Solid Edge vs SolidWorks surfacing comparison

This is a comparison of the tools in  SolidWorks and Solid Edge for advanced surface modeling work. This is the type of work that I do most in my day job. I’m learning the SolidEdge tools as I go, so there is some definite inequity built into the comparison, but I’ll do my best to be fair. Dan Staples (director of development at SE) helped me a little with some facts.

The tools

Solid Edge surfacing tools

BlueSurf is roughly equivalent to the SolidWorks Boundary. The SE Help references a Loft feature, but I can’t find it in theinterface (there is a solid loft, but no surface loft). The SE Swept surface actually sounds like the SW Loft to me, since it allows multiple cross sections, but is limited to 3 paths. SE does not have a Planar surface type, but the Bounded looks to be able to do that. The SE Bounded surface would be roughly equivalent to the SW Fill. The BlueDot is something that is clearly beyond what SolidWorks is capable of, and to me seems to be bringing the Synchronous type of functionality to the ordered feature side of the software. And if other CAD companies wanted to copy something from Solid Edge, the BlueDot would be my choice.

SolidWorks surfacing tools

The main things missing from the Solid Edge tools are the ruled surface and untrim. Well, that and Freeform, but Freeform in SW has enough drawbacks that you might not consider it to be much of an advantage. When it comes down to it, SE BlueSurf mostly covers Ruled and Freeform. Delete Face exists, but it appears to work only on solids, and only works with the heal option enabled, which is not exactly a surface-friendly way of operating.

First of all, working with complex shapes in Synchronous mode is kind of a “create-only” adventure, since Solid Edge does not have the capabilities to edit complex general NURBS. So you have to use ordered (history based) modeling when working with complex surfaces. This takes away the most  attractive part of SE ST3 right out of the gate.

Splines

What SolidWorkscalls splines, SE calls curves. Same thing. The quality and control of complex shapes rests in part on the quality and control of your splines.

A Solid Edge user corrected me in my last post. You actually can create a 2 pt spline in SE. Click-drag (in a freehand sort of drag) the shape you want, and you get a spline with just 2 control points – one at each end. But then the discussion turns to the control polygon. When you create a spline in SE using the click-drag method, you only get 2 points, but you get a control polygon with 4 total points.

In SW, a 2 pt spline can only be U or S shaped, and the S shape only comes with tangency (or handles) applied to both ends. In SE, the long squiggle (3rd down on the right) is a 2 pt spline. You can get SE to give you a SW-looking and acting 2 pt spline (top 2 on the right) by creating a 3 pt spline and deleting a pt. There are cases where the control polygon of 2 pt splines in both SW and SE have 4 points on the control polygon, but this depends on if you fiddle with the handles in SW, or the method you use to create it in SE.

In the end, I can get the SE splines to do almost everything I can get a SW spline to do. The one exception is that I can’t find a c2 sketch relationship in SE, which is a big deal, but it may be the only big deal. SE doesn’t have the handles, but the type of control the handle gives you is duplicated in the control polygon.

BlueSurf

The SE Help’s description of the BlueSurf makes it sound essentially like the SW Boundary. It can use all of the different input curve arrangements like Boundary, and it can apply curvature continuity across both directions. There are a couple of differences, though. First the BlueSurf does not seem to treat direction 1 and dir2 the same. There are additional conditions available on dir1. I can’t really tell quickly if this is good or bad, there are just additional options. Second, the weighting handles for tangency in a given direction are easier to use than the SW Boundary and Loft handles.

In practice, I tried a fairly simple surface with a section trimmed out of the middle, and then used BlueSurf to rebuild the missing section. The result is shown above. I tried to apply c2 all the way around, but it failed. So I was able to get it to work with a single side using c2, and even this put some serious creases down the face. It worked ok with the tangent on 4 sides, but the result was not as smooth as you might hope for.

To the right is the dialog with the BlueSurf options. I’m guessing that the end capping is for capping closed loop profiles, which would be a nice touch when needed. It is also nice to be able to see the tolerance being used for your sketches. Controlling this can be a dangerous thing, but knowing what it is can be valuable.

