Siemen’s Solid Edge ST4 is a revolutionary mid-range engineering CAD solution that could be better understood by the engineering industry. What makes it unique is its synchronous technology, giving the user incredible power over 3D components in both the part and assembly environments.
Solid Edge uses synchronous technology to distinguish it among mid-range modelers.
While models can be approached from a history-based and/or a direct-modeled approach, synchronous technology is neither of these. It is a new way of creating and editing parts and assemblies, and is based on a way of thinking in which many limitations of history and direct modeling have been written out of the software.
Recently, I wrote about getting to know Siemens’ Solid Edge ST4 from the perspective of a new user, and previewed the product’s highlights. (See “Solid Edge ST4 – Ease-of-Use Review.”) I decided to look at synchronous technology again and dive deeper into its functionality by developing a 3D model.
In part 1 of this review, I discuss the following aspects of synchronous technology and 3D modeling:
- Smart dimensions and PMI
- Relationships, live rules, and face relate
- Triad tool
- Part modeling
In part 2, I return for a look at documentation:
- Explode-Render-Animate environment
Overall, the process used by Solid Edge to develop a component assembly is quite similar to that of other modeling environments: (a) sketch out some base geometry, (b) build up the part, (c) assemble parts together, and then (d) document the result. The difference in Solid Edge ST4 is how you get from point ‘a’ to point ‘d’.
Smart Dimensions offers a unique method of constraining geometric features. It can be applied to sketches or directly to the features of 3D models. When a sketch is constrained using Smart Dimensions, the dimensions are transferred automatically to the 3D model as each feature is developed.
Furthermore, these dimensions can be locked to enforce dimensional constraints, and unlocked to relax them, as needed. This gives users positive control in being able to lock down important features while allowing Live Rules to control other features. (More on Live Rules later.) The sole drawback to this level of wonderful control is that it can be difficult to remember which dimensions are locked while working in the assembly environment. When Live Rules experiences a feature limitation, it reports it but in a manner I found somewhat generic. This inconvenience is minor, nevertheless when a locked dimension is encountered I would like to see more specific reporting in the assembly. (Siemens tells me that this limitation is addressed in this month’s release of Solid Edge ST5, which shows dimensions related to moving geometry and allows users to relax them dimension on-the-fly.)
Tip: Try to lock only dimensions that are critical to the design, such as datum surface offsets and key hole locations. Leave all non-critical dimensions unlocked so that they can adjust fluidly in the assembly environment, should movement be needed.
Dimensions are color-coded to help users understand their status, such as reference, locked, unlocked, or disconnected. These are further catalogued in the browser with status icons, making it easier to assess the current situation.
Dimensions are managed as variables, and so populate the Variable Table. From here, equations are built to relate one dimension to another through formulas. This is accomplished through the Copy Link function, which copies absolute file paths to the file from which the variable is resolved. Links provide a unique manner to gather information, and so can be resolved from any navigable location.
Once a link is established, it is cataloged in the browser for easier access to the link as well as to its position in the Variable Table.
PMI tab in Solid Edge’s ribbon
PMI [product and manufacturing information] can be applied to 3D part models and catalogued in the browser as dimensions and annotations. These permit users to specify much detail about the part right inside the 3D modeling space, including Smart Dimensions, datum references, numerous tolerance options, welding instructions, and almost every feature symbol typically used by industry.
The PMI objects are accessible by directly picking the object or through the browser. They can be turned off globally or individually, as desired.
Annotations are created and edited through respective builder interfaces that allow users to assemble customizable annotations, such as datum frames. Users save them in convenient fields that can be applied to labels as needed.
In addition to tolerancing, PMI dimensions can carry alternate units and a host of other formatting options that make the system quite robust.
There are numerous advantages to applying PMI in the 3D model space:
- Enhanced ability to visualize datum features in 3D
- Better understanding of critical feature dimensions and the role they play in the design
- Easier hand-off to other users, as dimensions are not hidden in sketches
- Viewing of PMI by downstream team members using the Solid Edge viewer, thus allowing engineering markup and manufacturing review
- Importing of PMI dimensions and annotations into drawing views, bringing with them all respective tolerances and annotations
- Efficiency of applying dimensions once only
Relationships are a well-built feature that dictates to Solid Edge how component surfaces should co-exist with one another in assemblies. For example, a shaft is to remain aligned to a hole and so forth.
