Whats the best way of accurately milling circular parts? Could I also do them on a CNC and how?
Any videos/demos would be awesome if you know of them.
Thanks!
You really can’t on a manual mill unless you have a rotary table (some people will put a lathe tool in the vise and the work in the spindle, but realistically you’re not making round parts on a manual mill without rotary table). That is a huge PITA though.
It’s trivial on a cnc. depending on what the part looks like you can do as much contouring as possible in the first op then flip it and hold the round portion in a 3 jaw chuck bolted to the table/clamped in a vise, 5c collet fixture, soft jaws, etc.
If it’s a thin part with through holes you can also bolt it to a sacrificial plate and contour the outside to be round.
I have a rotary table to do round stuff and it’s a process to set up, indicate, and work with stuff. Not too bad if you’re used to it but for new mill users it’s a challenge to get things perfect.
I’ve also done reverse-boring to turn stuff with a boring head but that’s really if you’re desperate and/or bored.
If it’s a CNC router, drill any holes first, screw down with woodscrews to the bed, and then contour the outside. Pretty easy. For a CNC mill the process is much the same, but you can use tabs to hold the part until you cut it out, or just fixture it from the center with screws or a chuck. It really depends on what you’re doing; I’ve considered making a versapattern fixture for doing all the various versaframe parts.
Thanks for all the suggestions!
On a slightly unrelated note, what kind of tools would we need to fab something like this:
Currently have access to mill, lathe, and CNC router.
I’d get a block, stick it in a vise, and use the CNC router to mill out everything except the bottom 1/8" of the block (which is being held in the vise). Then take it over to the mill and face off the bottom 1/8". You’ll need to do 2 toolchanges to drill those holes, unless you spot drill them or drill them undersized before finishing on a drill press.
The lower holes appear to be blind holes, so you might have to just flip it over on the router and do them on the backside. If the angle of them isn’t important relative to the other hole pattern, you can face off the back 1/8" on the mill like I said earlier before just drilling them on the mill, to avoid precision setups on the router. You would need to indicate the center though.
If you’re making several of these it would help to just make a fixture on the CNC router to let it do the whole thing in 2 operations.
Apple pi made essentially 16 of these for our swerve modules this year. In the offseason, we started by cutting the piece to the correct shape out of an aluminum tube on the lathe, then we used a rotary table on a Bridgeport to drill the smaller holes. What we ended up doing during build season was make them out of a block of aluminum that we cut on a circular saw then faced on a Bridgeport. Then that piece went in a Haas mini mill where all of the cuts were made and then was cleaned up on a lathe.
With what you have I would recommend either doing the lathe then rotary table option or do all the main cuts on the lathe and then use the cnc router to do the smaller holes.
If it is possible for the cnc to make the whole thing, then I would start with a block of aluminum cut to the right height and then just put that in vice in the mill. You can leave the bottom part a square, but do virtually every other cut/hole, and then put it in the lathe and make the bottom circular.
I have made a lot of #25 and #35 chain sprockets on CNC routers. You need to have a flat sacrifice table that is a known depth so you can machine the web thickness down correctly.
On a manual mill, you can use a dividing head and a gear cutting blade to cut gears accurately. essentially mimicking a gear hobber, which is how most gears are made in production anyway. The difficulty of machining gears is the tight inside corner, with a CNC cutter it requires coming in with a tiny endmill. Laser or waterjet would be recommended over a router.
a 12 sided ratchet can be done easily with a collet block.
sprockets are probably best on a CNC.
and yes, rotary tables are a PITA to work with. after trying to set one up several times, its just not worth using. work holding and accurately locating center is difficult.
I would suggest using a lathe to produce the round OD and ID features first, it’s really the most appropriate tool for the job. Decent Carbide Insert tooling and a boring bar would make quick work of this.
With a Milling Machine equipped with a DRO; you could locate and drill/tap these holes without a rotary table. You would need to locate the center accuratily with a test indicator. Most DROs once centered, have very accurate Bolt Hole Circles funtions.
Flip the part over, relocate center, and drill/tap the lower hole pattern.
This isn’t exactly speaking to your question, but I thought it’d still help to share. NYC CNC’s has been a great channel to help me learn CNC without a dedicated machinist on hand. Here’s a linkto a little project of theirs in which they machine a Tie Fighter. It’s a decently similar setup to your question as the main body’s a cylindrical piece.
hey adam,
Do you find any videos/demos to use CNC?
I have routertable, And I think only CNC videos will help me.