Gabi Jack's Blog

SolidWorks 2008: Virtual Components?

I’m still in the adjustment phase with SolidWorks 2008. I’ve been trying hard to resist the urge to do everything in SolidWorks 2007, just because it’s the “familiar” environment and I already know where everything is. Instead, I’m trying to spend more time working on SolidWorks 2008, and, as a result, I keep finding new things (or things that have changed) here and there.

This time, while practicing my top-down assembly modeling skills, I ran into something called “Virtual Component”.  Huh? Is it virtual because it doesn’t really exist? Well, not exactly. Apparently, in SolidWorks 2008, when you create a component in the context of an assembly (top-down modeling), you are no longer required to give it a name and save it right away, like before. Instead, the in-context component is saved inside the assembly document. You can work on it, delete it, insert more instances of it, pattern it, etc. You can do anything you would normally do with an in-context component! Anything? Yes, you can even create a component with no external references. “Hmmm, but what’s the catch?” you may wonder. Everything has a catch! Well, I haven’t found one yet. So far, the only catch is that, at some point, you may want to save those components as individual files… and you can do that too, so I guess it’s not much of a catch. The beauty of this is that, in the end, you only keep those in-context components that you really want, and the rest of them, the ones that used to accumulate inside your folder while you were changing your mind, those aren’t even there.

I tried this new functionality with a small assembly.  A simple experiment first, just to understand how it worked. So, I created an assembly, using this little part that came with the “What’s New?” document, as part of a tutorial for the configurations property manager.  The part (My_two_bolt_flange) has different configurations, and I wanted to see what happened to the in-context part when switching configurations for the referenced part and/or making changes to it.

I began by doing exactly the same I would’ve done in SolidWorks 2007 in order to create an in-context part: click on Insert Components, New Part, and choose a plane or a face where to place the in-context component’s base sketch. This will become the Front plane for the in-context component. In my case, I chose a face on one of the boss features of my first component, My_two_bolt_flange. Notice how a new part is added to the feature manager (Part7^My assembly), but I’m never prompted to name it or save it at this point.

I create my first sketch in this new part by converting the circular edge of one of the cut features in My_two_bolt_flange. Part7^My assembly is now an in-context part, referencing to geometry from My_two_bolt_flange.

Finally, I extrude the sketch and finish creating the part. I exit the Edit Component mode and go back to editing the assembly. This is exactly how I would’ve done it in SolidWorks 2007, except that here I didn’t have to save the part or even name it.

At this point, if I change the configuration of the referenced part (My_two_bolt_flange), the new in-context part updates too.

The same happens when I make changes to the referenced part. Here, for instance, I changed the diameter of the cut feature in the default configuration from 0.5 in to 0.7. After rebuilding the assembly, the new part updated, as well.

When the time comes to save my work, I am finally asked if I want to save the part I just created internally or if I want to save it as an individual file. If I choose to save inside the assembly, no other files are created. Next time I open my assembly, if any changes have been done to the referenced part (My_two_bolts_flange), all the parts in the assembly will update too, same as always.

If I want to save the part as an individual file, all I have to do is right click on it in the Feature Manager, select Save Part (in external file) and a dialog box will allow me to rename the file and select a path for it, which can be the same as the one for my assembly or a completely different one of my choice.

I like this new functionality, but I do wonder if it has the potential of creating huge assembly files.  As far as I know, assembly files used to be small in size, because they didn’t actually contain any of the parts. These new assembly files that result from using virtual components do contain some of the parts inside of them. This has to make them bigger. But how much of an issue can this really be? I compared the size of an assembly with the part included as a virtual component and the same assembly with the part saved as an individual file. The size of the one with the virtual component was 388 KB, versus 184 KB for the one that had none. That seems like a big change, but then again, it may not mean much for the overall performance if the assembly continues to load as fast as before. I didn’t notice any changes between the two assemblies, but that may also be because they are very simple, with only two components. What are your thoughts on this new functionality? Do you use it? Do you notice any change in performance?

