More thoughts on Synchronous Technology
The Fading Buzz
Well, the buzz has died down. The party has passed. Now we will see if Synchronous Technology is really going to turn the history-based CAD world on its ear. The pundits are nearly unanimous in saying that it is indeed revolutionary, and that it is going to make huge changes in the directions of all the current history-based CAD products in the not so distant future. But do people who will wind up using the software agree?
Disclosure
I have to make a couple of things clear before I go on. Siemens paid for a trip to Huntsville, Alabama with an overnight there. I spent the night before my meeting with them at Ricky Jordan’s SW user group. At the Siemens offices I met with several executives, technical and marketing types, and others. They gave me a demo and then some hands on training. I got to ask all the questions I wanted to ask. They have given me a copy of the software to use while exploring the possibility of doing some writing projects. In the end, the only writing that has come of it has been whatever you have read here at this blog and a two-part article for Desktop Engineering written months ago, which has yet to be published.
The folks at Siemens are bright, and they believe in what they are doing. They were excited to get an opportunity to put the software in front of people who both write blogs and use software. I believe they also approached other SolidWorks-using bloggers (or blogging SolidWorks users?) but I was the only one who accepted. I’m an independent and can be more flexible with my time than other folks who work for the man. They were courteous and curious, but kept me at arms length. They knew of my love-hate relationship with SolidWorks, and weren’t looking to fan the flames. At the same time they didn’t want to have any ire directed at them. I think they invited me because I was the one SolidWorks blogger who showed the most interest in Synchronous Technology, and I was at least trying to understand it.
Target Audience
Solid Edge with Synchronous Technology is aimed at people who think that history-based modeling is too difficult or time consuming. They want to create a market for CAD non-specialists. The Solid Edge people clearly believe that this brand of direct modeling is going to not just be competitive with history-based systems, but completely replace it. SEwST is somewhat different because it includes regular Solid Edge, along with SE’s assembly and drawing tools, and sells for the same price as SolidWorks. On the other hand, what’s new about SEwST is most similar to Spaceclaim, and in ways also related to Sketchup Pro, Key Creator, CoCreate and Iron CAD. While details of it are arguably new, I don’t believe you can make a serious case for SEwST being “revolutionary”. The functionality that goes to make it up is already found in other places. I’m not an expert in these other softwares, and I haven’t used them (aside from a short stint on CoCreate many years ago), but I have tried to keep up with the writings of people who have used them.
Available Sources
In addition to actually using the software, I have gone to a couple of sources to read about Synchronous Technology. There is of course the Solid DNA website, which takes the fanboy approach, which I take to mean claiming its just better without giving real concrete reasons. I have a hard time with this approach. There is of course the Synchronous Technology website, which I take to be a corporate blog because of its lack of objectivity. Probably the person who makes the best case for the concept of Synch Tech is Paul Hamilton, even though he is associated with CoCreate. I’ve even read a little Al Dean, Roopinder Tara and Evan Yares. Paul is an obvious cheer leader because he is employed by the industry, but what he writes is valuable if you are trying to understand what’s going on, even if he is writing primarily in favor of a different product. You have to filter out the unbridled optimism from what he says. The other press/pundit types are very enthusiastic, and while they have each actually used the software, I think it has been a long time since any of them directly used CAD to make a living. Their enthusiasm seems unexplainable to me. At least that’s the way I’ll leave it.
Eng-tips is another place you might go to read about user reactions to Synch Tech. I’ve been booted out of eng-tips a few times now, usually for doing what someone considered “advertising”, which turned out to be just stumping non-commercial sources of information. Really odd thing to do for a site that is plastered with advertising and is right up in your face with their sign in. Eng-tips has always seemed to me to be a place that enforces a smiley face, where everyone takes a hit of prozac before posting. This commentary is relevant because of the unusually negative tone eng-tips users display when talking about Synch Tech. Anyway, most of what you read on eng-tips is not favorable to Synch Tech, and it is all from the end user point of view. They seem primarily confused, then betrayed, even bewildered. Sometimes the information they give out is incorrect.
Evolution of Views
Early on, when I started writing about Synch Tech, I was just trying to spark a conversation about it. I obviously hadn’t used it. The other people who said I was wrong about things also hadn’t used it. They were right that I was wrong, but I think they were also wrong about what it was. At one point I called the combination of history and non-history based tools “FrankenCAD”. It turns out that was incorrect too. Frankenstein’s monster was a single being made from multiple beings. SEwST is really two separate beings. More like “Dr.-Jekyll-and-Mr.-Hyde-CAD”. You work in one or the other. You can’t go back and forth, and the features of one are not maintained in the other.
