Designing for Manufacture: Keeping the Production Team Happy
By Dave Lapthorne for Autodesk University
In this article, we will be taking a look at some design decisions which can make the jobs of our production teams much harder than they need to be. From features that are difficult to machine to part orientation considerations, the main takeaways will, if applied appropriately, result in designs which are easier to machine and produce efficiently.
Basics of CNC Machines and Tooling Geometry
A computer numerically controlled (CNC), milling machine is used to transform blocks of raw stock into finished parts by cutting away material. There are generally 3 axes to a milling machine:
For the purposes of this discussion we will consider the following directions when referring to the orientation of operations and tools:
X: Left to Right (sideways as viewed from the operator’s position)
Y: Forwards and Backwards (as viewed from the operator’s position)
Z: Up and Down (vertical as viewed from the operator’s position)
These three axes of motions let the spindle, which spins a cutter at high speed, carve away material and leave behind nearly any shape desired.
The part being milled is held in a vise, which is in turn attached to the table of the CNC.
There are more advanced machines with additional features and axes but understanding the simple 3-axis milling machine is an important first step to mastering manufacturing.
Types of Milling Tools
These are the most commonly available type of cutter. They’re efficient and cheap. Flat end mills are most commonly used for machining of flat bottom cuts and vertical walls.
The bullnose profile cutters are similar to Flat Endmill in that they share a common rectangular side profile but with an additional radius at the bottom corner of the flutes. They are great for quickly removing material while leaving a small bottom radius in pockets
The ball endmill has a full radius at bottom of flutes. These cutters can be utilized for complex surfacing as the contact point between the tool and material surface is constantly changing with variations in the slope of the surface.
Drills are used exclusively for making vertical holes in parts. There is no side to side or horizontal motion of the tool when using drills. The finished size of the hole will be dictated by the diameter of the tool itself. Subsequent operations can be used to alter the size of the hole (reaming, etc.) but those tools are not discussed here.
Additional Considerations Regarding Endmills
Besides the side profile it is also important to understand how the number of cutting edges, or flutes, are formed into the tool as viewed from the cutting end.
More flutes on a cutter restrict the amount of available space for the cut material (chips) to be removed. However, tools with a higher flute count perform better in harder materials.
The cutters shown on the right are center-cutting. This means that the sharp edge of the flute across the bottom of the mill extends all the way to the centerline of the tool.
Types of Milling Tools
But What about Tool Length?
Tool diameter, profile, and number of flutes are important things to consider. Another critical piece of information to consider is the tool length. Especially the exposed length of the tool that is exposed when the tool is clamped in the tool holder or spindle. This is commonly referred to as the tool stick out.
Tools which have a high ratio of stick out length to diameter are considered to be high aspect ratio. As the side of a tool comes into engagement with the material while cutting the forces involved work on the tool to create tool deflection. The higher the aspect ratio of the tool, the more deflection will be created.
Operations which create high side loading and therefore increased potential for tool deflection are:
- Deep pockets
- Large step down (changes in Z height) during operations
- High feed-rates (the speed with which the X or Y location of the tool changes while cutting)
One final topic worth discussing regarding tool geometry is the length of cut (LOC) that a tool can achieve. Some end mills have flutes that terminate at the same diameter as the portion of the tool which engages in the holder. Others have a reduced or necked down profile where the effective cutting diameter is less than the diameter of the holder:
Tool Aspect Ratio and Deflection
In the above graphic we can see the impact of tool aspect ratio on tool deflection. Deflection can be considered as the difference in location of the tool tip as a result of side loading.
For this example, doubling the length of the endmill while maintaining the diameter will result in an increase in deflection of around eight times.
Alternatively, halving the diameter of the endmill while maintaining the length will increase deflection by around 16 times.
If both endmills have the same side load applied, but the one on the right of the image is twice the length of the one on the left we will see much more deflection along the length of the tool.
This is a critical point to consider when designing parts. Having an understanding of available tools and their geometry can help to streamline the production process by ensuring that the features that are modeled are machinable with the tools on hand.
Shorter endmills with relatively large diameters, low aspect tooling, will allow for higher rates of material removal and a more cost-effective part.
When considering internal fillets on vertical walls, we can see how the previously discussed topics impact our design process.
The height of the vertical wall ideally should be less than the flute length of the tool and the radius of the fillet should be larger than the radius of the available tooling.
