dimensions.
Expressions let you incorporate design requirements and restrictions by defining mathematical relationships between different parts of a design. For example, you can define the height of a boss as three times its diameter, so that when the diameter changes, the height also changes.
Other NX applications can operate directly on solid objects created within Modeling without translating the solid body. For example, you can perform drafting, engineering analysis, and NC machining functions by accessing the appropriate application. You have to remember to save changes made to your layout before entering the Drafting application. If you do not save the changes, they are gone when you return to the Modeling application.
A model can be updated either automatically or manually. Automatic updates are performed only on those features affected by an appropriate change (an edit operation or the creation of certain types of features). If you wish, you can delay the automatic update for edit operations by using the Delayed Update on Edit option.
The manual method that I liked best was the Playback option on the Edit Feature dialog that recreates the model starting at its first feature. You can step through the model as it is created one feature at a time, move forward or backward to any feature, or trigger an update that continues until a failure occurs or the model is complete. The Edit during Update dialog, which appears when you choose Playback, also includes options for analyzing and editing features of the model as it is recreated (especially useful for fixing problems that caused update failures).
Synchronous Modeling in NX 6
NX 6 has two modeling modes – history and history-free – and you can take advantage of the benefits of each – sort of a best of both worlds sort of thing. The two modeling modes and the ability to switch between them are what set NX 6 apart and constitute Design Freedom, however, Synchronous Technology works in either of the modeling modes. Because you can use both modes in NX 6, you might find that the history-free mode is well-suited for the conceptual stage of a design and the history mode well-suited for the refinement stages of a design.
In history mode, you create and edit models using an ordered sequence of features that are displayed in the Part Navigator. This mode is most useful for parts that are highly engineered.lIt is also useful for parts that will be modified using predefined parameters based on the design intent built in to their sketches, features, and feature order used to model the parts.
In history-free mode, you create and edit models based on their current state without an ordered sequence of features – only local features without a sequential structure are created. Local features are unique because they are created and stored in history-free mode. Modifying a local feature affects only the local geometry without the need to update and replay a global feature tree. This is one of the primary reasons that local features can be edited much quicker than features in history mode. Synchronous modeling is also what lets you create geometry that adapts to a changing design context.
The Synchronous Modeling toolbar is your main ally for synchronous modeling and consists of the following commands that will provide you with a better understanding of what it can do (see Figure 1):
Move Face – Moves a set of faces and adjusts adjacent faces to accommodate the move.
Pull Face – Pulls a face out of the model to add material or into the model to subtract material.
Offset Region – Offsets a set of faces from their current location and adjusts adjacent blend faces to accommodate the offset.
Replace Face – Replaces a set of faces with another set of faces.
Resize Face – Changes the diameter of a cylindrical or spherical face and adjusts adjacent blend faces to accommodate the resizing.
Delete Face – Deletes a face or set of faces from a solid body and adjusts other faces to accommodate the deletion.
Copy Face – Copies a set of faces. Also used to cut, paste, mirror, and pattern faces.
Make Coplanar – Modifies a planar face to be coplanar with another face. Also used to make faces coaxial, tangent, symmetric, parallel, and perpendicular.
Linear Dimension – Moves a set of faces by adding a dimension and changing its value. Also used for angular and radial dimensions.
Shell Body – Modifies a solid body by applying wall thickness and opening selected faces. The wall thickness is maintained when the model is modified. Also used for modifying shell faces and wall thickness.
Group Face – Collects a set of faces together as a group.
Cross Section Edit – Edits a model by modifying its cross section.
Note: All of the commands except Shell body and Cross Section Edit are available in both history and history-free modes.
Figure 1: The Synchronous Modeling Toolbar
In NX 6 you can change the design mode between history and history-free, however, due to the differences between the two modes data unique to each mode is removed when the mode is changed. For example, when changing from history mode to history-free mode history data is deleted, including feature data. Geometry remains in its current state but features are removed, similar to using the Remove Parameters command. However, features that are local features are retained, so features such as holes and blends remain as holes belnds, but become local features.
When history-free mode is set, history-related commands are hidden in the interface. For example, Edit with Rollback, Reorder Feature, and Replay are hidden.
