Dezignstuff SolidWorks Blog

I’m doing some modeling for an upcoming writing project. I just need some additional and new models for demonstration purposes. One of the models I’m working on is a dump truck. It contains a lot of welded steel structural shapes and plate. I’m building it from a master model sketch placed in a part, and then that master model sketch part is placed into each of the individual parts going in the truck model, and all of the parts are put back together into an assembly. There are a lot of ways to manage a job like this, this is just one of them. I’m not convinced it is the best way, but it is the way I am doing this model. I like to try a lot of different techniques just for comparison sake.

The truck is huge, 21 feet from the ground to the top of the cab. I’m not going to do an incredible detailed set of parts here. I don’t really have time for all of that, but I do want to show a few part and assembly modeling techniques. Along with 6 monstrously large tires. CAD really doesn’t care much how big something is, and the physical size is not what’s important to me here. It’s really just the geometry. The tires have tread, and the treads have fillets, and the whole tread is patterned.

Just as there are several ways of driving the parts of an assembly through Layouts, assembly sketches, master model, multi-body techniques, there are also many ways to create the tread on tires. Here I will take a look at two. One method was the way that I just assumed was the best way to do it, and the other is an odd combination of features. Let’s see what happened.

Here is the tire I was making. Nothing too complex. Revolved shape with some treads and some circular patterns. Below is a screen capture of the FeatureManager for this part. I’ve put two FeatureManagers up to compare different methods for making this part.

The Split Line was just the outline of the tread groove split into the faces of the tire. Since it split more of the tire than I needed it to (created more than 1 closed loop on the face of the model), I used Delete Face to get rid of the extra.

Then I used Knit to copy the faces inside the split to a surface, because you can’t cut into a solid just using the solid faces of the split. In my view, both of those features (knit and delete face) are workarounds for lacking functionality.

Anyway, then I did a thickened cut from the surface to make the tread groove. That worked correctly, wrapping the cut around the side of the tire and giving a curved bottom of the tread groove instead of a planar bottom that you would get from a simple cut.

Add fillets and pattern.

But wait, You can’t do a mirror with an offset pattern like is shown on the tire. There’s just no way to do that. So I treated the knit surface from above as a separate body, and first mirrored it, then rotated it with the Move/Copy body.

But then you can’t pattern both cut-Thicken features with a single circular pattern (plus associated fillets) for some reason. But they could be patterned together if the fillet features were separated. So 3 fillets for Cut-Thicken1 and 3 fillets for Cut-thicken2 and then a single pattern works, if you use Geometry Pattern.

The rebuild time for this scenario is 44 seconds.

Here is the tree for a second method:

In this method I made several compromises to get the rebuild time down. The first compromise was to just make the tread groove as a simple cut. This did a couple of things. First it eliminated the need for the Delete Face features to clean up extra junk, but it also made flat bottomed grooves, which are technically incorrect. Plus, it required a second cut on the side of the tire to get the wrap around. This required further compromises, because the faces of the original groove were not parallel, and the cut from the side would create sloppy cut if the faces were not parallel.

Again, there was no way to directly mirror/offset this groove. So again, I knit faces into a surface body and moved that where I needed it. On one side we have a couple of cut-extrude features, and other the other side we have a cut with surface feature.

The single circular pattern feature is odd. I was able to pattern features and faces in the same pattern feature. This is rare enough because in my experience, few people use the Faces to Pattern option anyway, but I didn’t even know it was possible to combine it with Features to Pattern. Faces to Pattern winds up working like patterning a surface body. It worked well in this case.

Interesting. It’s good to know that’s there. I do think Faces to Pattern is under used, but in this case, there were a lot of fillet faces to select, and it all had to be selected manually. I couldn’t use window select for some reason, and the Select tangent would have netted the entire model.

Anyway, the rebuild time for this second scenario is 1.5 seconds. That’s a HUGE difference. The main difference is that one method gives correct geometry, and the other does not. But then on a “looks like” model like this one, is that really all that important? This model is primarily for demonstration purposes, so this kind of difference is always instructive in some way (except to eternal beginners who only want straight-line step-by-step tutorials).

So, here are some questions for the peanut gallery:

1. Do you sometimes accept incorrect geometry if it will save you 2900% rebuild time?
2. Do you ever try alternative methods to improve either on a geometrical or rebuild efficiency goal?
3. Do you visualize the features in your head before you start modeling a part?
4. When you are forced into a detour/workaround, do you take the question to someone like the forums, blogs, resellers, colleagues, a friend on email, etc?
5. How often do these adventures in every day modeling turn into enhancement requests or SR reports?

Its funny how many tutorials out there are starting to make you pay to get the tutorial. Whether its for a car or a motorcycle or a lamp. That tutorial is going to have to be pretty good to be worth the time to go through it as well as the cost for the thing itself. I’ve never bought one of these things, so I don’t know how good they are – either for the quality of the finished model or the generalized info you can apply to other modeling projects.

The danger with a tutorial is that all it teaches you to do is the specific task at hand, like modeling the seat from the SolidWorks chopper. How many times in your career will you do that? This is part of the reason I don’t like tutorials. They might be ok for students who are primarily interested in completing a class, not really in learning anything useful. But I do like case studies. I know, different words, same thing, right? Maybe, but not to me. To me, a case study is a look at the decision making process for how you made something. For example, how you model a Batmobile is unimportant. You will never need to know how to model a Batmobile. You may however, need to be able to apply some of the techniques used in modeling a Batmobile to other modeling projects, and that’s what I hope to convey here.

This will turn into a multi-section post, kind of like the Model A. Like the Model A, I’m not looking to do an exact replica of the Batmobile, but an interpretation. The tires from that era of car just remind me of Blues Brothers cop car chases.

I’m going to start with the problems I’ve had with SolidWorks while working on this model. There have been surprisingly a lot.

The primary problem that I have been having is caused by flipping connectors. I’m not sure what causes this problem. Possibly it is part of the enthusiasm for change that SolidWorks has made part of their product called Kneejerk – any intentional change causes a random change in an unexpected location. Because Change is Good, right? And SolidWorks is out to impose the maximum amount of Good on you that it can. For example, if I change a couple of spline points in a sketch used in a Boundary Surface, that Boundary or another one might see the connectors flip on it. Just so you know, the pink is supposed to connect to the pink and green to green. This was the first Boundary surface in the part, and it flipped after there were 60 other features dependent on it.

When you flip the connectors back, apparently it matters which curve you flip, but you don’t have any way to know which way is which. If pink are both on the left, the model will rebuild ok. If green are both on the left, all of the edges are renamed something SW doesn’t understand and the model is TOTALLY fubared. This is one of my favorite errors of 2010. In previous releases it was that the Trim features would flip, or the mates would flip, or who knows what.

Anyway, if flipping connectors is not your kind of thing, maybe flipping Ruled surfaces are. Here notice the orange surface that seems to be going the wrong direction. I wrassled with this particular one for quite a while. This uses the “tapered to vector” option, and (even though it worked correctly a couple of weeks ago when I first did this) I could not get all of the edges to taper in the same direction. I was able to trick it, however, which works almost as well. I reduced the angle until the edge did flip, then increased the angle to what it was originally. Yes, it worked, and no, it doesn’t make any sense. Why did I even think to try that? Because that I know making sense is not something you need to necessarily expect from this software.

Ruled surfaces are defined as surfaces that you can lay a straight edge on in one direction. So any extruded surface is a ruled surface, even an extruded spline. Ruled surfaces are great for creating draft, especially from a complex 3D edge. You can make Ruled surfaces from edges with the following options:

• tangent to surface
• normal to surface
• tapered to vector
• perpendicular to vector
• sweep

These are useful in so many ways, that describing each of the 5 options would take a lot longer than we have here. Just to say that “normal” means “perpendicular”, and “vector” refers to the normal vector from a plane (a line that is perpendicular to a plane). Why it is that they say “vector” when they mean “plane” when they don’t really deal with face or plane normals anywhere else in the interface or documentation is kind of a different issue. Its as if SW is just admitting that they expect users to learn surfacing from some source other than SolidWorks sources.

