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Archive for the ‘Tips and Tricks’ Category

Hey there!   How is your Summer? Mine, so far, is just as I expected: hot and hectic. But I won’t complain. Instead, I’ve prepared a document with step-by-step instructions on how to make this pair of scissors that were used for one of the examples in my Easy Surfacing Techniques presentation.

I had made this model just for fun and wasn’t planning on using it in the blog, but I’ve got so many requests for instructions and files that I ended up writing a short tutorial for it.  Hope it’s useful for someone out there. The files were all made in SolidWorks 2010.

To download the files and pdf document, click on the following links. I’m also adding links to these documents in the downloads  page.

Scissors Tutorial (pdf)

Scissors SolidWorks files (2010)

Hey there,

It took me a bit longer than I thought, but here it is: the tutorial for the hairbrush in pdf and the pack an go of the assembly. The model was saved in SolidWorks 2010, but the steps in the tutorial are good for previous versions too. Hope you guys find it useful!  You can download the files following the links:

Hairbrush tutorial on pdf

Hairbrush assembly pack and go

I’ll also add these links to the list of Downloads.

While working my way through the PDMWorks  Workgroup lessons in the training manual, I came across a bit of information about Toolbox parts that I never knew about before.  Some of you may have known this already, but it was news for me.

If you’ve noticed, every time you add a Toolbox part to an assembly, the component shows up with a special icon in the Feature Manager that looks like a fastener and that is used to identify it as a Toolbox part. This is true regardless of it being a copy of the master file or a configuration.  Well, that icon is associated with an internal flag that is placed in the file to identify it as a Toolbox part. An add-in, such as PDMWorks, reads the flag and uses this information to handle the part according to the rules that have been previously established by the Vault administrator.  

If the Vault administrator allows it, users will be able to check the Toolbox parts into the Vault with the rest of the components of the assembly.  This is not advisable, but it’s reasonable as long as your Toolbox components are copies of the master file and not configurations.  However, more often than not, the Vault administrator will decide that users won’t be allowed to check Toolbox parts into the Vault and these components will be listed in the assembly as links and in a separate project in the Vault as Toolbox references and library components. The following image shows those two last options have been selected by the Vault administrator.  

The reason for disabling the check in of Toolbox parts is simply because these components don’t require revision control. These are components such as fasteners, library parts or purchased components, and so they are usually located in a directory that is common to all users, instead.  In addition to the flag, PDMWorks can also identify these parts as Toolbox parts by the name of the folder they are located in. Folders containing \Toolbox, \Toolbox Parts or \SolidWorks Data are identified as Toolbox folders.

All this is nice and good but it gets more interesting yet. Did you know that you can add this same flag to components that were not created by the Toolbox? That’s right!  By using a file called sldsetdocprop.exe, which is usually located inside a directory such as SolidWorks/Toolbox/data utilities, you can add or remove the flag from files, thus causing SolidWorks and add-ins such as PDMWorks to change the way they handle them.  I prepared a little example of this.

I had this assembly of some scissors with only three pieces. You can find this assembly among the files for the surfacing tutorial in my downloads section. It’s the same one. There is a fastener in the assembly that shows up in the Feature Manager as a regular part. I’ll first try to check this assembly into the Vault as it is.  Notice in the image below that all the parts of the assembly appear as regular parts in the summary, that they can all be checked into the Vault and I can also take ownership of all them once inside the Vault.

I cancelled that check in operation and used sldsetdocprop.exe to add a flag to that fastener, instead.  This is very easy to do, you simply click on Add files, browse to the location of the component and select it, check the option Property State: Yes and then click Update Status, as you can see in this image.

The following dialog will appear, letting you know that the property has been changed, that is, the flag has been added.

When I try to check the assembly this time around, the fastener shows up as a Toolbox part and I’m no longer allowed to check this part into the Vault.

So what happens with this Toolbox part? Well, once the assembly has been checked into the Vault, the Toolbox part is listed in the assembly as a link, as you see in the image. That little mark on the left of the icon indicates precisely that the part is used in the assembly, but it’s not saved there.  The Toolbox part is not inside the Vault at all; it is simply referenced and shows up listed in the project Toolbox references. It cannot be opened from the Vault either.

