How feature-based modeling influences shape

The kind of things I’m working on lately are all surfaced on the outside, and all shelled, ribbed and bossed on the inside. Recent projects have included sports equipment, and an industrial handle. I can’t show the entire model for either project, but here are some images of the interesting areas. Both parts had the same approximate workflow, and the same problems. Getting the outside shape about 90% of the way there is relatively easy after years of experience of pushing this software. On parts this simple, the problems usually come from just one area, and usually a comparatively simple area at that.

On the sports equipment model, I was trying to use features to model over mesh data created in Zbrush. Just for reference, Zbrush lets you do insane stuff like this. It’s not product modeling, and it’s not CAD, it’s just insane 3D mesh. Mesh modelers don’t have the limitations of needing to break the shape up into artificial “features”. So trying to match the shape with features that was originally created with mesh was a little different. It’s like going to Southern Indiana and trying to fit in with their accent without sounding like you’re from Western Kentucky. In one area, I had to cut a section out and model it using another method to get the same shape using features that the original mesh data had. This is the “hack and whack” school.

The end product on the left looks ok, but when you see how I got there on the right, it’s a bit ugly. The edges represent what I had to do to get the shape correct. There were conflicts between using fillets and splines or boundary surface to smooth out an area, and sometimes the boundary surface could not be coerced to give the proper shape through 100% of the feature, which accounts for the elliptical patches on the right.

After the outside was done, the part had to be split in two and shelled in sections. I had two areas that could be shelled automatically (with the shell feature), but the middle section had to be shelled manually, and then the three sections joined. Shelling a part like this can take an 8 hour project and turn it into a 3 day curse fest. I don’t feel good handing over a model like this to the customer, but it is the price you pay for not using software that is intended for this kind of work. Using SolidWorks for this stuff is agonizing. Even finding the area of the model causing the shell to fail can add an hour to a project, especially when rebuild times for complex features is accounted for.

In the industrial handle project, I was reverse modeling from a combination of plastic parts and fully dimensioned autocad drawings. It always amazes me how clean things are in 2D drawings, especially when what is depicted is completely impossible in 3D. Anyway, I was thankful for the drawings because they give me the opportunity to make a 3D model much closer to the actual part, but there is nothing like a 2D drawing for imposing an artificial feature set on a model. In the end, I wound up fighting the software to make a couple of shapes, and especially fought false changes, where every now and then 90% of the model would just erupt in a sea of red marks in the tree.

Once the shape was created, the feature history was doing me no good, in fact, it was causing problems by failing randomly. This is why the “Feature Freeze” in SolidWorks 2012 is so important. It essentially begins to compensate for some of the implementation problems of SolidWorks tree management. But this customer specified SW2011. Bummer.

The problems I ran into with both of these projects are directly related to feature-based modeling scheme. Shapes are not always easily broken into areas appropriate for specific features. Very often in product design work, you need direct control over the shape. Fiddling with sketches and feature settings is indirect control at best.

Ed's marked up bottle, showing the flow of faces
Ed's SolidWorks model, edges showing features

To the left is a picture taken from Ed Eaton’s Curvy Stuff 201 powerpoint presentation. Just for reference, it was presented at SWWorld 2004, so the model was made in SolidWorks 2004 at the latest. This is the best illustration of the difficulty of using a feature-based model to make a general complex shape that I have seen. Ed took a physical bottle and marked it up with a marker to determine the flow of various areas of shape. This is important with NURBS modelers because all of the faces are essentially a mesh of curves that want to be perpendicular to one another. Ed is trying to represent the 2 directional mesh of the NURBS data using the marker lines. What he’s really doing here is establishing which areas would be made using different features.

Matt's try at the same bottle, with different feature breaks

To the upper right is Ed’s modeled bottle. The edges represent each feature. I made a version of the same bottle, working through Ed’s exercise, and came up with a somewhat different feature set, shown to the right. You can see I didn’t round off the sharp edge going around the bottle. Looking at it now, after 7 years, there are some things I would do differently, but it serves as an example of how different feature breaks on a model can subtly (or not so subtly) change the character of a product’s shape.

