Solid Edge vs SolidWorks interface comparison

Just as a warning, there is a lot to say on this topic, and this is going to be a huge post. Maybe you should read it in chunks, but I”ll let you decide that. I”m not going to go all deelip on you and break it into 40 small posts. A lot of people argue that comparing SE to SW isn”t worth the time because of the installed base or lack of installed base. I don”t really care about that. I”m just interested in the tools. The more you look at the Solid Edge tool, the better it looks. I will be doing several of these posts comparing or discussing various aspects of Solid Edge.

The interfaces of Solid Edge ST3 and SolidWorks are different. There are elements that are similar, but when you work with them, you will not get the feeling that they are the same basic interface the way you might have many releases ago.  They started out almost indistinguishable many years ago, and then evolved on different trajectories. They are both Windows based, 3D CAD programs, but the philosophies of the interfaces seem to be somehow different. Solid Edge interface in general seems more compact and icon driven, while SolidWorks uses a lot more text and seems bulkier. In this post I want to compare the two interfaces, and give my impression of which is better in various cases. I obviously don”t know Solid Edge as well as I know SolidWorks, so I will tend to avoid saying anything really drastic unless I have confirmed that with someone more knowledgeable in the software.

Solid Edge has some nice interface bits, but it does not have Real View type capability, which Dan Staples confirmed for me. When you look at some of the other available functionality, you may not care about the shiny bits. Although SE does have some capabilities around shiny metallic materials, as you will see later in the evaluation, SE doesn”t really measure up to SW in this area.

There seem to be some differences between the interface when using Synchronous as opposed to ordered features. I have to say that the Synchronous interface makes tons more sense to me. I think the workflow for ordered features is more structured, and it is structured differently from SolidWorks, so I”m not quite comfortable with it yet.  This interface evaluation really doesn”t have anything at all to do with the push-pull direct edit side of ST3, because those bits are not available in SW for comparison (unless you consider Instant3D as an equivalent of ST3, which it sorta is, but not really).

If you think I am being harsher on SW than on SE, well, I am (but wait for the next post on SE surfacing). That”s because I know SW”s deficiencies much better than I know SE”s. Am I taking sides? Well, I”m trying to be fair, and when SE falls down, I won”t hesitate to call it like I see it, but when it comes down to it, SE is not the one falling down much in this comparison. That”s just the way I see it after having used the software that Siemens provided for this and other blog posts I”m writing. I”m not getting paid by either party for this comparison, and this will not be as one-eyed as the recent SolidWorks vs Inventor mess.

This is a comparison for SolidWorks users, like the rest of the blog, so I will not post side-by-side images of all of the interfaces, since I assume that readers are already familiar with the SW interface. I know a lot of people use this blog for purposes other than what I intend (SW competitors), but I don”t think I”m required to make your jobs easy. This is a blog for users, not for marketing.

Ribbon

Yes, Solid Edge has been afflicted with the much reviled ribbon. Although, I have to say, if you have to have the ribbon, this is not a bad way to go.

The ribbon, on top of being fully customizable, also works like the SolidWorks CommandManager. I know the CommandManager isn”t exactly 100% popular, but I like it, and it works for me. I”m sure I could make this work for me as well. The names at the top look like menus, but function like the tabs of the CommandManager, and below the ribbon is what SE calls the Quick Access bar where you can put anything you like. It looks to me that SE has banned the concept of conventional toolbars altogether, but you can use this Quick Access as a custom toolbar. You can”t show just a regular toolbar in addition to the ribbon, so when you are sketching stuff, you have to sketch, change ribbon, make a feature, change ribbon, sketch… very inefficient, unless you use the Quick Access as a sketch toolbar. Quick Access can be placed up in the title bar above the ribbon to save space or under the ribbon to make it easier to get to. Nice options.

One really nice thing is that you can minimize the ribbon so it doesn”t show up until you click on a tab. This saves space but ensures an extra click to access everything. SW doesn”t have an equivalent, unless you consider the F10 functionality which hides the toolbars to be equivalent (which it sorta is but not really).

