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Solid Edge ST 6 First Looks: Assemblies with Synchronous Technology

By Scott Moyse, September 23, 2013

In my First Look series of Solid Edge ST 6, I looked at the new features for parts, assemblies, and drawings as an expert user of Autodesk Inventor. In this article, I'd like to describe some of the new assembly functions that caught my eye.

Creating Synchronous Geometry from Assembly Part Features

Now that assembly part features can create synchronous geometry, this new feature will be a relief to those users who aren't using multi-body workflows, as well as those who need to insert holes or cut features at the assembly level. Its purpose is to apply features to multiple components simultaneously, therefore ensuring correct alignments.

The first step to ensuring that these assembly features get added to sub-components synchronously is to ensure we have the options set as shown in figure 1. (The dialog box should pop up automatically the first time we use it.)

Figure 1: Assembly feature options set to create synchronous part features

In figure 2, I cut through three parts in a sub-assembly that was applied from the main/parent assembly. I then applied rounds to all the new edges. All of the features were pushed down to the parts automatically, while maintaining their synchronous state.

Figure 2: Cut and rounds applied to assembly, then pushed to parts

Unfortunately, it seems this workflow is not without issues. A number of times I struggled to get features to apply themselves. In what I figure would be the most common use case for this tool (create holes simultaneously through multiple components), this would be a face-to-face feature in most cases. When I selected the From/To extents option for the hole, Solid Edge completed the command without reporting an error; upon inspection, however, I found it hadn't created any hole features (see figure 3). A workaround for this is to use finite extents and then select the components we want the hole to go through.

Figure 3: From-To extents not working for holes

Fortunately, I found that it works perfectly for cuts, and so I successfully modeled the clearance cut detailed in figure 2.

I stumbled across another issue during the Round command, but found an easy work-around; indeed, experienced users probably won't have an issue here: after we apply the inputs, the command stays active so that we can continue to place more rounds. In my wisdom, however, I thought I'd end the value of my round through a newly created PMI dimension. Double-clicking it resulted in an instant crash; the solution is to not take my shortcut. I have no doubt the issue will be ironed out with some maintenance update as the release matures.

Autodesk has some of these features in Inventor in the form of an add-in accessible from the Exchange Apps store, and initially an experimental Autodesk Labs tool. It's better, however, to have the function baked right into the product, integrated with core Solid Edge functionality -- something Autodesk often falls short on with new features.

Editing Large Assemblies: Pathfinder Enhancements

Throughout my Solid Edge ST 6 learning experience, I found it difficult to look at the Pathfinder and immediately know where I am at any given time. (Inventor grays out parent components in the browser and dims inactive components as we drill down through the assembly structure, allowing our eyes to filters out the surrounding view complexity to focus on what matters.)

So I'm glad that Siemens PLM spent some time improving the way in which selection feedback is provided to us in Solid Edge ST 6; I imagine it would have been harder for me in previous releases.

And yet, as time has gone on, I suppose the Siemens PLM approach has sunk in with me. I do like the way in which there is a definite difference between components that are added to the selection set, versus the currently highlighted component (see figure 4).

Figure 4: Highlighting parts in yellow, with selected parts in blue

The other visual feedback feature I appreciate is how the parent is always highlighted in a lighter shade of either yellow or blue; this provides a nice bread crumb trail. I hope that Siemens PLM will add browser dimming in a future release.

Body Support for Simplified Assemblies

Previous releases of Solid Edge supported only faces in simplification of assemblies. I imagine it must have been a dreadful process to go through, although I suppose it gave users greater granular control.

To try out assembly simplification, I decided to simplify all the gearing on the planetary gearbox model I referenced in my earlier First Look write-up (see figure 5). It has a reasonable number of components with a degree of complexity, as well as a number of occurrences of identical assemblies, which meant I could give the Duplicate Body tool a try.

Figure 5: Internals of as-designed gearbox, before simplification

After switching to the Simplify environment (from the Tools tab), I used the new Pathfinder features to establish the sub-assembly for the first planetary gear that I wanted to simplify. I found the Enclosure tool pretty straightforward to use once I had all the component bodies selected. I chose to use Solid Edge ST 6's new Inside Cylinder simplification option, and found it perfect for what I needed it for (see figure 6).

I would like in the future, however, to see window selection supported with this tool, as selecting smaller internal components for inclusion can be difficult without Pathfinder.

Figure 6: Straightforwardly using the reliable Enclosure tool, once selection set is sorted

After the resulting body was created, I was able to make further rough modifications to it. For instance, to add back a degree of detail I applied out the new Subtract Assembly Body tool on a shaft and bearing simplification; it worked flawlessly (see figure 7).

Figure 7: Assembly Subtract Body command at work

With the simplified body just the way I wanted it, I moved to the Duplicate Body tool I'd been itching to use. This tool allows me to create and constrain very quickly copies of the same body, wherever a component of my choosing is located (see figure 8).

Figure 8: Duplicate Body tool, a pleasure to use

That is to say, it doesn't have to be exactly the same; I can select other components on which to use it. Obviously, this makes sense only when the end result of a simplification is so close to the one I just created. In my case, the assembly has three planetary gear assemblies to each set (see figure 9). I see this tool being a hug timesaver for a many users.

Figure 9: Completed simplification of gearbox assembly

I have just one gripe with Solid Edge's simplification environment: compared to Inventor, the resulting geometry may be too simple. Inventor's approach is along the shrink-wrap method; on the other hand, Inventor now has too many simplification tools and so it has become too complex to use.

Nevertheless, I trust that Siemens PLM matures this toolset to include greater geometric intelligence. We users find it necessary to remodel areas of simplified bodies and to make sure the recipient of the model has the interface geometry needed to complete their work.

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About the Author

Scott Moyse is the design manager for SMI Group, a super yacht interiors company in New Zealand. His background is in motorsport engineering and CNC programming. Scott has been using various Autodesk software for 9 years, most recently he has been implementing Vault Pro. More...

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