The importance of “going with the flow” is that if you have an edge that goes through a face at an angle to the NURBS mesh, that edge is going to look smeared, or like it has actual woven fabric going over it at an angle.

Below is an exaggerated surface showing this effect. It is a boundary surface with 6 splines. The splines have a peak that moves from left to right in each successive sketch, going front to back. The pink and blue lines are the U-V 2 directional mesh, and notice that the peaks in each spline want to follow the blue lines, not the artificial edge we are trying to produce by having a moving row of peaks. This sends little creases down the surface where you don’t want them. Just so it’s clear, this is highly undesirable.

There are two ways to get rid of this effect. One is to line up the U-V direction with the line of peaks, so effectively turning your planes and sketches by 45 deg.  The other way would be to use a connector in the boundary surface to connect the dots between the peaks. This rearranges the U-V mesh. It could cause other problems too, like scrunching up the U-V mesh in the upper right corner, and stretching it out in the upper left corner. The connector is the row of pink dots that go across the surface in the image below along the peaks in the splines.

You never want your modeler to drive the kinds of shapes you can make, but when you’re doing NURBS modeling, and we all are, you just can’t avoid it. Your choice of features can have a very negative effect on the shape outcome. And sometimes the available techniques limit the kinds of control you can have over shape. Mastering this kind of control over shape takes a lot of practice, and more than anything, a lot of failure.

To me, this is why real product design requires direct U-V push and pull (direct edit) capabilities in addition to feature-based tools. You often just can’t get there with straight feature-based tools. What kind of tools am I talking about ? Tsplines is one you can get to play with your SolidWorks data. I keep mentioning other tools like SolidThinking and Siemens NX for this kind of work as well.

If you are interested in the model used to make the last two images, you can download it here (280 kb – SW2011 format). It uses configurations to show both examples.

41 Replies to “How feature-based modeling influences shape”

  1. No, come on, you are twisting stats to suit yourself. You moved from quarters to halves without blinking there.
    Hidden in there is the revelation that sales are consistently scraping along the bottom at about 1.9-2.5% which is on par with natural global growth which is pretty poor going. No wonder DS want to replace it, capture their customers and kill piracy.
    Actually by your own figures the last quarter was down on the previous 24021-11748= 12273. So last quarter was down 4.3% on the one before.
    You also flipped from talking about SW to all DS products in the same paragraph.
    As I seem to remember from the last financial reports a good deal of recent SW sales action is from simulation products not seats. Following on some fairly steep declines in seat sales in the order of 26% which you previously quoted as 19% I am not sure the figures you quote are even correct.
    I think you should go away and come back when the thread is about damn lies and statistics.
    In the mean time cash up your shares and buy physical gold and silver and wait for the real meltdown.
    Not too far away now.
    I cant promise not to talk too loudly to prospective new customers about how their shiny purchase is going to be redundant soon and that while the software has been quite good it is going nowhere these days.
    I already determined SE isn’t suited to my particular need. Thanks for giving them a plug though. I am sure they will make use of your recommendation in their sales blurb. ‘SW insider says buy SE’.
    OK so back on topic…..

  2. @Neil

    First half sales were up 22% from the previous period to 24,021 seats. Across all Dassault products revenue from maintenance was up 19%. And all of this when there are fears of another GFC.

    I’m sure that you can find some numbers to try and substantiate your position… the Arctic’s polar ice cap is melting at a rate of 9% per decade so there’s almost another percent for your equations… only another 15 to 20% and you’re there!

    It couldn’t be that SolidWorks is great software and companies see that and buy it because it adds value to their business?

    BTW… I thought you were going to swap software… why not try Solid Edge Design1… only $19.95/month!

  3. Btw just out of general interest I note from wikipedia that the world population grows by an average of 1.1% pa and that world gdp growth varied from about 16% down to 2.5% for the top 123 countries and the global average is 3% or so. Even Guatemala managed 2.6%. Bearing that in mind its kind of hard to know how to interpret a 2.5% growth in new SW sales. 11748 sounds good at first hearing. It doesn’t necessarily follow that is sustained in consecutive quarters though and nor does it tell you anything about the numbers or trends in upgrades. To me the figure seems kind of flat or possibly even negative in light of the bigger picture but then you probably expect that for a variety of reasons.
    I guess a sale is a sale….

