Beginners questions for resources

[xHemi]

Hi, this is my first post so I’ll give some background quick, my name is Andy I’m 28, I work in a production cnc lathe shop in New York. I mainly repair the lathes and am more of a mechanic than machinist really. I have a 2 year mechanical tech degree that was machining oriented, but focused more on manual machines.
I have a good handle on Solidworks and just recently started teaching myself Gibbscam with online resources. I have been playing around with some easy aluminum programs using mainly volumill style tool paths and have been getting good finishes and have been having fun with it.

My buddy is building a wood processor and asked me to put a 4 inch hole into a 3 inch thick mild steel plate, of course I said no problem.

My main problem and the reason I’m posting this is because I have been milling aluminum with nice rigid 1/2 solid carbide coated endmills and felt I could do no wrong. Now I am attempting to mill this massive hole with a tool that I’m not sure can do it. The only endmill long enough we had was a 3/4 inch hss endmill with flutes just over 3.1inches. My plan was to drill out a starting hole in small depths and then mill out close to 4 inches and then repeat until through, then clean it up with a small cut at the end. I did this on a small test plate and the drilling went went ok but the endmill started chattering badly instantly so I stopped it. Was running around 2500 rpm and 20 ipm feed.
This is starting to feel like I’m writing an essay so I’ll just put some pictures in and finally ask a question.

What book would you recommend to me for learning to find feeds/speeds for modern machining?
And also any advice on my approach to cutting this specific plate would be appreciated. I don’t have the ideal tools/work holding for something this large and I know I’m beyond my skill set currently but I want to learn. There is no rush to have this done quickly, it’s just an after hour job i wanted to try.
Machine is a Fadal vmc 15-xt

 

[EmGo]

Just to stick in your head ? In steel for hss use 100 fpm, for carbide use 400 fpm. That's just a general general general rule, in about five seconds someone will be along "no, this new coating ..." but those are safe numbers, they work, as a starting place and a generalized, overall rule you can live with that.

And two flutes for aluminum, four flutes for steel. Gong to get backlash on that too but hey, there's fifty year old rules of thumb for a reason

Doing that in a mill I'd have probably skipped the drill and done a helical roundy roundy roundy path then a finish pass instead of trying to take it all out but that's personal preference.

Maybe your cam has high speed options, where you go a lot faster taking tiny cuts but not sure that's a good place to start ? Basics first ? Probably get argument there too. We argue a lot here

 

[xHemi]

Just to stick in your head ? In steel for hss use 100 fpm, for carbide use 400 fpm. That's just a general general general rule, in about five seconds someone will be along "no, this new coating ..." but those are safe numbers, they work, as a starting place and a generalized, overall rule you can live with that.

And two flutes for aluminum, four flutes for steel. Gong to get backlash on that too but hey, there's fifty year old rules of thumb for a reason

Doing that in a mill I'd have probably skipped the drill and done a helical roundy roundy roundy path then a finish pass instead of trying to take it all out but that's personal preference.

I was hoping to avoid this but I already tried the helical boy on the last .75 endmill we had so now I really am on the last endmill. Not sure what feeds/speeds I was running on this but I was going extremely slow, possibly too slow?

 

[guythatbrews]

Just to stick in your head ? In steel for hss use 100 fpm,

EmGo is correct. For a 3/4 em that's 509 rpm so you were wildly too fast! At 20 ipm the chipload/tooth was .002 so that was reasonable.

Since you've got a hole through on one piece I'd be inclined to run 80 sfm and .002-.003"/tooth. Drop all the way through and spiral out at a small radial doc, maybe .050. Climb cut and be sure the chips can fall free. There will be tons of em. Slow but steady wins this race.

 

[Stoney83]

Gibbscam technology expert is pretty good. When you open the volumill dialogue box it’s on the top left. Click that and It’ll recommend feeds and speeds based on what you tell it.

Gibbs will factor radial chip thinning so chances are it’ll recommend slightly more aggressive cuts than the 500 rpm and 20 ipm…. But it should be in that ballpark and there’s even a setting for how aggressive/conservative you want to machine. It’s a nice software tool that will usually get you close. You can play around with it and get an idea how different tools and even machines are likely to preform.

Volumill will also take into account what you’ve already machined in a couple ways. In your case if you drill a threw hole you can toggle the geometry to “air”… with a right click. The outer hole needs to be a teal color and the inner hole red. For a cleaner path there’s some spiral generators under the plugins.

 

[BajaFire]

As far as a book for referencing the speeds-n-feeds stuff, the Machining Data Handbook put out by the Machinability Data Center gives pretty good numbers for working on various materials. They'll get you in the right ballpark, and you can adjust from there to suit your setup. I think the Machinery's Handbook has numbers too, but I've never tried them to know how realistic they are.