I think it”s also a nice touch that the window controls are not taking up space inside the window. And the CommandManager tabs are not hanging down in the way of everything else. And the interface elements actually work. I mean it doesn”t look like SE thinks the interface is an afterthought, they don”t seem to think that if major portions of the interface don”t work, that that is some how ok. I have to say that all of the interface stuff I”ve used in Solid Edge seems to actually work, and at no point does it give an amateurish sort of feel.

Solid Edge also has flyout toolbar buttons for stuff like the rectangle, where there are several ways to create the rectangle, just like in SW.

Like the Microsoft ribbons, you access all of the stuff that goes on the “standard toolbar” by clicking on the Solid Edge icon in the upper left. It works well enough once you know about it, but I don”t think this is very intuitive interface design. Also like the Microsoft ribbon, you have tools and features in the same area, so you frequently find yourself covering over the tools you need to do something specific. With the ribbon, I think there is a lot more flipping back and forth between tabs, which is wasted energy in my opinion.

Sketching

Solid Edge does not seem to allow what old time SolidWorks users know as click-drag sketching. You must use click-click sketching. Which might be just as well, because Solid Works used to allow both, but now in some situations you can”t use one or the other, SolidWorks has become very inconsistent in this regard. Lacking functionality is certainly a fault, but inconsistency is a far worse fault.

When preparing to sketch on a face, there is an indicator of which edge any dimension text will be parallel to, and you can change this with the N hotkey. Interesting interface bit, not exactly something I find myself wishing for, but it”s there.

There are a number of ways to quit a sketch tool in SW, if say you are sketching a series of lines connected end-to-end. In SE, you can”t double click to end a sketch chain, but you can hit Esc or right click. Right click also works in SW, but you get the RMB menu. The nice thing about SE is that after right clicking to quit a sketch command, you can just start sketching another chain of lines. In SW if you hit Esc, it gets out of the sketch tool command altogether (turns off the line tool), but double clicking just interrupts it, and SE works the same way, replacing the right click for the double click.

SE is less rigid about the whole “which sketch are you editing” bit. This is all very confusing in SW. When I used to train a lot of beginner users, it was often a question whether you were “in or out of a sketch” and then beyond that, “which sketch were you in”? I”m having trouble describing it, but in SE, you just sketch, and you can sketch on this face, then on that face, and all of the sketch entities from sketches on other faces are still active and can be edited. It”s almost like you”re sketching in a 3D sketch in SW, but sketching on planes, except that everything still works. I guess what they have done is make your sketches solve as if there is no question of history between your sketches. Come to think of it, my part was in synchronous mode when I was doing this, so this is exactly what is going on. Hmmm. Ever get frustrated because you wanted to work on multiple sketches without having to flip back and forth between them? The only way to do that in SW is to use 3D sketches which are terribly unstable when it comes to relations and everything else. SE just seems to handle it beautifully. Ok, this is a huge out-classing of SW right here, just in case you were wondering.

This all reminds me of a failed function SolidWorks tried on a few releases ago, called Rapid Sketch. I don”t know if SW copied SE and decided the function sucked or if SE copied SW even though the function sucked. It allowed you to just start sketching immediately on whatever plane your cursor was over. The problem was that you couldn”t place the starting point of the sketch at an existing point like the origin, because it had to be on a plane, not a point. So if you were drawing a circle, you would have to place the circle out in space somewhere, then drag it to the origin. It decreased the number of clicks for some types of sketches in SW, but it increased others. Sketching in Synchronous mode seems to work like this, but it works much better, because you can at least sketch without needing to select a plane. You can hit F3 or click the lock icon to select the plane, and then start sketching from the origin or other point. This gives you the Rapid Sketch type functionality when you can use it, and the control of being able to start a circle or a line at a point. Again, SE solved this conceptual interface problem that SW seems to have just brushed aside.

Splines

Interesting thing about splines in SE, I don”t think you can get a 2 point spline. I use those frequently. Although, it looks like you can very easily change the degree of the spline. This may just be something similar to Simplify Spline, but with the added benefit that you can increase rather than just reduce the number of spline points. SE also appears to have an equivalent of the SW Proportional Spline, but I don”t see a conic equivalent (SW doesn”t have a conic either).

