CNCCookbook: Be a Better CNC'er

Do you want to be a better CNC'er in 37 Seconds?

Get Better Tool Life, Surface Finish, and Material Removal Rates Fast.

It's that easy. You can install and get results now.


CNC Design for Manufacturing (DFM)

This article is part of our CNC Machining and Manufacturing Cookbook.

What if there were changes in your design for a part that could make the part radically easier to manufacture without reducing the value of the part in any way? Wouldn't you want to make those changes up front instead of learning about them the hard way as you actually started making the parts?

It turns out there is an entire body of thinking around this topic and it's called "Design for Manufacturing" or "Design for Manufacturability." It's often abbreviated as "DFM".

What sorts of things come into play for DFM?


Overview of Design for Manufacturing

Let's break down Design for Manufacturing into some high-level ideas and categories, with some specific examples for each:

Material Type

The type of material chosen for the part will affect manufacturability greatly. Plastic, aluminum, and brass are very easy to machine compared to titanium and hard steel alloys, for example. If the part must be accurately made of steel, specify low carbon hot rolled rather than cold rolled. It is much more stable whereas the cold rolled will warp and require multiple machining operations to be accurate.

Take time to choose materials whose physical properties are adequate (but not overkill) for your part's needs.

Next, choose materials that satisfy those needs at the lowest cost for the material and at the lowest cost in terms of machining. Sometimes you'll want a more expensive material because you'll more than save the time in reduced machining costs by choosing a material that's easier to machine.

A good example would be choosing 303 stainless steel instead of 304, because it machines more nicely than the 304. Or perhaps you can use a tougher aluminum alloy like 7076 instead of some grades of steel because even though aluminum is more expensive, it can be machined much faster than the steel on most CNC machines.

Hardness tester

A typical hardness tester...

In general harder materials are more difficult to machine. Be aware of the different hardnesses available for different materials and their alloys and conditions. The condition of a material is, for example, different degrees of hardening. Information on Hardness for various materials, alloys, and conditions, is contained within G-Wizard for your reference.

Material Shape

Consider which shapes are cheaper to acquire versus which shapes are closer to the finished part and hence require less machining to complete. Bar stock can often be had for 1/2 the cost of plate for a given material, but you can waterjet more parts out of a plate. It'll take some careful calculations to tell which is cheaper to manufacture. If volumes are large enough castings or extrusions may further reduce machining time.


Material Size

When deciding your part's dimensions, visualize how they will interact with the rough stock sizes that are available. You need an allowance for machining that doesn't require too much step up in rough stock size lest you waste the time and material cost of turning that extra stock into chips.


Rough Stock Preparation

The cheapest form of material removal often comes at the rough stock preparation stage. For example, if you can start machining operations on a waterjet cut blank, you may only need one pass instead of a bunch of roughing passes followed by a finish pass.


Keep Tolerances Loose

The tighter the tolerances, the higher the manufacturing costs. Don't specify tight tolerances unless they're really needed. One of the most expensive tolerances is thread depth, and it often doesn't matter. Specifying thread depth to three decimal places is seldom going to accomplish much other than driving up costs substantially. More on the cost of tight tolerances.


Depth of Cut vs Radius of Corners

You can't cut a tight corner radius with a tool whose diameter is more than twice the corner radius. At the same time, the stiffness of a tool changes with the third power of length and the fourth power of diameter. Making the tool twice as long makes it 1/8 as rigid. Making the tool twice the diameter makes it 16x more rigid. Therefore, avoid designing parts with tight radius corners that are very deep.

A good guideline is keep the ratio to 3:1 depth vs diameter (2x corner radius). So, a pocket with a 1/4" corner radius should be no more than 1.5" deep or you'll greatly increase the manufacturing costs.

Here's another tip: choose a corner radius just slightly larger than the endmill radius that will be used to make the corner. This reduces the loads on the endmill due to lower tool engagement angles in the corner and will reduce your manufacturing costs as a result either by allowing the endmill to be fed faster or by causing it to last longer.


Through Holes and Deep Holes

Where possible, specify through holes as they facilitate chip evacuation. This is particularly important on holes that will be reamed or threaded.

