Solid Edge vs SolidWorks: Sketching, Part 1

There’s nothing meaningful I could do to compare the entire Solid Edge and SolidWorks programs in a single blog post. That’s why when I have taken the topic up on the Dezignstuff blog, I would bite off “small” areas like surfacing, sheet metal, or the overall interface. In this case I’m going to look at sketching, arguably the single most important function of any CAD program.

You might think Solid Edge and SolidWorks sketchers are pretty similar because they both use the (Siemens) Dcubed constraint solver. In the end, that similarity probably means that they share the strengths and weaknesses of Dcubed, but the comparison can’t be limited to that. The differences between them are much more structural. When you consider that Synchronous Technology has a big impact on sketching, the conceptual differences become even larger.

The Tools

The one thing I will say right off the bat is that I like the SolidWorks way of adding items to toolbars better than Solid Edge’s. I like to select an icon from a list, then drag and drop it where I want it. The SE method requires you to find the command from a set of cascading drop-downs, then find the area of the ribbon where you want to put it, and then use the Add>> <<Remove buttons in the middle. I remember this from a ’90s version of Netscape.

Also, where SW (in the Tools>Customize interface) gives you a block of icons, SE gives you a linear list (cascading drop-downs). The rectangular block is less organized, but more space efficient. This probably belongs more in the interface discussion than the sketching function.

3D Sketch

What is SE missing? Well, 3D sketch is missing. There is the Frames functionality, and it can draw lines in 3D space, but Frames in SE are done in an assembly (weldment equivalent in SW). I would like to see the 3D sketch capability added to parts. It took SW a long time to get 3D sketches to the point where they were only difficult to use (as opposed to impossible or frustrating). It’s my understanding that SW uses a different solver for 3D sketches vs 2D sketches, and the constraints in 3D sketches in SW are what makes it so unbearable. I’m not saying that SE 3D sketch equivalent is any better, being a noob and having no experience with it.


SW early on had this concept that you should be able to sketch with either the click-click or click-drag. And that worked well. You had a choice depending on your preferences or what software you had used before. Then they started adding things like the Enable Onscreen Numerical Input On Creation, which only worked for click-click mode. So. Solid Edge sketching works click-click. No games. It just works the way its supposed to, and you can count on it.

SW had a cool idea of having dimensions added immediately as soon as an item was sketched. At first I thought I would love this, but in the end, it turned out to be one of those things that you might want to use selectively, but not all the time.

In Solid Edge sketches, you can add numbers as you sketch, and it seems to flow well.

SW has Modify Sketch, as well as Move, Copy, Stretch tools. Again, duplicated tools instead of one thing that just works. SE has the Move, Copy, Stretch, Mirror, Rotate, Scale. Just one copy of each, as far as I can tell.

SE has this little visual tool with the Tangent Arc that gives you a target for which quadrant to aim at to get tangent, perpendicular or anti-tangent. SW has the same function, but no visual target.

The reason I bring all of this up is that SolidWorks sketch workflow, like much of the rest of the workflow in the program, is all over the map. There are duplicated functions. No wonder they had to gut the software and start all over again. The Solid Edge guys seem to have done better homework, and much better housekeeping. The two software packages are the same age, yet SE just seems cleaner, much less sloppy.


SE doesn’t have Face Curves, but it does have Intersection Curve. It also doesn’t have the weird schizophrenia about sketches and curves that SW has. In SW, curves are kind of bastards. They follow different rules, and are generally harder to deal with than sketches. Also in SW, some sketch types are called curves, which I’m sure would be confusing to my counterpart, an SE veteran learning SW. Projected Curve is a curve, but Intersection Curve is a 3D spline. In SE, so far as I can tell, curves and sketches are treated about the same. In fact, what is called a Spline in SW is called a Curve in SE.

SE doesn’t have a parabola or a conic (but it does have conic fillet/blend option). Of course SW doesn’t have conics either, but the parabola has improved at some point over the last several years in such a way that it’s actually usable. SolidWorks just got the CtrlA for Select All in a sketch in 2012. I notice this is also in ST4, but I don’t know when it arrived.


But then SolidWorks doesn’t have Freesketch.  Freesketch is a very cool tool, and I can see that it’s the kind of thing that some people will love and others hate. You can just drag your cursor to sketch a shape and SE interprets that as lines and arcs. It’s the quickest way I know to get a bunch of lines on the screen without clicking. I’m sure it’s a mainstay with the demo jock community, but I can see some practical use for it, especially for concept creation. I’ll bet with a Wacom tablet it’s really nice.

