Gabi Jack's Blog

Creating revolved sections the easy way

Revolved sections (also known as rotated sections) are really useful for adding clarity to drawings of parts with features that have a constant shape throughout the length which can’t be easily shown in an external view.  By using revolved sections, the shape of the cross section of a bar, rod, arm, spoke or other can be shown  in the longitudinal view of the object, instead, as a section that’s been revolved 90° onto a plane perpendicular to the center line or axis of the object. The visible lines adjacent to the revolved section can be then broken out and the surrounding space used for dimensioning the section. Neat, huh?

Here’s how to do it, really easy, in SolidWorks.  Let’s start by assuming I already have a few drawing views placed on the sheet. In the following image, you can see the top and front views of the part named Master Rod. 

I want to create a revolved section on the front view. For that purpose, I will need an extra front view that I can use to create a section view.

At first, the section view looks pretty much like this. This is not what I need, but don’t be alarmed; there are a few changes that need to be made before clicking “OK”.

After flipping the direction of the section line and selecting to Display Only Cut Faces under the Section View area in the property manager on the left, I’ve finally ended up with the desired section (section B-B).  Now I just need a few extra steps in order to add it to the original front view as a revolved section.

First, I need to create a broken view in the original front view, by using Break (Insert, Drawing Views, Break or click on the icon), and make the gap big enough for section B-B to fit in between the broken lines.

Next, I need to drag section B-B and place it in between the broken lines in the original front view. Because I didn’t do it from the beginning, I need to break the alignment section B-B has with its parent view (the second front view added to the sheet) by right clicking and selecting Alignment, Break Alignment from the menu. Like I said, I could’ve taken care of this from the beginning, simply by pressing Ctrl while placing the section view I had just created.

OK, so now I just need to get rid of the extra front view that was used to create the section. I can do that really easily by right clicking on it and selecting Hide from the menu. A small window will show up asking if you also want to hide all dependent views, make sure to answer no to this one, otherwise, the section view will be hidden as well.

The annotation that reads “Section B-B” can also be hidden in a similar way, by right clicking on it and selecting Hide from the menu. The result is a revolved section, which can be dimensioned if desired. Simple, isn’t it?

In case you ever wondered...

I know this little piece of information is extremely basic for those with lots more experience in SolidWorks, but believe me, I just found out about this one while working my way through the SolidWorks Drawings training manual. Well, you know there are multiple views you can choose from to display your part or assembly, right?  You have top, bottom, right, left, isometric, trimetric, etc.  Did you know you can also create and name your own custom views? I kind of suspected this was possible, because I had seen some parts used in other manuals that had views you don’t usually find available in the toolbar, like Reverse Isometric and such, but until now I had no idea how to do it. Well, it’s very simple, all you need to do is position your part and assembly just the way you want it or need it to be for your custom view by using Shift and the arrows, dragging it around with your mouse, using Roll, Rotate or whatever way works best for you, then click on View, Modify, Orientation to display a little menu of views (Note: you can also use Spacebar to get to the same menu).

From the menu, choose New View (second icon from left to right).

Type the name you wish to give to your new custom view.

And that’s it! Your new custom view will be available for you next time you need it and it will save you the work of dragging and rotating the part or assembly to achieve that particular orientation again.

All for one and once and for all? Display States in SW2008

The inspiration for this post came from a question a friend asked me about an alternative way to have a component in an assembly display in different colors, without using a configuration for each of the colors. He complained that the assembly was growing large in size due to all the different configurations. I suggested he used Display States, instead, since I remembered I had done something similar in the past, although I wasn’t exactly sure if it would produce a smaller file or not.  So, I decided to try it myself using an assembly I had just created in SolidWorks 2008. As it happens very often to me these days, while doing this I stumbled on something else that has changed since 2007.

As it turns out, Display States are no longer exclusive of a particular configuration. What does this mean? Well, in SW2007, every configuration had its own display states, that could be copied from one configuration to the other, but not exactly shared. In the past, whenever you created a new configuration, a new and unique Display State was assigned to it by default. In SolidWorks 2008, you can choose not to link the different Display States to any configuration in particular, which means they can be shared by all configurations in the assembly.  Why is this useful? Well, if you think about it, a Display State allows you to define different combinations of settings for the appearance of the components in your assembly: color, transparency, display mode, texture, whether  the component is hidden or showing, and RealView options, in case the RealView Graphics is on. This means that, for instance, you can define a Display State in which all similar components are hidden or transparent or a certain color or texture.  If you have configurations that use all the same components and these components only change in size or position, then you may very well benefit from creating Display States that apply to all configurations.  You create it once and it’s good for all!

So, how do you get started? Well, first of all, go to the Configuration Manager and there you will see the configurations on the top section and the display states on the bottom section. Right click on an empty area of the Display States section and select Add Display State from the menu.