SW2008: Creating a Configuration Property Manager

Last week’s meeting and all the talk about automation got me really inspired, so I decided to try some of the suggestions myself.  While searching through parts and assemblies that I could use for my experiments in automation, I happened to notice something that is actually new functionality included in SolidWorks 2008. RMB clicking the part icon on the top of the Feature Manager for a part with multiple configurations, the menu displayed an option that wasn’t there in SW2007: Create Property Manager. This option wasn’t available for a different part that had no configurations at all. Being the curious cat that I am, I clicked on it. Hmmm, it wasn’t quite clear for me what this was about, except that it somehow had something to do with the different configurations of my part. So, I finally took a look at the “What’s New?” document and found out that, for parts that have two configurations or more, this new functionality allows you to create a property manager that will let you, or others, select which one of these configurations to use when inserting the part in an assembly.  There was also a small tutorial, included in the pdf file, which teaches you how to create a property manager for a part that has seven different configurations, each one a variation of the same part, only with different dimensions for a couple of features.

Now, before starting the tutorial, I wanted to know what difference it makes to insert a part with and without this property manager.  First, I tried to insert the part that was included for the tutorial by dragging it into a new assembly from the SolidWorks search. This is the part BEFORE creating the property manager. An option to select a configuration is given as soon as you drop the part in the assembly, but you really don’t know what the dimension is applied to from that list. See the following image.

I also tried to insert the part into the assembly by the traditional method (Insert Component). This time, I didn’t get an option to choose a configuration for the part as soon as it was inserted, so I RMB clicked on it and chose Configure Component from the menu. The following image shows you my options at this point. Again, I can’t quite say what feature of the part those dimensions apply to.

Once I followed the instructions in the tutorial and created a Configuration Property Manager for that same part, however, I was able to see this property manager every time the part was inserted into an assembly. As you can see, from this property manager you can select a configuration not only by its name, but also, provided that you label them correctly and meaningfully of course, you can see the parameters that are being configured and have a better idea of what you are choosing in each configuration.

Creating one of these Property Managers is really easy. After solving the tutorial, I tried my own with a part I had made some time ago: the clothes hanger. First, you RMB click on the parts icon at the top of the feature manager and select Create Property Manager, a dialog box appears. On the left side, you have all the parameters that are being configured in your part, and on the right, a preview of what your property manager will look like. In the case of my hanger, I didn’t have dimensions to configure, only suppression states for several features in the part. The column Display State gives you three options to choose from: enabled, hidden, and referenced. If you choose Hidden, the property won’t even appear in your Property Manager. Notice how I chose to hide Plane4 and Sketch12, and that’s why they are not listed among the parameters on the right side of the dialog box. If you choose Enabled, the parameter will appear in the property manager, and, if there’s anything to choose for that particular parameter (a dimension for instance), a selection box for the parameter will also appear, listing all the possible values available for it in each configuration of the part. If you choose Referenced for a parameter, it will appear in the property manager, but you can’t really choose anything about it.  The column Label allows you to assign a name for each of the parameters. It’s a good idea to assign names that may be meaningful to you and others. I really lack some finesse on that area; I simply assigned the same name of the features in the part. All I wanted was to see how the property manager would look like.  The Order column is merely to organize the parameters and how they will be listed in the property manager. This is the dialog box for my clothes hanger.

And this is the dialog box for the part included with the tutorial. Notice the selection boxes under the parameters labeled as Boss Diameter and Bore. The parameter Bolt Distance appears as Referenced, and displays a value of 3, that will remain the same for all configurations.

This is how the property manager for my hanger looks like when I’m inserting the part into an assembly.  In this case, I have chosen the configuration named “Hanger – Style 2”.  The list of parameters in the property manager shows all the features that are being configured, and those that are unsuppressed for this particular configuration display a checkmark on them.

This is how the property manager looks like when choosing a different configuration for the hook.

Neat! Here’s my hanger part, in case you want to take a look at it.

Download hanger.zip

Tri-Valley SWUG Meeting (June-18th-2008)

Just as promised, here’s the second part of the post.  For this one, I managed to film Brian Titus as he was introducing the group to several strategies and tools for automating SolidWorks, such as macros, part and assembly design tables, mates, smart mates, smart components, and KBE tools. I was impressed by the KBE tools he demonstrated, since I had never heard of them. Others in the room seemed to find them attractive, as well.

