Are You Using the Wrong Drill Geometry? Burrs, Crooked Holes, Broken Drills

Drilling a hole might seem simple, but the wrong tool choice can lead to poor quality holes, shortened tool life, and even costly scrap. The geometry of your drill can make or break the results. Get it right, and you’ll achieve a clean, straight hole with a great surface finish. In a previous Tips and Chips episode, we compared indexable insert drills, tip drills, and solid carbide drills. But in this episode, we’re zooming in on your solid carbide options, standard, straight flute, and even flat bottom drills. I’ll break it down where each should be used and show you how to improve chip control, get cleaner holes, and extend tool life. All hopefully without unexpected headaches.

So, before we dive into when to pick a standard straight flute or flat bottom drill, let’s first take a closer look at why drill geometry matters so much. Here’s the thing. Drill geometry is more than just an angled tip and a helix. It’s the chisel edge, the web thickness, the number of margins and their thickness, and also the coating all working together to create a chip. Break a chip and get it out of the hole, all while controlling the heat. High performance drills can work well across many ferrous materials, but when drilling through alloys such as Inconel and titanium, abrasive materials like cast iron, or softer gummy materials like aluminum, specialized drill geometries are designed to handle those challenges effectively. Choosing geometry matched to the material gives you a big advantage when working with tool life, performance, and reducing chipping, chatter, and wandering of holes, as well as overheating. When choosing the right geometry drill for this application, consider these three things. The material, is it hard? Is it soft? Is it gummy or heat resistant? The hole itself, is it a through hole? Is it a blind hole or on an angled or rain surface breaking through into another hole? The next process is the hole finished with the drill or does it need further machining such as reaming? Does it need tapping or counterboring?

Now that we’ve covered why geometry is critical, let’s start with the baseline. Standard twist drills. the everyday workhorses of drilling. But like any tool, they do have limitations. Standard twist drills usually come with tip angles of 118 or 135 to 145°. These are most common because they self-center well, run faster, clear chips easily, and can drill holes in a wide range of materials all day. But what if you want to create an angled hole or drill on a cast surface or into a radius? or you need a cross hole or a flat bottom hole, a counterbore or open up an existing hole. Running an angled tip drill here is going to cause you problems with wandering, skipping, and poor hole quality along with premature wear and damage. This is where a flat bottom drill comes in. Flat bottom drills do what a regular drill can’t handle. They handle these tricky applications because of the end geometry of the tool. Instead of an angled tip, they’ve got a flat surface that bites in the material and starts cutting the instant it connects. where an angle tip drill would slip causing out of round holes or if feeding aggressively snap the drill. So, what are a few real world examples of when to use a flat bottom drill in aerospace? You may need to open up an existing set of flange holes from an earlier operation. Using a flat bottom drill instead of an endmill here will make holes far quicker. In the mold and die industry, you may need to drill into a curved surface or use a flat bottom drill to drill a hole for location pins. In the power generation or automotive industry, you may need to have intersecting holes that require a high level of accuracy. A flat bottom drill will cleanly break through into an existing hole without damaging the corners of the tool or creating difficult to remove burrs from the part.

Let’s talk about other specialty tools that often get overlooked. Straight fluted drills. Most of the time, we default to a helix flute drill because they are effective at evacuating chips, reducing thrust, making high-speed drilling easier. But there are real situations where straight flutes can offer advantages, especially in high hardened materials or very soft gummy materials and thin-walled parts. Straight flute drills excel when you’re drilling into abrasive materials like cast iron, glass filled composites or materials with high elements such as silica or molybdenum. You need to minimize tool deflection, especially in short hole drilling. you’re working with thin-walled components where a twist drill might lift the part or distort the hole or when drilling materials with a high hardness above 55 rockwell. Because there’s no helix, straight flute drills are very tough, lending themselves to machining hard, brittle materials very well, reducing the risk of cracking or chipping the material during drilling. And for burr control, straight flute drills can create cleaner entry and exit holes in some applications. They shear material more like an endmill, which reduces the outward push that causes burrs on the holes edge. The main tradeoff? Well, chip evacuation isn’t as efficient as it is with a twist drill. So, stick to shallow holes and use them in materials that easily like to chip. Unlike twist drills, you’ve not got that helix to help carry the chips out of the hole. So, you need to rely on forming small chips that can be easily evacuated during cutting or by coolant or air at the end of the cycle. So, while it’s not your everyday drill, when a hole quality matters more than the speed, a straight flute drill might be your best move.

