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Archive for April, 2008

Wow! I haven’t really experienced SolidWorks 2008 ( I wish I could). I’ve seen some people complain about things they didn’t like about it, like the user interface, but apparently all the other great things about SolidWorks 2008 as a whole greatly outweigh any problems it may have, since it’s been awarded Product of the Year, according to the readers of NASA Tech Briefs.  You can read about it here. It may also be all over the news by now.

Good job SW!

Well, last week was so hectic that at times I wished I could be the one splitting myself into multi-bodies. Hmm, perhaps, what I really need, is a few good buddies (like Molly Maid and Supper Nanny) that can come over and give me a hand every now and then.  Anyway, not so long ago, I was telling you about my little exercise in creating new parts using the Split command. But that isn’t the only way to create new parts out of a multi-body part in SolidWorks. Because multi-bodies can be the result of  something as simple as creating an extrusion that doesn’t merge with the rest of the part, and aren’t always the result of  slicing the part by means of the Split command, there are also other ways to save those bodies as parts or to insert the bodies into a new part.  I know, both options sound the same, but the results are slightly different.

As part of my exercise, I created a copy of my original part and named it “Buggy Two”. This time, I cut the part in half by means of an extruded cut, instead of the Split command.   The cut removes a thin layer of material, right across the middle of the part, and creates two bodies. SolidWorks then prompts the user to choose whether to keep all bodies or only one of them.  I chose to keep both bodies and ended up with a multi-body part, just as I wanted.  Now, to create new parts out of these two bodies.

First, I tried Save Bodies. You can find this option by RMB clicking on the bodies folder from the feature manager.  You will then see the following dialog box, which looks and works very similar to the Split command, but without the Trim tool.

I gave my two bodies a name and saved them as two new parts, “Buggy Two Top.sldprt” and “Buggy Two Bottom. Sldprt”.

In the parent part, Buggy Two.sldprt, a new Save Bodies feature has been added to the feature manager. The references and dependencies between the parent file and the two new files that were created this way  are very similar to those of files created by using the Split command. Any change done to the parent part BEFORE the Save Bodies command, will spread to the new parts. Changes done AFTER the Save Bodies command won’t. Also, if the Save Bodies feature (or the extruded cut) is suppressed in the parent file, the new parts won’t be able to load at all, unless the parent file is closed or can’t be located, in which case, the new part will open with an out of context reference to the parent file.

 

Inserting a body into a part, however, works a bit different.  To test this option, I saved a copy of Buggy Two.sldprt as it was just before saving the bodies, and renamed it “Buggy Three.sldprt”.  I opened the bodies folder in the feature manager and RMB clicked on each body, selected Insert into Part from the menu, and  gave each of my new parts a name.

 

The two new parts have references to the parent file Buggy Three.sldprt, but there is no trace in the history of Buggy Three.sldprt, that may provide a clue about the two new parts that were just created this way or when in the history of the parent file were the other two created. There is no way to access those files from the parent part, either.  Also, any changes made to the parent file, at any time, will spread to the other two files, unless the reference to the parent part is broken or out of context (file can’t be located or was renamed).

 

Out of curiosity, I suppressed the extrude-cut feature that created the two solid bodies in Buggy Three.sldprt, just to see what would happen to the other two parts. Unlike with the Split command, both parts were able to load, but can you guess how they looked like? Yes, they looked exactly like the parent part before the cut!

   

 

So far, I think I like what can be done by using multi-bodies in SolidWorks, specially when creating objects that contain many pieces that must fit together like a puzzle, following a shape in particular, but I’m a bit concerned about  all those references. It seems to me that in order to avoid potential trouble for ourselves or others that may have to work with our models, we must try to be a bit organized: document what we’re doing, keep the files and their parent together, etc.  Now, that’s a bit of a challenge!

Apparently, in part thanks to a certain Robin of Locksley from the 21st century, SolidWorks has just made the SolidWorks World 2008 proceedings available to everyone, along with podcasts, videos, cool photos and all! Oh, and the website is the coolest too! To get to them, just go to the Customer Portal, sign in and look for the link to SolidWorks World 2008 on the left. Enjoy! Oh, and thanks to the guys at SW for their generosity!