Deep holes are also much more expensive to manufacture. Try to keep the ratio of length to diameter under 4 (no holes more than 4 diameters deep) for best results. Any hole over 10 diameters deep is likely to be problematic, there are tools like G-Wizard's Deep Hole Wizard to help.


Edge Preparation

It's generally cheaper to chamfer an edge than to radius the edge.


Avoid Mirror Image Parts

Mirror image parts are generally used in pairs in an assembly. If the assembly can be designed so that both parts can be identical, great savings can be had because you'll be producing twice the volume of half the part types.


Avoid Thin Walls, Thin Webs, and Similar Features

Thin walls and webs are prone to chatter (which slows down machining speeds), distortion (so it's hard to hold tolerances with them), and are more easily damaged on the assembly line.


Avoid Undercuts and Similar Features that Require Special Machining

Undercuts are a lot more trouble to program and machine in most cases so make sure you really need them before specifying them on a part. Undercuts can be eliminated in surprising ways if you can learn to Think Like a Plastics Engineer.


Provide Tool Clearance When Turning

90 degree shoulders provide less tool clearance than tapered shoulders and so are more trouble. Also, if you're turning down an area to achieve a tolerance, if the shoulders bordering the area are perpendicular a burr is more likely to be formed than if they're not.


Threads and Tapping

There are a myriad of ways to minimize the costs associated with threads and tapping including:

- Minimize the threaded length in the hole. 1.5x the major diameter often provides sufficient strength.

- Avoid blind holes where possible. If you must thread a blind hole, allow room at the bottom of the hole for 1/2 major diameter more than the threads.

- Don't over-specify the thread percentage. A 75% thread has 95% of the strength of a 100% thread but only requires 1/3 the torque--so it is much less likely to break a tap. G-Wizard Calculator can help you select the right twist drill for particular thread percentages.

- Avoid tight tolerances on thread depths as they're expensive to implement.

- ProCNC has a number of good DFM guidelines for threads and threading.


Use Bosses Instead of Large Flat Areas

Where precision mounting is desired, consider using bosses around the dowel pins or fasteners rather than specifying the entire area be flat. It's cheaper to make the bosses flat and the flat area may not be adding any value to the part.


Make Floor Radius Smaller than Corner Radius in Pockets

It's easy to turn out a CAD drawing where the radius on the floor to wall edge is the same as the radius in a corner, but it'll cost more to produce because it will likely require a ballnose cutter to do the floor radius which means an extra pass with an extra tool. Specify a small radius for the floor that is available on a bullnosed end mill that can be used to do all the machining in the pocket.


Minimize Setups

Where possible design parts to be made in as few setups as possible--preferably in one setup.

For turning, try to put all the precision features so they can be turned in one go without having to remove or "flip" the part. Especially avoid rechucking to machine features that must be concentric with features before rechucking.


Design for Multiple Setups and Fixturing

If you must use multiple setups, follow design practices that minimize the cost.

When a part will require multiple setups, design the fixtures and parts so it is impossible to put the part into the fixture incorrectly. This can mean adding keys or asymmetrical features such as the placement of holes that interact with the fixture. Making it impossible to orient the part wrong in the fixture will ensure greater success for our operators and avoid costly mistakes on parts that already have prior machining operations invested in them.

Even better is to make every part symmetrical so that no matter which way it is oriented in the fixture, it will be correctly machined.

Provides features on the part that make alignment in the fixture easy.


Minimize Tooling Requirements

Be cognizant that the machine tool has a limited number of slots in its tool changer and each one is valuable. Try to design the part to use as few different tools as possible. For example, you may be able to use a spot drill to countersink a flathead cap screw. You may be able to reduce the number of drill sizes needed by using interpolation and an endmill for several hole sizes. You may be able to reduce the number of taps needed by using thread milling. If you're working on a very expensive assembly that needs to be tapped after lots of hours of machining, consider thread milling instead of tapping--if the thread mill breaks it won't be stuck in the hole.

Each of those ideas carries trade offs that have to be evaluated to determine which will truly yield a lower cost of manufacturing.