Solid Edge is able to save out surfaces, but you have to edit the default options to get them to go. Solid Edge considers multiple bodies and surfaces to be construction entities, which is OK, it’s just something you have to be aware of and prepared for. The Options box is on the Save As dialog, just like SolidWorks. SE ST3 can save to up to Parasolid 23.0, SolidWorks2011 to Parasolid 22.0.

SW Boundary with no creases and 4 sides c2

Once in SolidWorks, I copied the face with a 0 distance offset, then made the boundary surface with c2 on all 4 sides, without any creases or failures. There was no fussing around to make it right.

Here’s something that SolidWorks cannot do. You know how SolidWorks can loft to a point, right? That’s great, and sometimes you need that. BlueSurf can do that too, along with the tangency end condition to make it round at the end (here is a video clip from Dan Staples showing this technique). But what happens when you want to loft say a circle to a line, to make a chisel point or something like that? Well,SolidWorks just doesn’t do that directly, so you have to manually cobb it together to make it work. Well, guess what. Solid Edge BlueSurf can loft from a closed profile to an open profile other than a point. In the case shown to the right, there is a rectangle lofting to a line.

Here’s another plus for Solid Edge. SE BlueSurf enables you to start or end a loft parallel to the sketch profile. SW won’t do that. So SE BlueSurf can come in tangent to the sketch plane. This is a nice option that SW doesn’t give you.

Solid Edge seems to have no previews for end condition/tangency settings. You have to set the setting, and hit OK. Any change you have to go back to the options dialog, make the change and pray. That’s not so nice.

And there’s more. The Advanced tab in the BlueSurf Options is home to the Vertex Mapping. This is what we in SolidWorks call Connectors. It seems that with BlueSurf, you have to have existing endpoints in order for this to work. In SolidWorks of course, we just make a connector and move it around even between endpoints of profile elements.

Digging more into the BlueSurf seems pointless. It becomes clear that Solid Edge is a solid modeler with some surfacing features, but doesn’t have a lot of horsepower compared to SW. SolidWorks has most of the tools needed for real surface modeling, and while they don’t work all of the time, you will get more surface modeling done with SW than with SE.

I sent Dan Staples an early draft of this post, looking for some of his comments and corrections, and he added some information which will give you much needed clarification.

First, the BlueSurf is meant to be a kind of everything sort of tool. It superseded the Loft surface, which is why there is no Loft surface in Solid Edge. (SolidWorks intended to obsolete the Loft as well, but there were a couple of functions in Loft that Boundary cannot do).

One thing BlueSurf can do that SW Boundary cannot is add profiles in both directions. Boundary can’t even do this in one direction, but Loft can. Still, if you use BlueSurf, then add sections, and put BlueDots between the curves, you’ve suddenly got a nice mesh you can work with without worrying about sketch order. This is nice. A definite plus for Solid Edge. Here is a link to a little video clip Dan sent. This actually addresses the Freeform surface functionality in SolidWorks as well.

Dan says that you can also do Ruled surfaces with the BlueSurf, which you can, but… well,  the SE BlueSurf doesn’t have all of the SW Ruled functionality built in. In the SW Ruled surface, one direction is always a straight line, so the feature does that for you. You just provide the other direction and some settings.

The Centerline Loft in SolidWorks is covered by the Sweep in Solid Edge, because it Sweep uses multiple profiles.

The BlueDot

The BlueDot is a way to tell Solid Edge to solve sketches without regard to sketch order. It is simply a blue dot that you put at the intersection of two sketches.  Of course you can avoid the BlueDot altogether by sketching in Synchronous mode. I think the more people use this, the more important this is going to become. Even if you don’t believe in history-free modeling, I have not yet found anything to dislike about history free sketching. History free sketching may turn out to be one of the best parts of SE ST3 that no one really talks about, and no one really understands until they use it. SolidWorks has tried something similar with the push to 3D sketches a few years ago, but they were not able to make 3D sketches work reliably enough. I thought that SW was actually going to eliminate 2D sketches just because of all of the development they were putting into making 3D sketches work like 2D sketches back in say 2007. But it never happened. It’s hard to say why they didn’t keep going with the idea. Eliminating sketch history would be huge. Wonder if anyone is going to realize the little gem SE has here?