  4. Hmmm is that Matthew 1,2 or is this a third corporate minder?
    Really i dont know why you guys hang out there and obsess about things like this.
    Why not contribute something relevant to the actual discussion? Maybe you don’t use SW or Tsplines and just want to make a PR statement…
    OK well 10,000 in a quarter doesn’t seem very impressive when taken as a percentage of total SW seats claimed- is that about 2.5 % growth pa?
    Not exactly flying of the shelves is it but then its a mature product or rather in run out phase.
    I don’t know how that % equates to Tspline sales specifically (no doubt you can quote some figure although it isn’t your business) but I suppose DS will be happy to take the money and run regardless. Not a lot of honesty in the corporate world these days is there…
    Did they even tell Tsplines folk SW is about out of gas and they are helping to keep the dream alive until SWv6 makes it obsolete? Probably not. DS haven’t actually owned up to their customers about the ‘killing’ of SW yet officially I believe…wonder if they ever will..
    At least I was sincere with my contribution here about Tsplines present shortcomings.
    They might consider what I had to say when evaluating what to do to improve things.
    Any changes they introduce could just as well benefit any other Tsplines user though whether it be in conjunction with Rhino or some CAD vendor picking up on the SDK. Doesn’t have to be SW of course. I am sure the Tsplines folk will be just as happy to sell to SE users or Inventor users or who ever. Possibly their core business comes from Rhino users presently?
    Tsplines might like to consider where their long term interests lie which is what I am sure many SW users are doing despite the past success of SW. The dream run SW have had most conspicuously before DS started calling the shots could well end as a nightmare with the cloud. That n!Fuze thing was pretty much a fail. I wonder how sales of that are going -10,000 per quarter? Do you know? Hopefully the numbers are not something other MCAD vendors can only laugh at.
    All said and done Matthew its probably better to try to stick with the thread topic which wasn’t about SW sales but thanks for the random post anyway. Matt seems to be having a wee break at the moment and things have gone fairly quiet.
    Perhaps seeing as you seem to be involved with DS in some way you could give someone a poke about getting out some SWv6 details to anxious customers before it becomes a lost cause.

  5. @Neil

    With 11,748 new seats over the last quarter and you don’t think it’s worth developing tsplines for SolidWorks?? These are numbers the other MCAD systems only dream of.

  6. Because SW is almost in the grave I wouldn’t spend too much time on improving tSplines specifically for it.
    However if you want to better it for engineers use it doesn’t need to be more intuitive its needs to be more precise and analytic.
    Intuitive in SW terms inevitably means dumbed down, poorly documented and feature incomplete or having frustratingly inaccessible variables and lacking useful relations to other sketches or geometry and exacting control.
    This is exactly what we don’t want. SW have a fetish for this less is more stuff as being a substitute and excuse for things not done properly or things they don’t want to revisit to improve. Thinking users have a constant battle with SW to do things that really benefit them rather than look cool in the coders opinion and make a marketing bullet point.
    If you can augment the workflow such that the desired shapes are more deliberately articulated ie more mathematical and held fair over specific areas with edits rather than somewhat indeterminant in outcome and being waterbed like that would be appreciated HTH. 🙂

  7. Hi Matt,

    I’m late to the party on this one but just came across this thread on your blog. It’s helpful to hear this dialogue and compare it with our current development plans. Obviously, this is an area that is of huge interest to our company – it’s exactly the problem we are trying to solve. I feel like the current strengths/limitations of T-Splines has been fairly represented by a number of comments here. It’s true, T-Splines does give you freedom from many painful parts of surface modeling, but it does introduce its own unique paradigm and rules. We are currently working to make it more intuitive and also to make it available to the crowd that doesn’t already have Rhino.

    Regards,
    Matt Sederberg
    CEO
    T-Splines, Inc.