I imagine this can be useful for companies that create their own libraries of components that don’t require revision control. They can mark the components and make them easy to identify by PDMWorks this way.  Neat!

Bloggers don’t blog?  Sorry guys!  I was dealing with quite a few health issues and going through a lot of antibiotics as part of a trial and error strategycareful scientific methodology and thoughtful planning devised my doctor, and all because I’m allergic to Penicillin. But I’m finally feeling better and back with some goodies that, I hope, many of you will find useful.

First of all, let me tell you about the SWUGN San Jose Technical Summit that took place just yesterday, March 23rd, in the city of Milpitas, CA.  As I mentioned before in a previous post, I was there to present about Easy Surfacing Techniques for Solid Models. I was extremely nervous because this was actually my first time presenting for the SolidWorks community… well, OK,  my first time presenting anything for anybody since my last year of college, back in 1996. Yes, I know… 1996… I’m old.  So what?

I was fortunate to find quite a few familiar faces at the event: Richard Doyle,  Alex Ruiz (SWGeek), Matt Lorono (fcsuper and SolidWorks Legion), Phil Sluder, Brian Titus, Kenneth Barrentine, Elise Moss, and a few other people that I’m absolutely sure I’ve seen at SolidWorks World before.  Richard, Alex, Matt and Elise were presenting too, but I couldn’t stay and attend their presentations because I had to run back home to be with my younger son and allow my husband to go back to work. See, my husband selflessly sacrificed his morning to allow me to be at the summit long enough to present, but I couldn’t ask him to sacrifice his whole work day.

Anyway, at least, the time I was there was lived to the max. Despite the butterflies in my stomach, my presentation went a lot better than I had expected. In fact, quite a few people told me that  it actually went great!  And all those things I had worried for days (finishing too soon, making lots of mistakes, presenting for an empty room,  forgetting everything, having an accident in the freeway, wearing my clothes inside out) never actually came true.  This may seem silly to some, but it was a great victory for me. As I left the building, I felt so happy I was practically doing the jig on the way to my car. I just hope nobody saw me.

And now to the goodies. Because I promised it to the people in attendance, I have prepared a pdf document with step by step tutorials of each and every single one of the eight examples I showed yesterday at the summit. It’s 38 pages long and loaded with illustrations. I’m making that available here, together with all the parts and assemblies used in the examples, plus the solved examples to compare.  To download them, just follow the links.

Easy Surfacing Techniques for Solid Models

Example files

Example files (Solved)

I’m thinking I may as well start a new page to list downloads. Writing those tutorials was a fun experience, since I was able to include more detail than I usually do in a blog post, so I may be creating and adding more of those in the future.

I hope you are not growing tired of my SolidWorks World chronicles just yet, because I still have a lot more to write about. This was a particularly good SolidWorks World for me and I want to share what I learned with you.  This time, let me tell you about yet another hands-on session I attended. This one was presented by Michael LaFleche, Regional Technical Manager for CAPINC, and it was an introduction to direct modeling techniques in SolidWorks for those of us that hadn’t really tried that functionality before or didn’t know how we could benefit from it.

He began by showing us some common ways to do modifications in the geometry of an imported part. As you know, usually when you import a part -step, parasolid, iges, etc-  you are not going to have access to its features to modify any dimensions. Since all you usually have is an imported feature (dumb part) or imported surfaces,  it’s common practice to do modifications via the “Butcher Approach”, as Michael calls it, and that is basically slashing, moving and  then reconnecting and patching parts of the geometry.  He demonstrated this approach through an example.

Michael started with a step file that he opened in SolidWorks. After running import diagnostics and healing a couple of faces, we had no features on that tree. Michael used the “Butcher Approach” to make the legs of this part you see here  a little longer. First, he began by slashing the model using a line that was sketched on the Front plane and the Split command (Insert, Features, Split). This way, he cut the model in three solid bodies: the frame and two of its legs. They are all in the same color in the image, but you can see there’s actually three bodies and each one has a callout right next to it.  The three solid bodies will appear in the Solid Bodies folder in the Feature Manager tree.

