Synchronous Technology In NX 7.5

I have been fiddling around with NX 7.5 for some time now and am beginning to understand how Siemens PLM has implemented Synchronous Technology in the product. Its a little different from how they have implemented the technology in Solid Edge. When Synchronous Technology first showed up in Solid Edge a couple of years ago, the user had to decide at the start whether he wanted to use the traditional history based parametric modeling method or the direct modeling method to model his part. He couldn’t switch back and forth between the two methods in the same environment. However, in Solid Edge ST3 the user has been given the option to split up the feature tree into two parts, one meant for direct modeling (synchronous) and the other for history based modeling (ordered). So now the user can use both modeling methods on different parts of the model. If you are interested in knowing how this is done and what are the implications of doing do you can read my 11 part series titled “Synchronous Technology In Solid Edge ST3“.

Siemens PLM has implemented Synchronous Technology in NX in such a way that the user can switch modeling methods in the same environment with just a mouse click.

So the obvious question is “what happens to the feature tree after I switch from history mode to history-free mode?”. Well, the features are lost and the model is “flattened” to a dumb solid. This is the confirmation dialog box that pops up before you make the switch.

Say I create a box in history mode by extruding a rectangle. At that point if I switch to history free-mode the extrusion feature is lost and I end up with a dumb solid in the feature tree as can be seen in the following image.

While in history-free mode, features can be added to the model using traditional methods employing sketches or by using push pull type direct modeling techniques. But there is a difference here. In Solid Edge, if I add a feature in synchronous mode, something called synchronous features are added to the synchronous side of the PathFinder (the Solid Edge feature tree). For an explanation of synchronous features see part 2 of my ST3 series. But in NX, when I add a feature in history-free mode, a new feature is not always added to the Part Navigator (the NX feature tree) . This needs a little explanation. For example, in Solid Edge if I create an extrude feature by extruding a sketch a “Protrusion” feature is added to the PathFinder on the synchronous side of the tree. If I do the same thing in NX, no new feature is added. The faces that makes up the extrusion feature are added to the dumb solid and that’s the end of it. But if I add features like fillets, chamfers or holes, new features are added below the dumb solid in the Part Navigator.

From the image above you will notice that apart from a fillet, a chamfer and a hole I also added a shell feature. But it is nowhere to be seen in the Part Navigator. This is what I mean by only some features are added to the feature tree in history-free mode. I’m still trying to figure out why. If you know the reason please leave a comment.

The next question is “what happens to the features added in the history-free mode after you switch back to history mode?” Well, they get lost as well. This confirmation dialog box pops up before you make the switch.

As expected, all the features added in history-free mode are “dissolved” into the dumb solid and any new features added in history mode grow from the dumb solid.

As you can see in the image above, after switching to history mode, I added another fillet, chamfer and hole and they were added to the feature tree. Now here is something interesting. At this point if I switch back to history-free mode again, these new features that I just added should be dissolved in to the dumb solid, right? Wrong. Take a look at the image below.

After I switch to history-free mode the feature tree contains a dumb solid and three features listed under it: the fillet, the chamfer and the hole. They didn’t get dissolved into the dumb solid. I can even go ahead and edit their parameters and the model rebuilds itself. I went ahead and changed the fillet radius, chamfer distance and changed the hole from a simple hole to a tapered hole. Take a look at the image below.

So did NX lie to me? It does looks that way. NX told me that I would not be able to edit the parameters of features when I switched from history to history-free mode. But as you can see I just did exactly that. So what is going on here? Actually I’m trying to wrap my head around this myself. Here is what I think. Remember what I told you earlier about only a few features being added to the feature tree in history-free mode? I think what just happened is related to that in some way. NX appears to understand only some features in history-free mode or something like that.

Stay with me for a while. Let’s undo and revert back to the point after I created the three features in history mode and just before I switched to history-free mode. At this point if I add a fourth extrusion feature and then switch to history-free mode, the extrusion feature does not show up in the feature tree. But the other three features (fillet, chamfer and hole) do. So basically, if I had modeled a part in history mode using a bunch of extrusion features only and then switched to history-free mode, I would end up with a dumb solid and no features below it. In that case NX would have been telling me the truth. So to be on the safe side, NX always tells me that I will not be able to edit the parameters of features if I switch from history to history-free mode.

From all this back and forth we can conclude that only some features survive a switch from history to history-free mode and no features survive when switching back from history-free to history mode. Contrast this with how Synchronous Technology is implemented in Solid Edge. Depending upon what you are trying to do with Synchronous Technology you may find the implementation in Solid Edge ST3 better than that in NX 7.5. Why? Because in Solid Edge if you split the feature tree properly you can switch between ordered (history) and synchronous (history-free) modes over and over again without losing the features in the ordered side of the feature tree. In NX you will lose some features when you go one way and all of the features when go back the other way. So if you are going to go back and forth between the two modes, you will pretty much end up with a dumb solid at the end of it. Whereas in Solid Edge if you know what you are doing you can end up with a feature tree nicely split up into two parts with features on both sides.

