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Archive for May 19th, 2008

Perhaps the most frustrating and rewarding thing about being a self-learner is that you have to figure things out on your own, and, for the most part, it means that  you’re likely to find at least ten wrong ways to do something before you can find the right one. And then you have to figure out what was wrong about the other ten! The good part about this process is that (hopefully) you’ll learn something along the way, and won’t make the same mistakes again (now you’ll make new mistakes).

I’ve been going through the Advanced Assembly Modeling manual, learning about top-down assembly modeling and assembly features.  Talk about challenging!  Editing or creating parts in the context of an assembly isn’t really the complicated part, but keeping track of all those references is! So far, so good, but I’m still struggling with some of the assembly features. More in particular, I’m still struggling with the Hole Series.

An assembly feature is one that exists only in the assembly. It won’t propagate to the part level. This means that if you have your parts already placed and properly mated in your assembly and you extrude a cut through two or more of those parts, the cut will only exist in the assembly. If you open your parts separately, you won’t see the cut. This is true for all assembly features, with the exception of the Hole Series. The Hole Series is the only assembly feature that exists both in the assembly and part level. It creates hole features in each individual (unsuppressed and not hidden) component of the assembly that intersects the axis of the hole. The holes exist both in the assembly and in each individual part as externally referenced features (in-context). At first glance, the Hole Series is a very nice tool, because it allows you to set different hole sizes for the first and last part, and all the parts in between them that are affected by the Hole Series. It also gives you the option of applying matching smart fasteners to the holes automatically. For instance, consider this simple assembly of only two parts.  Preselect a face and click on Insert, Assembly Feature, Hole, Hole Series. This will open a dialog box and allow you to position your hole or holes in the graphics area.  Every time you click on the graphics area, you create a point that defines the position for a hole, so be careful where you click. You can first create as many holes as you need and position them later, by applying relations and dimensions, just like you’d do with any other sketch. This first step also gives you the option to automatically add a Smart Fastener, or to use an existing hole (one created with the Hole Wizard for instance) as a seed for the series.

Click Next to select your options for the first part affected by the hole series. This part looks pretty much like the Hole Wizard, but these options will apply only to the first part or component in the series.

The next dialog box allows you to select options for the size of the hole in the middle part(s). This little assembly doesn’t have any parts in the middle, so it’s OK to choose the option Auto size based on start hole.

The last dialog box is for selecting options for the hole in the last part. Same as the middle part, it can be custom sized or auto sized based on the start hole.  It can be a simple hole or a tapped hole, and it can go all the way through the part or have a different end condition (blind or up to surface).

I’ve found that the Hole Series feature works really well when used in assemblies where all the components have been created separately, with no external references to each other’s geometry. I don’t know. It may just be that I’m not really experienced with external references, but I suspect that, at least in some cases, it may create references that throw the system for a loop, trying to update a part that references another one, that itself references the first one. Does that make sense? I’m not sure why, but that seems to be what happened for one of the exercises at the end of the first chapter in the manual. I applied a couple of Hole Series, according to the instructions in the manual. Everything was OK after the first one,

but once I applied the second one, everything changed and now several parts in the assembly indicate the need for rebuilding. So, I update one part and another one needs rebuilding. Update the second part, and the first one displays the rebuild symbol again.

By the way, the file that contains the assembly in the last two images is available for download through SolidWorks. Simply go to the Customer Portal, and look for Training and Certification, there you’ll see a link to the SolidWorks Training Files that are available for download. These are just the files, no manuals.

Did you notice the rebuild icons in two of the parts in the assembly? I believe this issue is related to the references created by the Hole Series, because I later removed the second Hole Series and created the holes using the Hole Wizard. It worked perfectly, and no rebuild icons showed up. But of course, the holes will not propagate to the parts. Even when using the Hole Series with parts that have no external references, and because  the Hole Series will create externally referenced hole features in your parts/components, there are at least a couple of things to consider.   

First, you can’t use Hole Series with multiple instances of the same part or component. This one is fairly obvious. The part would be trying to add external references to itself. Doesn’t make sense! You can use Hole Wizard with multiple instances of the same part, however, because Hole Wizard won’t create any features outside of the assembly.

The second thing to consider is that the holes generated by the Hole Series can be edited, like any other feature, but only at the assembly level. In the part’s feature manager, it appears like a Hole Wizard feature, but if you try to right-click on it, you’ll see that you don’t have the option to edit the feature included in the menu.  If you open the part separately from the assembly and right click on the feature, the menu that displays gives you only the option to Edit in Context, which simply means that it will take you the assembly where the feature was created, so you can edit the feature at the assembly level.

I’m still wondering about that second Hole Series in the exercise and looking for answers. Could it be right to assume that the external references are the ones creating the trouble? What do you think?