Help Rant

Freesketch, by the way is tough to find with the Command Finder. It’s in there, but you have to click the “Show matches outside environment” link. You can find Freesketch in the Help, but it doesn’t tell you where to find it. I just stumbled across it yesterday, and for some reason, today I can’t find it again. I’m sure it was on the Line dropdown. I eventually found it on the Line drop down in the Ordered mode after starting a sketch. Not sure if that’s obscure or if that’s just me. Why isn’t this available elsewhere? I couldn’t find it in Customize Ribbon either.

I got called out for saying SolidWorks Help sucked without giving examples. So here are some examples. SolidWorks Help has no Index, so if you know what you are looking for, you can’t just go to it. Solid Edge Help has an Index. In the SolidWorks Help, I can’t use the Back button programmed on my mouse, you have to use the special Back button on the SW Help interface. On Solid Edge I can use my mouse. Solid Edge has all the help in one location, on your computer. You don’t have to fool with multiple locations to get the same information like in SolidWorks. Also SolidWorks Help is cluttered with all sorts of stuff that’s not related to CAD, stuff I’ll never use, and when you do searches, you get stuff from all those categories that just dilute the quality of the search. If you need more reasons, refer to old posts on the Dezignstuff blog.

Derived Sketch

SolidWorks has Derived Sketch. Solid Edge has Tear Off Sketch, which I think is just a copy, not a linked copy.

And then you get to the really odd stuff in SolidWorks. The stuff that people tend to not use. There’s Rapid Sketch, which I’ve always thought was a bit of a disaster in SW, but it’s roughly the way things work in SE.

There’s Instant 3D in SW, which should have been more popular, but wasn’t. This is essentially a weak response to direct edit as a whole. It gives you that direct edit feel for some types of features. If you use it. And I rarely see people use it. It used to be turned on by default, I’m not sure how they do it these days, not doing many totally fresh installs. It’s usually one of the first things I turn off when sitting down on a new computer. I’ve seen a lot of users have it turned on, but never use it. Instant3D is actually a cool idea. But it’s a bandaid compared to Synchronous Technology.

Here are some more sketching topics I’m working on:

Best Practice in SolidWorks is something that serves the needs of the CAD, not of the design. Solid Edge ST4 has less need for imposing best practice type rules

Create a plane and move it freeform using steering wheel

Reorient the axis of a sketch when creating it by using the B and N keys (on a face with non-perpendicular edges).

Solid Edge users are less obsessed with referencing the origin. They also appear to not care much about “fully defined” sketches.

Right clicking/ESC gets you out of just about anything.

Reattach dimension by clicking on dim line then alt-dragging leader to another edge.


Add a Comment
  1. Hello Matt,

    With regards to 3D sketching. Solid Edge has a Cross curve (see attached image) function which can be a very robust way to create a 3D curve.



  2. Great post Matt.
    3d sketches are lacking but you can use some of the curve commands as a replacement but a more robust set of tool would be nice.

    I draw a lot of irregular shapes and have discovered a trick.
    When the curve commend is invoked you can click and drag the curser to “free sketch or draw ” a spline. Then smooth it by using RMB simplify.


  3. Great post Matt!

    Just a comment on this statement:

    “Right clicking/ESC gets you out of just about anything.”

    Right click in Solid Edge validates and ends the current action/command.

    ESC cancels and ends the current action/command.



  4. Free Sketch is one of those things I recall seeing demo’d once but have never used nor remembered it exsisted.  I may play around a bit with this one! In an ordered approach I choose to define my sketches and constrain them. In Sync workflow this may not hold as much merit as it once did since the sketch no longer is the “driver”… 

    So the Noob become the teacher… Thanks Matt!!!


  5. Strike the last commetn…  Free sketch in an ordered mode command only at this time… I’m going to log an ER.

    Matt J.

  6. how about equation curves?

    Is ti possible to create a curve according to a equation in SolidWorks??

  7. Matt, you mentioned Tear Off Sketch.  This is an Ordered command and has the option to either Move the existing sketch, copy the sketch non-associative, or copy the sketch associatively.  This is set via the ever so familiar Option button on the command bar.

    1. I would also add that since sketches do not drive Synch mode models, there is no need for it in the Syncronous mode (use the Steering Wheel to move or copy a sketch non-associatively).