Relationships can be suppressed and unsuppressed with the same logic surrounding the locking and unlocking of dimensions.
Selecting a component initiates a pop-up list of all assembly relationships present for the component. This is one of my most favorite functions in the Solid Edge Assembly environment, and I’ll talk more on this topic during the section on assemblies in part 2, to follow.
A point worthwhile mentioning is that the Inter-Part Relationship tool allows users to add permanent relationships in the part modeling environment. Solid Edge develops a dynamic Inter-part Copy, and from this a synchronous face-face relationship is created for the part.
Live Rules is an interesting creature, and is the most significant portion of synchronous technology. There is nothing like it in any MCAD system from any other software vendor. Live Rules scans parts and assemblies looking for geometric relationships to maintain — regardless of the origin of the part file. For instance, I can import into Solid Edge a solid from another CAD system, and Live Rules treats its features in the same manner as a native part. This process is quite smooth and Solid Edge performs this function automatically, with no apparent performance lag.
The Live Rules interface panel pops up with controls that allow users to perform the following tasks:
- See, understand, and maintain surface relationships within 3D models
- Adjust relationships to be maintained, or not
- Provides on-the-fly control
- Determine where maintained relationships and design intentions conflict
Each button on the Live Rules panel is color coded to help users understand when relationships exists, if they are in conflict, and whether Solid Edge is maintaining the relationships or not. I found it is the ultimate situational awareness tool, and quickly becomes an integral part of my modeling process.
Tip: On more than one occasion I used the Live Ruled dialog simply to determine how a particular surface was related to the rest of the part, even though I didn’t intend to make an alteration.
Face Relate is the most addictive tool ever. The buttons on the Face Relate panel tells Solid Edge which surface relationships to apply, right now — without users needing to navigate through ordered history and sketches. Just pick the relate tool desired, such as concentric, and then identify the two surfaces that you wish to relate. It’s just that simple.
This tool panel can be used for both part modeling and in assembly environments without reservation. If an alignment slot in one part needs to be adjusted to a mating surface in another part, simply apply a quick mate relate. Wonderful!!!
- In the part environment, Face Relates becomes a permanently embedded characteristic, stored in the browser where it can be suppressed as needed.
- In the assembly environment, Face Relates is a temporary edit, leaving no trace or embedded constraint, which users should find to be a very good decision on the part of the Solid Edge development team. Once a geometric relationship is created, Live Rules continues to maintain the relationship without further instruction.
I will say, however, that an option to embed it on-the-fly, like a checkbox, would be a nice addition here. In addition, I would like some offset control over Face Relates to assembly component geometry, especially where planned gaps are modeled in; it took too many steps for me to accomplish this. (Siemens PLM agrees to the point that they plan to support offsets in Solid Edge ST6.)
The triad tool is a well thought out user interface gadget that allows users to directly affect the translation and rotation of part features and assembly components. It is employed everywhere in Solid Edge, and is easy to use. The triad acts as the base point for adjustments, and as well directs the alignment. When an alternate orientation is required for a move or rotation, the triad can be moved to the other feature location, where it automatically snaps to feature edges, faces, and so on.
All six DOFs [degrees of freedom] can be accessed through the triad. It is as logical in operation as it could possibly be.
Once an edit has been initiated, the triad disappears and is replaced with a field in which users may enter a specific value, or continue to drag to complete the edit.
I want to start off here talking about part modeling by pointing out features in Solid Edge that differentiate it from many similar competitors. In Solid Edge, each component can contain the following separate environments:
- Ordered – features are built in a history setting, each dependent on the previously added feature
- Synchronous – features are dissolved into the whole, in which subsequent alterations are not dependent upon the order of previous features; faces are maintained by Live Rules
- Simplified – simplifications are performed and subsequently stored inside the part for analysis and for simplified assemblies
Ordered and Synchronous environments work together to develop the final product that you desire. The only stipulation in Solid Edge ST 4 is that synchronous features must be generated prior to the ordered ones. Without this limitation, ordered features would not have a stable basis on which to be developed. Even so, radical changes made to synchronous features after placing ordered features can have adverse consequences. (Siemens PLM agrees with my point, but notes that this action is no different from making similar radical changes to the base feature of purely ordered models. Any time the foundation of an ordered model changes, there is some risk of “adverse consequences”.)