Aye, if I were to document all the stuff that went wrong with this model, I wouldn’t have room for other stuff. In the end, this is a cool looking model, and SW is able to achieve some nice results, if you know which rock to look under and you’re persistent.

Ok, well, here’s another one. I like the detachable propertymanager because its more manageable than using flyout FeatureManagers. But this is one of those features SW puts in but effs it up so badly that no matter how much you like the idea, you still can’t use it. The PropMgr is supposed to automatically expand to show the entire content of the window, but as you can see, it doesn’t, and it totally effs the interface.

Some PropMgrs like Delete Face even have an offset target area for the check. In this case, you have to hit about 20 pixels south east of the green check to activate OK. Annoying. Really interrupts workflow when you just have to remember that a couple of commands you have to hit in a hidden sweet spot to get them to work. And it never opens the window wide enough, and it always defaults to the same option, not the option you used last. At least the functionality works most of the time, even if the interface doesn’t.

I’ll be back later with another post on how I got started with the batmobile.

Now that the furor over direct edit has passed most users by unaffected, and it looks like SolidWorks is the only company that doesn’t have their hair on fire over this topic, maybe its time to reexamine it, especially in the context of history-based modeling. There is a lot of background reading that you can do here on this blog, by going to the Categories drop down on the bar to the right and selecting Direct Edit, or by going to Phil Hamilton’s blog, also with a link in the side bar.

I’d really like you to go back and read this one post on how SolidWorks could make their implementation of history-based modeling better. If you need something more basic, here is another primer post. The more I think about it, this blog post really contains what I think is the key to SolidWorks moving forward and laying to rest some of the silly accusations of the direct edit marketers. Who knows, it may even hold some keys to what Autodesk is messing with in Fusion. The ideas are from both me and people who have made comments on this blog.

Anyway, I want to take a more practical look at how some direct edit functionality currently works in SolidWorks, and some philosophical questions about if you are going to create the CAD equivalent of a black hole or a loop in time by using direct edit and history based modeling at the same time.

Phil Sluder is one of the better SolidWorks users you will find anywhere, and I’ve heard him express this sentiment before. He’s not the only one. I’ve said something like it from time to time. Phil’s tweet reminded me of this (and coincidentally gave me an opportunity to show what I think is a useful use of Twitter for work purposes, even though he didn’t fit his idea into only 140 characters).

Just look at what Phil has to say. He just moved some faces instead of changing dozens of dimensions. Is he being sarcastic? Is cutting down your work like that really that “sleasy”?

I totally agree with Phil. I think you can only understand what appears to be a sarcastic contradiction if you’ve actually gone slease yourself. Admitting it in public is the next step. I’ve done it a number of times myself, but the only part of it I’m proud of is how much time I saved by understanding advanced functionality. I don’t get a feeling of heroism for following the rules regardless of the cost.

Phil said the part deserved it. What could he possibly mean by that?

Well, here’s an example of a part where I used some sleasy modeling methods, and I saved myself a ton of time, and yes, I think this part also deserved it.

This is a part I’ve shown a few times because it has a lot of great examples of different kinds of modeling in it. First, it is part of a set with another very organic looking part, and they have to fit together perfectly on some organic shaped surfaces. That’s nasty. It’s really part of a family of parts that I’ve been working on for the last several years, including size and functionality differences. Originally there were some master model type techniques going on, but with all of the impossible changes and with the range of sizes, much of that is just a distant memory. In all, these parts have features that are long forgotten, some that were made and never used or removed, some that were created, then cut out but not deleted, and so on. In all, it’s like a concept model that never got cleaned up. And yes, hard tooling has been made from some junky data. With all of the changes the customer makes, from time to time, I have had to just go back and do a fresh remodel on a part rather than have another hack at it.

The point here is not the fact that from a parochial parametric point of view the data is ugly junk. The point you need to remember is that you don’t need to be so parochial about your data. You can actually work with “ugly junk”. In fact, there are several software tools that use this ugly junk method of modeling exclusively. In this case, I’m thinking particularly of something like CoCreate. The modeling I am calling “slease” and “ugly junk”, are what other people call direct editing.

Anyway, back to the part.

In this part, I just used the Move Face tool to offset the outer faces that were created by a set of features including sweep, split line, boundary, loft, trim, delete face and replace face. I could have gone back in history and changed a couple of sketch dimensions in a couple of different sketches, controlling different features, and take the chance that all those down stream features are gonna blow up, or I could just put the Move Face at the end of the feature tree. Oh, and there is a Scale feature in there somewhere too, so I would have to back calculate the sizes needed so the scale would come out correctly. Is your head ready to split yet? Do you blame me for going “sleasy” on this one? It probably saved 45 minutes, or possibly a couple of hours if I had to repair a bunch of features.

On the downside, next time I edit this part, I’ve got to remember what is driving the final shape. I’ve got to remember that the Move Face feature has final say, and not the Scale, or the sweep, or the loft, Move Face has some characteristics that make it a wonderful tool, but the same characteristics can be maddening. For example, if you use Move Face on a model, it does not rename the face or edges (unless it causes a face to intersect with faces different from the original intersected faces). So that means that if you click on a face moved by Move Face, it lights up the original feature, not the Move Face feature (unlike some features such as Split Line).

Here’s another one in the same part:

If anything, this one is even uglier than the first one. The image shows the result of an offset. The alternative to this was to edit a shape in another part that was inserted into this part, which would probably involve adding a configuration so that the one version would be used here, and the other version in the original context of the part. In short, the lip around the part shown here had to be treated like imported geometry. In the original part, the faces were created by a complex lofted surface cut, then the faces were brought into this part and made into a solid. So I could go back and try to mess with all of that, or I could just do what is completely natural in CoCreate, and just cheat, and use the Move Face tool.

I’m not sure what type of parts Phil was working on, but I recognize his conundrum. History-based modeling is all about process. Most of us recognize a lot of benefits from that history-based process, but it can sometimes be difficult to manipulate. Sometimes it is easier to just step outside of the process.

I’ve had a look at Spaceclaim, and CoCreate and Synchronous Technology, and I’ve got to say, that there are things I like about being able to ditch the process. The big argument is that the history is A) hard to undersand and B) bogs you down with rebuild times. These are true to some extent, but the marketers are trying to instill fear, while going short on facts. The history-based implementation in SolidWorks is not so hard to understand because you can click on a face in the model, and it scrolls the selected feature in the FeatureManager (requires a setting – Tools>Options>FeatureManager>Scroll Selected Item Into View). The demos for direct edit modelers represent people fumbling around with a tree trying to find which feature controls which geometry.

The rebuild times claims are true, but for the types of geometry that you can actually edit with something like Spaceclaim, the shapes have to be simple, so the trees are likely to be less complex than more complex geometry, and in that kind of part the rebuild times are not much of a problem. The direct edit marketers found a valid pain point in history based modeling, but I think have failed to demonstrate a relevant connection between their solution and our problem.

In the end, SolidWorks can currently handle both history and direct edit functionality simultaneously, but seeing a direct edit feature in a history based tree begs some underlying questions. I only use these methods when I have to, or when its not an option to do it the correct way. Even things like patterning or mirroring faces can be considered direct edit. These are considered valid ways of working in the direct edit world. I really think that if SolidWorks takes the ideas in the history implementation post and combine them with improved direct edit tools and functionality, they will have an unbeatable combination that will settle the history vs direct argument for the foreseeable future. The existing tools are good, but raise a lot of best practice questions. Additional control over rebuilds and the tree are needed to make this really make sense.

