Designing Parts for Small Batch Machining

CNC Machining when combined with 3D CAD/CAM has revolutionised workshop practice in recent years. It has opened up a whole new world of possibilities for designers who are designing machined components which are intended to be produced in small or medium sized batches.

But what has changed and what are the constraints from a designers point of view?

Ultimately the constraint on the designer is always cost. Almost anything can be made - somehow - if cost is not a constraint. What a designer needs to know is which features on a component are cheap and easy to produce and which are more difficult and therefore costly. This is not always obvious unless you have good experience of manufacturing parts using modern techniques.

As a starting point lets start with the easiest component to make and see what features can be added and what are the implications. What hasn't changed is that the easiest component to make is a parallel sided block with a pocket or other features on.
The reason this is so simple is that it can be held easily in a vice, machined around five sides and then put back in the vice upside down and skimmed to thickness. This process requires very little setting up and requires no special fixtures.

What has changed is that now the complexity of the pocket makes very little difference to the cost. When using a 3D CAD/CAM system the shape and depth of the pocket are simply picked from the model with a couple of clicks of the mouse and the software takes care of the rest. The complexity and size of the machine program produced makes no difference as modern machines have large memories and the files are transferred electronically.



This same principal applies to complex pockets with a number of different levels. Again the different pockets and depths are easy to pick from the model. The constraint which hasn't changed is the effect of the size of the corner radii. The smaller the radius in the corner then the smaller the cutter which must be used. As pockets get deeper then the more problematic it becomes as the cutter must get longer and therefore its aspect ratio increases so it becomes more prone to vibration and breakage. To overcome this problem the cutting depth and cutting speed must both be reduced to compensate and therefore the cost quickly starts to rise as the cycle time of the component increases. The golden rule is always to make these radii as large as possible even if it means creating more complex shapes in order to reduce the effect of these radii on the assembly.

Other features which might be added are tapped holes. The number of these and their positioning again make little difference to the machinist. Modern machines with a rigid tapping facility can tap holes very quickly and reliably. There is a common misconception that blind tapped holes are problematic to produce and ideally avoided but this is not the case at all - it makes no difference to the machinist. What does make a difference is the depth of the thread and the clearance between the bottom of the thread and the bottom of the drilled hole. Typically a thread depth of 2 x the thread diameter is easy to produce but anything longer becomes a real problem as the tap is much more likely to bind up and break. A good clearance between the bottom of the thread and the bottom of the hole - a minimum of 0.5 x thread diameter - is required as standard taps always have a lead in on the thread. Deeper tapping or threads taken to the bottom of the hole can be produced but are likely to require specially ground taps and to be tapped by hand which puts the cost of them up enormously.