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Posts Tagged ‘SSW10’

While at SolidWorks World this year I attended three sessions that were somehow different to what I had expected when I signed up for them.  The subject and purpose for each of them differed from one another, but what they all had in common was that they all required from the attendee to not only interact or follow through a tutorial, like in the hands-on sessions, but to actually provide the content for the presentation.  How can this be? What in the (SolidWorks) world is Gabi talking about? Don’t worry, I haven’t lost it… just yet.  These sessions did exist.  I’m talking about “Stump the Chumps”, “SolidWorks Clinic: Is the Doctor In”, and “Birds of a Feather”.

I think by far Stump the Chumps was the most entertaining one of the three. From what I understood, the idea behind this session was to have a team of SolidWorks experts answering really hard questions from the public on almost any subject related to SolidWorks, and showing the solution live on a big screen for everyone to see.  Those experts are the chumps and the audience is trying to stump them with difficult questions. I’m not sure what was supposed to happen if they did get stumped. Maybe the person who stumped them would win a cool prize or perhaps the chumps would get soaked on green slime, like in those Nickelodeon shows that my kids like to watch.  Never mind…  

We had a great team of chumps presenting that day, including Matt Lorono, Joy Garon, Alex Ruiz, Ricky Jordan, Charles Culp, Josh Mings, Rob Rodriguez, Phil Sluder, Ben Eadie, and I have the feeling I’m forgetting one or two more people. Please, if someone know their names, let me know to add them to the list!  You see, I tried taking pictures, but they all turned out really fuzzy, so I can’t tell who was who.  The team was put together by Jeff Mirisola, who was also a chump and performing as the moderator for the session, hogging  holding the microphone for everybody, coordinating the chump team, and giving away prizes to those that had a question to ask from the chumps.  It almost felt like attending one of those contest shows from TV, you know, like ”Who wants to be a millionaire” or “Are you smarter than a fifth grader?”  Unfortunately, due to budget restrictions the chumps didn’t have fifth graders to bail them out, but they didn’t need them, they all did  a really great job answering questions from the audience and also questions that had been submitted to them in advance.  Some of the questions were a bit strange, actually. One had to wonder what was going on in the mind of the user that asked that particular question or what difference it would make to know the answer, but the chumps strove to provide a solution just the same.  Many times I thought the chumps had actually been stumped, but they always thought it through for a few minutes and came with an answer or a way around it that did the trick. 

This was the second time Stump the Chumps presented at SolidWorks World, but the first time I attended this session.  I really enjoyed it. Perhaps, next year they should advertise more, to get more people to attend… and also get some green slime. Just kidding about the slime! It was a great session. Keep up the good work!

Birds of a Feather was actually more like a very brief meeting with other users that shared a common interest. I attended the one about Advanced Surfacing, hoping to learn something useful. This meeting reminded me a lot of last year’s focus groups. There was no PowerPoint presentation, nothing showing on the screen, no examples of anything, no particular problems being solved for the group,  nothing but a group of users discussing what they liked or disliked about SolidWorks surfacing tools. People from SolidWorks were there too, listening to what the users had to say, and asking questions hoping to start some form of conversation, since the users were extremely quiet in the beginning. I think most everyone there was expecting something different, just like me.  Once the users started talking, though, they also began giving advice to one another on what tools to try and what to do differently to obtain better results in the daily work, like breaking a loft in several parts instead of attempting to create one big, extremely complex surface, and saving a dumb part as a part adding some external features in the process.  Someone - I don’t remember his name- had a great idea for an enhancement request and asked from all of us in attendance to consider requesting it as well. It’s an Unknit feature. A feature that may do the opposite of  Knit. What do you think? Could it be useful?

And last, but not least, a bit about the SolidWorks Clinic.  This session was also not what I thought it would be, but turn out much better than I expected. Well, I thought it was a hands-on session where a presenter was going to show us tricks or techniques of some kind, but it turned out to be an opportunity to present a real-life problem to an expert and get one-on-one help from him or her. They had a large group of experts available that day, but, alas, I had no problem or question to ask from them.  It was then that I understood why some of my fellow bloggers were snickering in the back when they saw me come in and grab a seat behind one of the computers. They were making fun of me! I know they were! It could also be that I’m paranoid, because, how could they know if I indeed had a problem or not, right? Yeah, well, see the average individual could simply come to that conclusion and feel better instantly, but since I’m a real expert in the pursuit of unhappiness, I prefer to go with option A: they were making fun of me. LOL