You can add as many Displays States as you need this way. Notice the option at the very bottom of the Configuration Manager. It gives you the option of linking the Display State to the active configuration or leaving the Display States unlinked, thus accessible to all configurations in the assembly.  I created three Display States for my assembly. At this point I had only one configuration, so it made no difference whether I chose to link the Display States or not.

Next, you  can define the combination of settings for each of the Display States you just created by going back to the Feature Manager and showing the Display Pane (click on the >> that shows at the top right corner of the Feature Manager). Clicking on the icons that appear in the Display Pane for each component allows you modify that particular aspect of the appearance for that component in the assembly, for the active Display State. Here, for instance, I’m changing the transparency of one of the pistons.

You can also right click any of the icons in the Display Pane and a fly out menu will show up, giving you access to all the different settings for that particular component. From this menu, you can also add a new display state (Add Display State), rename the current display state, or change the current Display State, by clicking on Activate Display State and choosing a different one from the list.

If you have RealView Graphics on, clicking on RVAppearance allows you to change the PhotoWorks appearance, color and even transparency of your component.

As I said before, for my assembly, I created three Display States:  the first one with no changes at all, the second one where all the instances of Piston were colored blue, and the third one, where all the instances of Piston were made transparent.

At this point, I had only one configuration for the assembly, so I decided to create another two configurations, just to see how the option to link or not link worked like. Notice how, when the Display States are not linked, all the configurations (even those that aren’t active) have the same Display State: the one that is active at the moment. In this case, Display State 2 is active.

Display States can also be driven by a design table, if needed.

As a side note, and to answer my friend’s original question, I did try to do the same by using three configurations, instead of three Display States. One configuration with no changes, one with all the instances of Piston colored blue, and one with all the instances of Piston set to transparent.  The resultant file is a little bigger in size than the one that would result from using only one configuration with three Display States. The difference, however, is only of 200 MB or so. I remember reading somewhere in Matt’s SolidWorks Bible that using Display States instead of configurations in order to control the display of parts can actually improve the performance of the assembly, since changing configurations requires reading the model geometry again, plus, as I confirmed, they also take up additional file space and CPU time.

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!

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!

A block by any other name...

What is a block? Well, a block is something I wish my Dynamics of Machinery teacher had used many years ago, while he was trying to explain to us the way different mechanisms were supposed to work.  It would’ve been so much easier to understand with SolidWorks and blocks, but, alas, he had no SolidWorks or blocks, so we had to make do with his dinky drawings on a blackboard and the awkward ways in which he rotated his arms and head, trying to, somehow, use his own body to suggest the movement of the mechanism. Trust me, when you’ve seen a middle-aged man contorting like a four link mechanism, you’ve seen it all! And it isn’t exactly pretty.

In SolidWorks, a block allows you to group together different entities of a sketch, so that they move as one with respect to other entities inside the sketch, while always preserving the dimensions and relations between them. By using sketch relations, blocks can then be connected with other blocks in order to create layouts for assemblies, model 2D mechanisms, and even model pulleys and gears. Blocks can also be saved by themselves, independently of the sketch in which they were created, to use them later in a different sketch. Even better, you can automatically create assemblies from these layouts or mechanisms you create with blocks. In the assemblies created this way, each block is made into a part that contains all the sketch entities that conform that block, and special mates, called LockToSketchMate, are automatically added to keep the sketch geometry constrained to the part geometry. If several blocks were nested into one, then that one block is created as a subassembly and the nested blocks as parts. Neat, huh?

Modeling mechanisms with blocks is really fun and rather easy too, it requires only a little planning and keeping in mind that the entities that are grouped inside a block will not move with respect to each other, but as one with the rest of the block. I’ve included here another one of my DIY movies on working with blocks. I hope it’s a bit clearer than the previous ones!  I think you’ll find working with blocks easy and fun.  If you are a teacher or a student, you may want to try modeling the different 2D mechanisms inside your textbooks to better understand how they work, and if you have a little time, you may even want to create the solid parts for your mechanism, based on your sketches. Have fun!

Entertaining Angels

As a female mechanical engineer, I always feel an overwhelming excitement whenever I find other women venturing in engineering, be it as professionals or students. I rejoice whenever I find women involved in science and technology, but particularly in engineering, since, in my country at least,  engineering is still a mainly male-dominated area, slowly opening up to women.  And women have so much to offer!

