Design guide for CNC Milling

CNC milling is the most common fabrication method for professional prototyping, scaling well into the low- to mid-volume levels and sometimes higher. As with any manufacturing process, the more familiar the designer is the better and easier to produce the part will be. However, given the incredibly varied design possibilities and the flexible nature of the CNC milling process, it would be nearly impossible for one person to have a complete knowledge of the process and all its variations.

CNC milling

While a designer can be expected to know the basics, such as internal pockets requiring radii due to round cutters being used, knowledge of the nuances is less common. This short guide should help the advanced beginner design better parts when those parts will be milled.

Corner Radii

As you can imagine, since the cutting tools used in milling are round, it’s darn hard to make a sharp internal corner with a mill. The larger tool you use the faster you can cut, because of deeper possible radial engagement and more stiffness allowing more axial engagement and faster feed rates. So, the minimum radius of your corner is going to be the radius of the cutting tool.

1But that’s not the end of the story. Corners are tough on your tools. From happily cutting along one edge, your mill now engages in the corner and at the forward edge. In the picture to the left, the cutter is engaged for 25% of its diameter, and the red portion at the corner represents the extra portion of the cutter that is engaged for a pocket radius equal to the radius of the cutter.

It is common for the machine programmer to slow down the tool in the corners to prevent tool wear and maintain surface finish requirements. So, it’s critical to create corners that don’t stress the tools more than necessary.2

The larger the better, but a good rule of thumb is to size the radius to 130% of the radius of the cutter or more. The red portion of the image on the far right shows the additional cutter engagement at a corner sized to the radius of the cutter, while the other image shows how much less engagement is required by sizing the corner to 130% of the cutter radius.

3An additional step you can take to reduce tool wear during CNC milling is to remove corners completely, in a manner of speaking. The deeper your pocket (or the thicker your material, if cutting the profile of the part), and the tighter your corner radius has to be, the harder it will be to machine. However, it often doesn’t matter what the corner looks like. You just need it to be clear of material. In this case you can use a large-radius relief, as shown in the image to the left, to achieve the necessary material removal without requiring a tiny cutter.

Considerations for Multiple Setups of CNC milling

Often a part will need to be milled from multiple angles. While this can sometimes be handled by 4- or 5-axis milling, on a typical 3-axis machine multiple setups will be required. Each setup costs additional time and money, especially when the volume of parts to be machined isn’t very high. If possible, reducing the number of setups required to make a part is an excellent way to save time and money.4

Take a look at the example on the right. In the image immediately to the right, the sharp internal corner of the cut-out dictates that it will have to be milled with the right side up in a separate setup. By adding a generous radius, as shown on the far right, the cut-out can now be machined from the top, with the hole and cut-out being completed in a single setup.

When multiple CNC milling setups are required, be aware that re-orienting the part in the machine creates more possibilities for positional errors. Maintaining a tight tolerance between features produced in a single setup is far easier than keeping the same tolerance between multiple setups. Where function isn’t affected, try to design your part so tight-tolerance features are created in a single setup.

On a related note, it’s a good idea to limit the number of tools that will be required to make your part. For example, many holes of various sizes may be best accomplished through the use of many different drill bits. Each one of those bits will have to be loaded into the machine and their length measured, which adds setup cost. During machining, there will be some added time every time a tool is changed. Too many different tools, and the machinist may even run out of positions on their tool changer! If the designer can use a few common sizes for all holes, it will help reduce setup and run time.

Blind vs Thru Holes

All else being equal, thru holes are typically easier to machine than blind holes. This is because the machinist doesn’t have to worry about holding a depth dimension, and because the chips can be pushed out ahead of the tool instead of having to be evacuated out of the top of the hole or collecting in the bottom.

