Products & Services You
Need to Know About.
Only on CADdigest.com.
Find Out More!
By John Evans, Mar 13, 2012
Is Solid Edge easy to use? Any software, even CAD, can appear easy to use in the hands of a demo jock. But can a real user make real parts without any training? With companies getting tighter with budgets, that is often the case. CADdigest subjected John Evans, veteran CAD user but Solid Edge novice, to just such a case: here is your new software, there will be no training...now get to work!
When I was asked if I would review Solid Edge Synchronous Technology 4, I had never used the product. So, I felt it would be fair to evaluate some of its functions while looking at it from the perspective of a new user. Keep in mind that the following collection of comments are from someone who is experienced with Autodesk’s Inventor, and are based on my experience as a someone with little time to train, forming opinions while learning to become productive with ST4.
The first thing I saw after installing ST4 is the splash screen that gave me some top level options, including tutorials. I wanted to go straight in and draw before returning to the tutorials, so that I could report to you how “CAD friendly” the app is. So I choose ISO Part on the splash screen, and ST4 loaded into an empty part model.
Once I was in the part modeling environment, I was stunned with what I saw. It looked like a billion little icons. Once I got involved and became familiar with them, however, it wasn’t too bad. Half of them are understandable by any experienced CAD user; I invested a few hours a day over a week’s time, and learned 75% of the icon and toolbar functions. That’s reasonable, I think.
The interface overall is handled by two UI elements now standard in our industry, the ribbon and the browser. The ribbon is divided into panels, and the browser grouped into expandable trees, as I expected.
Part modeling is not too rough. The sketch tools are somewhat obvious. I quickly added an extrude and a revolve (which they call “protrusions”), and followed up with a hole and some chamfering. I saved the part, and then headed to the assembly environment. At this point I actually had to hit the help file, because I couldn’t figure out how to insert an existing component. I feel this should be obvious. (The solution involves enabling the Parts pane, which I describe later.)
Once I found the Parts Library, I was able to add two components and somewhat smoothly assemble these together. That’s where the fun ended, because I could not determine from standard workflows, how to resize a hole to a shaft (because I didn’t pay attention). So I returned to some part modeling and then hit the tutorials.
Figure 3: Selecting an origin plane to start a sketch
This is a really straight forward environment, with an exception that I’ll mention in a moment. Pick the geometry type, and then the origin plane desired. A toolbar appears at the top of the graphics area with a variety of sketch geometry options, including the width and height of the sides for easy entry and overrides.
As soon as the geometry is completed, the application looks to extrude the profile. The process was very simple, and exactly what I would expect.
Once the solid is developed, the sketch is a goner. That’s right: the geometry involved in the sketch has no further effect on the model. The only exception to this is the Smart Dimension. These are stored and grouped in the browser, and can be locked and unlocked as needed. Once created, they help carry the design intent forward through the rest of the process.
After the solid begins to take shape, solid features are added in the typical manner of editing. One thing I’d like to mention here is how fast the profiles are picked up, even from geometry intersections using non-closed curves.
Solid editing comes in one of three modes (see figure 4):
What’s kind of interesting is that as you work you can flip between these modes, and that each of these has its own interface. Here are some highlights of each mode.
This environment stacks features in an ordered state, grouped separately within the feature browser.
I found this environment quite user friendly. On the ribbon’s Solid panel, there are a collection of tools for automating the process of creating geometry and the feature, all in one action. These tools guided me through the sketch > profile > feature activities in a simple manner. As each workflow is completed, the next action starts by default, including the selection of profiles. As I noted earlier, the sketches are consumed by each feature automatically, and so are not accessible without editing the feature directly.
From Left to Right:
Figure 6: Ordered edits with simplified ‘on the fly’ work features.
Figure 7: Ordered tools automatically pick a profile.
FIgure 8: Ordered features are organized in a separate browser collection.
Synchronous mode is the one in which I worked the most, because it is the default state, and I really wanted to test the synchronous capabilities; I found comfort in modifying features on the fly, with no concern for the order in which actions had been performed previously.
Synchronous operations are similar to direct modeling in other applications, in that they are organized in the model browser and within their own group. These are applied to the model autonomously, and to function don’t depend on any historical build-order. When I built something on top of a cut feature, and then I removed the cut, there are no errors or problems. The software simply reworks the remaining features together again.
Planes, sketch geometry, and constraints are all available in ST mode, and feel similar to any other CAD application. As solid features are built, the sketches are not ‘consumed’ but are sent to a scrap bin named “Used Sketches.” They can be reused, but changes to them have no effect on the features previously created. That’s where Smart Dimensions and the Face Relate panel take over.
Smart Dimensions are 3D dimensions capable of controlling almost every aspect of the design. They carry permanent variables that are cataloged and accessible from the Variables table. The Smart Dimensions can be locked and unlocked as needed to develop the model using direct manipulation. When I had a key dimension that needed to be adjusted to allow another face to move, I didn’t need to delete it; I simply unlocked it. When I moved the face, the dimension updated, and then I locked it again.
