GD&T Basic(s) True Position and Tolerances

This post is a very simple explanation of Position as used in Geometric Dimensioning and Tolerancing. Why am I writing about Position? One of the most frequent questions people ask me regarding Geometric Dimensioning and Tolerancing is "what does that target bulls-eye symbol mean". That bulls-eye symbol is called Position and it seems to be the most confusing and mysterious symbols in GD&T for some people. Before I talk about Position you should go back and read - or read if you haven't read already - THIS post that I wrote about tolerances and size and maybe even THIS post I wrote awhile back. There is nothing really mysterious or even complicated about the concept of Position and how it's used with Basic Dimensions in GD&T. The application can get pretty scary and complicated sometimes but the concept is pretty straight forward. I'm going to try and explain it in a overly simple way and later tie all these Design Related posts together as I write more of them.

 

Square Tolerance Zones

The first thing that is important to point out is that Geometric Dimensioning and Tolerancing is all about the dimensions tolerances so I'm going to compare the 'traditional' method of tolerancing to Position as a starting point. So to start with have a look at a 'traditional' drawing below that uses linear coordinate dimensions. On a 'traditional' drawing that is using linear dimensions the tolerances are put on each of the dimensions either directly as in the picture below or in the title block (or notes) on the drawing. Have a look at the below drawings 2A and 2B that are dimensioned 'traditionally' with the tolerances on the dimensions themselves. I have left the dimensions of the block itself off the drawing for clarity.

Linear Dimensions with a Square Tolerance Zone

  

In the top view of the above picture (2A above) there is a rectangular block and a couple of dimensions to a point near the middle. Imagine that you want to drill a hole 1.5 inches from the left side and 1 inch from the top as the dimensions show. Note that each dimension has a tolerance of +/-.25 inches so to get the hole in the right spot you first measure down from the top of the block 1 inch +/- .25 inches, giving you a total tolerance of .50 inches. Same thing with the other dimension, measure from the left 1.50 inches +/-.25 inches - again giving you a total tolerance of .5 inches. To get the hole in the right spot according to the dimensions (and the tolerances) you would have to drill the hole so that the center of the hole was somewhere inside that .5 inch square tolerance zone. Does that make sense? It seems strange if you think about it that a round hole would be positioned in a square tolerance zone doesn't it? Read more and this will start to make sense...

So looking at the above drawing 2A again there is a square tolerance zone created by the +/- tolerance on each of the dimensions. The point in the center of the tolerance zone is the Nominal position or the exactly perfect place for the center of the hole. In other words the dimensions are to the nominally perfect point that the hole center can be and the tolerances are showing how far away from that nominally perfect point the center of the hole can be. 

    

Another way of thinking about this is: The dimensions on a drawing are locating tolerance zones and not the features themselves. Read that last sentence again and keep it in mind because it's a important concept and will be really important soon. So in the picture above the 1.50 and 1.0 dimensions are not dimensioning to the hole they are dimensioning to the tolerance zone that the center of the hole has to be in. It's easy to look at a drawing like the one above and think that the "dimensions are to the hole" but in reality they are not really dimensions to the hole, they are dimensions to the area that the center of the hole can be in. I'm going on and on about this concept because it's important to understand especially later (in future posts) when I'm going to write about more dimensioning concepts.

   

In 2B of the drawing above you can see the square tolerance zone with a dimension from the nominally perfect point in the center to the corner of the square tolerance zone. That diagonal dimension is .354 inches and that is the worst case position that the center of the hole can be in, or the farthest off nominal that the center of the hole can be and still be OK.

"Really, the hole can be off .354 inches" you ask?

At first glance you might think that the worst case position that the hole can be off from nominal is .25 inches, after all the dimensions are +/- .25 inches, but that isn't the case because the tolerance zone is square shaped. Now have a look at the drawing below of the square tolerance zone that has two possible positions for the center of the hole, both .354 inches from Nominal.

The Pitfalls of Square Tolerance Zones

The drawing above shows the square tolerance zone and a couple dimensions to possible center points for the hole. Notice that the orange .354 dimension to a possible hole center is outside the tolerance zone but the black .354 dimension is just inside it.  The center of the hole can be off Nominal by .354 inches but only if the hole is off diagonally from the nominal point. If the center of the hole is off by .354 either horizontally or vertically then the hole is out of the tolerance zone and the part is considered to be bad. That is a very odd way to dimension hole because the hole is round and it usually doesn't matter which direction a round hole is off from nominal, because the hole is round! A round hole can usually be off a little bit in any direction and still work in the design. If you dimension the drawing with a square tolerance zone you would have to reject all the parts that had holes off by .354 inches unless they were off diagonally. This odd situation is the result caused by the square tolerance zone.

    

In the picture above I put a bunch of points where you might expect to see the centers of holes if you were to make a bunch of parts and measure the hole centers on all of them. When you mass produce parts you tend to get a Normal Distribution around the nominal position for all the dimensions, those points represent what you might see if you made a bunch of parts and measured to the hole centers on all of them. Using a square tolerance zone would mean that a lot of parts would be rejected and possibly scrapped because the hole centers were outside the square tolerance zone even though the parts would probably work OK.