Anyway, I was lucky to seat next to Adam Scheible, who did come up with a question about Animation.  Adam had a model of an assembly he was animating as part of a lesson for his students. He wanted to know what else he could add to the animation to improve it or teach his students something extra. Adam got the help from Paul McCrorey, owner at McCrorey Digital and he kindly allowed me to watch what they were doing from the seat right next to his.  Paul showed Adam how to make some modifications to the already existing animation and also the use of cameras. I owe you that for a future post.  I’ll have to find a suitable model and make a video of what I learned from Paul, because it’s not easily explained without the visual aid. Paul also showed us some really cool animations made in Modo. Amazing stuff!  Since my hubby is a marketing guy always willing to give me a hand, I had considered buying Modo before, to start a little business doing renderings for websites and marketing literature. Seeing those animations made me wish I could get started right now.  

Sorry there aren’t tips and tricks or tutorials in this post. It’s simply part of the chronicles. If you attend any of these sessions next year (or a similar one), make sure to go prepared with some problems or questions you may have, and keep an open mind and a good attitude, even if you see some bloggers snickering in a corner. There’s always an opportunity to learn something new!

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.

Hi everyone! I hope you had a really nice weekend! It was a four day weekend for us here and it sure felt good to get a break, plus a little Valentine’s Day candy. Now it’s back to the routine… and the diet.  Anyway… I shall now resume my chronicles of SolidWorks World 2010.

As I mentioned before, this year I was really fortunate to be able to pre-register for hands-on sessions, and this particular session, The Connectors Workshop, is one of them.  This session was presented by Joe Galliera, who works for DS SolidWorks as a Simulation Technical Manager. 

During his presentation, Joe guided us through different scenarios where we used  connectors - bolts, pins, bearings, edge welds,  springs, dampers and many others - to simplify the analysis model. In all these cases, we were able to use connectors instead of modeling the parts because there was no penetration between the connectors and other parts of the assembly, and we didn’t need to investigate the stress or deformations in the connectors themselves.  If, however, we had the need to find out such information, we’d be better off modeling the connectors as real parts in the assembly and including them in the analysis.

 Joe Galiera was very kind to make the presentation and all the files needed to complete the tutorials available for download. Simply go to: http://bit.ly/aLd6mW 

Thanks to Joe Galliera for such a great presentation!

This one was the first ever hands-on session I attended at SolidWorks World. Last year I wasn’t able to get into any of the hands-on sessions, but this year I had the opportunity to pre-register for several of them and it was one of the best things I could’ve ever done. 

This session was presented by Dan Riffell, Projects Coordinator at Eltron Research and Development. Dan is also a very well known contributor in the SolidWorks discussion forums and engineering community. Dan prepared this session because, believe it or not, how to model a thread is an incredibly common question among SolidWorks users, so he wanted to explain a few different ways to do it that may be useful depending on our needs.

First of all, Dan began by pointing out that we usually don’t need to model threads. Unless we need them for an animation, mold creation or a photorealistic image, for instance, most of the time, we can get by with using annotations and don’t really need a physical representation of the thread in the model. We can add a callout in the drawing with information about the thread or use a special kind of annotation known as cosmetic threads (Insert/Annotations/Cosmetic Threads).  

This kind of annotation appears as a feature in the Feature Manager and you can suppress it or delete it if you don’t need it anymore.

He then showed us how to create revolved threads. He sketched a thread profile and revolved it around the temporary axis of the part, creating a cut ( Revolved Cut), then he created a linear pattern using the revolved cut as the feature to pattern and the part’s temporary axis to define the direction.

Notice that this is not a real thread, but only looks like one, and it’s actually the kind of thread that is usually generated for most Toolbox screws.

The next method that Dan demonstrated involved the use of Swept Cut, as you can see in the image. He used the same thread profile sketch as before as the profile for the cut, but this time we had to create an extra sketch to be used as a path. It was a simple sketch of a line that runs along the axis of the part. The option to twist along path is what makes the profile describe a helix as it travels along the path.

The next method is very similar, but he creates a helical surface first and converts its edge into a 3D sketch to use it as a path for the Swept Cut command. This is similar to what Charles Culp did to create the telephone cord, remember? Notice that this time around the path is already describing a helix, so there’s no need to use the option to twist along path.