  8. Freesketch looks very useful but there again its buried somewhere. Cant say as I noticed it in my brief trial, which is a pity because I probably came away thinking SE is more limited than it is. If they do a UI revision tuned for ID people (and hopefully they will get serious about that segment) things like this have to be readily available.

    Nice write up so far ;)

    1. Neil,

      Here is a customer of ours using Solid Edge for Industrial Design:

      See some of the products they developed and together with the new surfacing capabilities focus release of  ST6 next year, I believe SE will be a very strong option for the ID area.



  9. Hi, I follow your points of view from very close distance.

    Because of the issues with SW, specially the one related to the cloud and the Big Brother watching over our shoulders, and secondly because of the kernel change; I am testing replacements.

    Sadly it is really difficult to find tutorials about this software beyond the ones included with the software. Especially related a procedures in real world scenario. For example, it looks like there is no way to associatively inject a sketch from a part to another without to create a assembly as a bridge. Also, It looks like that skeleton sketches must be native to the assembly, they cannot be created in a part and to be injected into the assembly…. and so on…

    Perhaps as a noob in SE I am digging the help files and the internet in the wrong places. But may be not.

    I would like you might address this kind of issues in a near future.

    Note: English is not my first language, so accept my apologies if wrong grammar is present.

    Have my regards.


  10. Hi Matt


    Good first post to introduce the sketch,  Not sure what you plan for the next one, but one thing is sure, it is important to understand the role the sketcher play in both software before going too  technical.

    The Tools….

    Ok first about customizing the interface, not only we need to look at the good old  linear tree to select commands, you should also notice that we can create Split button and Drop button. Those two when use properly, will help you get higher command density to maximize and/or  optimize the space of the ribbon.

    *With ST4 we can also recreate the Ribbon from scratch. We have one user who have a giant screen, if i remember correctly, he have just one tab, one group and all the icons list.

    *Also icons can be display in different way, big, small, text, no text etc…

    At the top you can build  themes dedicate to surface modeling, for Solid modeling, for review (PMI) etc…. All them can be access using the RMB on the ribbon.

    Also if you RMB on any icon or group in the ribbon, you will have the option to add the command or group to the QAT (Quick Access Toolbar). This will give you the chance to use the ALT plus a number to launch a command.

    RMB on any element of the QAT and you can remove them.

    *Did not mention the radial menu first because it is kind of obvious for me, but like Dave mention, the radial menu can be customize per environment to give more flexibility.

    3D Sketch

    Most of SW users will probably back off after their first contact with SE because they expect to have the same kind of functionality in SE. SW users may need to give a second and maybe a third try… We need to remember  SW use the part environment to manage assembly process, Weldment and Frame are the two that came to my mind.

    Before the cloud and any SW database talk,  we could see Dassault philosophy to centralize anything and the part environment is one good sign. OK I stretch this one a little :-)  But I think that part configuration, Sheet metal info are also store in that same part file….

    So it might not be  the lack of 3D sketch but rather an understanding of how workflow are design in SE.

    As I have repeat this often, and sorry for those who are tire of hearing this, but the fundamental difference between SE and SW,  SE is a Feature base modeler  and SW is orient Skeleton base modeling.

    The sketcher in SW occupy a greater presence because, and this is base on what I was able to observe,  SW users are teach to create a wireframe skeleton to attach features. How many times we heard  SW users saying they wanted to create that giant sketch to control their model? And I still see this right from last week..

    So fundamentally SW focus on the tasks as oppose SE focus on the workflow. In traditional modeling (this is obvious) if you look at the Ribbon, you normally start from the left with:

    1.  Planes,  look on the command bar planes have no steps in their workflow, but you will find on the PromptBar few options keys that can be use N B T F P before you click to create any planes. Those will not be enable on the three base plane, only when you place the mouse over a surface.

    2.  Next one on the right we have Sketch, when you launch that process, you have two steps in the command bar:

    •  First step select  where in space you want to place you sketch (select a plane/surface)
    •  Second step the profile ( what do you want to sketch)

    Notice the drop down list to define the plane on the first step. Just there you see that we do not need to prepare something to create a sketch because the command encapsulate in a workflow all the ingredients we need.

    3.  Then if you look at the next one on the right, you will find features. Launch one of them and you will find (for extrude) 5 steps. Look closely at the first two……. Do they look familiar.