My experience installing Windows 7 was not bad. I downloaded the 3.5 GB file, burned it to a DVD, and rebooted my machine with it in the drive. The Siamese Fighting fish is the default desktop image. Those are awfully big bubbles from such a small fish. The background appears to change every so often, like a background slide show.

I previously had this machine set up as a dual boot, XP32 and Vista64, but it quickly became aparent to me that XP 32 was redundant except for the software that came with a voice recorder. I figured that wasn’t enough reason to keep the dual boot. 

When Windows 7 installed, it took the old XP directory and renamed it. This caused some minor software installation problems on the Vista64 install. More due to sloppiness on my own part than anything to do with Windows 7 install quality. The install size for XP was about 17 GB, and for Windows 7 it is about 11 GB. That’s a good sign.

It seems to have messed with the computer’s time. The time was off by an odd number (like 2 hours 45 minutes). The time error carried over to the Vista side as well.

When Windows 7 installed, it automatically got a driver for my scanner, plus it automatically set up my dual monitor system, with appropriate resolution on each. The install took maybe 20 minutes, and required one reboot. 

If you haven’t done a dual boot system before, it’s easy. It takes a little guts and some faith that you’re not just overwriting all of your hard work. With a system that already has a functioning OS, make sure you have a second hard drive. Not a second partition on a single drive, but a physically separate drive. When asked where you want to install the OS, point it to the second drive. When you boot the system, it will give you 30 seconds to choose between Windows 7 and Vista, or whatever your other OS is.

When you dual boot using a non-Apple computer, you don’t need additional software to make the dual boot happen. You just install to another drive, and Windows updates the boot file so you have the option of which OS to run at boot time.

It recognized my stuff fine, including all of my external drives (although it got them in the wrong order) but Google Chrome browser doesn’t seem to work… bummer. It installs with IE8, which I haven’t used yet. I started this blog post on the Vista side, and am finishing it on Win7.  Snagit installed without a snag… and works. It comes up by default with the Win7 continuation of the Vista Aero interface. I learned recently that turning off the Aero interface in Vista is responsible for a graphics glitch where the only part of the screen that will update is the little section behind the context bar after it disappears. So on this install, I’ll try to leave the shiny sh!t turned on.

It didn’t recognize my printer. It knew what my printer was (Oki 5150n color laser printer), but there was no driver to work… so maybe here we go again with hardware and drivers. It installed the microphone correctly, although it made it look like a generic device.

Accessing the SW site, the Flash player installed in about a second. Far better than the minute of messing around you have to do in other OSs.

Overall, Win7 is noticeably peppier than Vista or XP. Because it’s dual booted on my everyday work machine, I have a good idea of how fast this computer is on Vista, and this is a good bit faster. Very noticeably faster.

While I’m wating for SW to install, some impressions. I like the way the new Win Explorer is laid out better than Vista. I guess if you’ve used Vista you’re a bit softened up for this. Almost all of the Win7 press has been positive, and most of the users are saying good things. Of course that doesn’t usually influence me that much, I’m not seeing a lot here to dislike. The UAC does pop up and darken the screen so you can’t do anything other than deal with it, but I assume that like in Vista, it should be easy enough to configure. I understand it has a slider so you can tell it how much you can tolerate.

Surprisingly, Win7 installed without any gadgets turned on by default. I like that. It doesn’t crowd me or overwhelm me with stuff to deal with right away, but I have the option.

The Alt-Tab interface is different. It will hide each window except the window the Alt-Tab cursor is currently on. I like it. It makes it clearer and more obvious to find what you are looking for.

Getting a screen shot of that was a little tricky. It wouldn’t allow the PrntScn to work, so I had to trick it and use a timer.

It also has a nice trick where if you drag a window close to the top of the monitor, it will automatically expand it full screen, but dragging your mouse back down undoes it. That is nicely executed.

So, after all that, SW is installed. I was able to activate it. Not sure how that works with two activations from different OSs coming from the same computer, but it did work.

I did a Scooby test, and it came out to about 22.7 seconds, which is almost 2 seconds faster than the same machine in Vista. 2 seconds isn’t much, but it’s 10%. At least that’s 10% in the right direction, which is more than what we are used to with successive versions of SW or Windows. I’m listed in Anna’s spreadsheets so you can check my old results anyway. For reference, this machine is an XI,MTower, C2D E8600 3.16 GHz, 4 GB RAM, Quadro FX1700.

There does not appear to be a setting for classic mode on the Control Panel. And while I’m at it, it looks to have recognized the fx1700 video card, and even installed a driver for it (8.15.11.8171). Still, SolidWorks is running in Software OGL mode. It was difficult to find the information about the graphics card. It was quite buried on the screen resolution page, click Advanced settings. I didn’t find any other way to get to the graphics card.

Anyway, this is a quickie test, and things look positive at this point. I’m not going to use this regularly, mainly because of Google Chrome and my printer. I don’t have any need at this point to be so far over the bleeding edge that all of my functioning appendages are cut off. Its nice to know this is here if I want to check or verify something, its also nice to know I don’t have to use it yet.

This is part 1 in a series just on Toolbox. It has started from the series on CAD Admin. Toolbox is not a topic that you can talk about in a single long blog post, there is just too much there, if you’re gonna do the topic justice. 

Toolbox may not be exactly what you think it is. The image to the left shows how SolidWorks describes Toolbox in their Product Matrix. They call it a “Standard Hardware Library”, and say that you have access to “pre-built SolidWorks models”. It may be picking nits, but strictly speaking, neither one of these statements is true.

When I think of a “library”, I think of a place where I can go to get something that is there, something that exists. Toolbox doesn’t really work that way. With Toolbox, you tell it the class of thing that you want, and it builds it for you. This may or may not be an important distinction for you.

Toolbox consists of 3 parts:

1. Toolbox application – software that “does stuff”
2. Library of blanks – SolidWorks parts used as templates, which contain all of the geometrical options available
3. Database – contains all of the dimensional and “metadata”  used in the finished parts

If you have a real library, all you have is #2. So having software and extra data in a database is extra, and should be better, shouldn’t it? 

Yes, and no. It is better than just a library because of things like Smart Fasteners. SF enables you to automatically place the correct sized hardware into holes automatically. The problem is that it only really works that way in special situations. So you could say that it helps some of the time, and just gives you something to undo some of the time.

So in a nutshell, here is how SolidWorks Toolbox works:

1. By default Toolbox installs as a single user installation, where the library is local. There are many options during install in 2009, and I’ll talk about those in a futurearticle. Libraries can be shared or local.
    
2. By default the Toolbox database installs locally, but it can also be placed on a network for a shared install. The database is called SWBrowser.mdb, is typically located in a folder called C:/SolidWorks Data/lang/English, and for SW09 sp3.0 is 87.876 MB. You can browse and edit the file using Microsoft Access.
    
3. Toolbox is an add-in, so you have to activate it using the Tools, Add-ins menu. It is really 2 add-ins, SolidWorks Toolbox and SolidWorks Toolbox Browser. What I am talking about here is mostly the Browser. This is the user’s first clue that Toolbox is not just a library, it’s also an application, software.
    
4. Toolbox is used by drag and dropping Items from the Task Pane into the Solidworks graphics window. (There are also other ways to get parts into an assembly.) But before you do that, this is what you are confronted with, shown in the image to the right: a list of standards. Yes, but you can trim down that list of standards so it isn’t nearly as irrelevant. True, you can, but why hasn’t it been done? This is the way it was installed, even though during the install you specified ANSI standard and Inch units.

   So you have to configure the standards a little. You might even find after using it for a while that what you really need is a custom standard. Fortunately, it’s easy to do, but the hard part is first figuring out that it needs to be done at all, and then where you go to do it.

