The Solid Edge ST3 Feature Tree

The feature tree in Solid Edge ST3 is made up of three parts. In my series on Synchronous Technology in Solid Edge ST3, I explained the first two parts – Synchronous and Ordered. This post is about the third part called “Simplify”, which basically is used to defeature a model. In this part of the tree you either remove faces, regions, holes or rounds. Its a very simple concept for anyone familiar with history based parametric modeling. But for the benefit of my 2D CAD readers who maybe looking at all this and scratching their heads, I will explain by means of a simple example.

Here is a model of a simple flange that I created using a combination of synchronous and ordered features. The main body of the flange was modeled in synchronous mode, whereas the holes were done in ordered mode.

The feature tree has two parts and looks like this.

Now in order to defeature this part I switch to the Simplify mode. This changes the UI a little and gives me these commands.

I proceed to delete rounds. Solid Edge give me the option to select my rounds by picking on their individual faces or on round features. I choose to select the rounds by feature because I will need to make just two mouse picks, one each for “Round1” and “Round2”. But when I do that and accept, something unusual happens. Take a look at this model.

The rounds on the other three instances in the circular array are still present. I expected all of them to go away. After all I picked a round feature and that feature was patterned. So the software should have automatically selected all the other instances as well. This looks more like a bug to me, or maybe a limitation. Anyways, the feature tree now looks like this.

A third section called “Simplify” has been added and a “Delete Round” feature has been added to it. Since the delete round operation did not remove all the rounds lets use the delete face command to do that. I select all the rounds individually by picking on their faces and delete them.

A “Delete Face” feature gets added to the “Simplify” portion of the tree.

And all the rounds on the part disappear.

So in summary, the feature tree in Solid Edge ST3 begins with the Synchronous part which contains all the synchronous features. Then comes the Ordered part which contains the traditional history based parametric features. And finally we have the Simplify part where synchronous and/or ordered features and even individual faces can be removed to defeature the model.

So as I see it, Solid Edge ST3 can still be considered as a history based modeler, just that its history tree is broken down into three very distinct parts which are calculated in a specific order. I say this because when you are working in Synchronous mode, the Ordered and Simplify features are missing because they have not yet been calculated. When you are working in Ordered mode, the Simplify features are missing for the same reason.

The beauty of splitting the history tree into three parts in this way is that the user gets direct modeling capabilities in a traditional history based parametric modeling environment. It’s brilliant. Hats off to the genius to came up with this idea.

  • Anonymous

    That is a simple example. I wonder what a complicated example would look like? It’s so much easier to simplify models using Direct Modeling – and with KeyCreator you have Facelogic which finds the features and patterns of features for you. No searching through complicated history trees.

    • I guess it would work the same for a complicated part. I picked the rounds by clicking on them in the graphics window, not searching for them in the synchronous or ordered sections of the feature tree. The other advantage is that you can create part families with some of these defeaturing commands supressed or unsuppressed. And there is a whole lot more that I haven’t quite gone through yet. Maybe someone from Siemens PLM can chip in.

      • Darn, asynchronous comments! I was replying at the same time as you, Deelip,

  • ssweeney, you can still use “Direct Modeling” like in KeyCreator along with logic to find the features. There is no searching the history tree.

    What Deelip is showing is a second option that supports the ordered geometry and lets you bounce around the 3 related representations. For example, I could do an FEA analysis of the simplified body while continuing to work with the full design body all in the same part.

  • Anonymous

    oh I see, and if you had say 100 of the same features it would find them all, you wouldn’t have to pick each and every one of them all to defeature them?

  • You have to be careful to not confuse the Simplified representation with Synchronous and Ordered features in the list.

    Simplified is just a visual representation of the model that helps speed graphics in large assemblies and drafts. (No reason to process minute details when they are hidden from view anyway.) It’s a different state of the model like a flat pattern is a different state from a folded sheet metal part. The geometry changes in Simplified are not propagated to the manufactured part.

    To clarify, consider running mass property analysis on the body before the simplified part and then after. Regardless of the state, the mass properties will be equal even though the simplified part has removed rounds, holes, and other geometry. Based on Mark’s comment, SE Simulation may deal with simplified parts a little differently, which is great because it allows pre-processing of my FE model without having to make family of parts. But really, FEA should be done on a different “promoted” body and not the manufactured part or simplified part.

    • Correct. Here I simply concuding the discussion about the feature tree. Your gist of comment is mainly the reason why I made it a point not to add the “Simplify” section in my 11 part series because this has very little to do with the new mixed modeling paradigm of Synchronous Technology.

    • Scott, you can do it either way – with a “promoted” part or do it all in the same file. I agree that for more serious FEA you want to keep your FEA data separate location.

