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So, after a short break I headed over to the meeting room Toucan 1 for the Weldments focus group meeting, hosted by Jay Patterson, SolidWorks Product Specialist for DS SolidWorks. Once again, this was an extremely small group, but luckily graced with the presence of Randy Ooms, from Granco Clark, who really knows what he’s talking about when it comes to SolidWorks and Weldments. Randy is also one of this year’s speakers; together with Nicholas Benner, he’ll be presenting about SolidWorks Network Implementation on Wednesday at 1:30 pm.

I must confess that I was feeling a bit out of place, because the guys that were there have not only been using SolidWorks for quite a few years, but are also very well entrenched in the industry. However, I’m grateful that they allowed me to be there and learn from them.

First thing that surprised me was to hear how some of the functionality provided by SolidWorks sometimes goes unused, because it really doesn’t cater to their needs. The weldment bead feature is an example of this. Most of them don’t really use it, unless it’s absolutely necessary, like in case it needs to be included in an analysis of the model. The limitations of the bead feature were also discussed, as well as ideas to improve it and make it actually useful.  Weldment profiles are another good example of this. In fact, Randy mentioned that in his company they have practically thrown away the profiles supplied by SolidWorks  for aluminum and steel structural members and substituted them with their own, simplified, custom profiles, because this way it’s easier for them to obtain the information they need  (and nothing else they don’t need) about the size of the profile by looking at the name of the sketch, while in the profiles provided by SolidWorks all sketches are called sketch1 by default and don’t provide much information at a glance. On this same topic, it was also mentioned the need for a way to obtain information on those weldment profiles that may not be accessible to the user, perhaps in the shape of a flyover little window that provides that info, even if we can’t really open the profile to examine it.

The desire for enhancements for gussets and end caps was also addressed, more in particular, the need for automatic properties to be generated, so the user doesn’t have to go and apply dimensions to them manually in order to make them parametric, and, in the case of end caps, it was also discussed whether it’s useful or even desirable by some users to allow the length of a tube to be shortened when applying an end cap, like it’s currently done in SolidWorks 2009.

One of the attendees spent quite some time explaining about the trouble he’s got when modeling something as a huge multibodies weldments part that he then would need to break down into several parts, each with their own BOM and detailing. That’s when Jay mentioned how weldments in the past used to be more assembly oriented, as opposed as the way it is nowadays, and posed the question to the group on whether it would be useful or not to somehow orient it to be more about assemblies again, instead of multibodies parts. Personally, I have no idea how this weldments functionality used to be in the past and the multibody approach is all I’ve known, so I can’t tell if this would be a good idea or not. 

As an added bonus, we learned a bit about using library features to flatten the ends of a tube. It was a good meeting, but it would’ve been even better if more people had shown up. After all, that’s the purpose of these meetings, to get the feedback from the users of the product, and hopefully, a few ideas for enhancements and new functionality that is really needed.

 

As I had mentioned in my previous post, by the time I was finished with this little piece of fence, I had already collected twenty five bodies that appeared listed under “cut list” in the Feature Manager. How can this cut list be used as a mean to convey information about the model? Well, first of all, it needs to be updated, which means that all the members in the weldment that are similar will be grouped together in folders. In order to do this, right click on Cut List in the Feature Manager and select Update.

As a result of updating the cut list, we now have six different folders of cut list items, each containing the members of the weldment that are the same. Notice that the number in parenthesis indicates the amount of items in each folder. Placing the cursor over the name of each folder or item lets you see which item it is in the graphic area.

The next step is to customize the cut list, so it can become really useful for us. The first thing we may want to do is to give each item in the cut list a more meaningful name by renaming the folders, like I’ve done in the image. To rename the folders simply click on their names once, wait a bit and click again, then the text will show up inside a white box and you’ll be able to delete the old name and write your own.

Once we’ve renamed the items, we now proceed to customize the properties of the items as we want them to appear in the cut list. Right click on any of the item’s name (the names of the folders) and select properties. This opens the following window. As you can see, Length and Angles have already been assigned and calculated by SolidWorks. To add another property to the list, click on an empty cell under Property Name and select from the different options, in this case I selected Description, to add a short name to identify the item.  Notice that whenever you use a weldment profile supplied with SolidWorks, there’s usually already a Description of the item, inherited from the profile. In my case, I didn’t have a description for my profile, so I’m adding one this way, instead.

On the corresponding cell, under Value/Text Expression, I wrote the short name/description that I wanted to associate with that item.  I could’ve also linked this value to a dimension in the weldment profile, for instance, by double clicking on the dimension in the graphics area. The Evaluated Value shows the way this information will appear in the cut list when you add it to a drawing document. It is also possible to add other properties, like Weight, Volume or Surface Area and let SolidWorks calculate them for you.