Dimension entry

SolidWorks has another function called Enable Onscreen Numeric Input which doesn”t work very well, and appears to be a very bad imitation of Solid Edge workflow for sketches. With SE you can key in numbers as you sketch, and it doesn”t look clunky or interrupt what you”re doing . In SW you can”t use click-drag sketching while using numeric input. This seems proof that SW copied it from SE, because SE only uses click-click, and when SW copied this data entry option, they copied the “can only use click-click sketching” thing as well.

Most of all, Solid Edge seems to understand about cursor focus and text entry, a very basic point of interface design. SolidWorks seems to be stubbornly opposed to anything so 20th century utilitarian as efficient numeric entry. Making reflective surfaces is much more important than entering numbers. After using Solid Edge for a little while, SolidWorks just seems difficult for the most basic of tasks, as if it is actively working against you. The Solid Edge interface is just more refined, and the workflow is more natural. That”s all there is to it.

Part of the reason for this sophisticated feel, I think is the Command Bar, shown below. This is a replacement for what SolidWorks users would call the PropertyManager. It is much more compact, more visual, and less in the way. Notice that it is horizontal instead of vertical like the PM. You can move this anywhere you like, but it snaps to the top by default. Best of all, there is no silly scrolling like you run into frequently in the SW PM interface.

To extrude a sketch region in SE, you just select it and pull on the handle that appears. This is very like Instant3D in SW if you have it turned on. While dragging the handle you can just key in a number. It just works, and it doesn”t get in the way. I think the SE folks understand workflow intuitively. It is possible that they didn”t hire PhD experts to tell them what should be intuitively obvious like another CAD company might have.

A nice little find in here is the Crown option, which is part of the Extrude feature. Crown allows you to create an extrude with curved sides. To create something equivalent in SW would require a sweep or loft, or an extrude and a couple of cuts. You could think of this as a curved draft, or draft with a radius instead of just an angle.

Open profiles

Solid Edge has some very nice functionality around open sketches. You can make open sketch cuts without worrying about if the sketch line goes past the edge or not. Fantastic function, especially if you are working in synchronous, and the “Best practice” of how you get there doesn”t matter, the geometrical result is the only thing that matters. You can add material as well as make cuts with open profiles, and you aren”t just limited to the SW “thin feature”.

Path Finder

The Path Finder is what SE calls SWs FeatureManager. The Path Finder is easier to manage…easier to move around, and has a transparent background so it seems less like a rigidly cordoned off rectangular area of the software and more like it just fits with the rest of what”s there. You can move it up and down the left hand side where it lives by default or you can move it around the SE window. Best, you can move it outside of the SE window onto a second monitor. Ok, this simply WAY outclasses anything SW has done in this regard. This is really useful stuff in terms of interface configuration.

Command Finder

Find commands without having to look through a lot of irrelevant crap

I want to mention the Command Finder. SolidWorks has the Help, which is sorta equivalent, but not really. With SolidWorks Help, I always wind up with tons of irrelevant junk, especially since they got rid of the index and started relying on search. Because Google relies on search to make billions of dollars, so Google must be a good model to base everything off of. Search makes everything better, no matter how crappy it turns out. Just think how good my great grandmothers corn pone would have been if she had been able to use Google. Solid Edge Command Finder gets right to the point. The Command Finder is down in the task bar area. Very handy for a novice like me. Plus, I understand that the SE Command Finder is programmed with names of functions from other software like SW, Inventor and Pro/E, er – creo elements/Pro. This is great because the one of the biggest obstacles to adopting new software is learning the terminology.

Apply options

The Solid Edge Options, equivalent to Tools, Options, has an Apply button. So you can see the effect of the change before exiting the dialog. It”s standard functionality, and very much missed from Solidworks for a long time. Warning, though, not all SE functions have an apply or preview option. But this one does, so make a happy face when you use it.