    It turns out that you have to go to Toolbox, Configure Toolbox, Select Your Hardware. From there you should just unselect any standards from the list that you don’t want to use. Be aware that when you open the Configure Toolbox dialog, it may take some time, because SolidWorks is opening up that 88 MB database file in the background. If you have a shared install, it may take even longer because the database has to be opened over the network.

5.  After you get the standards set up, you drag and drop the type of screw onto the edge of a hole. Toolbox should orient it correctly, but if it doesn’t you can always press the Tab key to flip it 180 degrees.

   At this point, Toolbox asks you to choose a size and gives you some other options. If your Toolbox is a fresh unused installation, the part that Toolbox is using has only a single size, which is most often the largest size in the library. When you select a size from the interface, Toolbox selects the dimensions for that size, and creates a new configuration in the fastener.

   But hold it. What if this is a shared installation? Or what if I get an existing assembly with my new Toolbox installation?

   Well,  in those cases you should have known something prior to getting put into that situation. Again, most users find all of this out by accident, and usually after they have lost a lot of design data in assembly files. There are answers to each of these questions, but the fact is that many users don’t even know that the questions exist until it is too late.

As you get deeper and deeper into Toolbox, you come across many scenarios that may not be ideal for you. In almost all of these situations SolidWorks has provided for a way to resolve the issue in some fashion. The problem is knowing there is a solution, because solutions are not always obvious, and in many cases knowing there’s the potential for a problem, again because the need for a solution is sometimes not aparent until it is too late.

The truth is that the default installation settings work well for a stand alone user who does not share data with other Toolbox users. But the default settings can be disastrous for other types of use scenarios.

This Toolbox subtopic of the CAD Admin series will continue in a future post.

Thanks again to everyone who submitted a model for this challenge. I’m getting some good feedback from people about this series, particularly from those who haven’t had the opportunity to do much surfacing work in the past. There’s no pressure, and we’re all just here to learn.

I want to start this by discussing the reason I built my model the way I did. I started with a sweep from an arbitrary position along the spoon. It’s not really arbitrary, I started it at the point where I wanted the decorative pattern to fade into the smooth face of the handle.

Because both ends of the spoon are going to be round, or come to a point, I just needed a place to start the sweep. A sweep can only come to a point on one end. Mark B at SWW this year showed that sweep paths no longer need to end in the plane of the profile, so that was one thing I wanted to show. Another reason I chose the sweep was to show something about splines. If I had chosen an arc for the sweep profile, the sweep would fail where the handle transitions into the bowl. That is because arcs cannot flip convexity (from being cupped up to being cupped down). So I had to use a spline as the profile. 

Also if you notice, the sweep itself is symmetrical, but I only have a guide curve on one side. You cannot mirror things like projected curves. The way I handled this was to establish a Symmetric sketch relation with the ends of the spline. Because a sweep rebuilds the sketch at every intermediate section (intermediate sections can be seen by clicking the eyeglasses icon at the bottom of the Sweep PropertyManager), which means that they convexity flipping and symmetry are important to build into the sketch. Boundary and Loft don’t do this kind of thing, so the sketches can be “dumb”, but a sweep profile sketch has to be “smart” enough to rebuild at every point along the sweep. 

Next I built the tail of the handle. Notice that I ignored the fact that the spoon is supposed to be round at this end. The reason for that is that it isn’t easy to draw the stepped sketch on a curved surface, so I just decided to build it this way and trim it off. Anyway, what I’m trying to do is to create a scallopped pattern that fades into the smooth face. I drew several 2 pt splines, using handles to make them J shaped, then mirrored them. Then I made a Boundary surface between the sketch and the edge of the original sweep, reusing the rest of the mid plane sketch. Reusing sketch entities is an important aspect of both modeling efficiency and associativity. 

Next I tried to thicken the spoon, but it wouldn’t work. The problem was this bit at the end where the sweep created a degenerate point. Get used to that word if you’re gonna work in surfacing. It’s not a new concept, it’s just that SolidWorks has been shy about using industry standard terminology. See the Surfacing Bible or Entry #9 of the original Spoon Challenge post for a description of “degeneracy”.

Because the degeneracy wouldn’t thicken, I cut it off with a Trim feature. Before I did that, though, I made a Ruled surface that goes around the part to maintain the edge of the tip that was being trimmed away. When I trimmed the spoon, I also trimmed away the part of the Ruled surface that I didn’t need. The best way to describe this is to just look at the part and see what happens in Surface-Trim3. 

Then from the trimmed edge of the spoon and the remaining section of the Ruled surface, I built a Fill. Notice that the Fill does not create a degeneracy. This is one of the best reasons for using a Fill.  

Next I trimmed off the handle end of the spoon, knit it all together and tried to thicken it. Again, thicken wouldn’t work. This time the reason was the sharp edges between the scallops on that Boundary surface. I tried different thicknesses and different directions. In the end, I wound up making little fillets to take away the sharp corners.

Notice two other things going on in this image. First, the edges between faces are all shown as phantom. This uses the setting View, Display, Tangent Edges As Phantom. Past versions of SW had a different interpretation of “how tangent is tangent enough”. SW09 seems to be pretty liberal, comparatively speaking. I think what we have now can be called a “fix” rather than just “sloppy”. We used to have the problem where tangent edges didn’t always display as phantom. I had hoped that the problem would be solved by making the modeler more accurate, but I think what has happened is that they relaxed the tolerance on the display. Is this right or wrong? I haven’t had any problems with it, and I do like to see edges shown as tangent. 

The second thing happening in the image above is the blue edge. You can set surfaces to show open edges (edges that bound only one surface) in a different color. This helps with other types of models where it is important if a model is open or closed. 

So that’s how and why I built this model that way.

This year I did 3 presentations at World:

• Go with the flow: Efficient use of the 2009 interface
• Tools of the trade: Plastics tools in SW 2009
• Skeletons in the closet: Horizontal modeling

You can download my stuff from the links above. These are powerpoint (Office 2003) presentations with files. The ppt files are not annotated.

This year, SolidWorks recorded the mic on the presenter and took a feed from the projector, and will be making the presentations available in that recorded audio/video format. That will be nice. I don’t know how/when they will be available, but they are coming.

Just a note on the Skeletons part. I was not able to edit out the relationships between the features. In theory you should be able to delete the first feature, and all of the rest of the features would remain except for the fillet features. Unfortunately in SW this doesn’t really work. SW makes relationships between features in other ways, but you can use the “also delete all child feature” (sic) option. It seems SW needs to re-evaluate how it evaluates child features.

Honestly I was overwhelmed with the response to the puffy cube challenge. I want to thank everyone who sent in a model or comments. There were a total of 31 responses, and I turned away a couple Solid Edge entries. I learned a lot of stuff, and noticed a few things about how people model and maybe even think.

The part originated in a surfacing class I used to give years before the surfacing book came out, and also by a disastrous demo I did for a group of Xerox ID folks many years ago. The demo was basically to make a box in such a way as to tug and pull the edges and faces. Of course I didn’t learn that until I had failed the test. It was a “do this, do that, now make it change some other way” sort of test, so I couldn’t really avoid failure. I equated the design they were looking for with a “smurf” house – you know, where everything is round and made of blue and white marshmallows. Anyway, the puffy cube became a way to represent something that looked easy, and maybe “should” be easy, but certainly wasn’t straight forward.

First, when I looked at this part, I saw a great excuse to do surface modeling. Several of you saw it as a solid with boolean operations. Almost everyone approached this with some sort of pattern, usually two patterns, or a pattern and a mirror. My initial model was like Mark Landsaat’s, where I revolved a surface, patterned it around, then trimmed it and made it solid. I guess the reason I did it that way is that after doing so much surface modeling, I tend to think of parts as consisting of individual faces.