    *Again everything you need is encapsulate inside the command. For a user that was teach to use skeleton modeling and be able to launch the extrude command without having to draw any sketch that is a big cultural shock.

    *If you still need to do skeleton modeling it is possible, create one or many sketches, Launch the extrude command  and look in the list of available planes, first one on the top “select from sketch”

    *If you need to reuse part edge in you sketch, look in the Ribbon when create your sketch for “Include” this command is the equivalent of share sketch. This command will project edge on the sketch plane.

    Now after creating you first cube, RMB on it you will see three choices at the bottom ( traditional)

    •  Edit definition
    •  Edit profile
    •  Dynamic edit

    Dynamic edit might be the one you will find the most interesting.  It allow you to edit live the sketch of that feature. Select multiple feature and dynamically edit those feature.

    If you like to work with the 3D feeling in space, I will recommend you to open the Solid Edge options, under general at the bottom right unchecked “Orient the window to the select plane”

    *If you choose edit profile and you require to have the sketch parallel to the screen, hit CTRL+H.



    Because of the fundamental philosophy  Feature versus Skeleton,  curves are in many cases derive from the solid or like you mention from Intersection. This give the curves a better DNA ( sorry could not resist opening  this door :-) ). In fact if we look with a bigger umbrella, 3D curves usually need a solid foundation to be create ( grrr did it again sorry…. lol) Has mention by Theodore curves command can be found under the surfacing tab.

    One thing I learn with the time, in solid modeling the curves (edge) are driven by the surface in surface design  the curves (edge) drive the surface.  Again look at the history of Dassault  it came from the wireframe/surface world and we can see this influence in SW philosophy.

    «…Some of the underlying work on what eventually became CATIA started in 1960 at Renault where the mathematician Pierre Bezier developed a series of mathematical techniques for describing the curved surfaces of automobile bodies. Bezier’s work led to the eventual development of the widely used Bezier Curves for describing mathematical surfaces. In 1976, Dassault Aviation acquired the technology, then known as UNISURF, from Renault for in-house use to complement its CADAM system….»  one of the good side about CAD I think you mention this one once



    FreeSketche in a way show that sometimes Siemens is a little bit ahead of its time. This was present in SE as far I can remember.  I would say in 2000 we had this feature. However we did not have any good support (physical support in mean) to push this further. Now that we have those cool pen enable  tablets and people seems to  yell for enhancement with the surface modeling…. If were ask to use candy at ST5 to get something in ST6 count on me to place most of them for surfacing tools…. I think I might be willing to pay a beer  to get everyone’s candy… Ok I might just get my self in trouble.



    I would just refer to your first post…


    Ok enough for now….. first day off since a long time and I spend it commenting here. Hope you don’t mind doing this Matt,  promised I will get a life one day :-)

    have a great night all

    1. Luc, Wow, that’s a lot of stuff. I agree that the sketch is more important in SW than in SE. I also love what you can do with planes in SE, and the fact that you don’t have to make a pile of them or keep them around if you don’t want to.

  11. A sort of “Freesketch” thing here. You can draw a line through sketch elements and clean up/delete that way.

    Command finder is your friend. When you have a question type in what you are looking for and go.

    The radial menu is also very handy and can be easily edited for each environment or indeed for each job if you wish.

  12. I’m jealous of the SW slot and curved slot sketch tool – really nice. SE has something similar within the offset command but I find it cumbersome and really don’t like using it.

    1. Quote: “SE has something similar within the offset command but I find it cumbersome and really don’t like using it.”

      Are you talking about the offset or symmetric offset command? The Symmentric offset is a fantastic tool – draw a line/arc and click this with the symmetric offset to get an offset all around (like a buffer zone). Edit the original line (think centreline) and the slot modifies to suit.

  13. Matt-

    In SE can you save sketches for reuse, a library of sketches? For example, std drill sizes? Perhaps Drag & Drop?

    Thanks, Devon

    1. Hi Devon

      could you clarify the link between drill hole size and sketch, i think i know what you look for but wanted to be sure

      maybe a quick in context exemple

      1. In SW I can save any Sketch into a Library folder for reuse. I can also add constraints to that saved sketch to define it’s location, for example a given distance from another sketch point or a 3D edge. I can save this sketch and give it a meaningful name; i.e.5/16Dia or even something like 4X Bracket Holes Pattern.

        If I need to use any of those saved library sketches, I search by the name and then use it.

