GD&T: Multiple Datum's Referenced, More Than One Datum?

Datums referenced on a drawing using Geometric Dimensioning and Tolerancing can be really confusing, even on simple parts! When you get right down to it Datums are not that difficult to understand when you consider what they are used for. I have received several questions about Datums, why and how they are used and why use more than one. I'm going to answer those questions using a simple part that has one hole and has three Datums referenced. But before I go into the explanation about multiple Datums I recommend that you read THIS post I wrote about a parts size and how the dimensions tolerances determine what a part can actually look like. For a quick review there are THESE posts that I wrote about Geometric Dimensioning and Tolerancing Basic concepts. This post is a quick overview of the basic concepts of using multiple Datums. There is a lot more to Datums than what I'm writing about here and I'll get into those more complicated concepts later!

     

Lets start with a simple drawing of a part that has one hole in it and the hole is positioned in relation to three Datums.

 

Simple Part with Multiple Datums

The drawing above has a hole in it that is True Position to three Datums in this order: A B C. The reference to Datum A is holding the location and orientation of the center axis of the hole to Datum A (bottom surface). Take a look at THIS picture from an old post if that doesn't make sense. Another way to look at this is Datum A is the surface that someone is going to measure the perpendicularity of the hole to. So Datum A in this case is a place to start taking measurements. We'll start taking measurements with Datum A because it's the first Datum and we will continue measuring the part with the remaining two Datums in order from left to right. The Datums don't have to go in alphabetical order, they are in used in the order that you reference them when you measure the part. The important thing to remember is Datums are used to measure a part.

   

So what are the other two Datums doing? I'll explain the below... ;-)

To keep it simple I'm not going to go into great detail about what Datums are and what kinds there are in this post but I do want to mention what Datum planes are before I go too far in explaining what the above drawing means.

    

Datums are theoretically perfect geometric concepts that don't actually exist in the real world and there are several kinds of Datums that are used in geometric Dimensioning and Tolerancing. Datum Planes are the only type that I'm going to go over very briefly here but the concept is the same for all types.

     

A Datum Plane is a two dimensional collection of points that extend to infinity in two directions, like a perfectly flat plate. We can't create a perfectly flat plane that goes to infinity in two directions! The best thing that we can do in the real world is to Simulate a Datum plane with a really really really flat piece of something (usually granite) called a Surface Plate. For that reason the real world representations of Datums are called Datum Simulators and Datum Simulators are what are used to measure a part. Remember this is all about measuring the part!

     

Have a look at the above drawing again. It's a simple plate with a hole in it and the hole is positioned in relation to three Datums. To measure the part correctly a piece of tooling could be created that simulates the three Datums and holds the part while it is being measured. The Datum Simulator tooling might look like the teal colored part in the drawing below.

 

Simple Datum Simulator Tooling

The teal colored Tooling part above is simulating the three Datum planes in the drawing. To measure the red part (from the drawing) it would be placed into the tooling in the order that the Datums are called out in the drawing. What does that mean?

   

Datum A is the first Datum called out on the drawing so the part would be placed flat on the tooling with the three highest points on the bottom of the part making contact and establishing Datum plane A. Datum is B is next and the part would be pushed in the direction of the yellow arrow (1) until two points on the side of the part make contact with the tooling. To find Datum C the part would be pushed in the direction of the purple arrow (2) while keeping Datum A's three points and Datum B's two points in contact, until the highest point on the top of the part touches the tooling. There are a total of six of the highest points on three surfaces of the part in contact with the tooling, and the part can't move. Now measurements can be made from the tooling to the hole location to see if the hole is Positioned correctly.

 

To summarize the Datums are used to measure a part. Establishing the Datums is a way to hold and locate the part (constrain the degrees of  freedom) so that it can be measured. In the above picture showing the Datum Simulator Tooling it should be obvious that the order of establishing Datum's B and C doesn't matter. You could reverse Datum B and C and get the same results because the part is perfectly square and it's sides are perfectly flat.

   

So why does the order of the Datums on a part like this make a difference? In the real world things aren't so flat and square and that can make a big difference!