 

[Jatrox]

As far as resources, FS Wizard is a good place to find feeds and speeds to get a starting point. Machinery's Handbook can help with the technical side. Something to keep in mind is when machining an inside pocket the tooth engagement is greater in a radius than a straight cut. Backing off on the feed helps

 

[jaguar36]

As far as resources, FS Wizard is a good place to find feeds and speeds to get a starting point. Machinery's Handbook can help with the technical side. Something to keep in mind is when machining an inside pocket the tooth engagement is greater in a radius than a straight cut. Backing off on the feed helps

Beat me too it, FS Wizard is a great app and has always worked well for me.

In this case it gives 561 RPM and 9.5 ipm feed, which lines up with what other folks have said. Depending on which machine I'm using I will sometimes back off its recomendation by a bit as well.

 

[Mtndew]

a helical roundy roundy roundy path

A triple roundy path? Good god man this kid is new!

 

[EmGo]

A triple roundy path? Good god man this kid is new!

Okay okay, he could do one floor at a time then

Just outta curtiosity, that year fadal can do helical, I'd assume ? Should be pretty easy to tell it how many revolutions to make ?

Actually, I'm not sure on the K&T that I wouldn't just drill the hole a little off the inside profile, drop the mill all the way through, go around once to drop the block out and once to finish. Been watching too many of these nibble nibble videos maybe.

 

[Fadriver]

Hi, this is my first post so I’ll give some background quick, my name is Andy I’m 28, I work in a production cnc lathe shop in New York. I mainly repair the lathes and am more of a mechanic than machinist really. I have a 2 year mechanical tech degree that was machining oriented, but focused more on manual machines.
I have a good handle on Solidworks and just recently started teaching myself Gibbscam with online resources. I have been playing around with some easy aluminum programs using mainly volumill style tool paths and have been getting good finishes and have been having fun with it.

My buddy is building a wood processor and asked me to put a 4 inch hole into a 3 inch thick mild steel plate, of course I said no problem.

My main problem and the reason I’m posting this is because I have been milling aluminum with nice rigid 1/2 solid carbide coated endmills and felt I could do no wrong. Now I am attempting to mill this massive hole with a tool that I’m not sure can do it. The only endmill long enough we had was a 3/4 inch hss endmill with flutes just over 3.1inches. My plan was to drill out a starting hole in small depths and then mill out close to 4 inches and then repeat until through, then clean it up with a small cut at the end. I did this on a small test plate and the drilling went went ok but the endmill started chattering badly instantly so I stopped it. Was running around 2500 rpm and 20 ipm feed.
This is starting to feel like I’m writing an essay so I’ll just put some pictures in and finally ask a question.

What book would you recommend to me for learning to find feeds/speeds for modern machining?
And also any advice on my approach to cutting this specific plate would be appreciated. I don’t have the ideal tools/work holding for something this large and I know I’m beyond my skill set currently but I want to learn. There is no rush to have this done quickly, it’s just an after hour job i wanted to try.
Machine is a Fadal vmc 15-xt

If i were you, drilled bunch of holes around inner circle, next to each other, knock the puck
and finish fly cutting no expensive endmill.

 

[xHemi]

Thanks a lot guys for the advice I’ll order one of the books, might be a bit before I get back to the block but I’ll let you know how I make out

 

[Covenant MFG]

Tbh, if you want to be super duper safe, 125 surface feet and .0015" inch per tooth works with pretty much everything, with some exceptions when you need to be more aggresive, assuming you've got carbide. If it's a steel endmill, drop it to 75 SFM. It ended up being my go-to when I first started and was tired of things blowing up.

 

[dandrummerman21]

Is that a DA collet holder? Need to get that tool in a sidelock endmill holder.

Do not use a 3" long endmill to make 1/4" deep cuts. The thing is way too long.

Use shorter tools to rough it out. only use the long tool to finish the hole, and you'll want to use the whole length.


General rule, if you have chatter, slower rpm will help. If slower rpm doesn't help enough, you increase the feed.


If we are pretending that you needed to mill a 3" hole with that long tool you have, you want to bury the thing as deep in as you can go and take relatively light radial cuts. If you can bury the cutter the whole 3" deep, make small circles or spiral in at maybe .100" wide per cut.

Best way to really learn how to do it is to do it, and fail, a lot. Best place to fail without making terrible expensive scrap pieces would be to do simple things like milling the edges on a bridgeport. That'll give you manual "feel" that you can translate to cnc world.

 

[kenton]

What kind of machine are you using? With the 40 taper ProtoTrak I use at work I would drill 3/4 a pilot hole .03" from the edge and write a 2 axis program so I could plunge with the quill around the perimeter every .200" and then mill to clean up the scallops.

The "roundy mill path" idea would be good to on a more rigid machine. For one part, you might rough from both sides with a shorter and more rigid (and cheaper) tool and save your long endmill for the finish passes.

 

[Freedommachine]

Use shorter tools to rough it out. only use the long tool to finish the hole, and you'll want to use the whole length

^^^ this... do this. Unless you're running a great big, slow HBM or something. In which case you can either use a trepanning tool (sp?) Or drill a big hole and rough it out with something like a 1.5" diameter corn cob mill.

This would be a great application for a kennametal Harvi 1 TE end mill - if they weren't so darn expensive. You can really beat those things like they owe you money... because they do lol.