Generally speaking, the fillet radius (R in the graphic) should be greater than one-third of the vertical wall height.
It is also important to ensure that the part fillet radius is less than radius of the tooling. This ensures that the amount of tool that is engaged with material stays more consistent.
If the tool radius is too close to the radius of the part then the result will be a spike in tool engagement as the tool rounds the corner. This can lead to breaking tools or the tool chattering (rapidly deflecting and bouncing) which will degrade the surface finish.
Bottom Edge Fillets
Often the design will require internal fillets at the bottom of pockets or walls. In fact, parts without this feature can experience unplanned failure of the final assembly as a result of stress risers caused by a sharp corner.
In order to minimize potential machining challenges when producing these parts, it is advisable to make the following allowances in the design.
If the pocket is for lightening of a design, then the fillet may be able to be deleted from the design entirely.
For fillets that are required, consider selecting a fillet radius that matches to the corner or ball radius on multiple tools. This can allow the operator to use a suitable ball or bullnose endmill to machine the fillet.
If you are unsure of the corner radii available to the operators, then it is better to select a larger fillet radius to allow for usage of larger diameter tooling.
If the design intent allows, it is worth adding fillets to vertical external corners. This will allow for in-process deburring of those edges.
Since the toolpath will already be running around the profile of the part, these fillets can be added without appreciably increasing machining time (provided the fillets are of reasonable radius). The smaller radius selection is not as critical on external fillets as it is on internal ones. This is due to the way that the tool engages with the material. It is not experiencing a spike in loading or deflection on the outside corners.
Chamfering and Deburring
It is preferable to break the sharp edges on parts during the manufacturing process. This is because of the way that milling machines are capable of creating incredibly sharp edges which can lead to workplace injury when production workers are handling parts.
Unless it is critical for preventing interference with mating components, or some other important part of the design intent, avoid using fillets to deburr top edges of parts.
The tooling required to create these features in simple linear moves of the machine will need to be matched precisely to the radius (form tools).
Form tools can be expensive to purchase or require excessive time to fabricate in house.
In these situations a simple text callout on the drawing that states “BREAK SHARP EDGES” can reduce machining time by not holding the operator to a specifically toleranced dimension. This will also allow the operator to use readily available chamfering tools and negate the requirement of purchasing custom tooling.
Only model a chamfer if you need a specific toleranced dimension. In this case, it is recommended to use a 45-degree chamfer. This is a very commonly available chamfering tool. Different widths of chamfers can be produced with the same tool depending on where the toolpath is programmed.
Holes and Threads
Several factors can impact the manufacturability of hole features.
Hole Bottom Profile
When creating blind holes (holes which do not pass all the way through the thickness of the part) it is best to permit a drill point bottom rather than a flat-bottomed hole.
Due to the cutting geometry of drills, there is a natural angle (usually 118 or 135 degrees) that can be used to form the bottom of the hole.
When comparing the machining loads involved in machining a flat-bottomed hole versus a drill point bottom the thrust loading will be lower for the drill point hole. This will result in cleaner holes, lower temperatures during machining, and also allow the operator access to a wider range of options for tooling.
As a general rule, keep the depth of the hole less than or equal to six times the diameter of the hole. It is possible to machine deeper holes but they may require specialized tooling or different operations on the machine.
If the design requires through holes, consider specifying two holes, one from each side of the part. The downsides to this approach include the requirement for an additional setup on the mill (discussed later) as well as the potential for some misalignment of the holes where they intersect.
For tapped holes it is important to be mindful of both the depth of the threading as well as the bottom profile of the hole.
Thru holes are preferable to blind holes. This is because a through hole will allow for the chips to fall out the bottom of the hole as well as ensuring that sufficient coolant can flow in the area that is being machined.
For a blind hole, ensure that the remaining untapped material is at least half the hole diameter if at all possible. Holes that are tapped all the way to the bottom require different tooling than holes where the threading stops short of the bottom.
For thru or blind holes, there is not an appreciable increase in the connection strength when threading deeper than three times the diameter of the hole. Specifying a thread depth in excess of this is only putting added pressure on the operators who are making the parts and most likely drastically increasing machining time.
Proximity to Other Features/Edges
Always be careful regarding how close to an edge or adjacent features holes are placed. Holes placed on uneven faces or next to edges can be very difficult to machine accurately.
Holes where the diameter breaks through an adjacent wall can result in tool breakage, sharp corners, and poor surface finish.