Let’s take a moment to talk about how different drills perform in the same material using titanium 6Al-4V as an example. For this heat resistant alloy, a good starting point with a standard two flute coolant through drill with a single margin design would be around 168 surface feet and 0.007 inch per revolution, which works out to about 9 in per minute on a 1/2-inch diameter drill. The single margin design helps reduce friction and heat buildup, and the coolant through design is critical for flushing out chips and keeping the cutting edge alive in this material. Now, if you switch to a flat bottom drill in that same material, you’ll see a much higher cutting force. To manage this, you typically need to reduce your parameters closer to around 128 surface feet per minute and around 0.005 inch per revolution or equaling about 5 in per minute. That’s nearly a 45% reduction compared to a standard twist drill, but it prevents chatter, protects the corners, and gives you the accuracy needed for the applications like intersecting holes. The key is understanding that geometry drives performance. Single margins and through coolant help with stability and heat in titanium, while flat bottom geometry requires more conservative speed and feeds to avoid overloading the drill. I’m not saying you cannot run in excess of these parameters, but I just wanted to take a second to highlight the starting differences of different tools in the same material. As always, dial your parameters to suit your application.

Of course, parameters are only half the story. how you actually set up the drill and approach the cut can make as much difference in tool life and hole quality. Generally speaking, it’s best to avoid pilot holes or pecking cycles when possible. Though, of course, there are times when this is necessary. The goal should be to get the drill into the material, make the hole, and get the drill back out as quickly and as cleanly as possible. Every time a drill engages and re-engages the part, it wears faster. You’re loading up the drill torsionally, then unloading it each time it stops cutting, only to load it up again during re-entry. That repeated cycle accelerates tool wear and can shorten tool life significantly. If you do find you do need to peck, try to stagger the steps, progressively reducing the depth of cut. So, for example, if you’re making an 8×D hole, try doing it in a 4×D, 2×D, and then two one times D cuts. This way, you’re taking out half the material out before it gets difficult to evacuate chips. Then progressively reducing the amount of chips generated, giving them more time to evacuate. One more tip, avoid pulling the drill out completely during the pecking if you can. In deep holes with long reach drills, the drill can start to whip or wobble, especially at higher RPM. Taking the drill in and out of the hole increases the risk of damaging both the cutting edges of the drill and the whole surface. A useful exception here is with flat bottom drills. If the hole is pre-drilled, you can often increase your cutting parameters significantly without adding wear since the center of the drill isn’t being forced to do the heavy work it normally would. Finally, think about setup. Just like with endmills, keep the stick out as minimal as possible and use a rigid high quality holder to minimize runout. Ideally, keep the run out under 0.001 inch. Otherwise, you risk concentricity issues. And remember, drills today are available in diameters from nearly an inch down to just a few thousandths. And for perspective, a human hair is about 0.004 inch thick. And there are drills far smaller than that.

Even with the right setup, the biggest factor in drill performance is what happens inside the hole. How the chips and the coolant and the heat are managed. More often than not, a drill will fail due to one of several issues. Poor chip evacuation can cause the chips to jam and break the drill. Poor coolant delivery or excessive speed can cause the drill to overheat, breaking down the coating and then the carbide substrate. Incorrect feed rates will cause built-up edge, specifically in softer materials like aluminum or copper, which will increase the load on the drills causing them to fail. A lot of modern drill lines offer through coolant capability, delivering coolant right to the cutting edge. This helps control the temperature, provides lubrication, and improves chip evacuation. In practice, you’ll usually find through coolant drills are available in lengths starting at around three times D and extending out to 12×D or more once you’re above an eighth of an inch in diameter. And don’t forget through coolant technology is also available in very small diameters, sometimes down to around 1 mil or 0.040 inch, making it practical for both deep holes and fine feature work. If you’re having issues with exit burrs, try adjusting the feed rate for that last one times D of the cut. Halving the feed rate will reduce the thrust on the drill and reduce the possibility of the drill pushing its way out the hole rather than cutting. This generally eliminates exit burrs. If you start seeing exit burrs after the drill has been running for a while, you’ll likely come to the end of the drill’s life. As always, don’t forget about coatings. The coating you choose should be matched to the material you’re cutting and the problems you’re trying to solve. For aluminum, either run uncoated or use a low friction coating like TiB2 based options. These coatings are thin, hard, and slick, which helps control built-up edge by keeping the tool sharp and effective at shearing material. If you’re cutting materials like titanium, steels, or other heat resistant super alloys, go with a heat and wear resistant coating such as TiAlN or AlTiN variant. These boost wear resistance, help fight flank wear and tip damage, and also protect the cutting edge when the heat builds up. The bottom line, pairing the right drill geometry with the right coating not only extends tool life, but it also improves the performance and reduces costs overall in the long run.

Let’s start wrapping this up with a few final takeaways. Standard drills are great for straight through holes, deeper holes, and simple setups. Flat bottom drills are great for angled faces, radiuses, cross holes, clean cuts, and counter. That’s where they shine. Match your drill for the material. Don’t forget to focus on your feeds, speeds, holder, and stickout. You’ll save tools and time. Thanks for joining us today on Tips and Chips. If you found this video helpful, please like, subscribe, and hit that notification bell. Got any questions or tips you’d like to share? Leave a comment below as we’d love to hear from you. If you need any help, please visit the links in the description for more resources. And as always, keep those chips flying.