Thin walled parts are a real pain because the thin walls want to vibrate like a tuning fork. When that happens, you’ve got trouble, big trouble, and its name is chatter. I was reading a fascinating article recently that made the point that when milling thin walls, climb milling is a must. Because climb milling cuts with the part instead of against the part, it transfers less energy to the part and is therefore less likely to make that thin wall vibrate.
Using cutters with more flutes is also helpful. Depending on the engagement angle of the cutter, the more flutes, the more that are engaged on the part, which helps stabilize it. With a 2 flute cutter, there is only ever one flute engaged, which is the worst case of beating the material until it vibrates. Higher helix tools help too, because they pull up on the part, which keeps it in tension and reduces its tendency to chatter.
If you’re working on a material that doesn’t dissipate heat well, like titanium, thin walls are a problem because the heat builds up more. You’ll need to focus on better cooling, and either lower the spindle speed or reduce the cutter engagement to keep the heat down.
If you reach very far down into your thin wall cavity, you’ll need to look at tapered shanks or even tapered tools. Even though you’re only cutting at the tip, having that thin wall rubbing on the spinning shank still injects vibration and chatter into the job.
Tool deflection is a big deal with thin walled jobs. Be sure to keep it to a minimum. G-Wizard’s Cut Optimizer will tell you how much you can cut for a given tool deflection allowance.
Here is another tip: make sure your tool’s radius is less than the minimum internal radius needed for the part. This insures the tool is always moving. If the tool radius is the same, it will come to a stop in the radius of the part and that starts the chattering again. Keeping the tool radius a little smaller than the minimum part radius is a good idea in general, not just for thin walled parts. It will lead to a better surface finish.
A challenge is designers who are unaware of the relationship between cutter radius and the radii in their designs. They make the radii of their parts in round numbers because that’s the typical way people think. So, for example, the smallest radius may be 1/4″. But cutters are sold in round number sizes too, so you’ve probably got a 1/4″ cutter on hand and your next size down may be 3/16″. There are two good possibilities to make life easier:
– Get your designers to make their internal radii just slightly larger than your standard cutter sizes. That’s the best answer if it doesn’t matter to the design, and its very easy to do.
– Lay in some cutters as close to the standard sizes as possible but just smaller. For example, MariTool lists a 15/64″ endmill right below the 1/4″. It’s more expensive, unfortunately, because they aren’t called for as often. Or you could drop down further to 7/32″ and save a little more money.
There is a trade-off in tool rigidity that creeps up pretty fast, so don’t downsize the endmill too much. For example, G-Wizard’s Rigidity Calculator tells us the following:
If a 1/4″ endmill is a factor of 1 in rigidity, the 15/64 is only about 76% as rigid, and the 7/32″ is 59% as rigid. If we fall all the way back to 3/16″, our endmill is now only 32% as rigid, which is really going to slow down our production.
Now you know what those odd-sized endmills are good for!
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!