Figure 10: During assembly synchronous editing, unchecking PMI this shuts off dimensions globally (shown here with PMI turned on).
Unlocked dimensions are shown in blue, locked in magenta, and unlinked (dead) in gold. Dead dimensions are ones that were attached to features, but then were discarded in the back and forth process I used to work up this model until I was satisfied with its design.
Smart Dimensions are permanent features in the design. They persist within the design from start to finish, because they are intended to handle formatting and manufacturability, such as tolerancing and standardization.
I developed a shaft and a block in the synchronous environment. I built the shaft from one side of the block’s inner bearing recess, and then extruded it in both directions from this reference. I developed the shaft symmetrical to a common center plane, and referenced it back to key faces in the block -- without any other sketches or work geometry.
I simply picked the circle, picked the face, and then pulled it, allowing the feature to extrude; no dimensions and no extra worry. Once the protrusion was out, I simply used Face Relate to identify equal radii, common faces, and concentric cylinders. Occasionally I’d have to add a Smart Dimension at a critical point, which was performed directly to the solid.
Variables are synonymous with parameters, and are automatically entered when Smart Dimensions are applied. (Other feature dimensions used in the initial sizing of geometry are not stored and are forgotten, along with the used sketches.) They are accessed through the Variables table and the Variables panel on the Tools tab of the ribbon.
Like parameters in other MCAD programs, variables allow me to reference other key feature dimensions and item counts to use formulas on the sizing of the model. I did not spend much time on this aspect, but thought a little usability could be added.
This table displays the status of each variable, along with various other bits of information. One nice feature was that as each variable is selected, it is highlighted in the graphics view area. This was quite useful in both the part and assembly environments.
Each variable has rules that can be activated, transforming the variable from a static component into a substantially more versatile feature.
About this time I ran headlong into what people at Siemens PLM warned me about: Live Rules. It seemed like something sinister enough to prompt a Web conference turned out to be a beautiful thing. I watched as Siemens professionals worked synchronous technology and Live Rules over a solid part, with very little dimensioning applied.
Live Rules enforce run-time geometric constraints along the features of the solid. Each time a feature is modified (such as pulling a face), Live Rules searches the solid model for relationships, such as concentricity and parallelism. If it finds any, then it checks the Live Rules controls to see whether it should enforce the relationships it found.
The controls for Live Rules (or temporary constraints) are maintained in a pop-up toolbar, which activates any time a change is in progress. This includes modifications to Smart Dimensions. .
Figure 13: The Live Rules control toolbar.
The rules that are activated are in orange, and deactivated ones in white. Various configurations can be made and saved if desired. Additionally, there is an undo and a suspend button, allowing changes to be made that ignore all Live Rules.
Live Rules are named as such because they apply only to part features that are moving; they are not stored in parts or features. Furthermore, since Live Rules determines these characteristics on the fly, each time a feature is adjusted, it successfully maintains these feature relationships on solid models that have no dimensional or geometric constraints whatsoever, such as with an imported STEP file.
Once a rule is established during a feature adjustment, the Live Rule bar alerts the user by changing the pertinent active Live Rules icons to a green color. This gives the user some on-screen validation of the relationships that were found and enforced.
n my case, I initially dragged the inner face and found that the opposing face did not respond in kind, nor did the Live Rules for symmetry activate. Some small factor had changed of which I was unaware. I realigned the face for symmetry, and then when I again tried the adjustment, the Live Rule activated and both faces moved.
Simplify mode allows users to reduce the model complexity before being sent off for other operations, such as simulation
I found an awesome capability in Simplify mode of editing: each change is organized in a separate browser group. Like Ordered features, these can simply be ignored when not in this particular mode.
The functionality is much like Level of Detail in Inventor, but operates on part files. This is a variation of what I had in mind for models created in other software that are intended to be moved to simulation and so needed feature simplification.
In addition, the simplified and the designed versions of the model can be used in assemblies, as in a "simplified level of detail."
Figure 19: The Pane configuration button.
I found it fairly easy to learn how to assemble components. The first thing that we usually do is to place (or insert) an object. This is done through the Parts Library pane through which users navigate to their component sets, and drag them into the graphics view area. Pretty simple. The nice thing about the pane is its ability to keep it ready and focused on a specific group of components, getting rid of additional steps of opening and navigating a dialog.
Finding this was, however, not fun, and I required some help. Then of course I closed it, and had to learn all over again how to activate it. Fortunately, I followed instinct and found the pane visibility group almost immediately on the View tab on the ribbon. Score another for Siemens usability team.
Assembly is handled by the standard procedure of inserting components and then constraining them through relationships. Most are the same as in other software, with a few additions. For example, Key Points allows me to select radius points and the like, while filtering out faces.
As I reviewed components in the assembly, I tried to determine where the relationships were displayed. I mean how do you tell how the parts are constrained together?
I picked a component group from the browser, and something amazing happened. A pop-up toolbar activated in the lower left corner of the graphics area. It contained a summary of all the relationships affecting the selected component group. If I had to pick one thing that was my favorite Solid Edge feature, this might be it.
