Gabi Jack's Blog

Configurations and drawings revisited

Back in February, when I made my first attempt at creating multiple configurations for a part, some people warned me, with their own good reasons, that configurations are not really all that great, since they usually cause more trouble than they do help. Among those problems created by configurations, there was the one about not being able to tell what configuration had been used when creating a drawing. Well, back then I tried to create drawings using my configurations and I thought that there really was no way to get information about configurations being used from the drawing document. I just couldn’t figure out how. I recently learned that there is, indeed, a way to keep track of what configuration has been used in each view of the drawing, and there’s even a way to link the name of the configuration that was used to a note in the drawing, for added clarity. Of course, I’m talking about configurations for parts. I haven’t messed up with assemblies just yet.

So, this is what I’ve learned. When you insert a model view in a drawing, you can specify what configuration to use, simply by clicking on More Properties at the bottom of the dialog box. This will open the Drawing View Properties dialog box, and there, under Configuration Information, it will let you know what configuration is being used to create that particular view, and it will also allow you to select a different configuration from the drop-down list. If you ever wish or need to change the configuration later on, you can also access this dialog box by right-clicking on the view and selecting Properties from the menu. The following picture shows the two dialog boxes. In this example, configuration Size1 is chosen.

To link the name of the configuration to a note in the drawing, all you have to do is double-click the view before creating the note, so that the note is associated to that view. Then, create the note by clicking on  Insert, Annotations, Note  or clicking its icon from the Annotations Toolbar. On the Note property manager, click on Link to Properties.

This will open a new dialog box that will prompt you to choose what property to link to the note, and where to get it from. In this case, we need to use custom properties from the Model in view to which the annotation is attached and the property we want to link is the configuration name.

This is what is called a parametric note, because it is linked to the value of a document property, a custom property, or a configuration specific property. If the value of this property changes (if we change the configuration), the text in the note will automatically update to show the new value.

Never underestimate the power of a midget

Coach Mark, who trained my son during last year’s baseball season, was proud to lead a great team of “midgets”.  He led them from mere midgets, all the way to becoming last year’s champions of their own division. Most of the kids in the team, including my own gentle giant of a son, were not as big or tough as many kids in the rival teams. Some were scared of being hit (yet again) by the ball. But, whenever in doubt, Coach Mark would always say to them: “Never underestimate the power of a midget”.  And he was right! Midgets can grow, and they often do, in amazing and unexpected ways. They can also become stronger, resourceful, skillful, and develop character, often as a result of being treated like a midget.  That’s a good thing for the midget (guess who’s already making the MVP list this year), but not so good for those that never saw it coming and certainly would’ve never expected it from a “midget”, like that coach of the rival team that lost the championship to Coach Mark’s bunch of midgets.  It is also not a good thing if the midget in question happens to be a small error in any of the features in your model. It may be an insignificant error, but one  that has the power to cause most or all of the features in your model to fail.

The following example is something that actually happened to me while preparing for the CSWA test. I was working on the exercises in Planchard’s guide that required changes to be made to models that had been previously created.  Just for extra-practice, I decided to edit this particular one that you see in the picture, and change a few of its dimensions.

I made a mistake, however, and added a tiny extra line to one of the sketches. The line was on top of another one, and was so small that I didn’t even notice it. Well, guess what happened to my model. This happened.

One small mistake and now 90% of the features in my part fail! What do you do when something like this happens? Do you…

a)    Tap your heels three times and reload, wishing that the errors will be magically gone?

b)    Proceed, from the bottom of the tree up, deleting dangling relations and dimensions left and right, in hopes that it would all be better once they’re gone?

c)    Make use of the different editing tools that SW offers in order to find information and repair the model?

Well, if you know exactly what you did that may have caused the problem, just go and undo it, but if you have no clue, then letter c is your best bet. Now, how do you find out what’s wrong with the model? Well, the way SW will handle the errors when they occur, depends on your choice of settings. If you go to Tools, Options, System Options, General, you will find that you can check the option “Show errors every rebuild”.  This ensures that an error dialog box appears after every rebuild, showing a list of everything that is wrong in the model, including errors, that prevent features from even being created, and warnings, that don’t prevent them from being created, but will still show problems, usually with dangling relations and dimensions. You can also display the “What’s wrong?” list of errors if you right-click the name of the part in the feature manager and select “What’s wrong?” from the menu. The list you will get looks more or less like this for a part (it can look much worse than this).

And can look like this (or worse) for an assembly.