Brian Titus holds a B.S. in Mechanical Engineering.  He spent 10 years working for many companies and various industries here, in the Silicon Valley.  He’s got experience using most CAD systems including AutoCAD, Pro-Engineer, CADKEY, and SolidWorks, which he has been using since 1995.  He spent the last 8 years working for a SolidWorks Reseller as an Application Engineer doing pre-sales, technical support, and training.  His SolidWorks Certifications include:  Professional (CSWP), Instructor, Support Technician, COSMOS Core and Advanced, and PDMWorks. He now works for himself, and proudly declares that life is much better this way. He’s the founder and owner of Zeometric LLC, an independent design, engineering, analysis & CAD consulting company.

Brian’s presentation was a bit long, so I had to break it into three different videos. Hope you find them useful! Again, I apologize for those times when I seem to be FUI (filming under the influence). I know. That’s what tripods were invented for.

Part I

Part II

Part III

Tri-Vallley SWUG Meeting (June-18th-2008)

Last week I attended the second meeting of the Tri-Valley SolidWorks User Group. I’m glad I was able to make it to this one, because it turned out to be a great learning experience for me and, I think, for many of those in attendance. Meetings such as this one are great for getting exposed to tools and strategies that otherwise you may not hear about. The agenda was changed a few days before the meeting, and, as a happy consequence of these changes, the whole meeting ended up devoted to the topic of how to automate SolidWorks  in order to increase productivity and make our work easier.

I was able to film great part of what was presented at the meeting. I have edited the content and put it together in a few videos.  I apologize for completely missing the plane during Jim Doxey’s presentation!  Jim Doxey, from Solid Partners, talked to the group about a product called Activault, and that is very similar to PDMWorks.  His presentation was so casual, relaxed and open to questions from the group, that I didn’t notice it was the real deal until he was almost done. I guess I was too busy eating my sandwich… I’m sorry!  Anyway, you can always find more information about Activault by visiting Solid Partners website.

We also had Jeff Lyo, from Hawk Ridge Systems, presenting about DriveWorks Express and design automation.   I was fascinated by this tool that, until now, I didn’t even know existed in SolidWorks… and completely free of charge! But I don’t feel so bad; I wasn’t the only one unaware of its existence. Quite a few users in the room, and not precisely the newbie kind,  had never used it or even heard about it before. Basically, DriveWorks Express allows you to create multiple variations of parts, assemblies and drawings based on a set of rules you establish previously. It reminds me a bit of programming: If this happens, then do this…  At the meeting, we were given “The Little Book of Rules”, by Ian Yates, to help us get started. You can get the book for yourself by visiting their website at DriveWorksXpress.com.  There you can also find tutorials and videos that illustrate how to use DriveWorks Express. I was able to film Jeff’s presentation and here it is for you. I apologize for the times when the camera moves a bit. I really ought to get myself a tripod!

So, without further ado, I give you Jeff Lyo, presenting  about DriveWorks Express at the second Tri-Valley SWUG meeting.  Stay tuned for the second part of this post, with videos of Brian Titus’s (owner of Zeometric LLC) presentation on strategies and tools for automating  SolidWorks  and make your work (and your life) easier.

Update on A Matter of Looks. Another way to do it.

This suggestion for extruding text on a curvy surface (See a Matter of Looks) came to me as an email from Jason Stats, CSWP, from Bard Access Systems, and I thought it was a great idea to share it with everyone here.

“The way I usually do it is to extrude the text using the "Offset From Surface" end condition with the sketch being behind the surface as you mentioned.  This requires no creation of a surface if you are only offsetting from a single face. 

If I need it to span multiple faces, I make the surface offset distance set to zero, or just use the "knit surface" tool to make the surface without having to specify a distance of zero.  Then I select this multi-faced surface as my "Offset From Surface" end condition.  This gives me two advantages:

1.  It gives me the added option of "Translate surface".  Using this option rebuilds faster, but it is like extruding up to a copied surface profile that has been moved (in a single direction) by the distance specified instead of a true offset (in all directions).  You may not notice a difference if the surfaces you are offsetting from are not too curvy.

2.  It makes so I can simply double-click on my extruded text and see the offset dimension and edit it from there instead of having to go find the surface in the FM to edit the distance.”

Thank you, Jason!