Display

Solid Edge has more anti-alias display options so you can set the level of anti-aliasing. SolidWorks has 3 options: none, edges and sketches, and full scene, but does not allow you to control the level. I noticed a couple of other areas where SE allowed you control over the quality of the display to affect performance.

The overall display between the two softwares leaves little doubt that this is an area that SolidWorks has concentrated on while Solid Edge was working on perfecting interface workflow and cursor focus. Here is a comparison of the batmobile I did. The black one is from SW, the silver one is from SE:

I used a setting which allowed SE to cast shadows on itself, which seems like the equivalent of the elusive but fun to say “ambient occlusion” in SolidWorks. Notice that there is a difference between the Drop Shadow and the Cast Shadows. Drop Shadow is under the item, Cast Shadows means inside the item. I also used a Reflections setting, as shown below. I applied an aluminum style from the Color Manager (yes, a manager in SE).

To be sure, the display options seem to have a much bigger range in SolidWorks. I also found the Cast Shadows setting to take an additional 2-3 seconds to process after changing the view in Solid Edge, so it was not dynamic. Without that, though, the reflections seem to work plenty fast, and while not quite up to the same range of possibilities as Real View, the SE stuff does look ok. The Part Painter functionality in SE is much easier to use than the Appearances stuff in SW, but again, it lacks a range of shiny stuff that SW seems to revel in. Aside from the metallic styles in SE, I was not able to get a really glossy painted color. So you have to make up your own mind on this. How much is the Real View stuff worth to you, when it comes right down to it?

By the way, the import of the batmobile model came through parasolid, and it worked ok, except that SE saw the multiple surface bodies as an assembly. The wheels were in SolidWorks as separate inserted parts (separate bodies), and also came into SE as assembly components. If you do a lot of multibody modeling, the transfer from SW to SE might be a bit of an issue, but again, I didn”t research this in any depth, so there might be some operator error issues here.

Summary

When it comes down to it, as long as this blog post is, it is still just a cursory look at the two interfaces in just a few areas. I”ve used SolidWorks for 15+ years, and Solid Edge for about that many hours. My final impression here is that Solid Edge has spent some time recently focusing on their product, and the scope of their product is much smaller than the scope of SolidWorks. Because of this, I think Solid Edge as a product shows much more attention to detail in the interface. The areas of the software I have worked with seem to have a more cohesive flow. Working with SolidWorks over the years, I detect areas of the software going in different directions, so the software is less cohesive. If I had to give a grade here, I would give SW 75% (mainly due to interface bits that have not worked for a couple of releases, and nothing is done about it) and SE 90% (mainly due to the better workflow and spatial management).

I welcome discussion on the topic. Please leave comments.

32 Replies to “Solid Edge vs SolidWorks interface comparison”

  1. @JES and Jery – Gentlemen – it is usually a fact that you are much more comfortable with your existing software. I can show you as many SW users that have swithched to SE and are enthralled with the ease of use. I certainly understand mindsets, I have a few of my own – but being an old “board guy” and never having used CAD (at least 3D) – I did a one year study to determine what product appeared to be best. At that time, SW had better sufracing, but SE handled much larger assemblies, had better sheet metal and the 2D side was far superior to SW (V7 SE) – and they owned both the “Parasolid geometry kernel” and the D-Cubed Constraint Manager. Since that time, it appears to me that the technical advantage and forward thinking has to go with UGS (now Siemens). Siemens could have purchased Dassault, PTC or UGS – and they made the choice for an obvious reason. Synchronous Technology is rapidly becoming the leader (you can tell this by the way everyone is trying to emulate it) – Imitation is said to be the “greatest form of flattery”. That aside, I anxiously await the “kernel change” and the “cloud” endeavors to see where Dassault is going with SW. I must admit that for purely “business reasons” – I was very sure I wanted to go with a company that “owned” and did not lease the technology that I considered the “engine’ and “transmission” under the hood.