Entry 4 from Clay Corbett skipped the pattern altogether using a pair of lofts from 3D sketches and a knit. Entry 26  from Mike Wilson used a Move/Copy Bodies rather than a pattern, and Entry 30 from Pilun Chen used a curve driven pattern to overcome the need for multiple patterns.

Another trend that I liked was that people are beginning to get the hang of the Boundary surface. In most cases, boundary can be used as a direct replacement for loft. There are very few places where lofts can achieve something a boundary cannot (the exceptions being centerline lofts, closed loop lofts without direction2 curve). Chris Cole and Brian McElyea made good use of the Fill surface.

Several folks also used surface bodies as reference geometry, which is a use of surfaces that I like to promote amongst solids users. Mike Wilson used a surface as an Extrude Up To reference. Others used surfaces for their edges or to create curves.

Entry 29 from Matt Cummins was the only one to use partner software to achieve changes. Matt works for Tacton Works, a knowledge based engineering software vendor. I think Matt’s example shows the strength of KBE for work of this sort.

Many of you used 3D sketches in a way I wouldn’t have thought of. The first thing I learned about 3D sketch was that you can combine a lot of things that would otherwise take several 2D sketches into a single 3D sketch. Of course this makes the 3D sketches much more complex. Most of these techniques used planes inside the 3D sketch. 3D sketch planes can sometimes be difficult to control if your sketch is underdefined.

Pilun Chen (entry 30) gets points for the successful utilization of a curve driven pattern. I thought this was a very creative approach to solve the patterning/mirroring issue.

Clay Corbett and I tied for use of least features. I think Pilun Chen’s model could have been reduced by a sketch with a little effort.

For breaking the rules, I liked Mark Kaiser’s model with the straight edges, and several of the solids approaches. 

The most novel approach I have to give to Pilun Chen for that curve driven pattern. 

What did you learn from this exercise?

PS: the next challenge will be posted in the next week before SolidWorks World.

The winning blog post suggestion from the recent contest came from SolidWorm, and he suggested a monthly surfacing challenge. You all voted for him and agreed, so here we go. We’ll start this one off simple. This is a nice example of justification for surfacing. We will build up to more difficult surface modeling challenges as we go.

Sometimes instead of a flat face you need something with a little bulge to it. There could be many reasons for this, including general looks or even to increase stiffness.

The challenge here is to create a box with puffed out sides. Each side must have curvature in two directions, so they could be created by revolving an arc, but not by revolving a straight line.

Any method other than import is valid, and you can use any technique as long as a surface feature is used at some point. The finished puffy box must be a solid body.

Make the distance between adjacent corners 1 inch (25.4 mm), and make the part centered around the part origin. Each side should be the same size and shape, so I’m looking for something cube-ish.

Use the comments to ask for hints or suggestions.

Since this is an easy one, and SolidWorks World is a month from now, lets make this one end on Monday, Feb 2 – Ground Hog Day. Send in your model to me at matt (at) dezignstuff (dot) com. On Feb 2, I’ll post the way I would do it, but I’ll also post my favorite methods from models submitted. I always learn something when I see how other people model stuff, even something relatively simple like this.Â

There are no prizes this time, but I’ll be looking for:

• fewest features
• most robust through changes
• most novel approach
• most creative way to break the rules

Best of luck to every one!

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Entry 1 is from Kalpesh Navale. Click the feature manager to the left to download his part. This is a very interesting part. Extruded surfaces are used to create intersection split lines, which are lofted together to create the faces of the puffy box. Very interesting! How will you make the part?

 

 

 

 

 

 

 

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Entry 2 is from Charles Culp. Another interesting model. Charles made curved sketches forming a X and then used the Boundary feature to make the surface, patterned it, then trimmed.

 

 

 

 

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Entry 3 is from SolidWorm. Again, this is a solution I wouldn’t have thought of. Â This involves a solid as construction geometry, planes, sketches, and a boundary surface patterned around.

 

 

 

 

 

 

 

 

 

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Entry 4 from Clay Corbett. This one uses an extensive 3D sketch with planes to minimize features, and then makes the faces of the part with lofts. Clever, and nicely done.

 

 

 

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Entry 5 from Brian McElyea. Five entries and not a duplicate yet! Nice job on this one. Just a single surface creation feature, and the first Fill surface entry. Brian created a framework using a 3D sketch, and used a Fill to make a surface between the 3D sketch elements. Then pattern twice and knit.

 

 

 

 

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Entry 6 is from Garrett Brooks. This one uses another clever method that I wouldn’t have thought of. This is also the first to use a revolved surface. Garrett revolved a surface, then extruded a square with draft and used that to trim the revolve. Then the familiar pattern and knit.

 

 

 

 

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Entry 7 is from Steve Martin. Steve started with a 3D sketch, built planes, then sketches, and built a boundary from the sketches. Then he patterned the boundary, and built 2 more boundaries from the pattern. Very nice.

 

 

 

 

 

 

 

 

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Entry 8 from cgroh. Another boundary suface user, but this time with a twist- a Thicken and a Scale, presumably to get the dimensions correct.

 

 

 

 

 

 

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Entry 9 from Arthur Young-Spivey. Arthur made 2 versions, separated with folders and configurations within the same part file. The first uses a 3D sketch and a boundary surface, patterned, then two more boundaries, and finally knit.

 

 

 

 

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Entry 10 from Arthur Young-Spivey. Arthur’s second entry is called his “robust” version. It uses a layout sketch, a series of planes, a series of 2D sketches, a Boundary surface, circular pattern, then two lofts and a knit.

Two patterns seem to be employed in most of these parts, either patterning a face twice in opposite directions or once, then using additional features to cap off the first pattern. A variation on this is to make a single feature with 4 sides. 3D sketches are popular because they reduce feature count, but notice that Arthur doesn’t use the 3D sketch in the one that is “robust”. 3D sketches are prone to failing for reasons other than ones you might expect.

I think there is a lot to be learned from seeing how several people make these models. I will analyse in more depth after the end of the challenge.

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Entry 11 is from Mark Kaiser. Mark took a different approach, with straight sides on his box. He used a single loft created from a set of 2D and 3D sketches.

 

 

 

 

 

 

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Entry 12 is also Mark Kaiser. Similar to previous with a boundary surface instead of a loft.

 

 

 

 

 

 

 

 

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Entry 13 is from Mark Reader. Mark notes in his email:

“Something happens tolerance-wise if I replace the surface-revolve sketch with a single spline curve coincident with the wireframe cube corner. Â It builds find of course, but measure to the corners and it’s not 1.000Â consistently. Â Some measure just over and some under.”

Something to look into here… Also notice that all of the Origin icons in the FeatureManagers for these parts are red except for this one. Odd.

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Entry 14 comes from John Travis. John starts from a solid cube, makes some planes, then sketches, then patterns, knits a solid and combines solids. Nice job!

 

 

 

 

 

 

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Entry 15 comes from Jason Knox. This one is actually the closest to what I would have done. Revolve, pattern, pattern, trim. I have another trick up my sleeve if no one comes up with it, where I can get away with making a single face and a single pattern, no mirror or additional face features.

 

 

 

 

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Entry 16 again fron Steve Martin. An interesting method that copies a face of a 4 sided Boundary surface to pattern around and close off the open ends.

 

 

 

 

 

 

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Entry 17 from Chris Cole. All solid, but creative use of the Combine/Common feature.

 

 

 

 

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Entry 18 again from Chris Cole. I think this is the first one to start from a triangular slice.

 

 

 

 

 

 

 

 

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Entry 19 from Matt (me). The key to minimizing features is to use a 3D sketch, but there is a huge price to pay. Reliability and ease of use are not the best traits of 3D sketches.

