The SolidWorks Geek

We are back this week with some more ASME goodness after taking a short break. This week is all about Tolerance Accumulation per Section 2.6 of ASME Y14.5. You maybe asking yourself right now, “What is Tolerance Accumulation?”. Tolerance accumulation, or tolerance stack-up, is the dimensional variance between two features of a part based on the tolerance range of the intermediate dimensions. How you apply dimensions and tolerances to features on a part can have a huge effect on the finished part. Today we will look at some simple parts and how different methods of dimensions can give you dramatically different results.

Chain Dimensioning

Chain Dimensioning is the method of dimensioning the beginning of the next feature from the end of the last. It seems pretty straight forward but some may not realize that this gives the greatest amount of variation. The illustration below shows a simple revolved part dimensioned using this method. The part shown was modeled to have a mean distance of 3.500″ between surfaces A and B. Adding together the tolerances of the three intermediate dimensions, you will see that the actual variance is +/- .015″. This would make the maximum distance between A and B to be 3.515″. This may not seem like a lot but it may be enough to affect the overall performance of the design.

Base Line Dimensioning

Base Line Dimensioning gives you a better result then Chain Dimensioning. With Base Line Dimensioning each feature is dimensioned independently from each other, all off the same origin. By using this method you are creating less variance between features since the actual variance is the tolerance of the two features added together. Using the same part as before, this time using base line dimensioning, the actual variance is +/- .010″ because you are only going to add the tolerance of the dimension that affects A to the tolerance of B. This will make the maximum distance between A and B to be 3.510“. This is better then before, but we can sill do better.

Direct Dimensioning

Direct Dimensioning will give you better control over the finished dimensions of the part since you will be tolerancing the specific features you wish to control. In this part we have been concerned about the true distance between A and B, so why don’t we just control that dimension. By adding adding a dimension between A and B we cut the variance down to +/-.005″, this would give us a maximum distance of 3.505″.  I am not saying that you should not use any of the two previous methods. Each method has it’s place and you should consider what variance you can accept when dimensioning your parts.

Dimensional Limits Related to an Origin

As you saw in the previous sections how you dimension a part can seriously effect the final results. Where a dimension originates from can also have an effect on the final shape of the part. The method shown below designates a feature as the dimension origin using a Dimension Origin Symbol instead of an arrow. This is not the same as designating a “datum” as you would in GT&D (we will cover Datums at a later date) instead this method is used to create a tolerance zone that the feature must lie. Look at the 1.000+/-.100 dimension, the shorter side of the part is being designated at the origin. This means that the tolerance applies to the other side of the dimension, the longer side.

The figure below better illustrates what the tolerance zone created by designating the shorter side as the dimension origin. The entire longer surface indicated must lie within the tolerance zone created.

In case your wondering why it makes a differences as to what side the dimension originates, the view below shows how the part could be made of the other side was designated. Big difference, right?

Designating a Origin

Now that you know what is a dimension origin, you probably want to know how to add the symbol to a dimension. I must admit, this stumped me for a while and I must thank Josh Mings at Solidsmack for helping me figure it out. The key is to make sure that your the intended dimension is not set as a Smart Dimension. If you right-click on the dimension and you see Smart Dimension selected, de-select it. Then on the dimension itself, when you select it, you will see nodes on each arrowhead.

When you right click on the node, you will be presented with the available arrowhead types. Click the Dimenension Origin Symbol, the one that looks like an empty circle.

Think Before You Place…

If there is one thing should learn today, it should be “Think before you place your dimension”. As you have seen, if you don’t take into consideration how you place dimensions, you could be in for a big surprise when you get your finished part.