OK, so now we have a list of errors, what do we do next? Well, we start editing and repairing the model from the top, from the very first feature that shows an error or warning, and go working our way down. It could be that solving just one or two errors that were made early in the process will solve all the problems in the part. OK, this doesn’t always happen this way, depending on the complexity of the part, but it could. Remember to always hope for the best, even when you are expecting the worst.

In my case, at least, it happened that way, because the mistake I made was located precisely in the base sketch. This extra line in the geometry was causing the base feature, Extrude 1, to fail, and creating all sorts of problems all throughout the model, since all the other entities that depended on that first feature were now failing too and/or had dangling relations and dimensions, now that part of the geometry was missing. When I edited the base sketch, and with the aid of the Check Sketch for Feature command, I was able to pinpoint the culprit. The extra line in the geometry is highlighted in green and now I could simply delete it, rebuild my model, and proceed to repair the next error(s), if any. In my case, there were no more errors and my part was finally able to rebuild correctly.

There are many other midgets that can be causing the features in your model to fail. Some will be easier to spot, like if you made a typo and wrote a value for a fillet that is way too large. Some may not be that easy to spot, but can also be repaired, like if you established relations or dimensions that reference to things that no longer exist in your model. For this situation, you can use Display/Delete Relations while editing the sketch, in order to find the entities that are used by those dangling relations or dimensions and, if possible, replace them according to your design intent, so the model makes sense again.

From this experience I learned that it’s always worth trying to repair a model first, instead of going on a deleting frenzy, which may actually make the problem even worse. Of course, how long it takes to do such repairs depends on how complex the model is. I know many of us will probably have to spend several hours repairing something that someone else (or even ourselves while trying to do changes to it) messed up, and I’m sure it won’t be fun. Sometimes it may be easier to start from scratch? Then again, if it’s still possible, I guess it’s worth trying to repair.

Oh, just to share. Here’s a picture of Coach Mark and his happy bunch of midgets.

And speaking of good customer service...

I just thought I should mention the awesome treatment I received from SDC (Schroff Development Corporation) not so long ago, as an example of what I’m talking about in my previous post. Schroff Development Corporation publishes a great variety of tittles on CAD, CAM, FEA and Engineering Graphics.  They have plenty of tittles on SolidWorks and COSMOS, commonly used as textbooks in school. They also have other books for professionals.

Anyway, this is what happened. See, a few weeks ago, I bought yet another Planchard and Planchard book from Amazon.com. The book was supposed to include a CD of files that were necessary to understand the lessons and solve the exercises. In other words, the book was pretty much useless without the CD. However, yes, you guessed it, when my book arrived, I discovered it did not include a CD. I quickly contacted Amazon and inquired about this issue. I was advised to simply return the book and they would send me a replacement. The second book arrived a day later and, yes, you guessed again, this one didn’t have a CD either! This was so frustrating, especially because, according to the cover of the book, the CD was supposed to be included with the book. There was simply no other place where to get the files from. So, it occurred to me that perhaps I could buy the CD from the publisher, SDC, and so I sent them an email explaining my problem, and asking about that possibility. I was very pleased when I received an email from Ms Karla Schroff herself, just a couple of days later. Not only they were willing to help me with my problem, but they even sent me the CD free of charge! This is really good customer service, don’t you think? I mean, what was I buying? A book that costs only a few dollars, not thousands, and I didn’t even buy it from their website, I bought it through Amazon, but they still cared, they were still willing to help me out and they did. Now, this is what I’m talking about!

Wishing on a star

I thought about writing this for a long time, because I didn’t want it to sound like a rant or mere whining. Before I say anything, I want to assure everybody that I love using the software and I deeply respect SolidWorks as a company, as well as all the great folks that work there. OK, so here it goes. If you watched the movies I posted on the blog just recently, you may have noticed that Vic Leventhal does mention several times that SolidWorks really cares about their customers, and that is also a great believer in education.  As someone who is trying to learn the software and doesn’t really have the means to afford buying the commercial version of SW just for that purpose (not that I have given up on that dream because I’m saving my pennies), I greatly appreciate that SolidWorks is one of the very few companies out there that offers a fully functional student edition of their product, and for such a low price, that makes it incredibly affordable for students everywhere.  Being able to use SolidWorks this way has been tremendously helpful in my learning process, and I’m really grateful for that. However, I can’t help but wish that SolidWorks considered the users of the student edition as part of those customers they care so much about. In particular, I’m talking about the lack of technical support for the users of the student edition, especially when it comes to installation problems.