  8. Interesting example Matt. I’m in the same boat as Jeff, mine usually fail, then cut/patch/fill.

    But I’m not faulting the software, my own skills are lacking.

    Here’s a question, this works on a single feature, what about when this condition is the result of multiple features?

    Matt’s reply to Devon “Try it yourself and see” LOL!

    Thanks,
    Devon

  9. @Mark Biasotti

    @matt

    Thanks!

    Matt, I didn’t think that would work as a single fillet feature. Looks like the fillet diminishes to zero in the middle where the surfaces would essentially cross from convex to concave (makes sense). Whatever reason—and maybe because of some kernel stuff as Mark mentioned—most of the situations I try to fillet like this don’t work out. And those are the cases I cut out material and patch it back in with a filled surface to get what I need.

  10. Hi Jeff,

    I believe it it comes down to the definition of what is called “rolling ball” fillet. this methodology that is common in many modeling kernels and simply does not take into account that the concave that the ball rolls in, would suddenly or eventually change to a convex – that, in essence is the problem and something I know that Parasolid or CGM can not handle. So the solution is to augment two concave or convex fillets with a transitional surface. Like I said, ProE has done this for quite a while and it is very powerful, although very quirky in that it’s hard to get it to work in many cases.

  11. Thanks, Mark. This is the first time I’m seeing use of the terms “transition” and “fillet” used like this. How does this work in the context of convex and concave requirements for something like a fillet? Are you saying the new fillet would tackle (for instance) concave and convex areas separately and then create a junction between the two as an automatic second step? If so, that would probably work great—depending on execution and how robust it is, of course.

    But if it’s possible to create a blend between the convex and concave fillets, why not simply treat this as a simple fillet, since the blend is already at work between the two faces (or sets of faces)? Assign tangency or continuity, assign a set-back distance from the edge (or radius) and let the feature handle the rest. Wouldn’t that work with similar effect? I think it would be much simpler from a interface/in-use standpoint.

  12. Jeff,

    What I’m suggesting is a future fillet feature that would be able to:

    A) create two fillets (in the same fillet feature) limit the extent of those fillets and then B) have the fillet feature create the transition between them. ProE has had fillet transition feature for quit a while. This is similar in concept to fillet setback where you define the fillets at three (or more) intersecting edges, and then the setback creates a transition between them.

    Mark

  13. @Mark Biasotti
    Thanks for the thoughtful reply and proposal.

    So—I could define where the fillet moves from concave to convex? As opposed to the surfaces to which I apply the fillet doing so (which is generally what governs this)? This sounds OK, but I think it would be fragile. Suppose I edit the underlying surfaces such that the point of inflection moves a bit. Wouldn’t this break my distance/edge-constrained fillet, since my inflection point isn’t where I’d originally stated it as being? Am I understanding this properly? How would I use it when I’ve got several surfaces involved in this edge that are really creating lots and lots of small edge segments?

    I guess what I’m looking for is a nice balance between flexibility and stability. In the case of requiring a nice tangent transition between faces which change concavity like this, what I’ll do is create a split line, delete the faces, and use a filled surface (or loft or whatever works best). I don’t like this because it’s relatively fragile as well—there’s a long string of operations for a single goal. For instance, I generally use splines as split lines because they’re smooth. But the split lines often split multiple surfaces on each side of the edge I need for the fillet. If this moves around much in editing, my splines each must be readjusted to create the ideal gap, the fill may fail, causing the knit feature to fail, causing the creation of the solid and all solid-related features to fail. Everything then depends on getting this split-surface/fill to work again or all is lost. Fragile. And not very flexible, since the splines for my split surface really cannot be pegged well to the edge I need to fillet.

    So my current tools work, but they set up the model for easy failure with foundational edits. It would be cool if I could select an edge—and really not just an edge, since my edge is most likely made up of loads of fractured edges—and drive everything from this. Maybe somehow connect all tangent edges into something similar to a composite curve and apply the fillet to that? The fillet would really be more like a macro that splits the surface a given distance from the edge and filling with options of tangency, continuity, whatever.

