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.