If you have used Synchronous Technology in Solid Edge ST3 and NX 7.5 I would love to hear what you think. Please leave a comment.

Disclosure: SYCODE is a Siemens PLM partner. But our partnership covers only Solid Edge, not NX. At least not yet. Siemens PLM provided me evaluation licenses of NX for Windows and Mac.

  • Ken

    Deelip, both products have true Synchronous features. These are features with attributes, internal sketches or some other construct that controls and preserves the behavior of that feature (holes, rounds). I think the big difference is that in SE, SE captures those items that are not really Synchronous features (protrudes/cuts) as “face sets” and calls them features in the tree. It appears that NX does not.

  • Paul Hamilton

    Great article Deelip. This aspect of having some features survive when going from history to history-free is nothing to significant. If I take a model from Elements/Pro (or any other geometry creating tool) to Elements/Direct, chamfers and rounds also survive (or at least can be recognized). Although we don’t list them as features in the structure browser, they are fully editable either with dimensions or tug and pull. Good direct modeling must be able to handle rounds as rounds and chamfers as chamfers (and so on) – regardless of where or how the feature was created.


  • Great article, but you missed to explain the part that you could used all the Synchronous tools in the history mode to, whit out changing to the history free modeling.
    Synchronous tools also have the ability to be modify in a history tree (as features) I think this other differences between NX and solid edge.

    • True, the menu items in “Insert -> Synchronous Modeling” sub menu are enabled and can be used while in history mode. But that is not direct modeling. For example, if I use “Insert -> Synchronous Modeling -> Detail Feature -> Resize Blend” to resize a blend in history mode a new “Resize Blend” feature is added to the feature tree. The existing blend is not resized. If I do the same thing in history free mode, the existing blend is resized, which is the essence of direct modeling.

      In history mode, these so called synchronous tools merely add new features to the feature tree. That has been happening for years now in a number of MCAD products. This is nothing new.

  • Garrett Koch

    I must be missing something in CAD methodologies of today.

    It seemed to me that the purpose of ST was two-fold: 1) you could “gracefully” edit non-parametric models (dumb solids) and begin to accumulate parameters to capture the design intent and 2) you could work in more of a “bushy tree” instead of the traditional single-trunked tree structure of NX.

    In the position I’m currently applied, I am supporting a migration from Ideas to NX and it is already clear that the Ideas users are uncomfortable with the lengthy, serial dependancies of NX features built “onto” other features. I get that. But it also seems to be a case of the users not having a clear and complete understanding of feature editing in NX. It can be intense.

    Then again, NX has always been designed to ALLOW users to capture design intent with intended and expected associativity. Then again, they offered multiple Primitives too if you really wanted to cut the tree into firewood!

    But what is really puzzling me here is switching back and forth between history modes. Huh? Why are you doing that? What possible benefit could there be other than to investigate the software, meaning… see if you can break it.

    – Garrett

    • The Ideas to NX migration situation you describes is itself an excellent example where you would want to switch modes. The whole point of direct modeling is to be free from the history when you don’t want it and have it when you want it.

      Suppose you create a model using history and if someone else (or yourself after a while) go to edit it to effect a design change, you should be able to simply push and pull faces to make that change happen and not have to mess with the feature tree. That’s one of the times you would want to switch modeling modes. Conversely if you started with a history-free mode and you wish to grow features using history mode for some reason, you should be able to do that as well. To do so you will need to switch modes again. In an ideal world, features created in both modes should be maintained when switching from one mode to another. That’s what Autodesk is trying to do with Fusion. Are they there yet? No.

      • Tomas

        In my perspective you have not played enough with it in NX to state this,
        I do not see the purpose to switch off ( kill ) the feature tree just to be able to push and pull, adding the ST features in History mode doesn’t touch the feature tree since they are added as “changes” to the end of the tree. – It’s more like writing revision notes on a drawing, ” rev3:changed the size of x, moved rib y .. mm, deleted hole z. etc” . If the total model history ( regular features + ST features) makes a total mess in the end, one can kill the history then when one’s finished.

  • Frank

    Solid Edge is:

    ST History Free
    ST History free with ADDED history
    Ordered (history) mode only.

    NX is:

    ST History Free
    History Mode with or without added ST Tools, it doesn’t matter.

    In NX there is no good reason for switching back and forth between the two modes.
    Both CAD systems have very good advantages with ST.

  • Dennis

    Hey if your new to Nx I would check out this guys blog. I don’t personally use NX, but have watched his Rhino stuff and it’s well put together.

  • Alberto Savelli

    I guess NX keeps only fillets, chamfers and holes in the history-free mode for two reasons:
    1) These features are more easily treated as feature when recomputing the model. For example for direct modeling is very difficult to manage fillet surfaces. It is much easier to recognize them as fillet surfaces and re-apply it.
    2) The user intent was very clear when he created features like fillets and holes. While when he uses protrusion, draft, etc maybe he is just using these ones to get a desired geometry, that could be obtained also in two or more other different ways.