  14. @Mark Biasotti
    Mark, about this fillet thing, if you guys are still developing stuff like this, I think it’s great. I have the same problem as Jeff only occasionally. An edge might go from convex to concave accidentally. Ideally stuff like that wouldn’t happen if I had better control over surfaces to specify “no inflections” or “no curvature of less than x”. or “no curvature changes of greater than x per inch”.

    As far as the fillet itself goes, I’d like to see maybe the ability to offset edges within the space of the surface (regardless of U-V directions) by percentage, and then to fillet – or maybe more appropriately, just call it a blend. The offset could be asymmetrical, and because it’s basically just a loft from one side to the other, it wouldn’t matter if there were a little convexity flip here and there.

  15. @Jeff Mowry
    Jeff,

    Let me run something pass you and ask you if it would be acceptable: what if you could create a fillet, and in the fillet feature limit the extent of it (actually control where the fillet stops. Then you could create a multiple edge fillet with a “limit” where you determine where it goes from concave to convex. Would that be suitable?

  16. Hmmm…. I wonder if mimicking real life doesn’t eliminate the potential to orchestrate something by means that don’t exist in real life…or is hard to do in real life by conventional means. Perhaps we don’t have tools to produce the physical results – yet, or perhaps complex missions can be broken down into conventional tasks we can handle.
    For instance not that long ago parts were fairly intuitive and based on a craftsmans experience. Today we can mathematically describe and produce things with multiaxis mills or robots that were not possible to articulate previously.
    Part of the attraction of computing is that you are manipulating data or can reuse data from other sources. If you like it is formless and can be rearranged in infinite ways to suit our purposes. Why not view CAD as a magical dimensionless space like a swarm of ideas or musical notes that can reinterpreted to suit the need. If you can utilise a computer to switch from focusing on points to curves to faces to lines on piece of paper and back – all of which dont exist in reality but are mathematical concepts why base your tool on what you can touch and interact with.
    Although it is convenient to model processes we are familiar with we can go beyond physical into notional where we aren’t limited by what is familiar to us. We cant see solar flares or see through walls ourselves but we can extend our awareness with sensors that can. I am not saying you should get lost in your imagination creating things that cannot be made but that CAD could evolve to be adaptive and open ended rather than a discrete collection of compartmentalised tools. 2d cad mimicked the draughting instruments we were familiar with then but we didn’t stop there.
    > concave > convex fillet feature something that’s irrational…
    Perhaps we should be more ‘irrational’ as a way forward.

  17. Thanks, Mark, for participating in discussion here. Nice to have a viewpoint from the inside once in a while, and to explore some alternative present/future options on the table in geometry creation.

    By the way, is the example I mentioned of a concave > convex fillet feature something that’s irrational or otherwise out of reach within the NURBS environment? Would it be something feasible to add to SolidWorks functionality if not?

  18. @Mark Landsaat
    Hi Mark,

    I do likewise (start with rhino surface etc. and convert) I agree about holes – and this is typical for any sub-d; that’s what I mean when I say it is not suited for all shapes. It’s been a while but it is possible to create holes “smartly” with a workaround sub-divide where you want the hole and then delete the patch holding cntrl ( or something like that), then do an extend to get the edge definition back.

    Where I see the real potential with T-splines is with their T-Skinning approach which takes Sub-D and applies it to conventional surfacing methodology (start with curves.) It has a lot of potential and promise but is not quite their yet.

    Also, it is possible with Rhino/Tsplines or Rhino/Tspline/TsElements to combine Sub-D NURB with conventional NURB; the entire model does not have to be sub-d but just the portion that needs it. Using the bridge command is one (but not the only way) of accomplishing this. I also like and frequently use the crease command.

    All this said, it is kinda sad, and does rub me the wrong way. that if you are going to be proficient at Sub-d, the technology defines the design process and that is something I do not want to see.I would like to see the CAD process mimic the real-life physical model making and machiningprocess – that is something that I’m hoping we work towards in a future modeler.