Specific synchronous modeling commands are used to modify a model, regardless of its origins, associativity, or feature history. A model can be imported from other CAD systems, neutral formats (IGES and STEP), non-associative, with no features, or it could be a native NX or Solid edge model with features. Synchronous modeling lets you use parametric features without the problems arising from feature history by working directly with a model that virtually eliminates time spent rebuilding or converting geometry. In short, if you have a parametric model that you want to edit quickly, use synchronous techniques in history mode.
I found that synchronous modeling is best suited for models composed of analytic faces, such as plane, cylinder, cone, sphere, and torus. This does not necessarily mean simple, geometrically primitive parts, since models with literally thousands of faces can be composed of these analytic face types. A deficiency that I noted in NX 6 is that synchronous modeling does not work well with blends that would be found in cast or molded parts, but the company is working on this for future release.
In either history or history-free mode, you can select a compete set of features regardless of whether they are parametric features or order-independent local features created in history-free mode. You use the Feature Faces selection type from the selection tool bar and select a face from the object or element you want to edit, and all faces related to that feature will be selected.
Figure 2: Synchronous modeling lets you easily copy, paste, and move objects.
History-free mode is an environment where linear history is not accumulated and there are no features to replay.
When working in history-free mode, you can:
Use both traditional modeling commands and synchronous modeling commands.
Use synchronous modeling commands to easily modify the model, regardless of how it was created. In history-free mode, not all of these commands create features that appear in the Part Navigator, as they do in history mode.
Use the Face Finder in commands to help you select faces to modify.
Edit local features by changing their parameters in the same dialog box used to create them.
Select local features from the graphics window.
Split bodies into multiple bodies (for example, using the Extrude and Trim Body commands).
In history–free mode, it’s important to remember that the Part Navigator has no timestamp order and expressions are created for commands that produce local features. There is no feature update or playback available (because there is no history), there is no rollback available (although Undo is available), and an assembly can include parts with and without history.
While this time around, synchronous operations are relegated primarily to faces, one of the more interesting objects that I modeled and modified in history-free-only mode in NX 6 was an adaptive shell. A shell consists of a wall thickness value and a collection of shell relations between its selected shell faces and partner faces (the offset counterpart of each of the shell faces in a shelled body). Shell relations in an adaptive shell can maintain the wall thickness of the shell when changes are made to it. For example, if you move a face in a shell body with the Move Face command, the shell partner face automatically updates to maintain the shell’s thickness. You can also
remove all shell relations in an adaptive shell by deleting or modifying a partner face using other Face commands, such as Move, Delete, or Shell. Modifying a shell showed me that even this relatively simple change required no design interrogation that would usually be required with most other history-based modelers.
Face selection has been enhanced in NX 6, and new capabilities have been introduced with synchronous modeling that increase the potential of synchronous technology, and include Face Finder, Feature Finder, and Active Selection.
Feature and Face Finder are capabilities that seek and designate additional features or faces to copy, move, delete, etc. depending on how their geometry compares to a selected face – actually a relatively high degree of feature recognition.
Face Finder is new to NX 6 and is the logic component of synchronous technology. Face Finder searches, finds, and selects faces by recognizing geometric conditions between an input face and a set of scope faces within the model. For example, two cylinders might be oriented and located along the same axis – a coaxial condition. With Face Finder you can select one of the cylinders and recognize the other as coaxial. The Face Finder interface is available in several synchronous modeling Commands, such as Move Face (see Figure 3).
Figure 3: The synchronous modeling Face Finder and Move Face Command. When selecting the cylinder and using the Face Finder Coaxial, NX automatically selects all the geometry meeting the criteria. You then select a vector direction and drag the geometry to where you want it. Meanwhile you can see how the blends from the base of the rib updates, traversing the new surface boundaries of the cylinder.
Feature Finder was introduced in NX 5 and is enhanced in NX 6. Feature Finder is used to select an edge-connected chain of faces where the face set topologically represents an interesting feature. This is not the same as the set of faces produced when adding a NX feature, such as an extrude feature. Rather, the feature is derived by finding faces that fit a topological description. The features (topological descriptions) that are recognized by NX include boss or pocket, rib, slot, and connected blend faces.
Active selection is new to NX 6. Active selection improves selection intent. Within the synchronous modeling command set the selection intent rule defaults to “Single Face” since modifying a single face is what you’ll be doing a majority of the time.