    

Round Tolerance Zones

At this point I want to finally talk about Position and what it means in GD&T. In a huge oversimplification I'm going to say that in this example "Position is a round tolerance zone". I'll probably get a lot of emails (ottobelden.@yahoo.com) and maybe even nasty comments on this Blog about that last sentence because Position is a lot more than a 'round tolerance zone' but for now in the context of this post, think of Position as a round tolerance zone (it's actually cylindrical in this case but for now just think of it as round). To start this off I've redrawn the above drawing of the block with the hole in it using Position. Have a look at the drawing below and notice all the rectangles with numbers in them. The drawing looks complicated but really it's almost the same drawing as I did above.

Block and Hole Redrawn with a Position Tolerance
(the square tolerance zone is shown for reference only)

 

In the drawing 2C above I redrew the block and the hole but this time a equivalent Position tolerance is used instead of the square tolerance zone. The first thing that is different between the drawings is the 1.50 inch and 1.00 inch dimensions have boxes around them. When you put a box around a dimension it's called a Basic Dimension and Basic dimensions don't have any tolerance associated with them, they are perfect. Most people freak out at this point and say "you can't have perfect dimensions without tolerances" because nothing can be made perfect. That is true, all dimensions must have tolerances but the tolerances don't necessarily have to be on the dimensions themselves. With basic dimensions the tolerance is someplace else and not on the dimensions.

   

The concept of having 'perfect' Basic dimensions is not really that different from the +/- toleranced dimensions in the first drawings 2A and 2B above. With the +/- toleranced dimensions the 1.50 and 1.00 dimensions are dimensioning to the Nominally perfect center of the square tolerance zone so they are really perfect right? In the case of Basic dimensions (with the box around them) the 1.00 and 1.50 are dimensioning to the Nominally perfect center of a round tolerance zone and they are perfect too. The same perfect dimensions with just different shaped tolerance zones. The Basic box around the dimensions is really just a reminder telling you that the tolerance isn't associated with the dimension as it was with the +/- dimensions, the tolerances are someplace else.

 

Have a look again at the 2C drawing above. The 1.50 and the 1.00 Basic dimensions are locating the center of a round tolerance zone that is .708 inches in diameter. The .708 inch diameter tolerance zone is being defined in the rectangular box under the hole diameter with the "target bulls-eye symbol" Position symbol. The rectangular box under the hole dimension is called the Feature Control Frame and just like it's name it is controlling the Position of the feature (in this case the hole). This is a handy way of specifying the location of the hole because the location tolerance for the hole is right next to the hole diameter.

   

In drawing 2C I drew in the old square tolerance zone for comparison to the new round Position tolerance zone. Notice that the square tolerance zone is circumscribed by the round Position tolerance zone. That is because the .708 inch diameter round tolerance zone is 2X the .354 worst case square tolerance zone hole center location shown in drawing 2B above. Remember in the case of the square tolerance zone the hole could be off nominal by .354 inches only in the diagonal directions and not horizontally or vertically. The .708 inch round tolerance zone allows the center of the hole to be located .354 inches off nominal in any direction! With the position tolerance not only is the round hole being located with a round tolerance zone but if you make a bunch of parts and the hole centers are normally distributed around the nominal 'perfect dimensions' all the parts will be OK and not rejected.

Cylindrical Tolerance Zone with Position

Earlier in this post I said that Position tolerance zones are round but that wasn't exactly correct. Position tolerance zones are actually cylindrical in this case because in the real world parts are 3 dimensional objects. Position tolerance zones can be other shapes too and I'll write about those cases in another post, for simplicity in this case think of Position tolerances as cylindrical.

In the Feature Control Frame below the hole diameter I've added the letter A in it's own box. The letter A in this case is referencing a Datum that is being defined in the lower view of the part. What this means is that the .708 diameter Position tolerance zone is located in relation to Datum A, in this case the flat face of the rectangular block. Have a look at drawing 2D above to see what I mean and note that the round tolerance zone shown in the top view is extending through the entire part perpendicular to the flat surface datum A.

   

Remember that for the part to be OK the center of the hole has to be inside the tolerance zone. The center of a hole is really the center axis of the hole because the hole is a 3 dimensional feature. Because the Position tolerance is referencing Datum A the cylindrical tolerance zone is Perpendicular to the flat face of the part. What this all means is that the center axis of the hole must be completely inside the cylindrical Position tolerance zone as shown in drawing 2D above. The Position tolerance is controlling not only the location of the center of the hole but also how perpendicular the hole must be to the Datum face A. Isn't Position cool? 

  

In the drawing 2D above the hole isn't exactly Perpendicular to the face of the part but the center axis is entirely within the tolerance zone so the part is OK. If you wanted the hole to be even more perpendicular to the face of the part (but not change the tolerance zone) you have several options and I'll write about those in another post. For now the important concepts to remember are:

Dimensions on drawing are to tolerance zones and not to the features themselves.

Position tolerance zones are 3 dimensional and the center of whatever they are dimensioning must be entirely within the position tolerance.

Basic dimensions have a box around them and they are perfect, the tolerance for Basic dimensions is someplace else on the drawing.

Square tolerance zones allow things to be farther out from Nominal than the tolerance on the dimensions state because the tolerance zones are square!

This post is a simple explanation of the Geometric Dimensioning and Tolerancing concepts of Basic Dimensions, (True) Position and Datum's. There is a lot more to all these concepts that I didn't cover in this post in the interests of keeping it simple. I intend to elaborate on not only the concepts in this post but the other posts where I wrote about GD&T HERE and HERE and tie them all together. I will also cover other Position concepts as well as  lots of other fun and exciting GD&T stuff!! If you have any questions or see something I might have missed please leave a comment or send me an email at ottobelden@yahoo.com and I'll be happy to get back to you!