    Mark

  19. Mark,
    I am amazed at the versatility of the fill surface when the guide curves are not connected to the boundary. I made a nice rippled swimming pool surface using a rectangular boundary, and 20 points for wave crests and 20 points for wave troughs. 3D sketches work fine for guide curves.

    I think it may be possible to make clothing for my mannequin using the fill surface. I will start with some points on offset surfaces, then a 3D sketch along the seams. Some points offset from the mannequin surface to make draped wrinkles. Then a fill surface. If I am really lucky this might work relative to the poseable assembly.

    I tried making close for the mannequin.The fill surface does not do the right things when the edge of the fill is complex. It refuses to be guided by some very sensible curves or points. It was worth a try. Naked mannequins, what is a designer to do?

  20. @Mark Biasotti
    SubD for defining precise shapes for manufacturing is not easy (try cutting a round hole through a subD mesh and have it stay round). If you go to the Tsplines tutorials you will notice that 95% of them are for models that if they look good they are good. However with that said. The most difficult thing in parametric surfacing is building nice C2 blends between your carefully created parametric surfaces.

    In general I think we can all agree that exact parametric definition of this blend/transition is not of paramount importance. Your parametric main surfaces should take care of this. This is where the “if it looks good it is good” comes back into play.

    So in the current Tsplines workflow. I build my large starting surfaces with regular rhino tools. Although this is not parametric in a lot of ways it is identical to SolidWorks. I set up my initial curves and create the surface I want having full control over cross-sections, dimensions and locations. (This is however where I miss parametric constraints but it works). With Rhino you have control over the degree and Isoparm count in the surfaces you build (very nice). If you build them carefully this will set you up for success creating your blends.

    Once all the main surfaces are in place I convert them to Tsplines surfaces (this conversion is exact) and use the Tsplines tools to create the necessary blends. Main swoopy shape finished with exactly defined surface geometry aside from the blends. Ready for mechanical detail.

    Now here’s where I don’t see TSelements making a lot of sense. I already have a Tsplines model in Rhino. If I start a new SWX part with the Tsplines model as the first feature I can always go to the feature and “edit in Rhino” This gives me the full feature set of Tsplines tools and as long as I don’t delete and recreate any surface geometry all my mechanical detail added in SWX will propagate once I go back to SWX. It’s just another parent/child relation to manage. I guess the question is what’s the real benefit of adding TSelements?

    Do I like all this back and forth between two different packages. No not at all. Even though you are not at liberty to speak of work in progress, one of the main reasons I jumped on Tsplines now is the prospect of having a full Tsplines feature set within SWX in the future. Hopefully soon. When it comes I will already be familiar with the feature set and ready to work with it inside SWX.

  21. @matt
    Hi Matt,

    “Lots of tools” – I empathize. This is what mainly, I believe, is holding back TSElements; you essentially need 4 products. My hope is that will change in the future.
    Obviously, I’m not at liberty to discuss what we are working on – although I’d like to, that is something that professionally I’m held to by DS, and I don’t mean to “tease”. T-splines is continuing to enhance TSelements with more functionality and I can not discuss when or how much (functionality) only that they are investing in that product currently as well as their Rhino product.

    Regards

    Mark

  22. @Rick McWilliams
    My experience has been that you can not use more than two constraint curves with fill, and with that they need to be constructed very carefully (good tangency or curvature)

    What really makes the difference (success) with Fill is constructing reference surfaces first for all the appropriate boundaries. Fill is very dependent on boundary isoparms to define it’s flow.

    Regards

    Mark

  23. @Mark Biasotti
    Mark, thanks for chipping in here. modo/tsplines/solidworks, lots of cool tools, but still lots of tools. It’s too bad there isn’t a single tool that can do product design shapes and shell/rib/boss engineering too.

    SolidThinking also has subd modeling. The main difficulty there is that there are few paths from subd for shape to nurbs for machining. I know Tsplines does it, but Tsplines also relies on other software as a base, there is no standalone tsplines.

    It’s kind of significant to me that the main swoopy guy at SW is essentially conceding the point. I definitely appreciate the candor, and this is one time that being right is more an annoyance than if I were wrong about this.

    So you’re just going to tease us with that last comment about research?

