So many mills! Which do I need.

[aforww]

Another topic specific thread.

So, I'm perusing 1/4 and 1/8 end mills trying to decide what I want, need, and have zero use for. I've ultimately decided to go with the sets from inventables but I was wondering. What are the most commonly used cutters for you all and what type of milling are you doing? From what I gather double flute straight seem to be the most commonly used. Along with V cutters and ball mills. My intention is to do mostly inlay work and fine detail carving. It also seems the 1/8" cutters aren't really used all that often. What are y'alls opinions on cutters to start with?

[Derek the Admin]

Straight flute cutters are good for wood. I would imagine that two flute up cuts are probably more commonly sold than straight flute tools though. There is an entire science behind this. Straight flute cutters do not leave you with the tear out that a spiral fluted up cut will, but by their design they don't clear chips out of the cut as effectively either. Down cuts have some advantages too, but they pack chips down into the cut. The advantage is that the tear is forced down so there is less fuzz at the edge of the cut (unless you profile all the way through, in which case your fuzz is just all on the bottom side now).

V bits and ball nose bits are good to have around as well if you want to do anything more than cut flat bottom pockets and profiles. V bits come in different angles. A 30 degree V bit is more of a knife point type shape then a 90 degree. The 90 is going to be less forgiving to uneven stock being engraved because it works out that a 90 v bit at 1mm of depth is 2mm of width and so on. So if one side of your stock is .5mm higher than the other then that side of the engraving will be 1mm thicker. The 30 degree bit is more forgiving, but the engraving isn't as prominent for the same plunge.

I like 1/8 mills alright because they are usually a good bit cheaper. It will depend on what size collet your router has though. If you have a quarter inch collect you will either need a 1/8 collect or a collet adapter to run a 1/8 shank mill. You can get them in 1/4 shank with 1/8 cutting diameter, however. There is nothing wrong with this at all depending on what you want to do. Some people like to run bigger diameter tools because they can push the machine harder, but you really don't need to be pushing this like it is a big production machine. Bigger end mills clear more material at one time, but they also exert more force on machine for the same given feed rate and depth. This is a trade off between removal rate and acceptable deflection.

Also Google chipload, keeping in mind many of the recommendations on feed rate assume you have a big industrial machine.

I hope this was somewhat helpful.

[aforww]

Yea upcut, down cut, and compression cut I'm familiar with from lots of experience with routers in my woodworking. I'm just trying to bridge the gap between the system and my knowledge. Obviously routing with a router is a bit different by hand because it's as rigid as your grip or router table. I definitely need to learn chip load for various cutter designs because that's completely new territory for me. I also need to become more familiar with the types of cuts. Step up, down, ramping in etc. Thanks for the input.

[Derek the Admin]

No problem. It is certainly a learning process. On the note of ramping... if using an end mill you should ramp or helix in if you can. Even center cutting end mills are not that great at drilling. Deep plunging is a great way to A) Dull a bit, B) bog weaker routers tools, C) break end mills, D) worst cast scenario, start a fire. If you absolutely need a hole the size of your end mill you should try a few different things:

Preferably, split the work into another operation, change tools, and use a smaller end mill.

As an alternative, you can peck drill it. End mills still suck at drilling, but pecking allows you to plunge a bit, say 1mm, raise to clear chips, plunge to 2mm, raise to clear chips, plunge to 3mm, raise to clear chips, etc. It's still not really a great way to go about it but it definitely beats a straight plunge (Plunge steps just an example).

Another alternative if you are already running other ops with an end mill and you need a hole the size of that end mill or there about is to mark the desired drill points with the end mill just a tad, then come back and manually drill through the holes with an appropriate drill bit using a drill press or hand drill. I especially like this method for smaller holes in aluminum. Aluminum is too hard of a material to try to plunge through using an end mill (seriously, don't even try it). If I need a pattern of small diameter holes in aluminum I just let the machine mark them them finish them with a drill. If it's a reasonably sized hole (say 30% or so percent bigger than the cutting diameter of the end mill), then I'll just let the machine do a nice and easy helix down through it.

[aforww]

Ah ok so ramping in or taking the helical approach is just a means of introducing the tool to the workpiece in the gentlest means possible, it's something that should be done as routine procedure or is it something you do only when a gentle approach is required? For example, if I want to bill out my logo and it's only going to be an outline 3mm wide. Do I need to ramp down into the cut or just send it on its way? While we are on this topic, how does one direct the machine to make these various forms of approaches?

[Derek the Admin]

Aug 10, 2016 4:59:41 GMT aforww said:

Ah ok so ramping in or taking the helical approach is just a means of introducing the tool to the workpiece in the gentlest means possible, it's something that should be done as routine procedure or is it something you do only when a gentle approach is required? For example, if I want to bill out my logo and it's only going to be an outline 3mm wide. Do I need to ramp down into the cut or just send it on its way? While we are on this topic, how does one direct the machine to make these various forms of approaches?

These entries allow the tool to do such things as clear chips properly. Bob Warfield at CNC Cookbook gives a decent primer on this. A lot of his tutorials ties into selling his software (no shame in that), but you can get a decent idea of things from this:

blog.cnccookbook.com/2012/03/07/helical-interpolation-ramp-angle-and-the-best-ways-to-enter-a-cut/

I usually helix or ramp to depth. I might not take my own advice if I am in a hurry and I'm working in something soft like MDF. You specify this in your CAM settings, but not all CAM software is created equal. For instance, I don't think Inkscape G Code tools actually has a working ramp setting. A more serious CAM program like Autodesk Fusion 360 gives control over the type of entry, ramp angle, helix angle, etc. These can be found on the "linking" tab (the last tab) in the set up of an machining operation in the CAM side of Fusion 360.

Another good one to look into is lead in and lead out. This can help keep you from leaving artifacts of the entry on your piece.

[aforww]

Noted. I think I'm going to end up trying to get familiar with Fusion as opposed to MakerCam. At least for the time being. I'll still be playing with the others but I know when I do move up to a larger machine I'll be using aspire so mine as well get used to using more comprehensive programs now. I'll do some reading from the link you provided. Thanks.

[kb9jlo]

Aug 10, 2016 4:59:41 GMT aforww said:

Ah ok so ramping in or taking the helical approach is just a means of introducing the tool to the workpiece in the gentlest means possible, it's something that should be done as routine procedure or is it something you do only when a gentle approach is required? For example, if I want to bill out my logo and it's only going to be an outline 3mm wide. Do I need to ramp down into the cut or just send it on its way? While we are on this topic, how does one direct the machine to make these various forms of approaches?

If you're not going to do the ramp or helix then you really must do a lead in / lead out maneuver.

As I mentioned before our Autocad to gcode software was horrible so I created a standard 'block' for Autocad that I would just insert into the drawing to give me the tool path geometry for the lead in/out. Most of the time with this particular gcode translator, after finishing drawing my parts, I'd just draw tool path lines! Ha, ha. It was quicker then trying to each the software where the object's 'perimeter' was.