Synch Tech and Traditional SE produce different types of parts. You cannot read ST parts in SE, but you can read SE parts in ST. So this is a one-directional translation. If you talk to resellers, ST is the future. Siemens hopes to eventually migrate all SE users into Synch Tech. This means they are forcing users into a completely different workflow. The interface is partially the same, but the workflow and the bulk of the tools will be a learning experience for SE users that get forced to ST. Some of the sketching concepts remain the same, but with ST, sketching is for creation only, not for editing.
I should mention that Synchronous Technology is also a component of NX (formerly Unigraphics). And if you’re one to look out into a crystal ball, Catia V6 is said to be based on a kernel that may contain elements of what Synch Tech does.
Siemens has had a lot of difficulty explaining exactly what ST is. Maybe it was their goal to create a lot of confusion, because it added to the mystery, buzz and hype.
Synchronous Technology Is…
In the end, Synchronous Technology is:
- direct editing
- history-free
- parametrics applied directly to the faces of a solid model
- treats imported models almost the same as natively built models
It is also more than that, but that does for an introduction. Some very clever functionality that recognizes face relationships and applies geometric relations on the fly helps you add relationships to the model as you make changes.
My Experience
What I found by using the software was that there is a reason why most of the demos you see for ST involve editing geometry. That’s because editing is the one area where it has some real strengths. If you need to edit an imported model, a direct editing tool is the only way to go.
Actually building things in ST can be a little frustrating, particularly if you are used to a different way of doing things that involves using construction geometry. This seemed to be an obvious lack, especially when it came to setting up symmetry in a part. I found the software to be just lacking in tools. If this is intended to be a tool for non-specialists, it has a long way to go. The couple of extremely basic tutorials that exist for ST were not adequate to answer the many questions people have about how the software works.
Relying on the Live Rules to automatically apply the geometric constraints with each edit means that you have to check that it got the right relationships each time you edit. In the end, I didn’t feel I could rely on this to automatically do the right thing.
The workflow didn’t work for me either. Selections were order dependent, which might be a Solid Edge thing rather than exclusively Synch Tech. Also there was none of the click-drag interaction, it was all click-click. Something SolidWorks users at least will recognize. Many settings or options would not preview, so you had to accept the setting before you saw the effect. Just didn’t raise my confidence. Maybe it seemed un-intuitive because I’m ingrained in another way of doing things. The direction of change was the wrong way for “ease of use”. SolidWorks is far more flexible when it comes to pre- or post-select, click-click or click-drag, and definitely better with previews.
Of course there is the major limitation of working exclusively with extruded or revolved shapes. This alone will be a deal killer for many users. Fillets in any system are dependent upon the order in which they are applied. The problem in ST is that you can’t change the order. The only good news here is that undo and deleting faces work very fast. Still, you might be surprised by the kinds of changes you can make around fillets. ST can definitely make changes where fillets are involved that would completely choke SW.
Even so, sometimes fillets would limit the types of changes that could happen. If you combine the ideas of entropy and model topology, changes in the model can only lead to simpler topology (fewer model faces). If you make a change that removes a face from a model, there is nothing you can do (aside from remodeling the feature) to get the face back. That is to say that once a face is removed from the b-rep, it is gone forever. In Solidworks, because the b-rep is built in stages, as long as a face is built by a feature at some point in history, you can get it back if another feature cuts it away or covers it over.
Siemens has gone to great lengths to establish the limitations of history-based systems. But I think there are a few things they didn’t count on. First, the types of parts that ST is limited to (prismatic face shapes) are not typically complex parts. I also think they have dramatically overstated rebuild times for the types of parts ST can edit. It’s true that complex parts have rebuild times in SolidWorks that are unacceptable, but ST cannot edit complex shape parts. I think their argument in this direction is misleading. If you can show me a part made from extrudes and revolves where it is built efficiently and has more than 400 features, I may retract that.
Further, I did a large pattern in ST one time, and it is time consuming to create and edit it. Patterns and other types of features such as holes and fillets are considered “procedural” features, which means that a feature definition is stored for those types of features. Large patterns take a lot of time in ST as well, maybe significantly less than SW, but still a lot of time.
On the up side
There are some things I wish SW could learn from SE and particularly ST. I know I’m always grousing about this CAD stealing ideas from that CAD, but I just want to point out that it is not all bad news for SEwST. First is the ability to select one side of a dimension and have the dimension change in that direction. In underdefined SW sketches, it’s a complete crap shoot as to which side of a sketch will change.
I loved the ability in ST to completely ignore rebuild times (because they didn’t exist).