I found it easy to constrain a sketch and get moving. In most cases, I’d rough-sketch the geometry I needed, and then fully constrain the part features after creating protrusions and cuts. I accomplished this using Face Relate and Smart Dimensions. The reason for avoiding too much detail in the sketch is that once the protrusion is developed, the sketch is tossed into a used sketch bin and so has no further purpose for the part. All control is passed to the 3D model through the triad, Smart Dimensions, Live Rules, and embedded relationships. In any case, more time spent in the original sketch becomes somewhat unproductive, and this becomes evident while editing models in the context of the synchronous assembly. (Siemens PLM adds that some relationships and dimensions do migrate from the sketch onto the model automatically, and so it isn’t necessarily as unproductive as it may sound.)
There was an instance where it became necessary for me to fully constrain and to dimension the part features in a sketch. This was due to the part having continuous curvature and intricate features that would be difficult to protect during push-pull style editing. As such, all the effort I put into the sketch transferred to the part, including all smart dimensions. There is no limit to the features available in the sketch environment, and users can easily accomplish any standard 2D sketch workflow.
Creating model protrusions is as simple as it could be: create a closed profile (which is highlighted slightly in the sketch), and pull the protrusion or, conversely, push a cutout. I’ll reiterate how nicely Solid Edge extracts (and detects) profiles from any sketch and model geometry. It there is a closed shape implied by anything, Solid Edge will create the profile. Probably the fastest I’ve ever experienced.
I’d like to point out the nice editing environment invoked from the assembly. A beautiful balance of dimmed components and highlighted features makes complex editing with component references a pleasure. A great feature is how easy it is during part editing to access and turn off components in the assembly right from the browser. This functionality is smooth and convenient.
The visual balance and component accessibility play a key role in making Solid Edge a contender in the mid-ranged CAD market. Furthermore, these features jump start component design permitting new model faces to be quickly sized to other components on-the-fly. Just Sketch – Protrude – Face Relate; that simple.
The Face Relate tool is unbelievably addictive, and I have found that I use it as much as the triad. When faces with the option to project geometry to a sketch, or rough it and relate the 3D faces, I usually turn to the latter.
Another example of this is roughing faces for a rectangular recess that needs to remain parallel to other surfaces. It is just too easy to use the Face Relate tool to align the surfaces, and slap a Smart Dimension between the two in order to maintain the desired separation.
The Ground tool (on the Face Relate panel) is valuable while editing in the Synchronous domain, allowing faces to be held in space, forcing any remaining DOF into faces where adjustments were intended. Like all the other part file embedded relationships, it can be removed at any time.
Working in the part environment usually invokes Live Rules. Anything that affects the geometry invokes an evaluation. I found it to be a constant reference throughout the design process, and came to rely on it. I didn’t take the time to save and restore different Live Rules scenarios, however I think that would be the next level in my learning process.During this review I discovered a few important points related to dimension editing. The decision of which face the dimension would shift is delineated by highlighted arrows and highlighted faces. Picking the opposing arrow in the dimension or edit dialog would produce the opposite effect: Solid Edge would preview the change by reversing the arrows and highlighting the opposing face. I also noted the usability associated with selecting dimensions (or for that matter, any feature) to edit. In most cases, as I moved from one dimension to another, the latter edit is closed, and the new one is activated. No escape sequence is required, making very fast edits possible.
There were times where I would suspend Live Rules to force a change, but then had to chase down and apply the missing relationships that were temporarily ignored. This is the downside of using suspend. (Siemens PLM clarifies that user-applied relationships are not suspended, only found relationships. They add that Solid Edge ST6 allows more granular control over the solution, which will help me get the result I desire.)
PMI Model Views
PMI Model Views are a bit confusing, as you see later in the drawing section (see part 2). They are created through the PMI tab, using tools on the View panel: Section and View. With these, pre-defined views can be created for use in drawing views, which are a key component in the importation of the PMI information. One important point to note is that this functionality is only activated when the part file is opened directly, without the context of the assembly — which I only learned after no small amount of kicking and screaming.