When drilling holes which start on non-flat faces, the drill point will often wander from the desired centerline and this may result in the part being scrapped.
Proximity to Other Features/Edges
When working with sheet metal parts that will be formed on a brake press, it is important to pay attention to the location and diameter of holes with relation to brake form lines.
The sheet metal is going to deform slightly during the brake forming process and holes that are placed too close to those edges can distort into a tear-drop shape instead of maintaining the full round shape.
A common work-around to this situation is to have the production crew drill the holes after brake forming. Precise locating of the holes can still be achieved by ensuring that small pilot holes are pierced by waterjet or laser during the production of the flat pattern. Alternatively, the center marks can be etched if that functionality is available on the machine.
In situations that require holes to be placed next to adjacent walls or at the bottom of pockets, always be mindful of the diameter and length of available tooling.
In this example, placing the hole in it’s current location will result in the tool holder crashing into the vertical wall before the hole is fully drilled.
If the design allows, consider moving holes further away from adjacent walls. If that is not possible then the operator may choose to drill the hole from the other side of the part which will require additional time for setting up the part in the machine vice or fixture.
Feature Height and Thickness
Components which require fins or ribs of material can present challenges beyond the ones outlined on the previous page. If the height of the machined features exceed approximately four times the width of the feature, the vibrations induced during machining can result in poor surface finish, scrapping parts due to them being out of tolerance, or even tool breakage.
High Precision Locations
In areas where high precision flatness is required, it is easier to maintain those tight tolerances in smaller regions. To this end it is recommended that the components are designed with raised bosses which will be machined with slower, higher precision strategies while allowing the rest of the part to be machined in a more efficient manner.
Machining Complex Surfaces
While complex surfaces can be aesthetically pleasing, they also require different tooling and more complex machining strategies. The net result is increased machining time which will drastically impact the cost of manufacturing.
Complex surfaces, such as those with compound curvature, are typically finish machined using smaller diameter tooling. Often times small ball end mills or access to multi-axis machining centers will be required.
Additionally, multiple passes running perpendicular to each other may be necessary to fully machine the surface to an acceptable finish.
Undercuts are sometimes required for assembly or fixturing purposes. In these cases, specialized tooling will be required for successful machining.
T-Slots on a milling table are a great example of this in order to correctly machine T-Slots, an initial pass or series of passes will be run with a straight end-mill followed by subsequent passes with a T-Slot cutter to machine the undercuts.
In situations where an undercut is necessary for retaining mating parts it is worth assessing the design and determining if an acceptable compromise can be met such as machining open slots and bolting flat bar strips in place to create the retaining slots.
When part marking is required it is recommended to use engraving rather than embossing. Embossing typically refers to text which is raised above the finished surface. To machine small features like this will require very small end mills (assuming the font face used for part marking is around one-quarter inch in height) to be able to get into the small inside corners and interior pockets.
Engraving is typically done with a ball or v shaped end mill and involves cutting the lettering into the finished surfaces.
Interfacing with Square Corners
Often times, when designing fixturing for machining parts the parts that are being clamped have sharp outside corners. In these cases, consider using a dog bone corner on your fixture.
This involves an oversized round cut at the inside corner to allow the mating part’s square corner some clear space without damaging the part.
When creating dog bone corners, make the circular cut as large as practical with the available tooling.
Whenever material is loaded onto a machine and clamped in place, this is referred to as a setup. In the example at the beginning of this article, all three axis directions are fixed. This means that if a part has machined features on the top as well as through the sides, two or more setups will be required to completely machine the component.
It may be worth considering adjustments to the design to permit fewer setups. Each setup on the machine will add to the required time to produce the parts and may also necessitate additional clamps or fixtures.
It may not always be possible to redesign a component to reduce setups. There is always a balancing act between manufacturability and fully capturing the design intent. Reduce setups wherever possible. The most important thing is to understand how the decisions made during the design process may impact the production team’s time or ability to easily produce the parts as designed.
Dave Lapthorne is an implementation consultant with D3 Technologies, an Autodesk Platinum Partner and Authorized Training Center. He is based at the Springfield Missouri office. Primarily focused on Inventor workflows, he also specializes in the CAM tools, drawing on more than 15 years of industry experience ranging from machine design, sheet metal design, CNC programming, and project management. Additionally, he has spent several years working hands-on with manual and CNC machine tools including water-jet, plasma, milling, turning, plus shear and brake forming operations.