  24. Hi Neal,

    I agree that with Sub-D you can really struggle, but I’ve found that, for certain shapes the overall effort (and struggle) is less than trying to execute it in conventional surfacing.

    Sub-D – no doubt is a completely different mindset when executing more complex models and is not suitable for every kind (indeed many kinds) of shape. I like to think of the difference between Sub-D and conventional NURBS surface modeling like this: conventional surface modeling is defined by the curves. Sub-D modelling is the opposite of that in that the shape is defined by the surfaces (faces) and the resulting edges are subordinate. The holy-grail, of course, is when the two can be combined into one modeler and there is some ways to do that, that both T-splines and Dassault (us) are researching.

    T-splines, does a good job in being able to precisely sub-divide a region without reparamertizing the surround shape. It is an option, I believe LMB on the tool to use the precision method. It (precision) isn’t in all their commands yet, but I believe they are working in that direction. Meantime there are workarounds to holding boundaries, say for instance, when you delete a face and want to keep the boundary precise.

    Regards

    Mark

  25. The trouble is that Tsplines, while cool to use, is quite hard to be specific with.
    Fitting to curves helps but you still need to manage your mesh and tpoints carefully to preserve the desired shape as you work with it, and the more divisions you have (which are necessary to apply detail) the more prone to minor waves and bumps it becomes.
    Scaling and tweaking positions and regions by eye doesn’t give confidence in the fairness no matter how careful you are, plus each movement impacts the zone out to two neighbouring faces.
    The more you play with things the closer you get to the overall shape you desire of course but the more the initial simple finesse disappears as well.
    I know SW changed the display of curvature across patches – thanks for that – and it ought to help (although I have doubts about relying on it since the accuracy and resolution is an openGL thing related to the graphic mesh and not to the real geometry), but there are still issues with getting a fair shape/panel. Could there not be a ‘conform to surface’ function in TsElements?
    By that I mean you set up a feature based target surface in SW, select some specific Tspline control points (on surface) or area that you want to be coincident and match them to the surface- like a shrink wrap or wet cling. This leverages more exactly defined and hopefully smoother geometry in the manner you make use of an auxilary surface to set up tangency for boundary and loft.
    In Rhino you have a bend function that makes nice general realignments of points in 2d that suits some cases but the whole thing gets messy in 3d and once again isn’t specific. There really isn’t a way to detect or fix things that may have gone ever so slightly astray while you were playing around. If you drag a point in one plane until it looks right in an orthographic view chances are its moving out of place in another requiring a further tweak. Eventually you end up with a subtle beaten copper effect.
    You want to impose some definite overall regime on it though, ie iron out the wrinkles from the sheets, sweeten those curves..
    I suppose the best example I can give is the side of a car where there is a definite intent to curve along it and in the vertical in a deliberate/controlled fashion but there is also some local sculpting or creasing. Even after many subdivisions and repeat local tweaks you want it to retain the global intent and fairness or be able to reset it to that.
    I suppose you could go back and edit the underlying SW reference surface later to induce a global warp if you needed to…dunno..
    Hope that makes sense to you.
    My feeling after using it some is that Tsplines while seeming to be a neat tool actually struggles to be useful in its present incarnation for engineering tasks. For nondescript organic forms its fine though, excellent even.
    Even though I don’t use Elements I’ll put in a request here and now for a ‘conform to surface’ tool or something similar for those that do. Sorry I can’t submit an ER.

  26. Hi Matt,

    On shapes like these, I think it is worth the investment to consider going the sub-D route via Modo or Rhino/Tsplines and TSElements. I’m more convinced than ever, that when the overall shape and style lines become more important than functional features (primary – i.e. planar solids and fillets) that the sub-D route wins out.

    Unfortunately, I’m also aware of the political/procedural barriers of using “non-native” SW workflow with a client or within a your company. If the designer can successfully make a compelling case (i.e. – ROI) for using a non-SW product as part of the SW pipeline then they should go for it.

    My 2 cents.

    Regards

    Mark

  27. @Jerry Steiger
    Hi, Jerry!