The key here is all else being equal. If you want to make a machinist go crazy, specify a 1/8” hole through a 4 inch plate because you think thru is easy. At some point, the difficulty of drilling a deep hole far exceeds the benefits of making it thru. I’ve found a good rule of thumb is that if the material is 5 times or less the diameter of your hole, make it thru regardless of the depth required (so long as your design does not require blind holes for some other reason, of course). More than 5 times thickness to diameter, consider making shallow holes blind.

Overall Dimensions

5CNC Milling is a subtractive process so you need enough initial stock to cut your part. It is good practice to make your part out of readily-available material stock sizes. But, be cautious. Plate stock, for example, is often produced with tightly controlled tolerances and good finish surface finish for the thickness, but less so on the length and width. Your machinist will often want to touch up all of the edges, so designing for a size slightly smaller than a standard stock size will make it easier for him. The same applies if you ask for specific geometric conditions (such as flatness or parallelism), or tight tolerances anywhere. Your machinist will probably take material off to make hitting these requirements easier, and that should be taken into account.

Another element to think about is the possibility of nesting your parts, as shown in the image on the left. Remember to aim for a stock size that leaves enough room to get a fair size cutter in between your parts. This technique can save on both material usage and setup time.

Tool Spacing Considerations with CNC milling

Remember to take into account the tools that will be used to make your part. For example, if you must create an undercut, you have to leave room for the tool to be fed in. As the tool is round, the added clearance required to allow the tool to be lowered into position is doubled for every increase in radial depth of the undercut. This is because the full diameter of the cutter must be accounted for, while the depth is determined by the tool’s radius.6

In the picture on the right, you can see the effect on necessary clearance of having to use the larger red cutter to create the larger undercut shown in the lower image.

In a similar vein, taps to create threaded holes generally have some tapered lead-in threads before the full threads of the tap engage. The pilot hole needs to be sufficiently deep to allow the lead-in threads to move past the fully-threaded depth, with a deeper pilot allowing more leeway for lead-in threads.

Metrology

If you are going to specify a tolerance, it has to be able to be measured, and not all measurements are created equal. When specifying tolerances, specify only what you need, taking into account the difficulty of measuring a given tolerance. For example, the exact depth of full threads in a threaded hole is not something that’s easy to verify to a high level of accuracy, and is not normally a critical dimension. Similarly, concentricity is a notoriously hard geometric constraint to measure, while runout, which is simpler to measure, will often do.

Close-up check measurement of detail by precision detecting head sensor probe

Close-up check measurement of detail by precision detecting head sensor probe

Obviously, the above merely scratches the surface of the various considerations for the ideal design. I hope this short primer will help you make better designs, and lead you to investigate the process even further. Cheers, and happy CNC milling!

2 Responses to Design guide for CNC Milling

  1. dynosor says:

    To prevent tool chatter when milling pockets with a light manual mill, or when using slim center-cutting endmills, I start by plunging holes at all of the corners; using coordinates that leave perhaps .01 to .015″ of material for finishing cuts.

    Not only does this speed material removal at these critical points, having the full depth holes serves as a visual references to help “join the dots”. This makes it much easier than watching the DRO continuously with an eagle eye.

    Several light finishing cuts are made, running along the wall of the pocket, “climb milling” for best surface finish.

    Obviously, the benefits of plunging corner holes are not relevant when using a heavy CNC mill; especially when running large diameter, non-center cutting endmills. Then again, the beauty of a decent CNC mill is that you can optimize the toolpath and speed; and make full use of an automatic tool changer.

  2. dbyram says:

    Such recommendations is exactly why future designers that will be involved in parts requiring machining should be required to take some machining classes. Nothing is worst than a manufacturing vendor coming back to tell you they cannot make the part as designed. Designers need to understand what happens in the machining process and how it affects the cost of making the part. Very few educational institutions consider this important but the companies you may want to work for would consider a plus to hire. If you want a part that cannot be manufactured by standard machining methods, go 3D printed.

Leave a Reply

CLOSE
CLOSE
Skip to toolbar