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Archive for June, 2008

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?

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

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

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.

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!