What Is The Best Way To Machine A Deep, Narrow Pocket In Titanium?
Boeing’s answer to a reader question emphasizes the use of high-feed milling tools.
Personnel from Boeing's Research & Technology group recently answered readers' questions. One reader asked the following. To see the list of experts taking questions from readers right now, see our Ask An Expert page.
I have a part to machine out of Ti 6Al-4V. This part has one pocket that is 4.5” deep and another that is 1.2” deep. The corner radius for the pockets is 0.25”, and the pockets measure 1-1/8” by 1-1/2”.
I was considering roughing out as much as possible with a 3/4” diameter end mill, then using sinker EDM to finish the pockets. Does that sound like a productive approach?
Response from Boeing’s Research & Technology group
Your pockets definitely pose some challenges with how narrow they are, and I'm worried that you are going to have issues trying to side-cut with a 3/4” end mill sticking out 4.5”.
An option to consider would be a high-feed mill. Iscar and Sandvik Coromant both make carbide screw-in button tools with high-feed mill geometries. High-feed mills are outstanding for small-diameter cutters that have a long stick-out. Their geometry puts the bulk of the cutting force in the Z direction, which helps to stabilize the cutter. These tools take small axial depths of cut, but they take big chip loads due to their chip-thinning affect. If you choose this option, I would program the pocket with the high feed mill doing a continuous ramp-down. Take note that during this continuous ramp-down you must not exceed the maximum axial depth of cut for the high-feed mill that you choose. But the smaller the pocket, the steeper the ramp can be.
The reason for the continuous ramp-down is that high-feed mills perform best when you are able to keep them engaged with the material. You do not want to nibble with these tools, so you want to maximize stepovers and minimize engages and disengages as best you can. Doing this actually increases tool life. Small radial cuts quickly beat this type of tool to death.
Parameters depend on which high-feed mill you go with, but we typically run these tools at around 150 sfm and 0.020” to 0.030” chip load. The chip load for your smaller-diameter tool will likely be around 0.020”.
We think you are onto something with the idea of using your sinker EDM to finish the pockets. We don't have enough experience with EDM to offer advice. However, your 0.25” corner radii are going to be tough to achieve with a 0.5” diameter cutter sticking out 4.5”. If you do end up milling these features, I would look at using the appropriate high-feed mill to plunge out the corners, because these tools do work well for plunging.
The more common twist drill point geometries often are not the best for the job at hand. By choosing the best point for the material being drilled, it is possible to achieve better tool life, hole geometry, precision, and productivity.
Economic efficiency is an important consideration when choosing tools for challenging metals.
With macros and canned cycles resident in the CNC on most contemporary turning centers, single point turning of OD threads can seem like almost a default process decision. However, for numerous applications, OD thread rolling has inherent advantages as an alternative to cutting threads.