Editing the relationships is as simple as picking them, and then making adjustments. Each relationship can be suppressed through a right-click context menu. Their offsets (if any) can be easily modified through the Relationship toolbar, which is invoked when any relationship is picked. When a part is picked, the relationship pop-up appears with top level information. From the pop-up, relationships can be suppressed (via right-click), or an additional toolbar will appear when left click picked.
A quick trip to the Variables Table verifies that the (V253) shown at the end of the relationship name in the toolbar is the name of the variable stored as a Smart Dimension. Each of these is given a different naming convention from other dimensional variables, making it easy to pick them out from the rest.
The ST4 environment was filled with all the standard graphical interface options you’d expect. Here are a few that I thought were worth mentioning.
The View Orientation control dialog appears after picking its icon on the status bar. Once opened, the view in the graphics view window updates dynamically as the cursor passes over the icons. Views can be saved, which appear immediately in the dialog. This provides a fast way to reposition your model in any way you choose, seeing the instant preview without having to commit to the change.
Figure 27: The radial menu in Solid Edge.
ST4 allowed me to type prompts for commands, similar to a command line. This is a little field just above the status bar, and is a nice touch for all the typists out there. The Command Finder field translates commands you have learned from other CAD software. I didn’t use either of these functions, but I suspect I might in the future, as I do quite a bit of command line work in other software.
Solid Edge ST4 employs both standard context menus, as well as a radial menu, illustrated in Figure 27.
A fast right-click produces the standard rectangular context menu, but a slightly longer right-click produces the radial menu. While not contextual, it differs with each environment and holds 16 useful commands; as well, it is customizable. It should also be noted that the inner ring on the menu understands gestures, meaning a click-pull-release motion triggers the command that was passed over.
The install went fairly smoothly, along the way asking for a license file, which I provided. One odd feature was that the install wanted the license file location (which we would naturally store along with the app) before it had created the file structure. I had to put the license file in a temporary location to get through the install. Everything else was smooth.
Siemens' Solid Edge ST4 is a good product. Seriously. There is a lot of power under the hood, and I only got a slight look at it. For a new user, it can seem a bit complex and overwhelming, but then that’s to be expected in any new territory, and especially when some complexity is involved.
I’ll start with the things I did not like, and there were a few. The application felt a bit sluggish for the small number of faces that it was processing. The reaction time pulling a face was just a bit too long, and required a little patience from me.
There were a few occasions when I did not feel quite satisfied with the workflows. These were related to my lack of complete understanding of the action-specific toolbars, and obviously I needed more time to study them. I failed to give much attention to the almighty parametric design capabilities. The Variable table is available, and permits these kinds of relationships to be developed, but I felt that certain solutions could have been more obvious and intuitive.
On the positive side, I liked how ST4 resized the application window to a 70/30 split and allowed the tutorial dialog to fill the right side of the screen. Smooth move. Other features gave me the feeling the product was developed by a well-seasoned team. Also, I’d like to give a nod to the Siemens' team for picking up on the presence of Autodesk Simulation 2012, and installing the toolbar automatically.
I liked synchronous technology, and oddly never felt like the model was out of control. The combination of Smart Dimensions and Face Relationships was easy to pick up and adopt.
I became quite fond of the separated modeling modes (Ordered, Synchronous, and Simplify); the ability to move in and out of the simplified model was sweet. The fact that these changes are stored with the model is beautiful. Not having to ‘design to simplify’ or save a version of the part for a test (only to throw it away later) was a big relief to me. Sadly, I did not learn how to leverage these to an advanced level. Who knows, maybe I’ll get to in ST5.
I found that the ST4 environment delivered a very sound feeling of situational awareness. For example, feature related Smart Dimensions would become visible when a face was pulled to show the associated constraints.
The Live Rules and ST4’s insane ability to determine feature relationships on the fly were unspeakably cool. I found Solid Edge a complex animal. There seemed to be no limit to the new ways I found to manipulate and assemble geometry and components.
We take an in-depth look at Synchronous Technology. Does it work as well in real life as it does in sales demos?
John Evans has 30 years experience in the aerospace industry, including mechanical engineering, design, fabrication, and CNC manufacturing processes. He expanded into MEP and civil engineering 18 years ago. In addition, John is certified AutoCAD Civil 3D and Autodesk Inventor.
Along with providing data management for a civil engineering firm in northwest Florida, John works as a design consultant for Autodesk digital prototyping, and has joined forces with an emerging clean tech developer. He continues to explore the Autodesk design industry on the Design & Motion blog.
John has been a regular contributor for Civil 3D and Inventor articles in AUGIWorld Magazine, and now serves as its manufacturing content editor. He has presented at Autodesk University. He speaks English and Japanese.
You can contact John at email@example.com.
TenLinks uses over 125 expert authors for unprecedented
coverage of CAD, CAM, CAE products and services. Find out more about
Independent Content and