Several months ago, when I first installed SW in my computer, I ran into so many difficulties that I thought I had been sold a defective product. I ran the installation wizard according to the instructions in the case, but the installation kept failing over and over. It just stopped in the middle of it and would not finish. I tried to find answers to my problem by reading all the help pages and places the instructions direct you to, and I couldn’t find a solution there. I tried emailing SW, but I got no reply. What I needed was a real person to tell me what to do, but, alas, there was none. I ran the installation many more times, and then I started to do things “the wrong way” just to see what happened. Instead of uninstalling the first attempt, like the instructions advice you to do, I ran the wizard a second time over the first installation. This time, the whole software got installed, but COSMOS still wouldn’t work. It needed something else that I couldn’t find anywhere… I tried the online licensing over and over and it wouldn’t do it. I emailed again and nobody answered. Short from giving up, I decided to try my luck in the SW users forums, and it was there that, after a few days, another user  directed me to a page where I could download a patch for those that were  running the student version on Windows Vista, such as me. After the installation was complete, the software ran correctly and I was able to use COSMOS, but my computer kept doing weird things, like freezing every once in a while, and so on. I blamed it all on Vista, as usual, and didn’t think much about it. “It must be my luck”, I thought. The funny thing is, ever since I started writing the blog, I get an average of 15 emails every week from users of the student version that are still struggling with similar installation problems and that write to me in hopes that I can provide them with a solution! But what can I say to them? I’m just another user! I don’t have the answers that they need; SW does.

Now, I’m sure that providing the kind of technical support that SW gives to their service subscribers must be expensive, so that’s really not what I’m talking about. Would be nice, but I know it’s not going to happen, especially since the users of the student version only pay an insignificant fraction of what the commercial version must cost, the license only lasts for two years (sometimes less) and they don’t pay for the service, as other users do. But, really, why not provide at least some help during the installation process? I know they don’t promise any kind of help or support with the student edition, but why not show a bit more concern about this other customers? After all, the students of today will be the users of tomorrow. Someday, these same students will be the ones making the decision over to buy SolidWorks or not, and they will make that decision, in part, based on the experience with customer service (or lack of it) that they got while they were learning. Wouldn’t it be great if they could keep a nice memory of how SolidWorks helped them out and cared for them, even while they were just students? Vic Leventhal did say one more thing during that meeting. He said that, if at any time we thought of something that they weren’t doing quite right, we should tell them, because they do care about their users. Well, that’s what I’m doing here. I’m simply, and very respectfully, stating my point of view and how I wish the users of the student version could get the kind of help and support they need from SolidWorks. Is this simply a wish on a star, or could it become true sometime soon?

Tri-Valley SolidWorks User Group First Meeting (Part II)

As I had promised before, here is the second part of my recount of the first Tri-Valley SolidWorks User Group meeting.

After enjoying Vic Leventhal’s  interesting story about the origins of SolidWorks, and having had a bit of fun with all the SW trivia questions he threw at us, we took a short break to stretch our legs. Some guys in the room went for another slice of pizza. Some made short conversation and mingled with other members. I began wondering how many of the guys in that room were experienced users, and if any of them was a beginner, like me. Later, I found out that there was a little bit of everything, from the experienced user to those that are just getting their feet wet.

Following the break, Matt Lorono spoke to the group about SolidWorks World, the international user conference that takes place every year, always in a different location, in the United States. SolidWorks World 2008, for instance, was in San Diego, CA. Next year, it will be in Orlando, Florida. You can learn more about it by visiting the following page: http://www.solidworks.com/pages/swworld08/index.html.   You can also go to Matt’s SWW 2008 Presentation PowerPoint download page, and see for  yourself what he was talking about. He’s got some very cool videos to go with it, and he’s willing to provide them to you upon request.

Finally, it was time for what we had all been waiting for: the tips and tricks! With Matt’s assistance, Kenneth Barrentine went through a list of very useful tips for when sketching, working with parts, drawings and assemblies too, and he demonstrated each one of them for us. Some of them I already knew about, yet some others were completely new for me. I noticed how some of the other users were also learning about some of these things for the very first time, many began asking more questions, some even contributed a few ideas or, at least, exchanged them with their neighbors. It was right there when it became evident to me what this group is all about: it’s a safe place to learn, to ask questions and find the answers you need, to share what you’ve learned, and to help others in their learning process. In the words of our fearless leader, Kenneth Barrentine, “We are here for each other”.