Different Approaches With Assemblies
For many MCAD packages, large assembly performance is what sets them apart from the competition. In the previous release, NX 5, significant architectural enhancements were the basis for major improvements in large assembly modeling. To further improve assembly performance, Siemens JT data format was also integrated into NX 5. JT simplifies the pervasive multi-CAD environment that most manufacturers now deal with, as well as offering lightweight assembly design functions for faceted assembly representations that improve performance when precise solid geometry is not required, such as design reviews. To a large extent, it is the JT format that improves NX’s large assembly capacity
and performance, while reducing memory usage and rendering time.
In NX, assembly part files point to geometry and features in the subordinate parts rather than creating duplicate copies of those objects at each level in the assembly. This technique not only minimizes the size of assembly parts files, but also provides high levels of associativity. This enables a user to modify the geometry of one component so that all assemblies that use that component to automatically reflect the change. These relationships not only affect assemblies, but also other associated objects, such as drawings, tool paths, and CAE meshes.
There are different approaches to assembly modeling and with NX you are not limited to any one method. You can create individual part models, and then add them to assemblies later (bottom-up), or you can create parts directly at the assembly level (top-down assembly creation). Additionally, you can start by using a top-down method, and then switch back and forth between bottom-up and top-down modeling, depending on your specific needs. It is this versatile approach that helps NX fit into a wide variety of workflows.
To assist assembly design, multiple parts can be loaded simultaneously. Load options in the NX Assembly Navigator load implicitly or explicitly as a result of being used by some other loaded subassembly. The Assembly Navigator also lets you display information and manipulate the assembly for selecting, hiding, or suppressing assembly components. Additionally, loaded parts do not have to belong to the same assembly. The part currently displayed in the graphics window is called the displayed part. You can make edits in parallel to several parts by switching the displayed part back and forth among those parts.
An assembly can contain a mixture of parts modeled with history or history-free mode. This is not actually new. Even prior to the NX 6 this combination could be used. If you import a Parasolid .x_t (or other) part into a NX part file it has no history. This part can coexist in a NX assembly with native NX parts complete with features and history. Also, an assembly can contain a mix of parts and JT files, so if you are working with a supplier or OEM who provides only lightweight data for building an assembly, you can reference JT data and build models that are the correct size and shape.
When the displayed part is an assembly, you can change the work part to any of the components within that assembly (except for unloaded parts and parts of different units). Geometry, features, and components can then be added to or edited within the work part. Geometry outside of the work part can be referenced in many modeling operations. For example, control points on geometry outside of the work part can be used to position a feature within the work part. When an object is designed in context, it is added to the reference set used to represent the work part
Geometric changes made at any level within an assembly result in the update of associated data at all other levels of affected assemblies. An edit to an individual piece part causes all assembly drawings that use that part to also be updated. On the other hand, an edit made to a component in the context of an assembly results in the update of drawings and other associated objects (such as tool paths) within the component part.
Final Thoughts on NX 6
Synchronous modeling has been somewhat controversial since it was first announced and has endured considerable scrutiny by a broad spectrum of people ranging from users to pundits. There is yet no consensus on synchronous modeling, but everybody seems to have an opinion – some well-founded, some misleading. Admittedly, this is the first release that employs synchronous technology. Its implementation is a good start to capabilities that will only become more comprehensive over time (and I mean relatively quickly based on conversations I have had with the company). While it does share some characteristics of competing history-free MCAD applications, even at this early stage it
also offers several unique capabilities.
By itself, NX has been a very capable MCAD application for a number of releases, and synchronous technology and modeling techniques make NX 6 a very significant release. Out of the box, the core package is well-rounded and versatile, and there are a large number of optional modules available for handling virtually aspects of CAD, CAM, CAE, and PLM. NX 6 is one the most comprehensive packages out there, with “heavy duty” solvers and a user interface that continues to improve. The addition of synchronous modeling and the range of optional modules make NX 6 a wise choice for complex mechanical and mechatronic design that you are very unlikely to outgrow. As you designs mature
and evolve, NX 6 will keep pace stride for stride moving forward.
There are a lot of things I could cover, but I could only hit some of the highlights. I easily could have written an entire article on each of the topics covered in the sub-sections. There are a lot of new and interesting features and capabilities to be discovered and used in NX 6 – starting with synchronous modeling and branching out from there. Is synchronous modeling perfect? Well, no, but it’s a great start to what’s possible in the future for mechanical design.