One of the things that I really like about this country is the encouragement that is being given to girls of all ages to pursue a career in science and technology.  I wish I had found that kind of support while I was a college student in Mexico!  Now that I’m a much older woman (a senile 34 year old), my college years way behind me, I often also wish that I could find a way to encourage other young women to become engineers, but right where I stand at the moment, in the middle of my own transition, there’s not really much that I can inspire or encourage others to. At least, that’s what I used to think, until recently, when I ran into this young lady at one of my son’s baseball games. I had noticed her once before. She was staring at me from the other side of the field, but it wasn’t until I put on my baseball cap that she came over to take a closer look. Yes, well, that particular day my husband and younger son had already taken the other baseball caps, and the only one left had the logo of the team my son was playing against, so I decided it was OK for me to look geeky in style and sport my SolidWorks baseball cap to the game. Anyway, she came over and asked me if I was Gabi, the blogger. Wow! Somebody reads this tripe! Well, it actually gets better than that, because she also told me that she’s a community college student, looking forward to transfer to a four year college to pursue a major in engineering. Then she said to me something that really made my day: she said that reading stories of engineer women like me and others has inspired her and, many times, kept her from giving up when times get tough.  Now, isn’t that something? To realize that this journey that I started for myself is actually helping others in their own journey is such an awesome thing… And it’s humbling too.

So, here it goes for this young lady, and for anyone else who might be interested. She asked me a question about Smart Fasteners and Hole Series (just my luck!). She wants to find a way to add  more than one smart fastener to a series of holes, to replace  a very long one that goes through several  parts in the assembly. After searching in the manual and online help and playing with it for a while to try to understand what she was talking about, I found that what she wants to do can actually be accomplished and is known as splitting a hole series. The tricky part is, however,  that you can’t really do this if the holes were created by an assembly feature. In other words, you can’t split the hole series if you used Hole Series command to create the series of holes. Does that make any sense? Each hole the Smart Fastener goes through has to be created by an individual feature, at the part level,for this to work.

So, imagine you have an assembly such as the one in the following image.

All the holes were created in the individual parts and then mated together in the assembly with concentric mates, so they would be aligned. If we use Smart Fasteners to apply some hardware to it, with this arrangement, we’ll get the following results. It doesn’t matter what hole we attempt to select, it will only allow us to select one.

If what we really wanted was to have a couple of short fasteners instead of a long one, we can split the hole series (break the fastener into two) as follows. First, if the Smart Fasteners property manager isn’t open already, open it by right clicking on the smart fastener icon in the feature manager and selecting Edit Feature from the menu. Once in the dialog box, expand Series 1, like in the image, to see all the hole features the Smart Fastener goes through.  Decide which hole features you want the new fastener to go through. In this case, we have four hole features and we want one fastener to go through the first two holes and the second one to go through the last two holes in the series. Drag the first hole feature for the new fastener (in this case, the third one in the series) and drop it on the fastener’s name at  the top level of the tree. By doing this, this hole feature and any other hole feature that comes after this one in the original series will now be part of a new series for the second Smart Fastener. The first two holes will remain in the original series. A message box will appear telling you that this operation will likely result in fasteners of different lengths. You have the option of choosing if you want to calculate new fastener lengths for both series or if you want to keep the original length for both of them.

Once the splitting operation is done, you now have two fasteners instead of one, each with its own hole series. If you don’t like the orientation of the fastener, you can always flip it, by right clicking on Series 1 and choosing Flip from the menu.

As a side note,  if the orientation of the parts in this assembly was slightly different, like in the following image, this whole procedure wouldn’t be necessary in order to have two fasteners instead of one. We could simply select two of the holes (see selection in the image) and two fasteners would be added.

So, there you have it. I hope it helped someone out there. And for all of you that may be reading this, if you have ever wished you could inspire others to pursue a career in engineering, mathematics, science and/or technology, please, consider becoming a mentor for women and others under-represented in these fields. Check out Mentor Net , if you wish, or simply go and take the time to share some of your knowledge and experience with others. You never know who you may inspire just by being yourself!

Everything that's editable...

I stumbled on this one almost by accident and thought it was something neat to share, for those that, like me, didn’t know it was possible. You know how easy it is to edit feature patterns, right? There’s an icon for the pattern on the feature manager, you just right click on it and select “Edit feature” and voila, you can make all the changes you wish. But what happens when it’s a sketch pattern? Editing the sketch pattern doesn’t seem that evident. There’s no icon for the sketch pattern on the feature manager. Only for the sketch. You can edit a sketch, but there’s no way to “roll it back”. Well, there is a little trick for this kind of situation. If, while editing the sketch, you click on View, Sketch relations, so you can see all the relations on the sketch, you will notice that the entities in the pattern all display the following symbol.

 

That means they are part of a pattern. If you double click on any of those pattern symbols, you will reach the following Display/Delete Relations dialog box.

Right click on any of the “Patterned#” relations inside the box and select Edit pattern… from the menu that displays. Voila! It takes you straight to the dialog box of the sketch pattern, and from there you can modify the number of instances, the spacing between them, instances to skip, etc. Neat trick, isn't it?