The next meetings are going to be full of content and hands-on learning opportunities. Everyone is expected to pitch in and contribute their doubts, ideas, challenges, and even their own solutions and/or tips and tricks that they have found to be useful. Everyone is expected to not only take, but also give to others in the group. This way everyone learns and we all benefit. It already sounds like a great place to be in, and I’m very glad I joined this user group. I’m looking forward to the next meetings!

If you are in the San Francisco Bay Area and looking for a user group, you may want to check the Tri-Valley SWUG. It serves the communities of Pleasanton, Livermore, Dublin, San Ramon, Danville and surrounding areas. Even if you are not in this area, I encourage you to find a user group for yourself and attend the meetings. It’s really worth it!

This just came in

I didn’t tell you before, but for this first meeting of the TVSWUG, there were prizes and gifts for everyone in attendance. Everyone came out of there with something! Most gifts were SW promotional items ( screen cleaners, bottles, jackets, backpacks, baseball caps), but there were also other prizes that were gracefully donated by the companies sponsoring the meeting. The one that was considered “first prize” was a 3Dconnexion SpaceExplorer, just like this one here in the picture.

One happy gentleman was lucky to take that baby home. Me? I got a baseball cap that has already been claimed property of Master Andrew Jack (my four year old son), because “It makes me look like Sonic the hedgehog”.

Anyway, if you feel like you really want one these, I received email from Kenneth this morning that you can buy one from this merchant for a very decent price and, if you look carefully, you can get also get a second one for free, as part of a rebate offer. The offer is only good until March 31^st, so hurry up. I just wanted to share this with you because I thought it was really cool, so, now you know.

Tri-Valley SolidWorks User Group First Meeting (Part I)

Wednesday evening, I had the great privilege of attending the first meeting of the Tri-Valley SolidWorks User Group, in Pleasanton, CA. This was a first for me, and a very enjoyable experience to say the least. I arrived early, way before many of the other users. Being as bashful as I am,  I must confess that I was a bit nervous, but I felt much better after introducing myself to Kenneth Barrentine (our fearless leader) and my fellow blogger, Matt Lorono, who came to the meeting to talk to us a bit about SolidWorks World 2008 and, together with Kenneth, to offer the group a few tips and tricks that will allow us to use the software in a more efficient way.

So, after signing up, making some short conversation with other attendees, and enjoying a slice of pizza, we listened to the special guest, Vic Leventhal, Group Executive from Dassault Systemes, as he told us about the ( often unknown and many times hilarious) history of SolidWorks. This part I enjoyed tremendously! I don’t know why. I guess I find great pleasure in learning about how huge companies got started from humble beginnings, about their struggles and even about their lucky coincidences. Some stories are so amazing that they almost seem like taken from that movie, Forrest Gump, where the guy happened to be in the right places at the right time all throughout his life!

Anyway, I took my camera with me and filmed for a while, until I ran out of battery (nobody is perfect!). There was so much more going on at that first meeting and I’ll tell you about it, but I also wanted to share part of what Vic Leventhal said at the meeting, so I put together a couple of videos, and well, I hope you’ll enjoy  listening to this guy as much as I did. I apologize in advance for the crappy resolution and for  all the times it seems I was FUI (filming under the influence), because the image moves so much. Next time, I shall take a tripod with me. I'm really not good at making videos. I guess it's a good thing that I'm not trying to make a living as a journalist or video producer, otherwise I would starve to death. OK, so here goes the first part...

And here you got the second part...

I see a hole out there

Ah!  Spring is in the air! So many wonderful things all around us are finally making their way back: flowers, birds, butterflies, higher temperatures, tree top squirrels, gophers digging out my flower bulbs, those darn raccoons that keep messing up my yard…, and, of course, Little League baseball season! While sitting on the bleachers for a good two or three hours, I read from one of my books and watch my son and his friends practice their game, as well as their cheers. They have quite a few fun ones, but there’s one they seem to love, since they keep chanting it over and over. “I see a hole out there. I see a hole out there. I see an H-O-L-E, hole out there.” This intrigues me, you know? Where is this hole they see? What is it really they are talking about? Is it even a hole out there? I guess I’ll never find out! It’s not anywhere in my trusty manual “Baseball for Dum-dums”, and my son won’t say a thing! Anyway, it also gets me thinking about holes in general. More in particularly, about using sketches to place holes with the Hole Wizard. Why? Well, because it’s one of those useful speedy short-cuts that helped me when I took the CSWA and  it may help me again when, someday, I finally take the CSWP test.