As I mentioned in a previous post, I’ve spent some time learning about the use of multibodies in SolidWorks.  It’s a fascinating subject, indeed! I had used multibodies before, when modeling the hairclip, but mostly I had limited myself to combining two or more bodies into one. Now, I’m learning to do the opposite: create two or more separate bodies out of one, and save them as individual files.

In SolidWorks, one body can be separated into two or more by many different ways:  an extruded cut, a revolve cut, cutting with a surface, etc. It is also possible to use the Split command to divide the body into smaller parts. Why use multibodies? Well, I guess you may want to take a look at what Matt Lombard had to say about it in his presentation “The Care and Feeding of Multibodies in SolidWorks”. He gives a very thorough explanation of why and why not use multibodies when designing with SolidWorks.

As an exercise in creating multibodies, I decided to try and reproduce one of my son’s Cooties, a little bug looking toy.  So, first, I modeled the shape of the body as a single solid using the loft feature and a few circular profiles. I named this part Buggy.

Then, I divided the part into two new ones by using the Split command (Insert, Features, Split).  In this case, the Right plane served as a trim tool, but it could also be a surface. After selecting my trim tool and clicking Cut Part, the body is divided in two and I’m given the choice to save the resulting bodies as two individual parts, which I named BuggyRight.sldprt and Buggyleft.sldprt.

Notice the Split feature that is added to the feature manager in the Buggy part. There’s also a reference to the Buggy part in each one of the two new parts created this way.

         

This means that the two new parts created are still connected and dependent on the first one, Buggy.  I tried opening Buggyleft  on its own, and notice how the reference to Buggy appeared to be out of context, but the file still opens and rebuilds. It will always appear out of context if the parent file isn’t open at the same time.

The same happens if I move the file to a different directory or if I rename the file. When reloading Buggyleft.sldprt after renaming  Buggy.sldprt to something else,  first I got the following message. I chose not to look for the file, and Buggyleft.sldprt still reloaded, only with an out of context reference to Buggy.sldprt.

So, up to this point it seems like the worse that can happen if you misplace the parent file is to have some  out of context references.  The changes you apply to any of the new parts don’t affect the parent file, Buggy.sldprt, so you won’t be needing to update that file, like you would with an assembly. However, if you make any changes to the parent file, Buggy.sldprt, BEFORE the Split feature, they will reflect on the two new parts, and any changes you make to the Split feature itself can and will affect the parts that were created by that Split feature.  I realized this when I chose the Top plane as a trim tool by mistake. I created two parts this way: Buggybottom.sldprt and Buggytop.sldprt.  When I realized that I needed to split the body using the Right plane instead, I went back to Buggy.sldprt and edited the Split feature, thus creating another set of files: Buggyleft.sldprt and Buggyright.sldprt. After creating the second set of files, however, I went back to Buggytop.sldprt and look what happened to it.

Hovering my cursor over the Split feature in the feature manager I get a message that says that the Split is not valid. The funny thing is, this happens only as long as Buggy.sldprt can be located. If I change the name of the file or get rid of it some other way, then Buggytop.sldprt  will reload with out of context reference to Buggy.sldprt.  I could break the references and then I’ll be able to load the part, it won’t be dependent of Buggy.sldprt anymore, although the evidence of reference will continue to be part of the file and the feature manager (notice the  x  next to the reference), indicating that the reference is broken now. Interesting, isn’t it?

 

I have mentioned before that I’m trying to learn a bit about plastics and molds, and  since I’ve bought some materials from the Society of Plastics Engineers, every now and then I receive some information about upcoming events. I thought this one may interest a few folks in the area.  Anaheim is a bit far for me, but for 35 dollars seems a good deal, if you happen to be in the area and have interest in plastics and molds.  I bet they have different chapters organizing this kind of events in other parts of the country too.