After adding all the properties to every item on the cut list, it is finally ready to be inserted in a drawing document. In the drawing document, select the view that will be associated with the cut list, then click Insert, Tables, Weldments Cut List.

A property manager will show up. It allows you to customize a thing or two about how the cut list is displayed in the document.

After you are done customizing, click OK and drag the table to wherever you want to position it on the sheet.

Finally, you can change the size of the table by dragging its corners, just like you would do with any other window. Notice how all the properties we specified appear in the table, except for the Angles.

I must admit that this is not precisely what I had in mind when I first heard about weldments in SolidWorks. I actually thought that it would be like a representation of the different kind of welds, but all I’ve seen on that is the Fillet Weld. It doesn’t matter; I think this way makes a lot more sense.

The house I grew up in was a Mexican colonial style, with beautiful wrought iron fences and gates surrounding the yards. There were also wrought iron details on stairs, windows and doors.  Here in my neighborhood I’ve found only houses with backyard fences made out of wood, and no fence in the front yard. They look nice, but at times I kind of miss the elegance of the wrought iron fences of my childhood. Maybe that’s why I decided to make this for my very first experiment with SolidWorks weldments.

As I found out, most of the time, when working with weldments, you will need to create a sketch that will work as a layout or skeleton of your design.  You also need a second sketch, known as a weldment profile, and that is actually a Library Feature kind of file (.sldlfp). Think about a sweep feature for a moment; the weldment profile will be swept along the path you specify with your layout or skeleton sketch. In the following image, for instance, the line in blue corresponds to Sketch 1, the layout sketch, and the sketch in pink is the weldment profile that is being swept along Sketch 1.

Layout sketches can be 2D or 3D sketches, but they must contain only lines and arcs, no splines.  As for the weldment profiles, SolidWorks provides a few, and others can be downloaded from the internet (subscription service members only), by clicking on the Design Library tab on the task pane and then on SolidWorks Content, and opening the Weldments folder. Once there, ctrl + click on the zip file of weldment profiles you wish to download, unzip the files, and make sure to add the path to their location on Tools, Options, System Options, File Locations, Weldment Profiles, so you can access the weldment profiles in SolidWorks. 

You can also create your own weldment profiles, and that’s what I ended up doing, since I couldn’t find one suitable for what I had in mind. Creating a weldment profile isn’t hard, but there are a couple of things you need to keep in mind.  The first thing to consider is that the origin of your sketch will automatically become the default piercing point of the profile, so you better take advantage of any symmetry your profile may have. The second thing to consider is that later on, while using the profile to create structural members, it will be possible to select any vertex or sketch point as an alternate piercing point, so make sure to plan for it.

So, with this in mind, the procedure for creating a weldment profile is quite simple. Open a new part, create your sketch, and then save it as a Library Feature Part (.sldlfp) in a location where SolidWorks will be able to access it later. This is one of my custom weldment profiles. As you can see, it’s a very simple shape of the cross-section of a rectangular rod.

Once I had my custom profiles ready, I made my first sketch on the Front plane. The circle you see there isn’t actually a closed entity; I used Split Entity on it, or else it wouldn’t work out as a path to create a structural member.

On the weldments toolbar, click on the Structural Member icon and this will open a property manager that allows you to select the weldment profile you wish to use, the path, and even the orientation of the profile, by rotating the sketch or changing the piercing point. In my case, I’m choosing one of my custom made profiles, Sq. 0.5.sldlfp that I saved in a folder called Created Rods. As path segments, I chose the two vertical lines in the sketch.  Notice that the same sketch can be used to create different structural members.

I can now use the rest of the sketch to create other structural members in a similar fashion. I start by choosing one of the arcs in the design in the middle. I want it to be one structural member, rather than three smaller ones, so after I select all three arcs, I make sure I mark the option Merge Arc Segment Bodies in the property manager.

Notice in the image that I need to reorient this particular profile.  I begin by rotating it 90°.

This works better, but I have interference with the other structural members. I can solve this by clicking on Locate Profile in the property manager and selecting a different pierce point in the sketch, one on the edge of the profile, instead of the origin. In the image, the point in pink is the current pierce point, the point in orange indicates that the point can be chosen as the new pierce point.

Here is the result of this last operation, plus doing exactly the same for the circular sketch in the middle.

Notice how each time a new structural member is created it’s also added as a new body, and listed under Cut List. This is, in fact, a multibody part with four different bodies, so far.

The rest of the structural members in the fence are created in a very similar fashion, using a couple of other custom profiles of mine, the four sketches shown in different colors in the following image, and the Linear Pattern feature (keep in mind that we are patterning bodies here). Notice in that same image that there’s now twenty five bodies listed under Cut List.

This post is way too long already, but in a future one I’ll show you what to do with that Cut List and how to use it in a drawing document.