 

 

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Entry 20 from the one and only Phil Sluder. Wow, this is exactly the way I did this originally, for the model shown at the very top of the article. Revolve, pattern, pattern, trim, thicken.

 

 

 

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Entry 21 from Ken Kronholm. Revolve, 2 patterns, series of trims. Nice alteration – Ken has a series of configurations from 1 to 36 that change the box from squarish to almost spherical.

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Entry 22 from Keven Bouwman. Kevin starts with a solid and makes surfaces to cut the solid. It’s getting difficult to make unique solutions after this many entries, but this is unique.

 

 

 

 

 

 

 

 

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Entry 23 comes from R. Paul Waddington. RPW used AutoCAD to create the shape. The two blue blocks are solid, and the varicolored one is surfaces. The DWG file is linked to the image above. Most of what’s interesting with this challenge is seeing how people did it, which we don’t get to see with the Acad data, but it is interesting that he was able to do it at all. RPW is a frequent and valued contributor to this site, although he is an AutoCAD reseller.

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Entry 24 is from Mark Landsaat. This is another version of the part I made for the image at the top of this article.

 

 

 

 

 

 

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Entry 25 is from Matt Lombard. In honor of Thomas Edison who discovered many ways to not make a light bulb before he discovered a way that worked, this is a failed attempt at using fewer features to make the puffy cube.

Here’s how the concept works: the only kind of pattern that can pattern all the faces of the cube at once in a single 3D pattern (instead of using 2 2D patterns or a circular pattern and a mirror) is a curve driven pattern where the curve is on a 3D face. I had to first make the face, which required making a 3D sketch with a lot of planes in it in order to use the sketch entities (with the selection manager) and the Boundary feature. Then I made a sphere, and placed 3D sketch points where each of the XYZ axes would intersect the surface, then I drew a Spline On Surface through all of the points, using the Tangent To Curve option, and a Face Normal selection.

The concept is great, except that it doesn’t account for the alignment of each face. In order for this to work, the Spline On Surface would have to go through each of the 3D sketch points in a particular direction, in addition to being a controllable length, because the Curve Driven Pattern only enables you to place pattern instances either equally distributed along the entire curve or at a given spacing along the curve.

I also tried this with a series of straight lines in a 3D sketch where the 3D sketch points were the midpoints of each line. Â I just can’t get it to work. I’m sure there’s a way to do it, but I haven’t found it yet.

I thought a Sketch Driven Pattern would work, but it wouldn’t do a 3D pattern, only a 2D pattern. Any ideas for this? I don’t think it’s impossible, just really difficult.

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Entry 26 from Mike Wilson. Yes, THAT Mike Wilson. And just as you’d expect from Mike, this solution is creative but simple, and different from what anyone else has come up with to this point. Mike starts with a revolved surface, then extrudes up to surface, then patterns the body twice with the Move/Copy feature. It’s getting harder and harder to add something no one else has done, but Mike pulls it off.

 

 

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Entry 27 is from Stacy Abel. Stacy’s differentiator is the use of several projected curves to create the surface. Nice job, Stacy!

 

 

 

 

 

 

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Entry 28 from Dan O’Neill. Another unique solution! This one uses extruded surface as reference geometry from which to build a Boundary surf.

 

 

 

 

 

 

 

 

 

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Entry 29 from Matt Cummins of Tacton Works. This is probably the model with the fewest features. It uses all solid features, which is a little surprising. Revolved solid, patterned bodies, then Combine. Nice job. Also, check out the download for this method. Matt has included a movie of Tacton Works controlling the cube.

 

 

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Entry 30 is from Pilun Chen. Ok, this one gets some credit for solving the pattern issue, although in a different way than I was thinking. Pilun was able to pattern all 6 faces with a single pattern. As I suggested, he used a curve driven pattern, but unlike me, he patterned a spherical solid body, and then booleaned out the cube. I was trying to pattern faces already shaped in order to skip a trim feature later. Patterning bodies and then booleaning eliminates the alignment problem I was having. Download the part and check it out.

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I’ve had submissions from people using other CAD systems, but I haven’t posted all of them. The Solid Edge entries didn’t make sense for me to post because I no longer have a SE license, and while SE folks lurk here, that’s not really the thrust. I posted R. Paul Waddington’s AutoCAD files primarily because I really like his commentary, and because it was interesting to me that AutoCAD could do that type of work.

Entry 31 is from Matt Sederberg. Matt is the CEO of T-splines. T-splines is the name of a company and a technology. It might be an oversimplification, but my understanding of t-splines is that it is a surface technology like NURBS except that t-splines allow partial isoparameter curves, and they need less data to describe the same surface. T-splines can be used with some surfacing programs such as Rhino and interestingly Maya .

Matt submitted his puffy cube model, but really, it looks pretty much like the rest of the submitted models, with only an Imported feature in the tree. Here is Matt’s description of how he created the puffy cube in T-splines/Rhino:

All of the “Xpert” features in SolidWorks are really pieces of functionality that are written to help automate tasks for non-experts. Other Xperts are the DimXpert, TolXpert, DraftXpert, and a few others. Interestingly, if you type in “Xpert” in the Help Search box, you get nothing. So if you’re looking for general information on the so-called Xperts you’re SOL, you gotta know what you’re looking for.

The FilletXpert is one of those pieces of functionality that I really want to love. You can find it attached to the Fillet feature PropertyManager. I understand that SolidWorks used a model I built for Rubbermaid to benchmark this feature. The part was one of those big carts with a lot of ribs underneath the tray to increase stiffness and plastic flow. The following image isn’t of that cart, but just a sample part with a few ribs.

The main advantage of the FilletXpert is that it can help you select a set of similar model edges. Activate the FilletXpert button at the top of the FeatureManager. When you select an edge, the toolbar shows up, enabling you to select one of a set of edge selections. So you can see the attraction. Selecting 47 edges in a couple of clicks. Definitely cool. You have to try this one for yourself if you make parts with a lot of small fillets. 

There are some downsides to this as well, such as the selections are not smart (does not update if rib config changes), but once you make peace with them, the FilletXpert is something that can save you a lot of edge clicking.

This was posted earlier, but I wanted to make sure that after the holidays hoopla that if you wanted to participate you got the chance. 

There are 3 ways to win a SolidWorks 2009 Bible, due to be released in February:

1: Submit a Top 10 list

You can submit something serious or silly. Just make a list of 10 things you like, or would like or don’t like in SolidWorks. 3 submissions have alreaady been made. SolidWorks has a more serious version of this, which resembles something I’ve been suggesting for a while – an enhancement list with transparency so people can vote on it. Some of those enhancements sound an awful lot like bug fixes.

Anyway, SolidWorks is not likely to give you a SolidWorks 2009 Bible. You can only get that here.

Submit entries as a comment to this post.

2: Stupid SolidWorks Tricks

The intention here is to submit a stupid trick that may or may not have practical application in real world modeling.  We’ve only had 6 submissions for this. The first was from Jeff Mowry showing a spiral around a circle that changes diameter. Click on the picture to download his SW part file.

And another one from the one and only Mike Wilson showing pushing bodies into a plate to create shapes. Click on the image to download Mike’s assembly file with parts (zipped).

And another from Mike Wilson. This one uses the Split and Move Face features to create some nice 3D shapeliness that you might otherwise wonder how to do. Click on the image to download the file.

Next are 3 from Charles Culp. The first can only be experienced. It’s one he first posted on the SW forum as a variation of a little trick I posted somewhere demonstrating Verification on Rebuild. This is trippy. Click the image to download the SW part zipped. It doesn’t look like much until you rotate the part, paying attention to what looks like two separate bodies.

Charles submitted another one, an optical illusion. Click an image to download the part file. This is another one of those, you gotta rotate it to believe it kind of parts. And then how would you go about modeling something like this?