SolidWorks 2008: The Shock and the Dissection

I finally got the new DELL configured and all the software installed and running. I also made sure to copy all my files and download the files I’ll need to work my way through Matt Lombard’s new Surfacing book.  And so, at last, the moment of truth had come:  it was time to fire up SolidWorks 2008 and see for myself what it really looked like!  First, it was the shock of the unfamiliar.  Looking at that first screen, I could recognize some icons for the basics (opening files, help, options, etc.), as well as the Task Pane on the left side. While it didn’t look so dramatically different from SW2007, I quickly noticed that the menus for File, View, Tools and Help were missing… at least I couldn’t see them.  Hovering around with the cursor for a few seconds, I finally found them, and pushed the pin button to keep them from hiding again. There! That certainly looked more familiar!

Still, it looks different … I think I like the blue background; it looks nice, and it’s easy on my eyes too. I tried opening a new file, and got momentarily confused by the rearrangement of icons, menus, and toolbars.

I know, I should’ve been reading the “what’s new?” document, but I was way too excited for that, so I began to search for the familiar items on my own… And it really didn’t take long to find them!  I found how to display the rest of the toolbars by RMB clicking on the first tab on top of the screen. This is called the Command Manager, by the way. I also found the tools for selecting View Orientation and Display Style on the center top of the graphics area.

So, as I was exploring, opening files, and finding what else had changed, it happened: the dissection.  It was around 11:00 pm when I turned my back on the DELL to check email on the Fujitsu.  Suddenly, I noticed that something strange was going on, SolidWorks seemed to be searching through my files, and a small window showed up, alerting me that dissection was taking place as scheduled. Underneath the window, there was a “click here” sign that read “stop dissection”… or something similar. Since I wasn’t sure what this dissection was all about, and I certainly didn’t remember scheduling it myself, I decided to stop it for now and find out more about it.

A quick search in the SolidWorks help documents revealed that this “dissection” was related to something called “Design Clipart”, that is new functionality in SolidWorks 2008. Basically, through SolidWorks Search, this Design Clipart is going to search through all the folders and files you specify in the search paths, and dissect the files, in order to extract data that can be reused in SolidWorks.  There’s that dissect word again… Well, it actually means that it breaks down the parts into features that could be reused, and creates a library with them. Later on, you can simply drag and paste those features in different document, pretty much like a clipart. The files themselves are not changed or damaged by this process. According to the help document, parts will be dissected into features (apparently only extrudes and cuts), sketches and blocks; features will be dissected into sketches; drawings will be dissected into general tables and blocks; and DXF/DWG files will be dissected into tables, blocks and views. This is one file from Matt Lombard’s new book that got dissected that way.

The dissection is pre-scheduled to happen every day at a certain (probably very inconvenient) time, but you can change this, or even prevent the dissection from taking place, by accessing the System Options. Click on Options, Search and, under Dissection, select the time that is most convenient for you, or clear the option altogether.

You can also select what folders and files will be dissected by clicking on Options, File Locations, selecting Search Paths and adding or deleting to the list.

Even if you decide not to perform the dissection as a routine thing, you can still dissect an occasional file by itself. All you need is to open it using SolidWorks Search and you’ll be asked if you wish you dissect that file or not.

I think I’ll prevent the dissection from happening on a regular basis, at least for now. It is pretty cool, though, and I think it can save me some time and effort too, but I think I prefer it as something I can choose to do to a file or two every now and then.

So, this pretty much summarizes my first encounter with SolidWorks 2008. So far, I like it. I don’t want to say that I love it yet,  just not yet, because I don’t know what surprises await me… but I really do like what I’ve seen so far.

Anyway, right now I’m editing some video from yesterday’s SWUG meeting, and, if it turns out right, you’ll get to see this dissection thing in action and used for noble purposes, together with many other cool tools and strategies, for automating SolidWorks, and making your work easier. Stay tuned!

A Matter of Looks

I learned this little trick while trying to help someone extrude some text on a curvy surface.  It wouldn’t surprise me if some of you knew of a different way to achieve the same results. That’s one of the things I like about SolidWorks: there’s so many different ways to go! I must confess it used to drive me nuts in the beginning, when I was constantly wondering if I was doing it right. I mean, it looked right, but was it really right? While I can’t exactly say that there is a right or wrong way to do things in SolidWorks, it is true that some can be faster or more efficient than others, or may work better for your particular design intent. So, if you know a better way to do this, by all means, do share!