        During the past 14 years, I’ve created many saved library sketches for various different customers. I also do this for 3D features, create saved library 3D features, i.e. a specific thru hole with a custom counter bore. Just askin’ :-)



        1. Thank you Devon,

          Let me finish few things ans i’ll be back to you.

          Update 2012-04-22


          For Draft

          Prior ST (v20 and less) we have the possibility to create sketch in the draft environment and save this draft and change the extension from .dft to .par. This gave us the possibility to drag and drop the rename draft  inside a sketch.

          With ST in synchronous mode this became much easier as we can simply cut and paste sketch to create a library and simply drag and drop to reuse it

          With ST in traditional the rename draft trick does not seems to work anymore. But we do not have lost any functionality because any sketch in synch can be use in traditional modeling. In fact the skeleton i often refer, can be create in ST and in Traditional we attach feature to that skeleton


          In term of building a library of feature nothing have change, cut/paste then drag and drop. This is true for ST and Trad

          Hope this answer the question


        2. Devon, SE Ordered also has a feature library that can save the 3D feature with sketch and constraints which can be reused.  In SE Synch, you can copy 3D features and reuses them much the same way, but no sketches with those…

          1. Great, thanks for the information guys.


  14. Matt I am having a fundamental issue with understanding things. In most history or associative based systems it is simple – the sketch drives the model. You edit the sketch, the model updates. In addition you can select a feature and update the feature.

    Now in SolidEdge there are two modes? History (ordered) and Synchronous (Direct). I assume ordered is basically like SolidWorks. What I don’t get is how you relate the sketch to the direct mode?

    What it appears to me is that in direct mode you create the sketch and then the geometry , but then to make edits you move features and faces rather than edit the sketch? If so – why is the sketch so critical then? Why go to the hassle of dimensioning up a sketch, creating relationships between sketch and geometry only to have them ignored, then have to recreate all those interrelationships as Live Rules?

    Or am I wrong and sketches can still drive Direct models, and you can still edit the sketch to update the model? In which case then, surely it is history or associative based.

    This is a point that has never been adequately explained to me by SolidEdge users or SolidEdge VARs.

    Is there a video someone can point me to that shows building a simple part in direct mode and how to edit it by editing the sketch? Like I say, if you cannot edit the part by editing the driving curves this seems a bit like double work to me. Setting up sketches then having to reassign rules to relate the features.

    1. Kevin, it sounds like you’ve got it until you ask about the sketch driving the synchronous model. The sketch does not drive the synchronous model. Once you use the sketch in ST, it is kept, but only for reference, there is no associative link.

      The dimensions you apply to the sketch get automatically associated with the corresponding faces in the model, so there is no double work that you mention. Relations are assigned on the fly by Live Rules so that you can change your design intent easily. You can assign relations more permanently if you don’t want/need the extra flexibility.

      1. OK thanks Matt. One further question then. Sometimes in a history/associative system it is easiest to just drag a sketch entity and see a whole chain of features update. In a direct edit like this you presumably then have to select ALL the faces affected before making the move?

        if you combine this with something like Instant3D where you can drag an curve in 3D  model space surely this is faster/easier/more logical than having to select all the faces that you think might be affected then applying the move? Sure there is a rebuild issue but for a lot of parts under a certain feature tree size, on a fast machine this is almost instant anyway.

        Also if you have patterns in a history system linked to dimensions or variables, how does this relate in direct editing (like say by dragging a part to be 100mm long instead of 50mm, and a pattern rule is defined as having a hole every 20mm – in history this is easy, but in direct can you just drag the faces to extend the part and have holes automatically added to the part as per the variable/rule?).

        Sorry for all the dumb questions but I’m just trying to see possible pros and cons. We are looking to add another seat to the company and I’m pondering to go for SolidEdge as well as SolidWorks, rather than just another seat of SW. Ultimately it comes to cost and benchmarking though.

        1. Kevin, Selecting ALL the faces is what the Live Rules thing is about. I’m going to have to write something about that, since it is so important and so many people are asking questions about it. Live rules have default settings for finding faces that are perpendicular or parallel, tangent, and some other types of relations.

          Patterns are treated in a special way in direct edit. I think they are called “procedural features”, and don’t have history per se, but do have some sort of internal association of faces. There are also live rules for “coplanar axes” which handles certain types of patterns, I think.

