Deep pockets with tight radius corners are a real headache. Imagine a 2″ deep pocket that needs 1/8″ radius corners. The biggest endmill that can get in the is 1/4″. But with a 2″ deep pocket, you’re facing an endmill with an 8:1 length to diameter ratio. It’s going to want to deflect like crazy, so you’ll have to go super slow to get it done. Plus, a smaller cutter is going to have to go slow everywhere else in the pocket. The bigger the pocket, the longer this will all take.
Consider how fast a 1/4″ endmill has to go (using our G-Wizard software to find Feeds and Speeds) to get it done in 2 passes:
We wind up having to use a tiny 0.0863″ stepover to get the Deflection just barely (99%) within limits. MRR on this cut is only 0.8987 cubic inches per minute. That’s slow going!
What if we could use a 1/2″ endmill instead?
We can use full slotting if we want to for a whopping 17.244 cubic inches per minute and the deflection is no sweat. That’s before we even optimize the cut to use an HSM toolpath like adaptive clearing or volumill to get even more.
Think of it, our MRR is about 19x faster. Now we’re talking!
Just one little problem. We can’t cut those 1/8″ radius corners with that endmill. What to do, what to do?
First thing is to ask the customer or whoever designed the part if they really need 1/8″ radius corners? Would a larger radius do? Because the part is a lot cheaper if it would.
But, assuming you must deliver those corners, it’s time to have a look at a technique called “Corner Drilling”.
Here’s a diagram to help you visualize the idea behind Corner Drilling:
You can see the small, finishing endmill sitting right in the corner of the pocket. A larger (2x the diameter) roughing endmill is sitting as close as it can get to the corner. And the short line segment marked “Stepover” is the amount of finishing allowance we want to leave for the small endmill.
The operation is going to work like this:
- Use a twist drill the diameter of the Finish Endmill (or the corner radius times 2) to drill a hole in the corner. Don’t put the edge of the hole right on the pocket wall because you’ll never it it to line up exactly right and look right. Rather, inset it diagonally away from the edge by and amount equal to the Stepover. We do this before roughing out the pocket so we’re not drilling a partial hole, which can lead to problems. BTW, if the pocket is deeper than 5x the drill’s diameter, you’ll need to do some Peck Drilling.
- Now rough out the pocket with the larger roughing endmill.
- Finish using the smaller endmill that fits the corner and a finish allowance equal to the stepover.
For this ratio of cutter sizes (e.g. Rouger is 2x the Finisher), the Stepover is 0.0884 times the Finish Endmill’s Diameter. That’d be 0.0221″ for our example, which is less than our Deflection-limited Cut Width of above, so we’re in fine shape.
You’ll need a toolpath that does “corner peeling” to finish the corners because the material to be removed there is more than the Stepover, but most HSM paths will do a fine job with that. They often don’t leave the best finish, so you might do 2 operations:
- Run Adaptive Clearing to get the whole finish outline to within the stepover allowance.
- Do a final finish pass with that Stepover from the perimeter of the pocket.
See how much faster that’ll let you manage that nasty deep pocket?
Like what you read on CNCCookbook?
Join 100,000+ CNC'ers! Get our latest blog posts delivered straight to your email inbox once a week for free. Plus, we’ll give you access to some great CNC reference materials including:
- Our Big List of over 200 CNC Tips and Techniques
- Our Free GCode Programming Basics Course
- And more!
Just enter your name and email address below:
100% Privacy: We will never Spam you!
Bob is responsible for the development and implementation of the popular G-Wizard CNC Software. Bob is also the founder of CNCCookbook, the largest CNC-related blog on the Internet.
I am currently a novice in this arena and look forward to these posts!
Thanks so much for this and please keep up the great work!
The corner bottoms are going to have a substantial amount of material left on from the twist drill point.
Tim, yes, the corner drill is inset away from the corner on purpose. The reason is that it will be noticeable on the wall if the drill doesn’t precisely cut and match the end mill’s path. You are still going to have to run that small end mill to take out the little triangular pieces where the big end mill didn’t reach.
Given that you have to run the small end mill and it is hard to get the walls to match perfectly with two completely different cutters, we chose to just use the twist drill to make the small end mill’s job easier, and let the small end mill do the finishing pass so all matches up.
I was referring to the corner bottom not the sides. The stepover is going to be considerably more as you get towards the bottom than the diagram above indicates. So be careful!
Tim, it’ll work out okay even though we have a non-flat bottom. In fact, the non-flat bottom is gravy because the deflection calculation assumes full material all the way to the bottom and the twist drill tip clears a bit of that away.
You can plunge the endmill into the hole to take out the drill point and leave a flat bottom before you run the rougher.
I use a similar method by drilling the corners undersize and then helical boring with an endmill, in this case, a 3/16. Now the corner is “finished” and when you finish the walls there will be no increase in tool engagement when it comes to the corner. Give it a shot, if you can use an endmill small enough to make even a small arc in the corner, it reduces deflection and chatter in the corner.
Also if your doing mold work, with lots of 3d shapes, slots and pockets, try using drafted endmills if the walls are tapered. The vibration reduction will be huge. slim shrink fit tool holders also do an amazing job when entering into the deep pocket arena.