  2. @JES I am trying SE after using SW for a couple of years, That is how I feel too. The interface is more like AutoCad and I have a hard time with that because of the click sequence. The “synchronous technology” is what drew me in but I am finding that it needs constraints to really work well. I do not dimension extensively because I change/tweak things so much it is faster not to. Any one else feel this way?

  3. Nice post!
    I’m using solid edge for past 5 years and it is awesome, but I found difficulties in drawing 3D curve when using Solid edge.

  4. escribo desde España. No se si podrán entenderme.

    El debate SW versus SE es para mi apasionante y complejo.

    Usé profesionalmente NX durante varios años.
    He practicado bastante con SW-2010 y 2011 y también con SE ST2.
    Actualmente trabajo en una empresa que usa SW.

    Reconozco que la tecnología ST supone una revolución en la forma de entender el diseño.
    Aporta gran flexibilidad en el manejo de la geometría, pero en mi caso, viene acompañado de cierta perdida del control sobre lo que queremos diseñar.

    Me gusta controlar lo que hago y saber exactamente los cambios que quiero producir en la geometría, y pienso que las reglas activas de SE ST aún no son la solución definitiva y tienen mucho que mejorar.

    Sigo de cerca la evolución de SE, pero de momento me siento más comodo diseñando con SW.
    SE se me hace muy incómodo manejando ensamblajes y sobre todo realizando diseño de piezas dentro de ensamblajes (descendente). Pienso que ahí SW gana por goleada.

    Con SE no se pueden dibujar dos solidos en contacto, dentro de un archivo de pieza.
    Estoy obligado a hacerlo en ensamblaje.
    Sin embargo con SW se hace sin problemas, igual que con NX.

    Aun reconociendo la gran transformación que esta haciendo SE, de momento me siento más cómodo trabajando con SW. Lo que pase en un futuro nadie lo sabe.

    Un saludo.

  5. I’ve run SW for years and am now running SE. Sorry to say but Solid Edge takes some of the simplest of things and makes them too user Un-friendly. Too many steps, and or you have to fight with it. I have a laundry list of problems with Solid Edge. No configurations within a part file, big time parts list problems, exploded view problems, too much manual updating, measuring works chaotic, custom scaling, relations, hatching, etc, etc, etc……the list goes on. Trust me RUN SOLIDWORKS it’s much more intuitive and you’ll keep your sanity.

  6. Great Post Matt !

    I have used both the systems in the last 9 years. Having used both, i believe SW is more user friendly, because Solid Works says so, their marketing says so, amusingly, even their sales guys say so.
    Arguably, i believe SE has more logical.

    Talking of Direct Modeling,
    Synch Tech in SE is indeed different from Instant 3d, which i believe can be compared to “Dynamic Edit” of SE which is about 6 yrs old in SE.

    It’s good to be passionate about a product one is using, however, from time to time, people just need to remove their glasses and genuinely evaluate. Many a myths will be shattered.

    Cheers !
    [img]http://www.dezignstuff.com/blog/wp-content/uploads/2010/12/SW Trained.JPG[/img]

  7. I’m afraid Solid Edge falls at the first fence for me – no multibodies – and therefore top down design becomes harder especially for large fabrications. Apart from that (compared to SolidWorks) it seems a bit clunky though this could be just because of my lack of experience with it. I appreciated the benefits of multibody modelling when I had to go back to ProEngineer to design a large 3000 feature casting having done similar on Catia V4 for the previous 3 years. When I started using SolidWorks it seemed to be the near perfect CAD package because it had this functionality and because it was so easy to use. Plus configurations seem to be so much easier to use (in both part and assembly) than equivalent functionality in ProEngineer (and from what I have seen in Solid Edge). However it is early days on SE so I am open minded – I have always found it better to play to the strengths of a particular software rather than try to work it like software I have used before.

    1. Solid Edge does have multibodies. It also has a special environment for weldments. This is not early days for SE, it is as old as SW.

      I have always found it better to play to the strengths of a particular software rather than try to work it like software I have used before.

      Yes, I’ll agree with that.