So, we were trying to extrude text on a curvy surface, a round (fillet) to be more precise. Using wrap was out the question, given the kind of surface, so we thought about extruding the text from a tangent plane, up to the fillet surface, like in this image.

It looked OK, but if you notice, the thickness of the text isn’t uniform.   It becomes more obvious in a side view of the model; notice how the extruded text follows the shape of the plane on one side and the shape of the fillet surface on the other. The size and depth of the text and the radius of the fillet can also make the uneven thickness more obvious.

So, after thinking about it for a while, we tried something different. First, we created a new surface, an offset of the fillet surface, by applying Offset Surface from the Surfaces Toolbar. Face 1 in the image is the face of the fillet and the 0.02 in, in this case, is the offset distance.

The text was sketched on a different plane, an offset from the first plane, and located behind the fillet surface. The text was then extruded from the sketch plane up to the offset surface previously created.

The result was text with an even thickness that follows the shape of the fillet surface.

So, how would you do it? Please, share!

Slow Motion

So much happening, only not as fast enough as I would like it to… Well, the “ Pepsi Challenge” went a lot better than I thought. I didn’t stutter (much), everyone had a great time, and they liked it so much, they even came back for seconds! It was good, but after this experience, I sure have  a greater respect and admiration for the real  SolidWorks representatives and salespeople. Their job is not easy!  It seems to me that they need to know the product inside and out, and be prepared to answer all kinds of questions  about  performance, installation, compatibility, prices, equipment,  etc.  I don’t think I could ever fill their shoes, but  it sure was fun to walk in them for a day!

I’m finally finished with the darn manual on assemblies! Oh, and what a struggle that last chapter was! Working with large assemblies made it overwhelmingly clear that this old Fujitsu coffee pot is really no match for SolidWorks. It kept crashing left and right, and just opening an assembly or performing any kind of operation with it took forever.  It’s got to be because of the computer… Or  could it be because of Windows Vista?  Or, perhaps, it’s all the other junk I’ve been loading in it? Well, I guess it doesn’t matter much. Now that the “Challenge” is over, I’ll be busy removing some of the other software from it, and restoring the whole thing. Maybe that way SolidWorks and Internet Explorer will finally talk to each other, at least long enough for me to try my luck with the CSWP test. Sigh… The new computer still hasn’t arrived!

Ah, but even in the midst of my struggle, I think I did learn a thing or two about best practices that can help create assemblies (big or small) that are both efficient and faster (faster to load and faster to edit).  The first thing I learned is the importance of breaking down the assembly into sub-assemblies whenever possible. The bigger the assembly, the more important this becomes. Using sub-assemblies allows for faster access to the components. Instead of editing a large assembly with hundreds of components, we can open and edit a small sub-assembly, instead. This is  also useful when working  as part of a design team.

Reorganizing the structure of an assembly can be done in different ways: we can dissolve an existing sub-assembly that doesn’t work for our purpose (RMB click the sub-assembly icon and select Dissolve Sub-Assembly), select a group of components from the top level assembly and form a new sub-assembly with them (ctrl-select components, RMB click and select Form New Sub-Assembly Here), drag and drop components in and out of existing sub-assemblies, or insert a new, empty sub-assembly and drag components from the main assembly  into it. Forming a new sub-assembly with a group of components does, indeed, create a new assembly document.  Dissolving an existing sub-assembly, on the other hand, does not delete the document from disk, it only  brings the components that were in the sub-assembly up one level in the assembly structure.

One important thing to keep in mind (one that I had to learn the hard way) is that all this reorganization needs to be carefully planned, because it can affect mates and features  that reference the components you are moving and regrouping in the assembly.  For instance, if you try to move a fixed component from a sub-assembly to the top level assembly, it’s likely to over define the assembly. On the other hand, if you move a fixed component from the top level assembly down to a sub-assembly, the top level assembly may end up completely unconstrained.  If you have features with external references and you move the referenced component, the features will disappear. The same will happen if you try to move the component that is the seed for a component pattern. The whole component pattern will be deleted!

