It’s Wednesday and you what that means…another Standards Wednesday! Woo-Hoo! What better way to celebrate the hump day then with some ASME goodness? Last week we finally completed our four part series on dimensioning of features per Section 1.8 of ASME Y14.5M-1994. This week we move onto the next section, Section 1.9, Location of Features. Section 1.9 describes the methods used to dimension the location of features. Basically there are two main methods to dimension the location of features; rectangular and polar coordinate dimensions. Today we will dig into both of these two methods.

General

The two dimensioning methods, rectangle and polar coordinate dimensioning, are used to specify the location of an individual or a group of features from an origin point or datum. Dimensions can also be used to locate features from other features. We will be covering datums in detail on a future Standards Wednesday.

Locating Round Holes or Symmetrical Contours

Round Holes or other features consisting of symmetrical outlines, such as slots, should be located using the center of the feature. However, if the design intent requires locating the hole by the edge, the center does not need to be located.

Rectangular Coordinate Dimensioning

Using two or three perpendicular faces or planes of your part, Rectangular Coordinate Dimensioning locates features using linear dimensions. It should be obvious and clear which faces, or planes, are used to located the features. In SolidWorks using the Smart Dimension will more then suffice for most Rectangular Coordinate Dimensions, although I do find myself using the Baseline Dimension tool since it cuts out extra mouse clicks.

The image below shows two examples of Rectangular Coordinate Dimensioning.

Rectangular Coordinate Dimensioning Without Dimension Lines

Section 1.9.2 of ASME Y14.5M uses the term ‘Rectangular Coordinate Dimensioning Without Dimension Lines‘ but us SolidWorks geeks know these types of dimensions as Ordinate Dimensions. Ordinate Dimensions are shown with the dimension value on extensions lines with no dimension lines or arrows. In SolidWorks, to use this method of dimensioning select Ordinate Dimension from the Dimension fly-out.

Before placing dimensions the origin must be indicated as 0. Click the edge that will be the origin and locate the dimension.

Place the dimensions by clicking the feature to be located. The dimensions will automatically be aligned to one another. To dimension the vertical locations, after dimensioning the horizontal, reselect the Ordinate Dimension from the fly-out. In Section 1.9.2, the diameters of the holes are indicated with a hole chart. In my opinion, this was great when we were doing drawings on a drafting table but with SolidWorks we want the diameter dimension to update with any feature changes. With this in mind, I strongly recommend dimensioning the diameter with conventional methods.

Tabular Dimensioning

In my opinion, Tabular Dimensioning is another one of those throw backs to the board days. As shown in the figure below, dimensions are not placed on the drawing, instead each feature is identified with a symbol and referenced in a table. I don’t like this method for two reasons. One, there is no clean way to achieve this method in SolidWorks. Two, the table is not linked to the part so feature updated will not be updated in the table. Like I said this is only my opinion, so take it for what it’s worth.

Polar Coordinate Dimensioning

As shown below, Polar Coordinate Dimensioning is much like Rectangular Coordinate Dimensioning except you’ll be using angles and linear dimensions to locate features about a fixed point.

Repetitive Features or Dimensions

Although I have seen many methods for doing so, repetitive features and dimensions should be indicated with the number of places follow by an ‘X’ and a space preceding the dimension value. For example ’3X R.125′ means the radius indicated is .125 and applies to three places on the drawing. If you are specifying a basic dimension the ‘X’ can be either inside or outside of the box. In SolidWorks the ‘X’ will be placed outside of the box when you specify a repetitive dimension as basic.

Use of ‘X’ to Indicate “By”

I am sure everybody has seen it, an ‘X’ used to indicate “By”. Most will see it being used when dimensioning a chamfer as in .125 X 45° which indicates .125 BY 45°. Another example would be when dimensioning slots as shown in a previous Standards Tuesday.

Well that does it for this weeks Standards Wednesday. Short post today but then again it’s a short section. Next week we will begin Section 2 of ASME Y14.5-1994, General Tolerancing and Related Principles. Keep those questions coming, I love hearing from readers, and don’t forget to comment on this and other posts.

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