How to place holes using the Hole Wizard was really hard for me to understand at first. I went through all kinds of trouble trying to avoid using the Wizard for that reason. It wasn’t until I saw how it’s done in one of Albert’s video tutorials, that it dawned on me that the position of the hole is determined by a point, a sketch, and that, as any other sketch, I can apply relations and dimensions to it just the same way. Now one thing to keep in mind is that the Hole Wizard can use both 2D and 3D sketches to place the center of the holes.  Basically, if you have a planar surface and you want to use the Wizard to place holes on it, then you want to use a 2D sketch for that purpose. In this case you need to preselect the surface before starting the Hole Wizard, otherwise, you’ll end up with a 3D sketch.

Using 3D sketches, on the other hand, offers an obvious advantage for when placing holes in non-planar surfaces, but they can be tricky to define, since several relations that are usually available for 2D sketches aren’t available for 3D sketches, and also because you have to be careful what you dimension your sketch from. It is always better to dimension from a plane or planar face, rather than an edge, vertex, line, etc. In the following image, the Hole Wizard was used to place a hole on the surface of the sphere. 3DSketch1 is the point that locates the center of the hole, and it’s position is dimensioned from  the front and top planes.

In addition to being able to define the placement sketch just as you would any other sketch in SW, there’s the added possibility of using linear and circular sketch patterns to place more than one hole. In the following example, a linear pattern was used to place a series of holes on this planar face. Notice how the entity to pattern isn’t the hole, but the point that locates its center. The procedure to do this is very simple: just preselect the face, activate Hole Wizard, choose the kind of hole you need and then click on the position tab, place the hole anywhere on the surface, and then deactivate the point command, to avoid placing any more holes.  Then you can proceed to insert the kind of pattern you need, linear or circular. The entity to pattern is Point1, the center of the hole you just placed there. Finish by dimensioning and adding relations to the sketch, just like you would any other one, and when you finish, click OK to close the Hole Wizard.

Just as a curious note, it is possible to do the same as in the image above by using the hole wizard to generate the first hole and then using a feature pattern to create the rest of the holes. The following image shows the same part, where the holes where created using a linear feature pattern, LPattern1. In this case, we are patterning feature, the hole that was created with the Wizard, and not the point that defines its center.

Both parts look just the same, but when comparing their file sizes I was shocked to find that the part where the Holes were created by using the Hole Wizard in combination with a sketch pattern more than doubles the file size of the part that was created using a feature pattern.  It’s 504 KB against 238KB! That is a big difference! I still think the Hole Wizard is useful, but, in order to keep my file size small, I don’t think I would use it in combination with sketch patterns if I needed to place quite a large amount of holes in a part.

2D Life isn't fair!

My brother spent a couple of hours chatting with me last night. He was really upset and, unfortunately, it seemed that whatever I said to him actually made him feel worse. Oops! See my baby brother (he’s ten years younger than me) is an Architecture student in Mexico city. He’ll graduate this year. For several weeks, all he could talk about was this contest he was participating in.  Several students from other schools all over the city were also in it. The students had to come up with a design for a new museum about water, “Museo del Agua”, and it had to be creative, functional and harmoniously integrate the elements of the environment, in particular, a small water body that is located in the area where the museum would be. According to what he told me, the design that wins first place will actually be built in Xochimilco, Mexico city. What an honor for a student, don’t you think? Of course, my brother would’ve loved to be that student! But not all wishes come true… At least, not all the time.

For several weeks, he kept emailing me AutoCAD files and jpegs, showing me his progress. His ideas were really good, and I’m not saying this just because he’s my baby brother. He worked the pre-Hispanic  Mexico theme, with narrow canals connecting the galleries, water everywhere, surrounding the whole of the museum, and a snake shaped main corridor. There were also chinampas, small rectangular-shaped areas of fertile land built on top of shallow water, that were used by the ancient Aztecs to grow crops in the lake beds of the Valley of Mexico. The artistic concept included figures of pre-Hispanic deities, like Tlaloc and Quetzalcoatl, carved in stone, as well as statues similar to those in the original buildings made by our ancestors. For several weeks, I kept telling him he should find a way to “translate” his ideas into 3D, but instead, he kept working in AutoCAD, created a few isometric views, and made a scale model.

On the day the projects were presented, he was shocked and mortified to find that most students from other universities were presenting computer generated 3D models with killer rendering jobs. The judges were delighted with the work of these students, even when some of the projects lacked creativity or functionality, simply because the 3D models allowed them to visualize their ideas in a way that no 2D drawing or even a scale model could do. My brother was not happy. I think I don’t really need to tell you who won the contest. No, it wasn’t my brother. Although he did get something out of this particularly painful experience: he learned that this is a 3D world now  and he has to go with the flow.  I would tell him to try SolidWorks, although I’m not sure if it’s used in Architecture at all. Is it?  For now, he said he would try something called REVIT, from Autodesk.  I hope he has better luck next time!

