Commenters have asked some great questions about Synch Tech. I’ll try to answer them as best I can.
…parametrics with no history is more of a 2D concept…
Yeah, kind of, or at least that’s one place I’m familiar with the concept. You can have a sketch which is parametric, and within the sketch there is no concern about history. Of course sketching is substantially different from solving a b-rep model. If you have multiple sketches, you introduce history effects. If you make a single 3D sketch, you can have the whole thing without history.
I’ll be interested to see the ST review and how this would work for consumer product design and how it compares to the above process.
Well, right now, ST doesn’t work well with consumer product type stuff. You can create lofts and surfaces and shapes, but you can’t edit them. The editing prowess of ST is limited to prismatic shapes.
It seems that ST is a middle ground between direct modeling and parametric feature modeling. It has strengths and weaknesses of both. I suspect that ST-style model edits could theoretically be captured as parametric features
Yeah, I think capturing the model edits as history based features is what happens in SolidWorks right now with the Move Face feature. This is the part that some SW gurus are calling bad practice. It really does chew up rebuild times, and puts some model faces in double jeopardy for where you go to make changes – to the original parametric feature that created the face or the direct editing feature that moved it.
I think the real question should be whether the benefits of capturing design intent, feature dependencies, etc. in an automated way is worth the baggage that comes with it.
Yes, I think that’s exactly the question.
How does this work in a top-down environment? Can the ST model automatically detect relationships to layout sketches, or other parts in an assembly?
In top down, you can assign relations between parts, and even edit more than one part at a time, if you want to make the same edit to multiple parts. I’m not sure the concept of layout sketches exists in ST assemblies. I haven’t delved into that yet.
In the case of what we’re seeing with ST, is there some form that allows for configurations?
I don’t believe ST has an equivalent for configurations, but I don’t see why it couldn’t. I don’t believe the concept precludes the use of configs for size variations or even variations with removed faces. Design tables don’t seem to be out of the question.
Something that interests me is the freedom NOT to rebuild the part in all its glory so often with ST.
Part of what I’m possibly not communicating well here is that everything happens in real time. You can drag faces and they move NOW. The concept of rebuild waits is nearly non-existent. In assemblies when editing multiple parts, you may see some hesitation, but changes are frighteningly immediate.
1.) What impact does ST editing have on existing drawings that were created from a previously history based model?
2.) What types of geometry are not supported?
3.) What happens to existing assembly mates if ST editing is used on a previously history based model?
4.) Is the user warned about external relations that will be negatively impacted?
1) I made a drawing of a traditional SE part, converted it to ST, went back and updated the view on the drawing, and it updated correctly, changing the correct dimensions.
2) Anything spline based can be created, but cannot be edited.
3) I’m going to guess that if the drawings update correctly, so will assembly.
4) Not sure how to answer this question. External relations are almost not needed. I don’t know how the “inserted part” type relation is handled, because I can’t see how to create it. I’ve said earlier that some of the multibody options seem limited. Might just be I haven’t found those tools yet. You can split existing parts, and make multiple bodies on the fly, but not sure about inserting another part as a new body. Maybe one of the other guys can lend me a hand with this one.
When you do convert from traditional to synchronous part, you do get a warning that says that you can’t go back, and that you ought to make a backup copy.
Given your recent comments about 3D CAD software being “too automated”, has ST and “Live Rules” prevented you from making edits that follow your intent?
Oh, yes. Fillets are the big culprits. But then in history-based systems, you know how much energy you put into workarounds for working against “design intent”. I’m still an ST noob. I know what a tyrant SW or history in general is.
On a simpler note, what would happen if this part had drafted faces for casting or injection molding? Would ST be able to make the same modifications you demonstrated?
Yeah, see the part shown below, which has draft and rounds.
In a similar vein, how would fillets impact the ST editing process?
In controlled situations, ST works well with fillets (they call them “rounds”). There is a difference between native rounds and imported rounds. Native rounds have the opportunity to become “procedural features”, which are treated in a special way. If you select to fillet between faces, new edges created by those faces can also update with new fillets, much like a history based system except better because it can do it live as you drag a face. So fillets have some ups and some downs compared against history based systems.
Is there any way to edit 3D spline based surfaces? At all?
You can move (translate/rotate) surfaces, but you cannot change the shape of a spline based face.
What about creating prismatic, or more importantly, slightly non-prismatic shapes and other more complex geometry. Not editing it later, but creating from nothing?
Yes, the tools to create complex shapes and surfacing commands are all there. Ironically, once they are created, you cannot edit them.
When I create a part I typically constrain it in the sketch. You’re saying not to constrain the sketch, but to constrain the geometry afterwards. Either way sounds like six of one and half a dozen of the other.
Once the sketch is used to create something, it is disassociated from the solid geometry. The sketch is typically kept, but you can delete it without losing any solids.
Also you mention “you can see the sides of the rib that are tangent to the top cylinder change when the outer cylinder gets bigger, so it is maintaining tangency, which is done in the Live Rules panel in the upper left.”
So this means that the software is making assumptions based on pre-existing geometry, and changing based on that? Wouldn’t it be far better for ME to decide what these rules are instead of the software making assumptions. You complain time and and time out that you don’t want the software to make the assumptions for you, you want to define these parameters yourself. I strongly agree. Is the software robust enough to have tangency constraints with face-face? Can I truely have a full range of constraints at the model (and not sketch) level? I think this would be a requirement for me before such technology would be an “improvement” over constraining sketches. I don’t need more software that makes assumptions for me.
Yeah, this is the heart of the question. The software makes guesses, and you can either disable or add to the guesses. This part of it actually works pretty well. The part of it that doesn’t work well is a bit of feedback so the user can see what relations are applied more immediately, or more visually. You can disable the assumed relations through the Live Rules panel. You can also use Selection Manager to manually establish rules. You can completely disable Live Rules so that you are always manually in charge. I think over time, and depending on the geometry you find yourself working with, you would learn to use the Live Rules automation, and disable it selectively.
2. Enhance instant 3d such that it has an option to override dimensions in features and sketches.
This already exists in SW. Go to Tools, Sketch Settings, Override Dims On Drag. For the record, I dislike most of the functionality of Instant3D. I never actually use it. I don’t think I’ve seen anyone actually use it.
I’d be interested in someone demoing ST with a really complex model with some prismatic features and some curvy stuff.
Well, I’d be interested in seeing how it handles a large complex part as well. The curvy demo would be short. Not much to see there. I’m guessing even some twisted ruled surfaces would be out of the question.
Here is one of the simpler parts I’ve done recently. Few lofts, lots of extrudes. 109 features, but it starts off with a base part where all of the externals were created for several housing pieces. I want to move a boss. Something that is concievably within the range of SEwST.
On a fast CAD box, the changes happen almost instantaneously, but the party doesn’t last long. I can only move the boss so far, and it fails. If I try to pull it straight, rather than off to one side, it still only moves so far, apparently due to the fillets. You could de-fillet it and then edit more quickly.
Notice that it knew enough to move the hole with the boss, and also extended some of the fillets.
How do you manipulate something that you can’t define with a dimension?
If it’s a spline, you can’t edit it. If it’s not a spline, you can define it with a dimension.