Next, he used Move/Copy Body  (Insert, Features, Move/Copy Body)  to translate both legs down by 20 mm. Note that Move/Copy Body also has the option of using constraints. We don’t want to use constraints, so make sure to choose Translate/Rotate under options in the Move/Copy Body property manager. You will see a Triad appear. You can use this triad to dynamically move the bodies down by dragging the green arrow, or you can enter numerical values for the new position directly from the property manager on the left.

By now, both legs have moved down and now there’s a gap that needs to be filled.

Michael used the Boundary Boss feature to fill the gap and reconnect the bodies. He could’ve also used loft or even a surfacing technique, but Boundary Boss did the trick this time.  So there you have it, the Butcher Approach.

 

Next, he showed us a direct modeling approach, using Move Face. First, we needed to turn on the Direct Editing Command Manager tab by right clicking on any of the other tabs and selecting Direct Editing from the list.

He used Move Face to translate those six faces you see here ten millimeters towards the inside of the leg. Notice that we needed an edge to specify the direction of translation, so we used the one you see highlighted there next to the pointer. The preview of the new location appears in yellow.

Something important: Once we accept the Move/Face feature, it will show up in the Feature Manager as an other feature that can be edited, but not only that, we can now use Instant3D to dynamically drag a face in this leg, for instance, as you see in the image below. Notice that dragging the face with Instant3D doesn’t add another feature to the tree because, in fact, every time you drag the face using Instant3D you are simply editing the Move Face feature that had been added previously.

Move Face can also be used to offset a face in a body, like you see in the following image. Here, Michael instructed us to offset the face highlighted in blue 1 mm towards the part. Once we accept the feature, all other faces around it will be modified accordingly and, just as before, we’ll be able to use Instant3D to dynamically drag this face.

There’s also an option to rotate the face instead of moving it or offsetting it. To use this option we need to specify an axis for rotation and an angle. In this image, the vertical edge on one side of the face was used as the axis and we rotated the face 15 degrees from its original position.

Notice that once we accept the Move Face feature the hole doesn’t show up in the face we just rotated, but that all the rest of the geometry has changed accordingly and the hole now shows up going through other faces in the part.

Michael corrected this situation by using Move Face again to translate the geometry associated with the hole. Notice the edge of the face that is used to specify the direction of translation. The preview of the new location shows up in yellow.

He also demonstrated the use of this technique in a large model when he used Move Face to change the location of some of the support ribs on this engine block. By the way, those ribs are not really part of a pattern, but Michael did mention that Move Face can be used to change the location of one, two or more instances inside of a pattern without disturbing the rest of the pattern.

 

He first changed the model to a Right side view and Wireframe display style to make it easier to select the geometry. He used Move Face command again to translate the faces of two of the ribs. He selected the faces associated to the ribs  by dragging a box from left to right as you see in this image.

Once the faces were selected, he used a horizontal edge in the part to specify the direction of translation and moved the geometry 2 in to the right. It’s a bit hard to appreciate in this image, but there’s a preview of the new location of the ribs. The lines in blue are the ribs in their original position, and the preview shows up in yellow.

Michael also showed us how to use FeatureWorks to recognize features in an imported part. This can be done locally, by right clicking on a face, for instance, and selecting Edit Feature from the flyout toolbar. FeatureWorks then will recognize features such as extrudes, holes, revolves, etc. that could be associated with the geometry selected. We can also recognize features in the whole model at once by right clicking on the imported feature in the Feature Manager tree and selecting FeatureWorks, Recognize Features, as you see in the following image.

FeatureWorks will then recognize features such as extrudes, revolves, holes, ribs, fillets, etc. and create a Feature Manager tree for the part. This can save some time and effort. For instance, after recognizing features in this imported part, I suppressed the ones that were associated with the engraved plate.

I believe the complete presentation with files and step by step instructions will be available in March. Until then, as usual, I hope my brief chronicle was useful for someone out there.

Thanks to Michael LaFleche for a great hands-on presentation. I really enjoyed it.