The assembly environment is one where everything comes together, including synchronous technology. The more I worked in the space, the more features I found.
Components can be created in the assembly context (which is how most of this review was performed) or by dragging them from the Parts Library. The Parts Library displays a list of components that can be inserted from the default workspace location, as well as navigation functions to view other areas where components are stored.
Additionally, the Standard Parts button is available to pull (selected) standard based fasteners and hardware from. This is installed from the installation DVD, and resides in a managed SQL database.
The automated relationship tool for inserted components was nice, once I learned how it functioned: the part hovers in space awaiting relationship inputs. It allows users to add more relationships to refine the component placement. The user interface and visual feedback are great. I didn’t use it as much as I would have liked, as most of my parts were created simply in the assembly environment on the fly.
As parts were developed it was easier to avoid specific diameters and lengths, and instead concentrate on the shapes in the part file.
Alignment pins that I created were simply three concentric cylinders, with equal diameters shared between the two outer faces. Little consideration was given to the dimensions of the pin. The critical parts were sized as needed, and the pin was placed; afterwards, its faces were related to the final size in the assembly. Thereafter, if feature’s size or position needs to be adjusted, the pin simply follows suit. Provided you don’t go overboard, this is a sweet deal.
Eventually I worked to a point where I had to make numerous passes at very small recesses that were partially concentric to the pin. These changes were likely making changes the pin’s position, which would cascade and alter related mating surfaces in other components within the assembly. Rather than fight this, I simply locked the pin in the assembly, which in turn locked the mating surfaces’ x-y translation. Additionally, I locked the dimensions governing that pin’s diameters, which further limited the nature of the design. However, the lengths were constantly free, governed by the assembly components as needed (if the assembly grows in width, the pins automatically adapt). Solid Edge can be as free or limited as you like.
I was looking for ‘Select All Occurrences’ or something similar, and so became frustrated when I could not find it. However Solid Edge had me covered: I selected a component and then changed its appearance. Once I completed the action, Solid Edge alerted me that there were multiple occurrences of the component, and asked if I wanted all of them to be treated the same. Nice save, Solid Edge.
Assembly Features is a good way to place fastener holes, permitting any number of components to be affected by the hole feature. These are driven by an assembly sketch and, like any other hole feature, are part of the Ordered domain. The sketch is easy to modify: to reposition the feature, drag the base sketch geometry along the sketch plane. I should note that sketches in the Ordered domain do not dissolve (as with the Synchronous domain), but remain active, thereby allowing future revisions by way of sketch edits.
Another situational awareness feature offered by Solid Edge occurs when dealing with assembly relationships. As the user hovers over a feature, the feature is highlighted and a tool-tip style notification activates next to the cursor, reporting the feature along with the component to which it belongs. When you have pins or shafts with multiple concentric cylinders, some of which overlap with mating components, it can be almost impossible to understand which face is being related. This tool-tip saves the day.
The component and feature tooltip activated while hovering
A right-click menu is available to select alternate faces, if the one selected is not the one desired. A tiny glyph appears next to the cursor when additional component faces are available.
Once the basic components were formed and the assembly began to take shape, I edited relationships to fulfill some intricacies. The first step was to add clearances for movements and a layer of oil. The easiest thing to do was to affect the mate relationships of a blade component: I simply picked the blade, and all pertinent relationships appeared in that great pop-up. From here, it was easy to see all the blade’s relationships, and then edit the ones I needed. After I applied the 0.05 mm gaps, Inter-Part Relationships caused the pins to adapt automatically.
Precise Mating of Moving Components
At this point I needed to create and tune the blade locking recesses. For alignment, I added an angular relationship with the datum surface of the mating part, and then dialed the blade from the open to the closed position. The stop pin locked at the desired location. Cutouts were developed in the part environment, and then related to the pin to establish the precise sizes and locations. Once the position was set, the part relationships to the pin were suppressed, allowing the blade to move without warping the mated cutout. After the blade was rotated, the process was repeated. Very smooth.
Solid Edge offers an Engineering Reference section, permitting numerous important components such as cams, gears, and shafts to be inserted into your design and then modified.
In part 2, I tell you about using the ERA (explode render animate) environment, and working with drawings.
This article was published at CADDigest, on July 20, 2012.