Another Tuesday is upon us and it’s time for another batch of fresh hot ASME goodness straight out of the oven. Today we are digging ever deeper into everyone’s favorite ASME Y14.5M-1994. Last week we finished on the Applications of Dimensions so this week will will begin digging into how to dimension features. As many types of features exist for a part there are as many techniques for dimensioning them. What are foreshortened radii? How do you dimension a part with rounded corners? What is a symmetrical outline? All these questions and more will be answered over the next couple of weeks. So grab your reading glasses and your thinking caps and lets go ahead and jump right in.

Diameters

When dimensioning a diameter you must precede the number value with the diameter symbol, shown below. I have seen some people try to sneak in the acronym DIA., but that doesn’t fly around here mister. Besides, if you are using SolidWorks you just have to click the diameter symbol in the PropertyManager. If you need to specify a spherical diameter, once again don’t type in SPHERICAL or any other variation, use the spherical diameter symbol shown below. In SolidWorks you can just plop an ‘S’ in front of the diameter symbol but this not exactly correct since it would create a space between the two. Instead use the Symbol Library to insert the Spherical Diameter symbol.

When dimensioning multiple concentric diameters, it is better to apply dimensions from the side view. Of course, this is not a rule, it is just good practice. Dimensioning a part from the front, looking directly at the diameters, could get confusing as to what dimension applys to which diameter.

Radii

As with diameters, when you dimension a radius; the radius value must be preceded with the appropriate radius symbol. Each radius dimension uses one leader and one arrow pointing to the arc. When a the position of the center of the arc is critical a dimension line is to be drawn from the center to arc with the dimension between the two, as long as space permits. When space is an issue extend the line beyond the radius center. When you do not dimension the center of the arc then center marks are ommited and the arc is controlled by other means such as the tangent surfaces. If you do dimension the center of the arc use a small cross to represent the center.

Foreshorten radii

A foreshorten radius is used when the center of the dimensioned arc extends beyond the limits of the drawing or the dimension may interfere with another dimension. In SolidWorks this is done by clicking the Foreshortened button in the Leaders tab of the Dimension PropertyManager.

The radius dimension is then foreshortened. When you dimension the centermark of the radius the dimensions will be foreshortened as well.

True Radius

When you are dimensioning a radius in a view that is not reflect the true shape of the arc the word TRUE precedes the arc dimension. In SolidWorks this is done automatically when you place the dimension but it may require some massaging.

Multiple Radii

When you are dimensioning multiple radii of the same radius you may dimension one of the radii and precede it with the number of times, as in 3X R.125.

Spherical Radii

As with spherical diameters, when you are dimensioning a spherical radius the dimension is preceded with SR. This however does not need a special symbol from the Symbol Library.

Chords, Arcs and Angles

Chords, arcs and angles are dimensioned as shown below. Chords and angles are simple to dimension but dimensioning an arc tends to be a sticky point for a lot of people. In SolidWorks, to dimension an arc with the dimension tool active click the arc. Then while holding down the CRTL key, click both of the end points of the arc.

Rounded Ends

The image below illustrates the techniques for dimension features that have rounded edges. First dimension the overall dimension by holding down the SHIFT key in SolidWorks and clicking both of the arcs. When the arcs is a full radii,only indicate the radius but it is not dimensioned. When the feature has partial radii, then they are dimensioned.

Well, I think that will do it for today. Next week we will continue all the fun. Until then, I hope you are making even better drawings with the information I have shown you today and all of the previous Standard Tuesdays. As always, I will always be here to help you with any questions you may have.

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