Gabi Jack's Blog

The bug that really wasn't

While chatting on Twitter a few days ago, a couple of SW users and yours truly got a bit confused about changing the display settings of annotations in a drawing document.  The misunderstanding began when one of our fellow users asked something more or less like this:  “In Document Properties, Detailing, Annotations Display, it won’t let me change the Text scale of the annotation. Why and how can I change it?” The answer came right away: “Clear the option bellow (Always display text at the same size)”. However, this didn’t seem to do the trick, because the option was grayed out, it was grayed out for our friend and for me, as well. Our friend even called his VAR, and the VAR saw the same, so, without any possible explanation for this, we all thought it was, perhaps, a bug. Well, while I don’t know if the VAR ever came back with a solution or an explanation for our friend, after seeing exactly the same happen in SW2007,

in SW2008,

and even SW2009,

I couldn’t help but wonder what was really going on here. It can’t be the same bug in all three versions, can it?

Puzzled, I did some research on my own and it turns out it wasn’t a bug, after all, and, in fact, there was absolutely nothing wrong. It’s meant to be that way!  According to the help files, Text scale and Always display text at the same size are options available only for part and assembly documents. They are disabled for drawing documents, which would explain why they appeared grayed out in all three versions of SW. When Always display text at the same size is cleared you can specify a scale for the default size of annotation text, like in the following image, where I specify a ridiculous scale of 8:1 for the size of the annotation text.

When the option is selected, all annotations and dimensions will be displayed the same size regardless of how much we zoom in or out. Again, this option is not available for drawings, because SW always adjusts the text height for drawing documents every time we zoom in or out. This doesn’t really change the size of the text as it would appear when we print the drawing; it only means that the text is getting zoomed in and out for better display while we are working with the drawing in the computer.

One more question remains, though… Was our friend actually trying to modify the size of the text? If that’s what this SW user was trying to do, then the easiest way to do it was to go to Tools, Options, Document Properties, Annotations Font,  select the kind of annotation, and then modify the font and size of the annotation according to his needs.

I’m pretty sure our friend figured this out in the end. We all have times when we get confused. I should know! But, you know, besides learning something new, this incident made me wonder about how many times something like this has happened to other users.  How many times have we found bugs or problems that really aren’t there? How many reports to the VAR have been made over something that really wasn’t anything at all? And how many VARS have actually figured that out and told you so right away? How many of them agreed with you it was a bug? (Gasp!) Perhaps, the biggest lesson here is that we should all start by reading those help files first… just in case.

Favorite Note

Learning how to properly do drawing and detailing in SolidWorks isn’t precisely the most exciting thing in the world, but it’s necessary, so I try to keep at it, even when it seems I’m making progress in an extremely slow fashion.

Anyway, I was learning how to create Annotation Favorites, when I noticed that something was different about Favorites for SW2007 and SW2008, when compared to SW2009. Well, first of all, an Annotation Favorite is any kind of annotation such as a note, weld symbol, surface finish symbol, geometric tolerance symbol, etc., that can be named and saved to be reused in the document.  They are called Favorites in SW2007 and SW2008, but renamed as Styles for SW2009. The extension of the file in which SolidWorks stores this information has also changed, but never fear, because you will still be able to use your favorites created in SW2008 and SW2007 in documents created in SolidWorks 2009. I’ll tell you all about it in a few minutes.

Using SW2008, I created a favorite by selecting a note (My Note in the image) and clicking on Add or Update a Favorite in the Note property manager on the left. I was prompted to enter a name for my Favorite, and so I named it My Little Note. 

The next step was to save this favorite as a file, so I could be able to reuse it in this or other document. Notice the extension .sldnotefvt given by SW2008. I saved this file in the annotations folder of SW2009 Design Library, just to see if I would be able to reuse it in a document created in SW2009.

And, yes, the Favorite was still available for use in SW2009.

Now, why did I do this? What made me wonder if I would be able to use the same favorites in SW2008 and 2009? Well, it’s just that, as I said before, the extension of the files for SW2009 is now different to the way it was for SW2008. In the following image, notice the extension .sldnotestl given to the same Note when it’s saved as a Style in SW2009, previously known as a Favorite for SW2008.

These favorites or styles can also be deleted and edited at any moment. To edit one of these favorites, simply make whatever changes you need to it, select it, click again on Add or Update a Favorite, select the name of the favorite you are updating from the list, and finally, save it again, same way you did before.

Crème de la Crop

Well, not precisely… This is just a quick tip on how to edit a cropped drawing view. As you probably already know, whenever you create a cropped view in SolidWorks, the two things you need are a model view and a closed sketch that will define the area of the view that you wish to keep. Everything outside the sketch will be eliminated. But what happens if you make a mistake while creating the sketch or if it doesn’t include everything you needed it to show in the cropped view?  Well, you can always edit the crop!

In the following image, Drawing View 3 is a cropped view, but I need to edit it somehow, so that it includes an edge that I left out when I created it.

All I have to do is right click on Drawing View 3, then click on Crop View, Edit Crop.

By doing this, I will be once again able to see the original view as it was before the crop, and I’ll also  be able to edit the closed sketch that defines the crop. Notice how I’m simply modifying the closed spline, to include the edge.

After all changes to the sketch have been made, all I have to do is click Rebuild.

And the new cropped view now also includes the edge, just like I wanted.

SW2009: Creating customized drafting standards

So many things that can be customized in SolidWorks 2009! This one in particular caught my eye, mainly because I’m still learning about drawing and detailing using SolidWorks. More in particular, I’ve spent the last few days learning about the different weld symbols available in SolidWorks and how to position them correctly in a drawing document. I’ll tell you more about that in a future post. For now, if you want to learn about what’s new for weldments in 2009, visit Ricky Jordan’s blog. He’s got some great posts and cool videos there.

Now back to the subject of this post. According to the “What’s new?”document, SolidWorks 2009 allows the user to create customized drafting standards in order to define their preferred specifications for annotations, dimensions and tables in a drawing document. This set of detailing properties included in the customized drafting standard can then be saved in a file and used in multiple drawings. It could be shared, for instance, among members of a team, to eliminate the guessing work and achieve uniformity.

Creating a customized drafting standard is really easy. First you need to do go to Options, Document Properties, Drafting Standard. On the right side, you will see a list of all available pre-defined standards. Select one from the list as the overall drafting standard.

Notice that at this point, you can’t specify a name for your customized standard or rename any of the fixed ones.  Select any of the detailing properties defined by the overall standard and modify according to your needs.  Notice on the top of the property manager, how as soon as you modify any of the detailing properties, the name of the overall drafting standard changes to reflect that you have modified it, and to avoid overwriting it. In this image, I changed the display type of the datum feature to Round (GB), which is different to what was specified by the ANSI overall drafting standard I had chosen in the beginning.

If you now go back to Drafting Standard, you’ll notice that you are allowed to rename the overall drafting standard and save it to an external file.

Later on, as needed, you can load that drafting standard to use it in another drawing.

I think this functionality has a lot of potential. What do you think? What would you use it for?

Stumbling... then learning about fit tolerances with SolidWorks

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.