So, what do you think? Is that a nice fence or what?

Learning how to use the different tools for drawing and detailing in SolidWorks is not precisely the most fun I’ve had with the software so far. I’d much rather work with the solid model!   Maybe that’s why I had been putting it up for later, and why I get sidetracked so often.  Anyway, after beating myself up for not being more diligent, I’ve spent most of this week studying and practicing with the different tools available for adding dimensions and annotations to drawings.  It’s not as bad as I thought it would be. In fact, it’s kind of fun… sometimes. It’s a bit confusing at times, because the books and manuals I have are based on SW2007 and I’m finding that a few things have changed in SW2008, if only in the user interface and the way to access some of the options. It’s no big deal because I’ve found everything so far, it’s just confusing. However, I must admit that I got stuck when it came to all the different tolerance and precision options.  More in particularly, I got stuck with the different options for fit tolerances.

Perhaps, it’s because I never really used such tolerances in the past that now they seemed so confusing. The SolidWorks help file explains how to use the functionality, but it didn’t help me much to understand what  they were all about, so I searched around in a few books here and there, and I think I finally got it. This kind of tolerance refers to the fit between mating parts, more typically holes and shafts. There are four classifications you can choose from in SolidWorks: user defined, clearance, press and transitional.

In a clearance fit, the shaft will always fit inside the hole and there will always be a space or clearance between the parts.  In the press or interference fit, the shaft is slightly larger than the hole and there is always an actual interference of material. The mating parts must be pressed together. A transitional fit may result in a clearance or an interference condition. Whenever one of these classifications is chosen, SolidWorks will filter the kind of tolerances available that, according to standards, correspond to that classification. Once the tolerance is chosen for the hole or shaft, the list for the other type is filtered once again to show only corresponding tolerances for the mating part. This can be tricky, sometimes, it may tell you that there are absolutely no matches for the kind of fit you chose, so it’s always useful to remember to select the type of fit depending on the use or service required from the equipment. Most of the time, choosing for the hole first is the way to go, but there may be times when it’s advantageous to choose a fit and tolerance for the shaft first, like if you have several parts, each with different fits, that are required to be assembled on a single shaft.

ANSI has issued preferred limits and fits for cylindrical parts in the shape of tables that recommend standard sizes, allowances, tolerances and fits.  These tables prescribe the fit for any given size or type, and they also prescribe standard limits for the mating part(s) that will produce the desired fit. Letter symbols identify five types of fits as follows:

            RC       Running or Sliding Clearance Fits

            LC       Locational Clearance Fits

            LT        Transition Clearance or Interference Fits

            LN       Locational Interference Fit

            FN       Force or Shrink Fits

These symbols, plus a number that is used to indicate the class of fit within each type, are used to specify a complete fit.  However, the choices you have to select the type of fit tolerance for holes and shafts in SolidWorks aren’t these ones, but the corresponding ISO symbols. At least, that’s all I see. According to the ISO system, limits and fits are divided into three different categories:  clearance fits, transition fits and interference fits.  So, for instance, according to this classification, the clearance fit would include those that were known in the ANSI standard described previously as Running, Sliding, and Locational Clearance fits. The Transition Fit would include those that were known as Locational Transition, and the Interference Fit would include those known as Locational Interference, and Force in the ANSI standard. The tolerance symbols include the basic size for the hole or shaft, followed by a letter that indicates the fundamental deviation (uppercase for holes and lowercase for shafts), and a number that indicates the IT grade. So, as an example if you specify the fit tolerance for a shaft as:  25 f7, it means that the basic size of the shaft is 25 mm, with a close running fit, and the dimension limits for this shaft would be Ø24.98-24.959 mm.

Sounds a bit confusing? Well, at first, but it really isn’t so bad once you look it up on tables, which are available, for example, in the Machinery’s Handbook or even in some drafting books. I actually want to learn more about tolerancing and dimensioning standards after this. It’s quite interesting!

One advantage you have here is that, unless you choose to do it yourself, SolidWorks automatically calculates the bilateral tolerances for you, according to the kind of fit you specify, so if the size of the part ever changes, they will be updated as well. And by the way, you can choose between three different ways to display the fit tolerances:  If you choose Fit from the Dimension Property Manager, under Tolerance/Precision, it will display as the basic size of the hole or shaft plus the tolerance code.

If you choose fit with tolerance, it will display the basic size, the tolerance code and the value of the bilateral tolerances.

You can also exclude the code altogether and display only the basic size and tolerances by choosing Fit (tolerance only).

There’s also the choice of including the type of fit for the mating part in the same annotation, if you wish to do so. This option only works for Fit and Fit with tolerance because they display the tolerance code. Note that the bilateral tolerances won’t be displayed in this case, only the codes.