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.