Anyway. To describe the BlueDot, I’m just going to rely on the SE Help:

The SE Help, by the way, is much superior to the SW Help. Not that it would take much, but that’s how I see things. SE Help still has an Index, so if I know what I’m looking for, I can be sure to find it. All Search does is give you a pile of irrelevant information. SW relies 100% on Search.

Bounded

The Fill surface in SolidWorks is one of my absolute favorites. The SE Bounded surface works in some ways similar to Fill. It is the n-sided patch. It is my understanding that the Fill surface is a function that comes from Catia, not from Parasolid. It isn’t clear to me why SolidWorks would choose to go to this extra bother, but the functionality delivered by this little portion of the Catia kernel must have delivered more power than what Parasolid offered. The main difference between Bounded and Fill is that the only edge condition available in Bounded is Tangent. No c2. While the surface created by the Bounded surface feature in the jagged boundary I trimmed out of this revolved spline looks pretty good, it is still a limited case. Sometimes you need c2. Another complaint about Bounded is that the only mass edge selection method appears to be box select. It works, but you have to have just the right geometry to make it work effectively. SW of course has the RMB options Select Tangency and Select Open Loop.

Trim

Solid Edge does not appear to have a mutual trim feature. Without this, you are going to have a lot of tedious work to get some sets of surfaces trimmed correctly. Solid Edge uses an arrow display to show the portion of the surface to be kept and which to discard, which is clearer than colored faces for simple trims, but is probably not workable for very complex mutual trims. It also appears that you cannot trim with a sketch.  It looks like you have to first project the sketch onto the surface, and then use the projected curve to trim. Alternatively you could extrude the sketch as a surface and use one surface to trim the other.

The other trim functionality that is missing is untrim. Life without untrim would be full of painful workarounds.

Fillets

SolidWorks has very powerful filleting, but mostly because of the power of the Parasolid kernel.  SolidWorks has these kinds of fillets:

  • face fillets
  • single and double hold line fillets
  • full round fillets
  • variable radius fillets
  • setback fillets
  • multiple radius fillets
  • constant width fillets

It’s not surprising, then that SE’s fillets should be in the same league as SW’s. Solid Edge does have fillets with conic section shape (called a blend), which is nice and something SolidWorks does not have. Solid Edge allows the scroll wheel to control the fillet radius, giving you an effective option to find the largest functional radius value fairly easily (SW has a nice radius control with Instant3D).  The options for fillet overflow that are rather obscure in SolidWorks are much more accessible in Solid Edge, but in some cases are also obscure. Solid Edge has Setback (suitcase corner) fillets and Tangent Hold line blends, which you might not find if you’re a noob like me – Dan had to point them out. Solid Edge’s advantages are more in the practical vein, so I would argue that there is some offset there in SE’s favor.

setback fillets

Tangent Hold Line fillet

Summary

While I didn’t go into complete depth on any of the features, to me it seems that the SE surfacing tools in most cases are almost equivalent to their mates in SolidWorks. I’d estimate that SE has about 87% of the functionality of SW when it comes to surfacing work. There are some offsets, though, because SE does a fair number of fairly major things that SW does not (add profiles to BlueSurf, loft open to closed, BlueDot, mix Synchronous sketches with ordered features, version ahead in Parasolid). Mutual trim, sketch trim, untrim, etc. while all secondary tools, are missing, and are still important to the overall package.  I’ll bet if you learned to do surfacing in SE, you might not ever miss what SW has.

17 Replies to “Solid Edge vs SolidWorks surfacing comparison”

  1. Matt, you can delete faces on a surface. The heal option is there exclusively for surfaces and can only be toggled when surface faces have been selected. I’m not sure what you’re doing wrong. The heal option is set to on when you are selecting a face on the body because if it wasn’t turned on, you wouldn’t have a solid anymore!