  8. Hi! I haven’t read all the comments so his onw might be rdundant but here goes:

    About the changing tabs in the menu thing, you know you can just scroll through it with your mouse’s scroll button as long as your mouse pointer is hovering over the ribbon? So no annoying clicking between tabs. It’s pretty intuitive. However, this doesn’t work if the ribbon is minimized…

    Also, I hadn’t even noticed that you can move the Path Finder outside the interface onto a second monitor… This’ll help a lot!

  9. I just want to know if I can open a SE files in SW or SW files in SE? Do you think I need to change the extentions? Do you have another way to do so?

  10. Wow, Matt, you really railed that interface hard.
    Good work. You know, you hear the attitude from vendors that 3D CAD is a known quantity and that what users really need are not new features but only cloud computing and SAS. Keep them honest. Last thing we need is SW turning into Autodesk.

  11. @Solid DNA

    Update on previous command

    There is another command you could try in your exploration. This command was implement way before pen enable device. Most of the SE users probably do not know it is there.

    It was remove in synchcronous mode.

    Using it with the mouse is a bit tedious, but with a pen device it could be easier to work with.

    The command could probably benefit from an update to catch up on those new pen device.

    In traditional mode, when you start a sketch, under the line command, you will find Freesketch

    [img]http://www.dezignstuff.com/blog/wp-content/uploads/2010/11/freesketch01.png[/img]

    [img]http://www.dezignstuff.com/blog/wp-content/uploads/2010/11/freesketch02.png[/img]

    Once the command is launch, you can draw like if you had a pen in your hand. Just press the Right Mouse Button to lower the pen.

    Reason i mention this, is you start your review by saying

    “…They started out almost indistinguishable many years ago, and then evolved on different trajectories….”

    And little bit further

    “..Solid Edge does not seem to allow what old time SolidWorks users know as click-drag sketching….

    I guess this is one of those evolution where a branch was create.

  12. Matt

    About the 2 points spline, the way i understand it, you need a starting point and end point and maybe a third one to help control the curvature.

    A two point spline would be closer to an arc.

    So create an arc, then in the same group, click the “Convert to curve”

    [img]http://www.dezignstuff.com/blog/wp-content/uploads/2010/11/Contocurve.png[/img]

    Clicking the arc will then convert it to a 2 points spline ( what i think is closer to what you are looking for).

    [img]http://www.dezignstuff.com/blog/wp-content/uploads/2010/11/Contocurve01.png[/img]

    Convert to curve allow us to start a sketch with primitive 2D elements and tweak them if need.

    The technique Jon recommand work also when you create arc circle and rectangle. As an example, when creating an arc, click and drag ( similar as when you use a pen). You will have a hand draw line preview, when relasing the mosue cursor, Solid Edge will interpret and create and arc that match the preview. If you have a pen enable device (Tablet pc or wacom) that could be interesting to review.

    [img]http://www.dezignstuff.com/blog/wp-content/uploads/2010/11/Contocurve02.png[/img]

  13. @Mark
    Yes, I’m curious about the separate windows comment as well???

    And pertaining to the SE users who left because they were annoyed by the introduction of a new, separate environment that was optional to use along side the existing one. I’m kind of confused by that one as well. We have been using ST1 and ST2 in Traditional mode which allows us to use the same modelling workflows we had been using in V20 and every release prior to that. Even with ST3, we still have the choice of using the same modelling workflows we had been using.

  14. @matt
    Yes, also possible to add and remove control points on existing curves. Simply select the curve… Then hold down the “Alt” key and select an existing point to remove it or select anywhere else on the curve to add a new control point.
    SE also has the option to edit the curve in 2 ways – local edit (moves the edit point or control polygon locally) or shape edit (tries to maintain overall shape). You can toggle the option in the command ribbon whilst the curve is selected.
    Have fun
    Jon

  15. @matt
    Hi Matt, no problem.
    If you are in the synchronous mode of the model (which I guess you are), you need to make sure you lock to a face first with either “F3” or by selecting the lock symbol. Then you will be able to use the click and drag method.

    The curve will run from the point you clicked to the point you let go… Its shape will follow whatever shape you made with the cursor along the way. The only 2 edit points on the curve will be one at the start and one at the end.