    I use elliptical areas for the Fill feature. I don’t like rectangular areas because they tend to bunch up in the corners and the opposite directions are some times unable to allow c2. When ever I have an area that kinks or wrinkles and I can’t control it, I just cut it out and Fill patch it. If I have to use a 4 sided patch, I tend to use boundary instead.

  28. Matt,

    Nice post. I would love to hear some more about how you made the elliptical areas work. I would never have thought to try that. I’m still a bit amazed that it worked. Nice comments as well from everyone.

  29. I heard slip on the last Tsplines webinar about a plugin coming for SW – not just Elements…not sure how real that is but you might get your wish for something a little more push pull. I guess that’s an easy way to extend SW life without doing development in house…come to think of it I think I said that to Mark B. on the SW forum a while ago. 🙂

  30. I am finding that the fill surface will accept all kinds of guides. This can generate very interesting wavy surfaces.

    We see surface shapes by the character and movement of the highlights. It would be nice to define these curves and drape a fair surface. Then use some digital sand paper to smooth the breaks.

  31. Sounds gloomy, but at the same time this sounds like a good advertisement for T-Splines. Speaking of capitalism, T-Splines + tsElements is a very cost effective tool-set to compliment SolidWorks.

  32. Ever need a fillet on an edge that must go from concave to convex? Won’t work with a fillet feature—you’ve got to patch-in your own feature to do this (boundary surface, fill, etc.)

    Ever have a convergence of radiused edges that won’t blend (because of the convergence)? You’ve got to punch a hole in the area of the surface that has the convergence so each radius doesn’t actually converge—and then patch the hole you created. And the shape of the hole you cut (rectangular) matters—as does its tilt—if you hope to get a nice blend with the surrounding surfaces. What I do for this is create a rectangular-shaped hole that can be spun around with an angular dimension (quickly) after the hole, radii, and patch are put together. I tweak the angular dimension of the hole (essentially controlling U/V directions by doing so) to see what produces the best fit. And yeah—the sketch is almost entirely blue (undefined)! Defined sketch rules slow development, and really aren’t the best idea all the time.

    The random feature crashes for projects like this are inexcusable, and I see them all the time with my projects. VARs don’t know how to solve these issues, so I suppose there are no real solutions. Buggy software? Not sure of the cause. But trying to track down the cause of feature failures that fail on one CTRL-Q rebuild, and resolve on the next is nerve-racking, and certainly can cause a net loss on a project. After all, if the battle is truly one with the software (and not against the chaos of the ether to create something of order and function), you’ve got two battles to win—along with split focus.

    Talk of the cloud with known issues such as these left unaddressed is maddening.

  33. @Kevin De Smet
    Kevin, yeah, I agree, it’s a model-to-model thing. I just run into the same type of roadblocks working with this tool. The Freeform tool has fallen short. This is a time where the 80-20 thing has reversed to a 20-80. Yes, it allows you to check the box that you’ve got a tug-and-pull freeform modeling, but no, it isn’t actually useful. I’ve tried several times to use it on real models, and I’ve only succeeded once, on a bit of a crazy model where I had to model frozen splashing water. It allowed me to give the surface of the water some randomness.

    @Mark Russell
    If they really intended SolidWorks to be used for product design, they wouldn’t hem and haw at adding conics for years on end, they would have better tools for evaluation and control of shapes, and they would allow more control over the tree. I mean, it’s ok for what it is, but it’s not really built to be a professional level tool for swoopy stuff.

  34. The management at Solidworks must dread your new posts -“the price you pay for not using software that is intended for this kind of work”. I feel sorry for the many new engineering students who pop up on FaceBook extolling the virtues of this awesome software. One day they will understand, what second-rate means. I seriously blame capitalism for the concept of second rate CAD.

  35. At the bottom line, it truly does depend on the model. Nurbs-only modelers would kill for the kind of procedural surfaces possible with parasolid and acis. But it is definitely not for every shape.

    I agree SolidWorks could use a more industry standard direct control point manipulation, Freeform comes close, but it tries to hard being a feature that holds your hands. Commendable… but is it the right approach?

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