Another Wednesday is upon us and it’s time for another installment of Standards Wednesday. This week we get to jump in right into Section 2 of ASME Y14.5, General Tolerancing and Related Principles. If you are new to Standards Wednesday, let me explain it to you. Every week I take a different part of an ASME standard and do my best at breaking it down into easy to understand English and try to relate it to SolidWorks.  Over the last couple of weeks I covered Section 1 and if you missed anything, I highly recommend going back and read them…they were pretty good.

A General Introduction

Section 2 of ASME Y14.5-1994 introduces you to the practices for tolerancing linear and angular dimensions  and how to interpret tolerances.  There are a few ways to apply tolerances to a dimension and I am not referring to the tolerance types. Since everybody likes bullet points, here are the different ways to apply tolerances to a dimension:

• Apply limits or plus and minus tolerancing to the actual dimension
• Use GD&T (Geometric Dimensioning and Tolerancing) *Future Post
• In the general notes referencing specific dimensions
• Specified in other referenced documents
• In the general tolerance block in your title block

Locating Features of Size

Although not required, it is generally preferred to locate Features of Size using positional tolerancing methods that we will discuss when we begin GD&T principles. If you are not comfortable or familiar with positional tolerancing then it is perfectly fine to stick to the conventional methods. Hopefully, after we cover GD&T you will feel 100% comfortable using the methods we discuss. Now I know some of you are asking “What the heck is a Feature of Size?” Section 1.3.17 of the standard defines a Feature of Size as:

One cylindrical or spherical surface, a set of two opposed elements or opposed parallel surfaces, associated with a size dimension.

Implied 90° Angle

When you have centerlines or surfaces of a feature being shown as intersecting at a right angle and are they not dimensioned then it should be understood to be 90°. A simple example would be a standard centermark, one centerline is vertical, the other is horizontal and they appear to be right angles. There is no need to dimension the angle because there is a implied angle of 90°. If the features being shown were actually 89.99° then they should be dimensioned but how often does that happen? If you apply a global tolerance to angles in the general notes or in the title block, angles that are implied 90° are affected as well.

Direct Tolerancing Methods

The following are the different direct tolerancing methods used per ASME. In SolidWorks, select one of the methods in the pull down in the Tolerancing/Precision section in the Dimension PropertyManager

Basic Dimension

We will cover Basic dimensions later when we dive into GD&T but since were here you might as well see how to specify a dimension as Basic. A basic dimensions is a dimension with the value shown in a rectangle. No you don’t break out the rectangle tool, instead select Basic in the Dimension PropertyManager.

The dimension is now shown as being basic.

Bilaterial Dimensions (Plus or Minus)

This is one of the cases when SolidWorks differs from ASME. When you compare the standard to SolidWorks, your eyes would probably cross.  In ASME a Unilateral dimension is a plus or minus dimension with one of the limit values as 0 (zero). However a Unilateral dimension is created using the Bilateral dimension in SolidWorks. A Bilateral dimension is a toleranced value with both a plus and minus value following the dimension. In the Dimension PropertyManager, select Bilateral and enter in the plus (+) and minus (-) values.

The dimension is now updated.

Symmetric Dimension

A symmetric dimension is a bilateral dimension with the plus and minus values equal. Yes, a symmetric dimension is a bilateral dimenison per ASME but is designated as symmetric in SolidWorks. After selecting Symmetric in the Dimension PropertyManager, enter the +/- value.

The dimension is now shown as a symmetric…or bilateral dimension.

Limit Dimensioning

When tolerancing a dimension using limits, the high limit is above and the low limit is below. When using one line, the low limit is before the high limit separated by a dash. To apply a limit tolerance in SolidWorks, select Limit in the Dimension PropertyManager and enter the plus (+) and minus (-) values.

The selected dimension will appear as below, with .005″ being added and subtracted to the nominal of 8.000″:

Metric Limits and Fits

I will be covering Limits and Fits at a much later date, once I replace my copies of the standards. Until then, if you know how to use them, you can add the Limits and Fits symbols to dimensions per ANSI B4.2 in the Dimension PropertyManager.

To be Continued…

That does it for this week, but don’t forget to come back next week. At this rate it will probably take me at least a year to cover ASME Y14.5 completly but it will do us all good

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