    Hope that helps
    Regards
    Jon

  16. @Mark
    @Cadjunkie
    @Quin
    Yes, you guys are right about the icon that pops up allowing you to make the cut a boss. I missed that one. Sorry. I’ll fix it in the text.

    Mark, I’ll be talking about direct edit functionality later.

    ST is completely avoidable in ST1, ST2 and ST3. I have not yet begun to talk about ST3, aside from the article a few weeks ago. All I’ve done so far is talk about history-free sketching. I’d be glad to hear what you have to say about that.

    What separate windows are you talking about? The point of the article is to compare interfaces, I thought that much was clear.

    @Kevin De Smet

    I don’t think that is part of the way this works.

    @Jon Sutcliffe
    I’m unable to get that to work. If I click the first point, then click-drag the second point, then hit Esc, I still get a 3 pt spline. Can you be more specific? I’d love this to work.

  17. The crown feature is one I have always wished SolidWorks had. I like single features that intelligently incorporate multiple options in one hit. I think crown was originally developed for plastic moulding design of more functional parts where you might have a heavier texture – increasing the draft angle with depth. I would use that.

  18. Matt,

    I look forward to more post. There are very few people lifting the skirt behind these programs a really doing a side by side.

    Side note, “SE has a manual override for this automatic option. In SW there is no option, just automatic stuff that might give you something you don’t want and can’t control.” The instant 3D should give an pop up icon that switches it from a cut to a base extrude. In this same box is the ability to add draft as well.

    It’d be nice if the sketch didn’t have to be exited in SW just to get the arrow for the instant 3D to work. Is this the same in SE?

  19. Crown looks interesting, but if it’s a constant radius maybe not so much. Can crown increase curvature near the ends of a surface only – like the way I’d imagine crown to be?

  20. dragging the sketch through the solid automatically results in a cut. SE has a manual override for this automatic option. In SW there is no option, just automatic stuff that might give you something you don’t want and can’t control.”

    In fact SW does offer you the option to create an extrude instead of a cut just wait for the pop up to show,

  21. I got half way through your write up and noticed a couple of things which are simply incorrect. You said SW is unable to do an extrude through a solid without it cutting, not true. There is a pop up which changes it to solid, or you can grab the sketch outside of the face if possible. Apart from you saying “which is sorta equivalent, but not really” far too much, Instant3D is not designed to be equivalent to ST. If you want a more comparable tool it would be Move Face. Or in fact anything on the Direct Editing tab in the SW Command Manager. Considering you’ve been using SW for 15+ years, your SW knowledge seems quite limited. Did you write this after having a bad day? SynchTech has annoyed many SE users to the point they have switched to SW. I have used both and SE looks mickey mouse and the separate windows are archaic. I really don’t see the point in this article.

  22. Hi Matt, great post.
    Maybe I can help out on the spline side of things. If you want a 2 point spline, just click and drag when you are in the spline command. This should give you what you need.
    Best Regards
    Jon

  23. This is very interesting. I have been following the development of Solid Edge with synch tech for a while and this is a cool post. You mention that Solid Edge does not have conic sections just like SolidWorks. Could this be because conic sections with rho control are available in the more expensive NX? Obviously the technology is available to Solid Edge.

    Despite the fact that Solid Edge might be a great tool, it will be hard to get people to switch. If I look at myself, I have thousands of dollars invested in SWX premium and am not likely to invest thousands of dollars in a package that has similar functionality. If they continue to work on synch tech and add funcionality that is not available in SWX there might be a tipping point, but I’m not sure where that would be.

  24. Awesome Matty! Great write up. Spending a long time in one tool, is like wearing a cage in front of our face… after a while we stop seeing the bars and look beyond those obstructions. Using another tool can open our eyes to other ways, better ways to skin the same cat. Looking forward to more on this topic. Thanks…

  25. very nice article. thank you. ability to work with multiple sketches at the same time is interesting.higher degree splines are cool if it allows higher continuity level that G2.

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