If you have any specific questions pertaining to NX 6 that were not covered in this review, feel free to contact me at
| NX 6 Evaluation Quick Guide
|Price: Starts at approximately $9,000 (US)
|For More Information: NX6
|Contact: Siemens PLM Software
The Week’s Top 5
At MCADCafé we track many things, including the stories that have attracted the most interest from our subscribers. Below are the five news items that were the most viewed during last week.
Autodesk announced a restructuring plan to reduce its annual operating expenses. The company anticipates the restructuring will result in annual pre-tax cost savings of approximately $130 million annually starting in fiscal 2010. As part of its restructuring plan, Autodesk plans to reduce its workforce by approximately 750 employees, representing approximately 10 percent of the company's global workforce. The company also plans to consolidate certain facilities. The actions are in addition to the ongoing cost reduction initiatives previously announced, which include a hiring freeze, business travel restrictions, and other reductions in its operating expenses. As a result of this
restructuring, the company anticipates taking a pre-tax charge in the range of $65 million to $75 million. Approximately $45 million to $50 million in pre-tax charges will be taken in the fourth quarter of fiscal 2009. Most of the remaining charge will be taken in the first quarter of fiscal 2010.
Lattice Technology announced its new XVL Plug-in version 1.2 for Adobe Acrobat 9 Pro Extended. Acrobat 9 Pro Extended supports the major 3D CAD data formats, such as CATIA V4 and V5, NX, I-DEAS, JT, SolidWorks, Pro/ENGINEER, Autodesk Inventor, and others. Lattice’s new Plug-in developed using the Acrobat 9 3D SDK allows engineers to open any of the supported files formats directly in Lattice Technology’s XVL Studio and Lattice3D Reporter applications. Assemblies can be edited, animated, annotated, and shared with others using PDF. 3D Parts lists and BOMs created in Lattice3D Reporter and Microsoft Excel can be easily shared with others by using the Plug-in to deliver 3D
data, parts lists and interrelated assembly tree data in PDF. The 3D PDF files created can be shared, and the 3D animations, interactivity and related assembly structure data can be viewed using free Adobe Reader software. Information about the XVL Plug In for Adobe Acrobat can be found at:
MSC.Software Corp. announced a new license and distribution agreement with FEV Motorentechnik GmbH. Through this agreement, FEV will continue developing the common ADAMS/Engine technology, and leverage its automotive marketplace expertise to make product enhancements using the technology. FEV will be the provider of new ADAMS-based Engine/Powertrain software products under the new brand: FEV Virtual Engine Powered by ADAMS. FEV’s position in the engine and powertrain technology marketplace makes it well suited to grow the use of the ADAMS/Engine technology in automotive and related industries. FEV is now licensed to develop, market, distribute, and support all MSC Software's
engine modules worldwide.
ESI Group announced the acquisition of Mindware Engineering Inc. (Mindware), recognized in engineering services encompassing CFD, and is also well versed in Fluid/Structure interaction and engineering data management. Mindware has established strong relationships with customers from automotive, aerospace, and defense companies by providing digital simulation based solutions driving product design and development. Through the Mindware acquisition, ESI Group will reinforce its global offering of end-to-end Virtual Prototyping of industrial products involving CFD functionalities. This deal creates an opportunity for both teams to leverage their complementary knowledge to enable
simulation-based design in multi-physics. ESI Group has taken control of Mindware by acquiring 100% of its shares through its American subsidiary ESI North America Inc.
PTC announced the availability of Windchill ProductPoint for sharing CAD and other structured data among teams. Windchill ProductPoint provides an opportunity for smaller companies to experience the benefits of PLM without a large investment while also giving companies with an active SharePoint strategy the flexibility to extend their product development system to broader user communities. Windchill ProductPoint combined with Microsoft SharePoint helps teams to connect to each other in a variety of ways including:
Instant access to colleagues via presence detection
Personalization of workspaces to organize relevant content
The sharing of rich product information throughout the company and with their customers
Jeffrey Rowe is the editor of MCADCafé and MCAD Weekly Review. He can be reached at
NX 6 –Synchronous Modeling Promotes Design Freedom
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- Yes but it's not new January 27, 2009
Reviewed by 'Adrian'
Hi Jeff Rowe
I am intrested in the noise about synchronous modelling, but is this not already a feature in Think design from the company Think3 now for a few years? Feature set certainly looks simular and Open Mind OEM Think Design in the product called hyperCAD. I certainly know i have been using this function called [censored] modeling for at least 18months.
3 of 12 found this review helpful.