Surprisingly shelling has some advantages with this system. You can selectively shell a shape more easily with ST than SW. By selecting the faces to “thin wall”, you can exclude an area from being shelled. In SW the workarounds for this are feature order or multibody modeling. Neither is as good a solution as selecting faces to thin wall. On the down side for ST is that if the number of faces is large or the topology is complex (split into many small sliver faces), selection can be nightmarish.
After using SEwST, I have a new appreciation for the Instant3D tool in SolidWorks. I still don’t think I will use it, but for people who are simply too lazy or really in that much of a hurry, it offers a way to edit the underlying history-based model without regard for the history itself. It doesn’t work all of the time for everything, and it will never find its way onto a best-practice list, but it is an interesting and useful tool. Also, the SolidWorks Move Face tool is a pale reflection of the “steering wheel” functionality in ST.
One huge topic SolidWorks could benefit from having a look at is feature tree management, rebuild management, and a few other things in that direction. Check out this blog post where I suggest a few things SW could do to improve overall rebuild speed by getting rebuilds and the tree under control.
Summary
The concept of direct editing as embodied in SEwST is beautiful. It solves problems from interoperability between different brands of software to version compatibility within a brand. Those alone are super compelling ideas for me. For editing imported models, this system is in its glory. How often you do that determines how much you need this.
For comparison, Spaceclaim (another direct modeling system) sells for as little as $775 at Novedge. SEwST has much more functionality, and sells for starting at ~$4k. If all you really need to do is edit imported data, you might consider something a bit less expensive.
For a system aimed at non-specialist users, SEwST is far too complex and process dependent. You can’t just pick it up and understand intuitively how to make changes or how to apply the parametrics. It will fail to edit sometimes, and if you are not a b-rep analysing type of user, you will never know why.
Solid Edge with Synchronous Technology is a nice alpha version of the software they are should one day create. I think the interface needs to be less busy, and less cryptic. It’s even worse than SolidWorks when it comes to replacing text with icons. It is great technology, and a fun tool to use, but with all of the limitations it is not a SolidWorks killer, and in its present state Solid Edge users will not be happy to be forced to ST.
Matt,
Great post! Glad to hear an independent assessment of ST now that the dust has settled.
While I hope more direct editing makes it way into SolidWorks, I certainly don’t want the “one direction” approach that SE has implemented.
When pundits claim 2-10X improvements, I get very skeptical.
I hate rebuilds as much as the next user, but don’t think that parametric CAD is a dead end. We need both parametric and direct editing, without limitations. To throw away history when a direct edit is made is just ludicrous.
People that claim casual users will some how become modeling gurus because of direct editing are dillusional.
Keep up the good work, and have a great holiday season (PC for Merry Christmas).
Hi Matt,
Thanks for taking the trouble you have in reporting as you have done. Balanced assessments and comparison of CADD software are hard to come across and they are very important.
John_P’s statement, “We need both parametric and direct editing, without limitations. To throw away history when a direct edit is made is just ludicrous.”, touches on my long held view. CADD tools need to be a mixture of methods. Whether they like it or not CADD developers are going to need to embrace this fact and build products to match.
Wishing you, yours and your readers a great Christmas, Matt.
Dear Matt, you said “For editing imported models, this system is in its glory” : is this comment coming from your direct experience ? Did you really try to load step files from solidworks to SE and try to edit them ? Were they complex with fillets/drafts ?
Thanks for the update on this Matt. I think you have hit the nail on the head with the comment “If you need to edit an imported model, a direct editing tool is the only way to go”. For me therein lies the big problem with a solely non history system. We don’t need to edit imported files – we create all our data.
Over the last 10 years there has been some intersting new developments in CAD – and I have tried most – but on closer inspection they all fall into that category – editing existing geometry. There is very little new stuff around for creation of complex geometry – accurate geometry not blobby geometry (by which I mean subtle complex surfacing as opposed to the extreme examples you usually see).
Most of the new stuff that has come around is based on global or local shape modification (like the GSM tools in ThinkDesign, or Morph in VX, or Freeform in SolidWorks) and these are useful and have their place, but, for any package to claim to be the future it has to encompass both forms of editing – history based (parametric features and curve driven via sketches) and direct face modification.
I’m still failing to see how and direct modelling system can handle an automated modelling scenario like those tackled by DriveWorks – which at the end of the day is targetted at precisely the extrude/revolve/shell market ST seems to be placed in right now.