More good suggestions included creating configurations of the assemblies and sub-assemblies  that represented the model in a simplified state, by suppressing details and features that are merely cosmetic and not precisely critical for the assembly. In order to do this, first the simplified configuration for each part is created, then a simplified configuration for each of the sub-assemblies, using the simplified part configurations. This can be done manually, by RMB clicking on each component in the feature manager and selecting  Component Properties from the fly out menu. The following dialog box displays,  allowing the option of choosing the configuration to use, whether we want the component to be resolved, suppressed or lightweight, and, in the case of sub-assemblies, whether  to solve the assembly as rigid or flexible.

It can also be done by using a design table, such as the one in the following image.

It is also useful to keep the number of mates to a minimum by using component patterns when possible, to adjust the image quality settings and the level of detail, from more to less, to improve the performance of the assembly, and to load all components, or at least most of them, as lightweight whenever possible, and as long as they don’t need to be edited, of course. 

These little pieces of DIY advice are useful for any size of assembly, I think, but when opening an assembly in Large Assembly mode, the software takes care of a few other settings that help make the large assembly faster, like disabling the automatic save of the model, suspending automatic rebuild, and hiding all planes, sketches, axes, annotations, etc.

I think I’m getting the hang of working with assemblies, sub-assemblies and their configurations. Of course, it would be easier if my computer cooperated with me… Or, if the new one finished arriving here.  Hmmm… Looks like it’s time to restore this old coffee pot!

Students, SolidWorks 2008 and Formula One

What a great combination!  Well, the New 2008-2009 student edition of SolidWorks has just been released, with all the functionality of SolidWorks 2008 Office Premium, plus COSMOSWorks, COSMOSMotion, and COSMOSFloWorks.  So, for up to 24 months, students from middle school all the way through graduate school will be able to take advantage of the full potential of SolidWorks, everything, all the bells and whistles, with the only limitation being that this edition can’t be used for commercial purposes; a watermark will be included in all print outs.

Ah, but there’s an extra added bonus this year… Taken from SolidWorks press release: “SolidWorks Education Edition 2008-2009 includes a new F1 in Schools™ curriculum for teaching middle and high school students about SolidWorks software, 3D CAD, and analysis. The curriculum includes lessons for designing, analyzing, simulating, rendering – then actually constructing – a scale model Formula One racing car. Students can enter regional, national, and global competitions.” 

Do you like Formula One racing cars?  Or should I better say, do you know anyone who doesn’t like Formula One racing cars? I love Formula One! I used to build scale models of the cars as a hobby when I was younger. Wow, what a great time to be a student! If I can’t make myself younger again, I have to, at the very least, find a way to get myself into teaching, just to see if I can lead a group of students in these kind of competitions! Your very own scale model of a Formula One racing car! Fancy that!

A Solid Ant on Wings Like Eagles

I can’t say I’m a very patient person. No, not really. That’s not me! My nature is to run straight ahead to wherever it is I want to go, and never stop running until I get there, no matter what. However, I’ve learned that in this life, sometimes, it does pay to wait and go little by little, just a little bit every day. Sometimes, it’s the only way to do it. You just need to keep at it, even when it doesn’t seem like you are doing much, or getting anywhere at all. Never stop… Before you realize, you’ll get the job done, exactly like the ant, one grain of sand at a time. It’s amazing how much you can accomplish this way, with a little patience and a little faith… and, sometimes, a little luck.  Well, this Solid Ant has gotten lucky in unexpected ways, and she’s also saved some money, little by little, for quite some time, and now she has just put some of that money to good use and bought herself a brand new computer to run SolidWorks 2008 in it.

Yep! After spending some time researching and comparing what others (like Anna and Devon) had bought for themselves, I finally made up my mind and bought a Dell Precision M6300 mobile workstation, with all the trimmings I could afford, such as 160 GB in hard drive, 4 GB SDRAM, and, for the first time ever in my life, a nice NVIDIA Quadro FX 1600 graphics card. I will finally know what Realview looks like! I ordered the computer this weekend. It will still be a few days before it gets here and I can load all the software in it. A few more days, and I can hardly wait! I’m really excited, so please, if you own one of these computers and there’s something about it that you absolutely hate, don’t even bother raining on my parade. I just don’t want to hear about it! Just kidding! Well, no, not really.

I’m still keeping SW2007 in my old Fujitsu. I’m still not done with it. You may see me jumping from one version to the other.  I wonder how different SW2008 will be and if I’ll like it better than SW2007. Guess I’ll find out in just a few more days!