Another method to create a helical path for the thread is to simply create a helix by using Insert, Curve, Helix/Spiral, as you can see in the following image. By the way, to use this method you have to start by opening a new sketch on the circular face of the part and converting the edge to use it as the base for the helix. A curious fact: I asked Dan if it made any difference what start angle we chose and he said the rebuild time changes with the angle, for some strange reason.

Once you have the helix ready, you can use it as the path for the Swept Cut, and, just as before, there’s no need for the option to twist along the path.

 

What Dan demonstrated next was the coolest part, because he showed us how to create a design library feature to add threads to other similar parts without having to go through the whole process again and again.  First, he opened the Design Library Tab in the Task Pane and dragged the SweptCut1 feature from the Feature Manager tree  to the Design Library’s lower pane. A property manager appeared, as you can see in the image. From this property manager we can choose a folder where to store our new library feature and/or add a tooltip to remind us what this library feature is for.

Once the library feature has been added to the design library, we’ll see it in the lower pane or in whatever folder we placed it and we’ll be able to use it in other parts simply by dragging it from the lower pane and dropping it on the graphics area. In this example, after we drop the library feature, SolidWorks prompts for us to select a placement plane. Other selections will be necessary, as well (an edge, a sketch point and a face). All these reference selections are defined by the relationships that were used in the thread profile sketch. For instance, the thread profile was sketched on the Front Plane, so the Front plane should  be our selection for Placement Plane.  A little display pops up to help us along the proces,s by giving us visual clues of what we’re expected to select. In the image below, for instance, we are expected to select that circular edge we see there.

Once all our references have been selected, the thread is added to the part.

Last but definitely not least, Dan showed us how to model an inner thread, such as the ones in nuts, to match the outer one. We started with the model of a nut and inserted the screw we had been working with before by using Insert, Part.  We located the part as you see it in the image by adding a concentric mate  and a distance mate between both parts.  Remember, this is not an assembly, we inserted a part into a part.

Next, Dan showed us how to use Combine (Insert, Features, Combine) to subtract the screw from the nut, as you can see in the image. The nut is the main body (in green) and the screw is the body to subtract (in blue).

As a result of this operation, SolidWorks will remove or cut away the parts of the nut that overlap the screw, creating the inner thread. Neat!

As I said before, the step by step procedures and files for this and other presentations will be available in March. For now, I hope my little summary may be helpful to somebody.

Thank you, Dan, for this great presentation!

The first training session I attended was presented by Charles Culp, who is very well known at the SolidWorks Forums.  Charles was introducing all of us to a series of useful surfacing techniques, including how to convert a solid body into a surface body, fix some geometry, and then turn it back into a solid, the proper use of Delete Face and Delete Hole, the advantages of using Replace Face, and the difference between a boundary surface and a filled surface.  I arrived a bit late, but still managed to see him fixing a funny looking fillet located in a corner, similar to the one circled in red in this image. I tried really hard to reproduce what he had, but mine doesn’t quite look the same.

Anyway, he showed us how to trim and delete faces from the fillet, and then use Fill Surface with tangent option to patch the hole with a new, smooth surface, just like you see here in this image.

Of course, like I said before, my example isn’t exactly like his, so I did a few things differently to be able to delete the right faces, but the method and result are pretty much the same.

He also demonstrated how to model a telephone cord, by first creating a helix that follows a 3D spline. This is what he did: He started by opening a 3D Sketch and creating a 3D spline on it. Next,  he created the sketch of a line on the plane normal to the 3D spline at one of its ends and used it to create a Swept Surface, using the option to twist along path, as you can see in this image. The result is a helical surface that follows the path of the 3D spline.

He opened a new 3D sketch and selected the edge of the helical surface, then used Convert Entities to create a sketch of a helix.

Then he created a reference plane normal to one of the ends of that helix and sketched the cross section of the cord.

Finally, he created the telephone cord using the Swept Boss feature, with the sketch of the cross section as a profile and the helix as path. No need to twist this time around.

I wish this had been  a hands-on session, if only to have a copy of the original examples Charles used for his presentation. It’s OK; even though it wasn’t a hands-on session,  it was full of useful  information just the same. I believe the procedures of this and other sessions will be available in March. Until then, all I have to offer is my condensed version.

Stick around.  More chronicles from SWW2010 are  on their way!