      On the other hand, it can also be nice to drag a face, solve your model, drag a face, solve your model without even leaving the CAD graphics area, let alone switching to another file, going to a different environment or starting another program.

      But like I said, we can work either way with whatever geometry representation you want. You can even mix and match design and simplified bodies for assembly level analysis.

      • Mark, don’t know where your planning is taking SE Simulation (as it’s going to be a few weeks before I get a demo license), all I can say is INTERPART COPY.

        Copy the part geometry as a dumb solid into another part and use the synchronous tools to push/pull the geometry and run another case study. Or use Synchronous PMI to attach parameters to adjust & record for the case studies. That would be my proposed technique until a new way to promote solid bodies is developed. Assembly FEA requires a bit more thought.

        • Actually Scott, tell me where you want me to take it 😉

          Point is – I’m both VERY accessible and VERY customer driven. The more folks email me or send enhancement requests for FEA to GTAC the more data I have for making sure we do the right things. (OK Scott – you already do this. I’m just trying to get more to follow your example).

  • ….

  • Paul Hamilton

    Are all modeling operations, synchronous(direct) or ordered, captured in the feature tree? Are all direct edits captured in the feature tree? Seems like this could get out of control quickly??

    • Paul, synchronous features are added to the Synchronous tree and serve as a “face set” for that feature. Synchronous direct edit modifications are not added to the tree. Ordered features always create a node in the tree.

      • Paul Hamilton

        That makes sense. But if you do make a direct edit to an ordered feature (like the delete face above) you do get a new feature, or is that just in Simplify mode?

        • Since your making a direct edit (DE) using an “Ordered” DE command (Delete Face, Move Face, Rotate Face) in ordered mode, you get a new feature in the tree. However, it is possible to DE faces of the Synchronous body while in the Ordered mode which will not create a new feature.

          • Correct. The ordered side of the feature tree works pretty much like a traditional history based parametric modeling system. The beauty is that while you are in ordered mode, you are free to edit the features on the synchronous side using the steering wheel.

  • Paul Hamilton

    Is there any concept of taking a feature or edit on the synchronous side and bringing it into the ordered side? This would be comparable to the change manager with Inventor Fusion. Or is it a one way trip? I think you mentioned this in part 6.

    • No, there is no such concept. It’s a one way process. Yes, this is close to what Autodesk is trying to achieve with Fusion. Siemens PLM is not going down that path. This also goes to emphasize my earlier point of how different MCAD systems are diverging in their workflows.

  • Alessandro

    Some comments about the way to constrain a model in sync mode (live rules, PMI, etc)? I think it is a very important factor to decide if sync is good for production or not. How does sync performs when the model is big and needs to be fully constrained? Is the model really lighter than a traditional one?

    I guess Sync was created mainly to:

    1) Make it better the inter-operation with step/iges/x_t files
    2) Make it faster the rebuild of the model
    3) Make it easier to understand a model when it passes from a designer to another.

    How do live rules behave about these problems? I’m afraid that the sync mode without the obligation to constrain everything could lead to too weak models.

    • The whole point of Direct Modeling is to have the freedom to do certain things. And that notion is exactly opposite to the rigidity of history based parametric modeling stands. So obviously you are going to have to give up some control to get some freedom.

      • Alessandro

        Mhhh, I not totally agree. Direct Modeling and ST are differents. In ST you have the possibility to drive the model imposing constraining between entities and not by means of history based features. For example, you can order to SE to make two faces to stay parallels and at a distance of 20 mm. It happens that if you push-pull one of the two faces, the other one follows the first one according to the constraint that you imposed between them.
        In my opinion, this a really smart and NEW way to model a part, more relate to the design intent than what it is possible to achieve with a trad. modeling. But it seems that when models are biog and complex, it is easy to create mistakes with conflicting constrains (no direct experience on this, I have just read something around).
        But, in my opinion, the possibility to fully constrain a model is mandatory for a m-cad.

        • Direct Modeling merely signifies that you are picking on a face and moving/rotating it, without having to pick apart a feature tree. It does not mean that that face cannot be constrained like you just described. That’s the part of Direct Modeling that is easily misunderstood by many.

  • Jon

    Has anyone notice how converting a model to synchronous significantly decreases the performance? When I move a complex model from ordered to synchronous, the file size decreases quite a bit, in my example from 55mb to 27mb, closing the model and opening it, spinning it around it moves quite fast just like the original one, however after making a change (in this case moving a hole 3mm one way and 2 mm another) after this the performance drops significantly, even when un-selecting everything. The only way is to close the model and open it again.

  • Jon

    Actually it seems like a bug in solid edge, does it with the original model too… back to ST2 it is I guess until the first service pack is released.