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

Gabi Jack submitted one too. A twisted knot. Click on the image to download the SW part.

And not to be missed, here’s one from Brian McElyea. Look at the feature list. Notice the sketches are all named the same, as are the features. Click on the picture to download the part:

Next is an entry from SolidWorm who shows a set of sweeps that are all made from the same profile, path and guide curve, just using different settings. Click the image to download the file and see how he did it:

Garret Brooks submitted a set of parts in the style of MC Escher. These are cool, and seemingly impossible. Click here  to download the zip file with all the parts.

You can email entries to me (matt (at) dezignstuff (dot) com).

3: New blog post suggestions

The last category is suggestions for new blog posts. The surfacing tutorials seem to be the most popular stuff. A good example of a great suggestion is the basis for a couple of posts such as the Wavy Edge or the Tricky Modeling Situation. These were both suggested by my friend Stan in response to real world modeling questions.

Submit entries as a comment to this post.

This will close one week from today, so submit stuff now!

Ok, this one is from my friend Stan. Stan was also responsible for the three-cornered dome modeling challenge from a few weeks ago. Now Stan wants to put a wavy edge on a pot. I see this same issue come up when people ask for a “wavy washer” or belleville washer. They will use the same techniques. 

I’ll show a couple of ways to do it. Because I was slow on the uptake, Stan came up with a solution of his own, which shows some nice technique with a Spline-On-Surface, relations to a layout sketch and a reference plane.

With the spline in place, he was able to sweep a cut. That spline must have been a lot of work, and as always with the spline you need to be careful. Sometimes sketch relations don’t work the way you think they should. Stan also said that he wanted more control over the shape of the spline at the bottom of the wave, so he didn’t want a completely top/bottom symmetrical sine curve.

Here is the way I would have done it. Much simpler, I think, and with easier to control shape:

So that’s a loft between lines on angled planes, mirror the surface loft, pattern the mirror, knit it all together, then cut with surface. Of course you can use an equation to drive the spacing and size of the waves. Consider using a global variable for the number of instances for the circular pattern. Because the angled plane happens before the circular pattern, driving the plane angle with the number of instances will cause some problems with history (might require 2 rebuilds to be correct).

Use the tangency weighting in the loft feature to control the shape of the wave. For example the lower sketch might have a 2 weight instead of the default 1 weight. This would make the lower part of the wave wider, and the top narrower.

Another way to do this, if the pattern were something other than a wave, would be using the Wrap feature. I wouldn’t use Wrap on a wave because you’d have to get the wrap to perfectly line up. But on something like the above, wrap and pattern works great.

Ok, Stan is bearing the load for you guys. Who’s next to step up with a cool modeling challenge?

Ok, you guys got me started on this. Now I can’t stop.

I’ve been reading a book about Rhino 4.0. After writing my own book, suddenly the flaws in other books just jump right out at me. It’s kind of painful reading, but there is some good content. In particular, this guy does seem to know something about splines, even if he doesn’t seem to know what to do with them.

Some terminology used in Rhino is not used by SolidWorks users, although it may be used by the people doing the SolidWorks spline programming. Words for this post are: kink, and knot.

Rhino uses the word kink to signify a sharp tangency discontinuity in a spline. In SolidWorks, you can get discontinuity within a spline, but the best way to get it is to simply create two splines that touch at the ends without any tangency constraint. Kinks in Rhino can be useful when you are trying to smooth a sharp edge into a continuous face. Again in SolidWorks, this is possible, but is usually achieved by using multiple features, which tends to break faces up. I believe this kind of thing can be done more smoothly in Rhino because Rhino allows internal kinks in the spline, where SolidWorks requires multiple splines.

To me, having used primarily SolidWorks for so long, splines are intuitively internally continuous, and its hard to think of any curve which is not continuous as a single spline. I’m not a big Rhino user, but this sort of thing seems to work out in Rhino.

The second word here is knot. What Rhino considers to be knots are what are called simply spline points in SolidWorks, the points along the spline used to create and manipulate the spline. As I understand it, SolidWorks splines are “piecewise continuous”, which means that a single equation is responsible for the curve between the spline points. So if a SW spline has two end points and an interior point, it would require two equations. In SW you can achieve a curvature discontinuity within a spline, but you cannot achieve a tangency discontinuity.This post doesn’t really add anything to the arsenal of what you are able to do in SolidWorks with splines, but it does make you aware that not all surface modelers out there have the same limitations that SolidWorks has with splines. It also gives us the knowledge that we could ask for something like a Rhino kink – a sharp tangency discontinuity It never hurts to ask. I would guess that SolidWorks has tried hard to maintain internal continuity, and may not have thought that internal breaks within a single spline would be something users deemed desireable. And maybe I’m the only one, but when you make a sharp edge that flows into a smooth surface, that sort of thing usually has to  be broken up into 3 separate surfaces (one on each side of the sharp edge, and then another on the other side of the end of the sharp).

A commenter recently suggested 3D sketches as a topic for a blog post. It is a great topic, and one that becomes increasingly important the more you get into modeling more complex geometry. This will also be the last in my series based on the Model A. It has been a fun series, and from the looks of things, visitors like the posts on splines and surfacing.

To talk about 3D sketches, I’ll use the motor of the Model A. I didn’t want this project to turn into a research project on car engines, so I thought I’d take the easy route and get an engine off of 3D Content Central. I have yet to get a really high quality model with any detail at all from that place. It never has stuff I want. I know a lot of people say they love 3DCC, but I wind up wasting more time looking through junk than I would just modeling something myself. In this case, I got a block with a couple of extrudes and a cut. That was the best car engine I could get. I added the covers, scoop, pulleys, distributor, wires and pipes. When people do nice work, they tend to not give it away.

Anyway, the pipes and plug wires are the 3D sketches in this part. In this case, the sketches are mostly splines, but there are some lines and arcs involved as well. Let’s start with the plug wires first. The plug wires run from the top of the distributor to points on the side of the engine. On the distributor, they connect at the centerpoint of a circular edge. When drawing a 3D spline, you can reference circle centers in the same way as in a 2D sketch. Just hover the mouse over an edge, then put it near the center, and it references it automatically. For each wire spline, I created two endpoints and one point in the middle. The middle point references a small guide clip that retains the wires in a neat bundle at the back of the engine. When drawing the spline, I referenced the center point of holes on the clip in the same way at the distributor end.

Finally, on the side of the engine block, I had sketched 3 construction lines, made them colinear and equal length, and dragged them to approximate spacing. This gave me spacing and positions for 4 wires.

To get the splines usable as sweep paths for the wires there is still a little work left to do. At each end of the spline I selected the spline handle and gave it an Along Y or Along Z relation. There are no such things as “horizontal” and “vertical” in a 3D sketch, we identify things by axis.

Once the relation was placed on the handle, I dragged out the length of the handle to make sure enough wire was there so the wires didn’t look too tight.

All of these splines were done in a single 3D sketch. In versions of SW long ago you had to create everything in separate sketches, but now you aren’t limited in that way, and sometimes it makes sense to put everything in one sketch.

Notice the way it all looks in the Feature Manager. All of the 3D sketches use the “shared” hand and also the “contour” symbol, indicating that the Selection Manager was used to select a single spline out of the 3D sketch spagetti.

Also notice that I’ve made use of derived sketches again. Derived sketches are great because they are easy to locate, and they all change together without creating link values or other links. They are very easy to create, especially if you make a hotkey for it.

The sweep profile sketches didn’t have to use individual sketches instead of gang sketches ( a single sketch with 8 circles in it, one for each wire), but that’s the way I did it for this model. You can use the Selection Manager for sweep profiles and paths.

 

 

 

Next I moved on to the pipes. These were a little less defined, but still relatively simple in the world of 3D sketches.