   

Below is a drawing of the part showing how it could be fabricated in the real world with the dimensions (and tolerances) given in the first drawing above. Notice that the four sides of the part are not straight but they are within the size tolerances called out in the drawing. The height of the part is 4.00" +/- 0.12 and the width is 3.00" +/- 0.12 and the part is within those size limits. It's worth noting that the top and the bottom of the part could be similarly wavy but for simplicity I drew them flat.

 

The Above Part Made To It's Extreme Width and Height

In the above part example the fabricator cut out a somewhat rectangular shape 4.00" +/- 0.12 in height and 3.00" +/- 0.12 in width. After having cut out the rectangle they used a straight edge to find the two highest points on the left hand side (Datum B) and one point on the top (Datum C) and measured to drill the hole. Putting this part into the Datum Simulator Tooling shows that the part is to print in this example.

   

A Part in Datum Simulator Tooling

In the above picture the part has been placed into the Datum Simulator Tooling just like it was before. First Datum A is established on the three highest points of the back of the part. Second the part is slid to the left in the direction of the yellow arrow (1) until the two highest points of the left side are in contact with the tooling. Lastly the part is slid up in the direction of the purple arrow (2) until the top highest point is found. The detail on the left side of the drawing shows a red circle that is in the Nominal Position of the hole center as measured from the tooling. The red circle is a 0.080" Dia. circle per the tolerance of position in the drawing (have a look at the first drawing in the post).  The center mark of the hole on the part is right in the center of the tolerance zone and in this example the part is to print!

   

What happens if we reverse Datums B and C? To show that the order makes a difference I took the same part and put it into the Datum Simulator Tooling but this time I used the top of the part as the second Datum and the left side as the third Datum and got different results.

 

Same Part With The Second and Third Datum's Reversed

Just as before the part is placed into the tooling with the three highest points establishing the Datum A surface. This time the part us pushed up in the direction of the yellow arrow (1) until the two highest points touch the tooling and pushed to the left in the direction of the purple arrow (2) until one point touches. Again the detail on the left side of the drawing shows a red circle that is in the Nominal Position of the hole center as measured from the tooling. This time because the part was placed in the tooling with two of the Datums reversed the center of the hole is not within tolerance! The order in which the Datums are used makes a difference.

   

The same sort of thing can happen if you use one side as Datum A when making the part and use the other side (the opposite surface) as the Datum when measuring the part. The order that the Datums are called out on the drawing is the order that the Datums should be established when fabricating the part and also when measuring the part.

   

The above part was shown with exceptionally 'wavy' sides as an exaggerated example. In reality you wouldn't expect to see a part made like that but if you were worried about it (and wanted generous size tolerances of (+/- 0.12) you could use a flatness callout on the Datum surfaces to make the 'smoother'. When selecting surfaces to use as Datum planes a designer would pick surfaces that make sense for whatever the part is. In the above example part the Datum A surface would probably be the side that mates with another part. The other two Datum sides might be important because the part fits into a corner (much like it does on the Datum Simulator Tooling). In fact the tooling designed to measure a part probably will look a lot like where the part is going to be used.

      

There are some real disadvantages to dimensioning a part like above. It's clear from the drawing the the position of the hole is rather important but the overall size of the part isn't. Measuring a part like that can be a challenge and even worse if the part is symmetrical it might be impossible to tell which side is which. Imagine if  the hole were exactly in the center of the part, there would be no way of telling which sides were used as Datums B or C and which face was used as Datum A. Where the dimensions are placed on the drawing, the Datums selected and the tolerances all determine how a part is made and how it is measured. There might be one (or maybe several) right ways to draw a part but there are a lot of wrong ways to do it. Everything depends on how the part it going to be used. 

    

One of the many ways to draw the above part is in the first drawing at the top of this post using three Datums. An alternate way of doing it might be something like the below drawing.

   

Alternate Method of Dimensioning the Part

In the drawing example above there are only two Datums and one of them is the hole. The Composite Feature Control Frame is using a Profile tolerance and is in relation to the Datums. This drawing is essentially saying:

"Take a big plate and drill a hole in it. Measure from the hole to find the edges of the rectangle and cut it out"

In this way the drawing is showing that the hole is the starting point (because it's important) for measuring and fabricating and the shape of the part is to be located around the hole. I'll write more later about Composite Feature Control Frames and multiple Datum uses. In the meantime I hope this post answers more questions than it creates ;-) If you do have any questions please let me know with an email or leave a comment!