          These are not dumb questions at all. I’m just about a step ahead of you with figuring some of this stuff out. Finding the pros and cons is what this blog is about.

          The thing with Solid Edge is that imported prismatic parts will be just as editable as native parts. Buying a license of SE would add capability and capacity, where adding a license of SW would only add capacity. SE is still not as capable for things like complex surfacing.

          1. Hi Matt,

            “SE is still not as capable for things like complex surfacing”

            You did a great surfacing comparisson back at the end of 2010 –

            You concluded that post with the line “I’ll bet if you learned to do surfacing in SE, you might not ever miss what SW has”. Has that conclussion changed over the last year? Since purchasing your surfacing book at the start of last year and having changed my tact to a pretty confident surfaces user in SW, I’d be pretty lost with out the same functionality these days.

            Thanks in advance…



    2. Hi Kevin

      Answer can we long because we need to explain many things, but let cut it short.

      The sketch is consume when we create the solid, by consumed i mean it is placed in a bin name “Used sketches” it is not delete, at any time that sketch can be recall and reuse .

      Classic example, i create a simple rectangle, then extrude that rectangle.

      Now i wanted to create a new rectangle, no need to redraw a new one as  we can reuse the existing one. However in many cases it could be much easier to just redraw. We have an option that prevent sketches from migrating to the “used sketches” bin in case you know you need to reuse it. This will cut few steps in the reuse process.

      For the dimensions, they are migrate to the solid body. Again to take the classic example of the cube, if you draw a square with two dimensions and extrude the sketch, the two dimensions are transfer to the solid.

      However, remember that dimensions can be add to the solid at anytime in the process.  In some cases, it might be easier to just redraw the sketch ( especially sketches with fewer lines)  with no dimensions,  near the final shape, extrude, then fine tune the model by directly manipulating the solid.

      As for geometric constraints apply to the sketch, they are not transfer to the 3D model. A portion of that intent in the sketch is carry on by the Live Rules. Each time you move a face the model is interrogate and Live Rules maintain the geometric condition of the model. LIve Rule is pretty good at finding the original intent. One of the strenght of the Live rules,( and i think Matt have show this somewhere) by adjusting the options of Lives Rules you can change the design intent on the  fly. By default Synchronous is develop to give you flexibility.

      For people that came from the traditional world, it is possible to lock the design intent with master dimension and persistent face relationships


      Let start with those basic explanations to begin the dialogue and let see where we go from there.

      I need to change PC to create quick videos then i will update the post



      1. To a SW user this construction (in the video) looks very fragile. Is this how you would work in practice or is this just to demo sketch reuse? I mean SW is a bit like mountain climbing, you pick a secure route, anchor your rope carefully and have 3 points of contact.  Matt already mentioned not being so fussed with the origin in SE and such but arent you going to get into trouble somewhere if you just attack you model any old how?


        1. sod this blog edit in Android not updating…

          I mean doesnt the lack of feature history encourage all sorts of poor modelling practices merely because you get the idea having a plan doesnt matter?

        2. Hi Neil

          Can you elaborate on “To a SW user this construction (in the video) looks very fragile.”

          I practice climbing (rock and ice) in the past and i understand you analogy. But i also remember that at some point we need to trust the material and that we need flexibility to climb that route and work with just one anchor point… Part of the climbing is also to look at what seem impossible 5  or 5.5 grade and realize that it is not impossible to climb.

          By reading your update about feature history  “…lack of feature history encourage all sorts of poor modelling practices…” I understand better the first post you made and better see why you think that synchronous modeling might be a fragile.

          Those are the first signs that you are entering in the first phase of your reflection where your modeling foundation are shaken because you loose the usual reference  :-)

          For the origin,,,

          I saw the mention of the origin in Matt post, but did not focus on this because, we start talking about design/modeling technique not really about the software.

          SE users care about the origin of the part. More then you can imagine. I would say that we care more because the origin is important in the overall workflow, (read sending the part to a CAM system, but this could be discuss in another topic)

          Maybe this have change, but if i remember well, SW deliver the software with the z axis pointing to the user instead of up. This have for impact that when we received design from SW it is not orient correctly.

        3. Neil,

          Your opening sentence “to a SW user” sums this up, SE is not a variation but rather a whole new way of doing things without the constraints of history based modellers. Sure you can do things in the ordered environment and feel secure that you’re doings thing the way you always have –  just with a slightly different flavour. Or you can embrace the synchronous way and create models that are more robust, still with your design intent (whatever that means) and way easier to edit and update. It is, however, a different way of thinking and a leap of faith for the SW faithful. I can understand that sometimes it appears just plain wrong but trust me it works and it works well.