The first thing to do was to establish the straight section of the pipe. Everything else would depend on this. So I just drew a straight line, and assigned an Along X relation. I wanted to control how high and how far from the mid plane this line was with dimensions. One thing you have to remember about 3D sketches is that dimensions in 3D sketches do not do the alignment, like horizontal and vertical, that dimensions in 2D sketches do. If you put a dim on an angled line in a 2D sketch, you have the option of getting horizontal, vertical or aligned dimension. In a 3D sketch, you ALWAYS get aligned. For this reason, if you want a horizontal dimension, you have to dimension from a vertical PLANE. So, to locate the straight section of pipe from the mid plane, I selected the Right plane with the Smart Dimension tool, and then picked the line. I did the same thing between the line and the Top plane.

This behavior of the 3D sketch is worthy of an enhancement request. So many things about 3D sketches have improved by leaps and bounds in the last several releases, but dimensioning has not.

Anyway, once the straight section was located, the rest of it was easier.

The pipes come off of an angled portion of the engine block. So, the pipes cannot come off it in one of the X, Y or Z directions. At the same time, there is no relation available to make a spline perpendicular to a face. You can make a spline tangent to a face, but not perpendicular. To achieve the perpendicular condition, I drew short construction lines and made the line perpendicular to the face, and the spline tangent to the line. Messing around like this should be unnecessary in a tool as sophisticated as SolidWorks, but that’s not the case yet.

Each of the curved sections of the pipes are made from a 2 pt spline. One point on the engine and the other on the straight section of pipe.

To finish the pipe, I swept each of the 3 remaining pipes only up to the start of the straight section. In reality, this is a poor way to do things. Because each sweep is ending in a relatively undefined way (at the end of a spline). If you require more accurate geometry, there are better ways of handling this, such as a loft or boundary. In fact, it might have been better to have used a single circle at the beginning of the straight section to extrude the straight away from the engine, and then sweep each curved piece back toward the engine. This would use the same starting sketch for all of the features, which would be ideal.

Thanks for your attention during this series of posts on my Model A cartoon car. Keep the suggestions coming for stuff you want to see.

One of the little secrets about creating complex shapes in SolidWorks is that they aren’t all as complicated as they look. The grille is one example of this. Once you know what you’re doing, something like this is actually very easy to create.

First, we have to select a feature type to use. This is going to have to have curves in both directions, so it could be a boundary. The profile needs to change, and doing guide curves to change the profile would be too difficult. So it will be either a loft or boundary. In this case it really doesn’t matter, so I selected boundary, just because it’s the future direction of development, and clinging to the past is oh, so gauche (he says as he models an antique car).

The first thing I’d do to model the grille is realize that the thing is symmetrical, and that there is a sharp edge at the plane of symmetry. This makes things much easier.

Of course something else you want to do is to get a picture of one you like and work from that. Realize that this is a cartoon Model A, so I’m not really trying to recreate this 100%. It’s gonna be a little exaggerated in some ways. This image of the 34 coupe captures the flowing shape between the front fenders and the grille together. This grille is taller and more narrow than what I’m looking to create, but it has the overall form that I want.

You can start to model this part in one of two ways: draw the curve that becomes the “direction 2″ 3D curve or path for the boundary, or draw the 2D sections for “direction 1″. Direction 1 and 2 are completely arbitrary in real application, but I’m pretty entrenched with the old way of doing things, so I think of Dir1 as “loft/sweep profiles” and Dir2 as “paths/guide curves”. It doesn’t matter how you use the two directions, which is part of the point of the boundary feature to begin with – both directions are treated equally.

Ok, so I select to make the 3d curve path first. The 3d curve is essentially a C shape, angled back and curved in both directions. You can do 3d curves in a couple of ways, but the most important are the 3d spline, and the projected curve. In this example, I’ll use the projected curve. A commenter suggested having a look at 3D sketches, and I will get to that in my next post on this Model A where I look at creating the exhaust pipes and the sparkplug wires.

Projected curves tend to be confusing for people. Not sure why. Some people get it immediately, and some just don’t. Anyway, there are 2 ways to “project” the projected curve. The curve can be projected onto model faces, or onto another sketch. Projecting one sketch onto another is where most people who are going to get lost usually get lost. The sketches that you project are usually on planes that are perpendicular to one another. Sometimes you have options to pick different combinations of planes, such as front and top or front and side. In this case, front and top will be the easiest. Sketch onto Sketch projected curves essentially extrude both sketches through space, and where they intersect, it creates a curve. You can think of this like extruding one sketch as a surface and making a sketch onto face projection with the other sketch. You could also think of the projected curve function as being like a reverse drawing. A drawing takes a 3D something and creates 2D views of it. Projected curve takes 2D views and creates a 3D shape.

Actually, the grille in the image of the 34 coupe is slightly angled back in addition to being angled to the side, but I didn’t model it this way. I just took the easy route, but I’ll also explain the more complex operation as well.

So here are the two sketches. The arc with the dimensions was sketched on the top plane, and the spline was sketched on the front. Notice that the spline has 2 endpoints and a midpoint. The shape is controlled by the handles. 

When you make a projected sketch from these, the grille will be essentially straight up and down because the arc is placed on the top plane. To get the grille to angle 

the way it is on the image of the 34 coupe, you would need to put the arc on a slightly angled plane. Anyway, this results in a 3D curve.

3D curves are not as flexible as 3D sketch splines, but they are far easier to control. There is a lot of overlap between curves and 3d sketches, and a future post on 3D sketches will talk about a lot of this. SolidWorks has not put much development into curve features in the last many releases (variable pitch helix was I think the last change of significance). But they have poured massive development into 3D sketches in general. Even the new Equation driven Curve is actually a sketch element. I keep wishing they could dig themselves out of the terminology quagmire they’re in but it just gets deeper and deeper with each new feature.

Anyway. So with a 3D curve in place, now it is time to draw the sections. On the side plane, I drew the section of the grille at the top, and then in the same sketch I drew the section of the grille at the bottom. You couldn’t get away with this in days gone by in SW, but you can now. I still don’t think it’s a great idea, but this was just a model to create an image. Too many things can go wrong when you combine sketches with separate functions into a single sketch.

 

 

This image shows the top and bottom in a closed sketch, and an intermediate profile in an open sketch referencing the curve created earlier. 

When making models for renders, remember that sharp edges don’t render well. Usually you want to have a small fillet on a sharp edge. In reality most edges that we characterize as dead sharp actually have a visible round. 

The next step is to create the boundary feature. Remember that boundary uses some of the same rules as loft. The one I’m thinking of here is that if you want a loft to not twist, select the profiles from the ends that you want to connect. Same applies here. It is nice that with the boundary, you can RMB on a profile in the propertymanager and select Flip Connectors. 

In this case we don’t need any end conditions unless you want to add some shape around the plane of symmetry. 

In the end, the result looks like this. Remember to apply a shiny appearance. Just doesn’t look the same without it.

The next part to worry about is the mesh inside the grille. No, I’m not going to actually model it. This is a “looks like” model, not a production model, so shortcuts like this are permissible.

The easy way to do this is to make a surface of the shape desired and then apply a texture, ahem, I mean an appearance to make it look like slats.

This surface is easier to create than you might think. On the side plane, I drew an arc with a suitable radius to add some curvature to the grille. The arc went between the open corners of the boundary feature on the side plane. Then I used a Fill feature to fill between the sketch and the inside edge of the boundary. And that’s it. It will look better if you turn off  ”optimize”.

Finally, add an appearance. The vertical slats probably look better than the horizontal ones.

Big headlights, baby. Don’t be shy. Mirror and you’re done.

By the way, if you are impatient with how little information is here on this surfacing stuff, just go and buy the Surfacing Bible. I’ve re-read it recently, and, well, I’m biased, but I think it’s a really nice book.