I feel that parametric history based modleling carries much of the design intent. I can change a few dimensions and the model changes in a way preserving the structural and aerodynamic properties. I designed the engine installation and cowling for a nice little amphibious airplane. Everything was modeled in Solidworks. The large assembly is at the limit of Solidworks on my computer. It takes about 5 minutes to load or save, rotations are blocky.
Yesterday I needed some quick direct editing. The airplane is in flight test. There is a flow separation on the pylon under the engine. I needed to communicate the shape of a fillet to the builder. I started from a solidworks assembly of the entire airplane. I then saved the assembly as a part. That converted all of the solids into surfaces and removed all design tree insformation. The model, she is dead. Solidworks refused to create solids from the surfaces, but would in some cases form a thin shell. Fillets were unreliable due to the number of surfaces. I really wanted a variable width chamfer. I projected some curves onto surfaces, made them into 3d sketches and swept a line to make the desired surface. A little thikening and trimming and the shape was created. It took way too long.
What do you mean about “You cannot read ST parts in SE, but you can read SE parts in ST.” ?
I’ve played with NX6 at home and I don’t h have this problem.
Are you regarding about different release ?
@cubalibre00
What he means is that in Solid Edge with Synchronous Technology, a part created in the Traditional mode (Traditional part) can be converted to a Synchronous part, but a Synchronous part cannot be converted to a Traditional part.
Ken
Matt,
First of all thanks for taking the time to do a serious look at the technology. I’m sure all your blog readers appreciate your critical eye and candor. I won’t take issue with any of your opinions – differing opinions make the world an interesting place. But I’d like to correct or clarify a few things if I may.
Before I do this, I hope what most folks can take away from your observations is that there is some great technology and concepts here, but some of the implementation needs to be rounded out. I don’t really take any issue with that. We believe that the premises are sound and extensible, but clearly we have work to do to finish some rough edges and to convince folks to look at what we believe is ultimately a better ways to do things. I’d just ask your astute readers to keep their minds open – they are designers and engineers after all – they are born to think “there must be a better way.”
Ok, so on to things that I’d like to correct/clarify…
Target market — A couple places you state that we are targeting the non-cad-specialist with ST, implying that this is our main target for the software. This is certainly not true. Our core target remains the mainstream CAD user, particularly users who have or are still going to transition from 2D. We have endeavored to ALSO make it approachable by the more casual user, though certainly your review points out that we have more work to do there.
Workflow — Here, I think the whole story wasn’t quite made clear. Yes, it’s true that history-based modeling and Synchronous Technology are quite different and you don’t mix and match the modeling styles within the same part design. But we DO allow and encourage mix/match at the assembly level – you can create models using either technology (both are included in Solid Edge even in the base package) and create assemblies of both types mixed. With the next release of Solid Edge, ST2, we will continue to expand this notion, allowing even more flexibility with assemblies with mixed part types. In general, you will continue to see us evolve and merge the two technologies to continue to leverage the best of each.
Users are not “forced to ST” – I think we are in agreement on the fact that if you push someone in a direction, they won’t like it. But we aren’t forcing ST-style modeling on anyone – though perhaps in our enthusiasm we’ve failed to make this clear. We know we can only succeed when people WANT to use the new technology. The technology has to be demonstrably better and applicable to a company’s complete breadth of work before they will want to work with it. For some folks that’s now. For some folks that’s later, when we’ve done more of the “evolving and merging” discussed above. And some folks can’t see how this will all play out and therefore want to keep doing the history-based thing for the foreseeable future. That’s fine; we don’t plan to pull the rug out from under anyone — in many folks opinion, Solid Edge was the best CAD system in many respects PRIOR to Synchronous Technology (sheet metal and drafting have always been strengths) and that hasn’t changed.
Revolutionary or Not? — Now, not really an inaccuracy, but a point of debate is the “is it revolutionary” thing. I would say that it’s true that MOST of the pieces have been piecemealed here and there in other systems and some would argue that that doesn’t make it new or revolutionary. The same of course could have been said for PTC in 1988 or so. The basic idea that editing a dimension does a solve and changes the sketch goes back to Sutherland’s SketchPad software from 1968 (yes 1968 – two decades before PTC . I’m sure you know this Matt, but some of your readers may not). And most of its other pieces can be traced to Romulus or other early solid modelers. But I would be the first to say it was revolutionary at the time. I think Synchronous Technology is revolutionary in the same way – yes, many of the pieces had been implemented here and there – but there was lots of invention (several patents filed) and new thinking on how to wire this all together more productively. Time will be the judge of this debate I suppose.