  2. Last year I designed injection molding plastic products on SE requiring a lot of complex surfacing features. I came to realize SE’s shortcomings in this regard. Building tools are somewhat OK, it’s the checking tools that are lacking and based on what you’ve shown off in your blog, I found myself wishing for SW features a few times. Problem is, the SE development team has not added anything to the surfacing tools like since V14, 7 or 8 years ago.

    My conclusion is that for product design and “freeform” plastic parts, SE is not up to par compared to SW. Plus since it’s not as popular as SW, it’s not working well with third-party software like KeyShot or Bunkspeed Shot (formerly Hypershot).

    BTW I want to thank you for your series on SE, and your fair and balanced review of the software. I’ve known too many SW aficionados trashing SE without a second thought. Keep it up!

  3. I use the extend surface mostly as a work around for the projected curves poor accuracy. The huge problem I have with Solidworks surfacing is a small change on one surface can break dozens of trims and fillets. Mutual trim is very nice but not reliable. Solidworks should recognize that many surface operations do not need to force the order of the feature tree. Untrim is nice, but scary, I prefer to make two identical surface features.

    Fillets between knit surfaces is rather flaky in Solidworks. I am usually filleting along an edge that was a surface trim. A regular fillet should work, but a face fillet is required and has all of the arrows mixed up.

    At the end of the day Solidworks usually allows me to create the desired geometry.

  4. @Jeff Mowry
    Sorry, didn’t see the question down at the bottom… too much going on here.

    If you have a Synchronous complex face, it would work just like if you had an imported surface body in SolidWorks and had trimmed it into or replaced face to get it into a block. You could move the face (translate/rotate) and maybe even scale, but you wouldn’t be able to alter its shape directly.

    I understand NX is the place to go for that kind of work.

  5. Oops—I just noticed my question above was worded incorrectly, and now it’s past the edit date. What I meant to say was, “If I have a swoopy surface on one side of a cube, what can I do with that in ST3?” Can that be modified, and if so, how?

  6. @Eric
    Curvature Continuous is not the same as a conic. The conic blend in Solid Edge will be a true “rho conic” which means it will be a conic section (hyperbola, parabola, etc) and the Rho value affects how much the radius is “pushed into the corner”. As I recall, a rho of .5 is an arc and any other value varies from hyperbola to parabolic. They can provide very nice looking blends, but also in some applications the rho value is important for other reasons.

  7. Thanks, Matt—this is exactly what I’ve been waiting to see.

    Frankly, SE has more capability here than I expected. If SolidWorks could keep surfacing features (such as Mutual and regular Trims) stable—particularly between SW versions—they’d really have some much stronger surfacing tools than anyone else I’ve seen at this level of CAD tools. As it is now, every time I bump a project up a version I’ve got headaches to solve on the order of hundreds of features because of these instability issues with certain surfacing features (seems to commonly forget which sides of Mutual Trims to keep/discard and crash everything downstream).

    How might an imported surface/solid be manipulated with the surfacing tools? If I have a swoopy surface on one side of a curve, what can I do with that in ST3?

  8. While I’m not happy with SW’s fillet creating options, I will say that you can create a conic fillet in SW. It is limited to the Face Fillet feature and you have to select it in the Options area of the feature, but it is there as “curvature continuous”. Maybe not the true “conic” as not all conics are curvature continuous. I wish that all the options available in the Face Fillet feature were available to other types of fillets.

  9. Matt

    I wonder if the G2 you talk could not be achive using the tangent constraint at the sketch level

    [img]http://www.dezignstuff.com/blog/wp-content/uploads/2010/11/Tangent_01.png[/img]

  10. Thanks for the informative post Matt. I would however, like to defend my lame videos as “only intended to clarify a few points for Matt” and not really of public-facing quality. No problem posting them, but they do represent “5 minutes of Dan messing around at a break from his day job” 🙂 and little more. I guess if they help clarify, that is all that matters. Thanks again for taking an interest in Solid Edge. I look forward to more…

  11. Thanks for this Matt very interesting. All I’ll say though that reading this I’ll stick to SolidWorks.

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