          FWIW these days I primarily use NX but I still have to break out SW and SE depending on what/who I’m working with. Incorporate better surfacing and integrated CAM into SE (both of which are on the near horizon I understand) and I’ll take SE over NX and SW.

          All IMVHO of course.

          1. While I realise Sync is more flexible and Siemens would like to promote it as wonder cure I really have concerns that working without regard to how you construct things isnt just begging for trouble to manifest later. Not every model in SE will be purely Synch based. Perhaps Matt is a better person to comment on this coming from a SW perspective. I think he will appreciate what I am getting at.



          2. I agree. Sync is not going to totally replace history (yet), but this is where Solid Edge has excelled – you can work with sync where appropriate and do the rest in ordered.

            I would also like to point out that history based is not infallible. How many times have you modified a model and had lots of features fall over? What happens when you open a model (more often when it has loads of features) that was modelled by someone else and you need to spend ages just trying to work out how it was built, just to make a tiny change? Sync is able to avoid all of these headaches.

          3. I agree. I am working on a blog to cover that very scenario.  Sync will work well with fillets around a single edge, but you get into trouble when these fillets (especially if they are of different sizes) intersect each other. When you get into this situation, you apply the fillets in ordered (Sync stuff edits live, while suppressing ordered stuff) and that way you will not get into an uneditable model situation.

          4. Here’s my take on it. Synch Tech is a great thing, but it doesn’t do every thing. I think there are situations where using ordered features are a good idea. For those times when you use history, it matters very much how you set things up. I have some ideas about this that I want to work through. Certain situations tend to fail a lot in direct edit. Like dragging things around with a lot of fillets. Fillets are one thing that I think might best be applied as ordered features. When synchronous fillets fail, they prevent your edit from working, and you’ve got to do something drastic like delete the fillet faces (if you can) or create some other left-handed workaround.

            When fillets fail in history, they delete themselves, but allow the overall edit to go ahead. To me this is simpler to deal with. Same thing in SolidWorks – you just have to find a solution that works.

            I’d like to do a “best practice” kind of post for Solid Edge. The thing is, you can throw away about 70% of the “best practice” stuff you have to carry around in your head to make SolidWorks work. But there are still going to be things like “apply fillets last”. That is still going to be a best practice rule for me working in Solid Edge, whether I’m in synchronous or ordered.

          5. Ok Matt a best practices post sounds good. To me it seems a user should still approach their model in a ‘traditional’ way but make appropriate use of Synch to hasten progress and ease revisions but perhaps that is too conservative an appproach? Anyway looking forward to the next exciting installment…

  15. Looking at this and all the videos on YouTube I can see the theoretical benefits of ST, but, I honestly think for the type of work we do it is only going to help is a few very specific cases. The difficulty we have – the time consuming bit – is creating new geometry in the first place.

    Whilst I see that ST would be useful for modifying some (simpler) parts where you have large feature trees, or parts where your build has been so convoluted that the best option is to just export as a .xb and import again as a dumb part. The problem is most of the parts we need to edit are complex, curve driven surfaced parts.

    The equation for us is simple. Stick with what we know, what we are comfortable with and what works most of the time, or dip our toe in the water and (yet again) start running different CAD systems that are (on the surface) quite similar. In many respects, I am coming to the point of view that if we did want something else I would possibly prefer to opt for Spaceclaim – which is a lot less expensive even with the add ons for Translators.

    But nothing is decided yet. I am waiting for the call from SolidWorks to show me what is coming :-)

  16. I do smooth shapes that are defined by skeleton sketches. An airplane begins with an inboard profile sketch. This controls the locations of all components and is the outline at the center. The plan view is used combined with a widest point curve from the inboard profile. The smooth 3d shape is then defined as a conic surface that has some defined rho value. Is this possible in SE? Perhaps I could eftine it as a rectangular shape and do a conic fillet eliminating all of the square surfaces?

    My comments do not seem to post reliably from an ipad.

  17. Hi< doe anyone know if there is a similar command for solidworks as the "include" command in solid edge?
    I have an part that I am adding multiple holes to and want to make sure they are concentric with the mating part.


    1. Solid Edge “include” is like the Works command “convert entities” in sketch mode.

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