Engineering Tips Forum – I will grant that I’ve been remiss in paying close attention to this forum and helping users with their questions. Solid Edge has its own internal newsgroup where much dialog has been going on and I’ve been in the middle of that. That said, I did go peruse Engineering Tips Forum after your article and did not find users “confused, betrayed, or bewildered.” There was some good Q/A and one rant, but all in all it was just “hey, here is something new, what do you think?”
Comparison to SpaceClaim – I suppose this was inevitable since both use the Microsoft Fluent UI and both have aspects of non-history. However, I do think SpaceClaim is limited, as you say, to being “targeted at the non-CAD-user” and “primarily an editor”. This is definitely not true of Solid Edge. Yes, as you say, it IS great editor of other peoples’ data. However, it is so much more than that and it really sells it short to sum it up as that. Just in the modeling arena, they differ quite a bit in how they handle features (procedural features – a lot more on this coming in ST2) and dimension driven editing (SpaceClaim has no constraint solver so you cannot do basic engineering like lock one dimensional value and edit another dimensional value preserving the first one or relate dimensions via equations). And, unlike SpaceClaim, Solid Edge is a true production CAD system with framing, piping, wiring, large assembly handling, unparalleled sheet metal, built-in PDM & FEA, top-of-the-line drawing production and more. If you want to compare, compare Solid Edge (history-based) to SolidWorks (history-based) and then give Solid Edge the ADDITIONAL credit for Synchronous Technology.
Sorry for being so long winded (didn’t start that way!) and thanks again for giving us your considered opinions. I look forward to your readers continuing to follow the ST thread as we continue to round out and prove that it’s the next big thing.
@dan_staples1
Dan,
Thanks for a great response. I’ll definitely try to remain open minded in that I’ll try to recognize change, but I don’t make any apologies for having an opinion.
I do need to apologize for your post getting thrown in the spam bin, probably because of the length. fortunately I fished it out before it was deleted. It should have posted a day or two before now.
Good point about being able to use both ST and trad SE parts in an assembly. I was just thinking on the part level.
It’s easy to get the idea that you’re targeting non-cad specialists. I’m pretty sure someone said this at some point. A big part of your argument against history is the you’ve-got-to-become-a-master-at-sorting-out-the-tree thing, which is close enough to cad-software-guru. With such gaping limitations, I can’t imagine ST being used for general CAD use. Certainly not in the same way that traditional SE is used.
In terms of people being forced to ST, you have stated that at some point you expect traditional SE to go away, and unless you have 100% adoption, that means someone is going to be forced.
Even if your comparisons about being revolutionary are correct, I see little effect on actual users. Other vendors are flipping out, but users are not. If Toyota put an 8track tape player in the Accord, you could watch Chevy get whiplash trying to put one in their equivalent car. Users really don’t figure into this equation much. It’s all about marketing perception, which doesn’t equal users reality.
Comparison to Spaceclaim: The only real reason for a SW user to be looking at Solid Edge is the Synchronous Technology, so I think it makes more sense to talk about the direct edit side of things than the comparison between history based systems. Anyway, with ST coming out on the heels of Spaceclaim, and trying to out-hype Spaceclaim, the comparison is certainly inevitable, with most folks perhaps assuming the software is equivalent from a modeling point of view. To me personally, anything outside of modeling is a non-issue (such as drawings). And with direct edit meaning that native data means that much less, the entire solution (parts, assemblies, drawings, rendering, analysis, etc…) can be thought of as component technology.
Anyway, thanks again for your input. I’d like the opportunity to do a follow up when your next version is available, if you can manage that.
ps. It sure is nice for an executive from a CAD company to be able to comment intelligently on a users blog while adding credibility to his product/company rather than becoming a major embarrassment.
Roberto,
Yes, this is based on personal experience, but it has to be qualified. First of all, as mentioned in the post itself, Synch Tech can’t edit complex shapes. Some of them had fillets and draft. Fillets also had limitations such as if editing must create a new face, then the edit fails. Also if editing would cause a fillet to extend in a non-tangent manner, the edit fails. So yes, the whole pile of qualifications that apply to other edits in ST also apply to imports. The only difference between imports and native data is that the native data has the “procedural features”, which enable you to specify parameters. Stuff like holes and patterns.
As for the means of import, I opened SW files directly or used parasolid. On many newer files, the SW direct conversion failed, so I used parasolid.
Have you looked at Solid Thinking? That one’s on my short list of stuff to play with.
Anyway, about the Driveworks thing, I think it is completely doable for direct editing to incorporate a table of values to drive sizes like a design table. It would be a different issue to add/remove features. Then you’d have to have a list of operations like delete face or extrude. And if you do that, you’re right back at creating a feature list almost like a history based system. I think a really clever person could figure out something to make all of this viable.