Design for Assembly (DFA)

Design for Assembly is a subset of Design for Manufacturing. The idea is to change the design to make it easier to assemble the parts. There are a lot of techniques around this, but here are two examples:

- Keep the tolerances on bolt holes loose to allow for faster fit against a wider array of potential misalignments.

- Use fewer fasteners. Bolts are primarily good for holding and so-so for alignment. Machine features into the parts that ensure alignment without requiring the bolts to do so.


Select a Gentle Entry to the Cut

Many CAM programs offer a wide variety of entry methods: plunge, ramp, helix down, etc.. Some of these methods are far gentler than others. Be familiar with the best methods and select these over the harsher approaches. For more information see our "Toolpath Considerations" chapter from the Feeds and Speeds Cookbook.


Give Bolts a Loose Fit Keep as much clearance as possible in the holes that locate bolts. This provides a margin for error if things don't line up quite right. Clearance may be achieved with oversized holes, or even by having slots rather than holes. Remember: you can't move threaded holes! If things don't line up, your best bet is more clearance in the non-threaded holes.
Avoid Flat Bottom Holes Blind holes must be cut with a drilling tool that has a conical bottom. To finish a flat bottom may require an extra operation or may make the overall operation slower.
Avoid Partial Holes Partial holes are those where the drill axis is less than a hole radius from the edge of the material. They're hard to machine accurately as the tip wants to wander.
Keep the hole axis perpendicular to the surface Drilling into an angled surface is prone to tip wander. To avoid it requires milling a shallow pocket before drilling which makes the hole more expensive to machine.
Avoid Deep, Narrow Slots Keep the final depth of cut less than 15x end milldiameter for soft materials (wood or plastic), 10x diameter for aluminum, and 5x diameter steel. Longer tools are prone to deflection and vibration which leads to bad surface finish, poor tool life, and poor tolerances.
Design with the Largest Possible Internall Radii The smaller the internal radius, the smaller the end mill that may be used, making the job more expensive. Ideally, make the radius slightly larger than a standard endmill size too.
Avoid Long Thin Parts When Turning They may require a tailstock or other means of support.
Keep straight parallel outside edges This makes workholding easier when outside edges are straight and parallel.
Keep straight inside edges If the walls of a pocket are not vertical, they will be more expensive to machine.
Minimize Tool Changes Any change that saves a tool change will save time. For example, using fewer unique hole sizes.
Inside Fillets vs Chamfers Inside chamfers are time consuming and difficult to create. Inside fillets are easier to make because round tipped endmills can be used.
Avoid smooth round edges Putting a radius on all the edges may make a part look better, but it also makes it more expensive to machine. Simply specify "break all edges" and let the shop find the most cost-effective way to do that. If a more extensive treatment is needed, chamfering is preferable to rounding. If you must radius the edges, at least make them all the same radius so multiple tools aren't needed.
Use GD&T Rather Than +/- Tolerances GD&T tolerancing can be more lenient than +/- tolerancing in many cases.

There is special Design for Manufacturing Software available that suggests changes to your designs to reduce the cost to manufacture. For example, our G-Wizard Calculator's CADCAM Wizards have a DFM hint window that makes Design for Manufacturing suggestions.




Try the Free Trial Version of G-Wizard G-Code Editor...


No credit card required--just your name and email.




Featured Articles

Step-By-Step Guide to Making CNC Parts

CNC Router Cutter Types

Why Use a Single Flute Endmill?

Step and Servo Motor Sizing

The Truth About Tool Deflection

10 TIps for Router Aluminum Cutting

2 Tools for Calculating Cut Depth and Stepover

CNC Machine Hourly Rate Calculator

Special Purpose CNC Calculators

Feeds and Speeds Guide

CNC Cutter Guide

Feeds and Speeds By Material

G-Code Tutorial

  Feed Rate Calculator

Sales, and Special Deals


GCode is complicated.
G-Wizard Editor
makes it easy.

Try It!


Feeds and Speeds:
Made Easy.

Try G-Wizard



Do you want to be a better CNC'er in 37 Seconds?

Get Better Tool Life, Surface Finish, and Material Removal Rates Fast.

It's that easy. You can install and get results now.


Start Now, It's Free!