Back in the saddle

Now that the euphoria of being officially promoted to the level of “SolidWorks Advanced Beginner” has finally worn off, and most importantly, that I’ve had some time to sleep, I can  go back to learning more about SolidWorks. I can once again explore a bit on the intermediate and advanced topics and techniques, confident that I have successfully managed to cover the basics. Yeah!

So, this week, I’ve decided to spend some time learning more about lofts and sweeps, since I’ve been intrigued by those two features from the very beginning.  Basically, what intrigues me the most is how to use lofts and sweeps with non-planar paths and profiles, with guide lines, and 3D sketches in general. But before I can do any kind of sweep or loft, I have to learn about how to create such non-planar curves and sketches.  I decided to try my luck first with the one that attracted me the most: the projected curve.

Basically, the projected curve command creates a 3D curve by means of projecting a sketch onto a face or  a sketch onto a sketch. Projecting a sketch onto a sketch  simply means that it will project those two sketches in space and create a 3D curve that will pass through the points where the two sketches intersect.  This reminds me a lot of the way we used to create isometric  drawings and perspectives back in the day, by projecting three different views, more or less the same way, and finding the points where they intersected each other. 

To create my projected curve, however, I only need two views of my sketch, or a sketch and the surface that I want to project it on. First, I tried to experiment projecting a sketch onto a sketch.  I decided to copy (or at least try) the plastic mask that my older son uses to inhale his medication (my son has Asthma). He’s got something very similar to this, and I only tried to recreate the mask, not the complete OptiChamber.

 

You can’t see it very well in the picture, but the way this mask looks suggests a loft from the edge that is in touch with the patient’s face, to the cylindrical part that goes into the OptiChamber.  The edge that touches the face of the person would be the 3D sketch that I needed to create by using the project curve command.  So, first I created  sketches of how the edge would look like when seen from the front and from the right.

By applying the project curve command  to Sketch 1 and Sketch 2, the result was  the 3D sketch that defines the edge of the mask. Just what I needed!  In the image below, you can see the 3D sketch colored in yellow, and the two 2D sketches in green.

Next, I sketched a circle on a plane parallel to the Right plane, and a couple of guiding lines joining both profiles.  The guiding lines would help shape the loft between the 3D sketch and the circle, so the transition between them wasn’t plain and straight, but rather curvy, like in the real mask.

The next step was a little shock, because SW would not allow me to create a solid loft using this profile, so I had to use a lofted surface and thicken it to a solid.

After adding the cylinder that connects the mask to the OptiChamber, it looked a bit more like the real thing. I’m just missing the “cushion” that goes around the edge and that makes the mask comfortable for the child.

For an example of the sketch that projects onto a curve, I tried to recreate a funky path for a circular sweep that I had read about in  a tutorial, some time ago. The path is supposed to go around, like a knot. There was no SolidWorks file with this tutorial, so I couldn’t actually see the part and roll it back. I just had to come up with my best approximation to it from what I remembered about the instructions I had read. Please, pardon my less than stellar use of surfaces and splines here!

According to this tutorial, the idea was to first create a surface by extruding a couple of arcs, like the one in the following image. The sketches that would create the path for the sweep would be projected onto that surface.

Next, the two curves that were sketched as a 2D line and a spline on the right plane, are projected onto the surface using the projected curve command.  This is very simple, really. All that is need to do is to select the sketch I want to project and the surface, like in the following image.

 

The two resulting curves are shown in red. The lines in blue are the 2D sketches that I projected onto the surface.

The next step is to combine both curves into one by using the composite curve command (Insert, Curve, Composite Curve).

Now we can hide the surface and use that composite curve as the path for a sweep feature. Mine didn’t turn out as nice as the one in the tutorial, but you get the idea.

The “knot” is created by making a circular pattern of the sweep, with only two instances, around Axis 1, like in this image.

The use of a sketch projected on a surface as a path for a sweep feature doesn’t need to be this funky all the time, but I thought this exercise was kind of neat and that’s why I wanted to try it.

Yes, I still have a lot to learn about all the different ways in which you can create curves in SW. I'm beginning to think that the more I know about this particular, the better my sweeps and lofts will turn out. What do you think?