Tips on Roughing , Please.

[lostkoss]

I work at a small tool shop.We have (1) Haas TM1 and and older Matsuura thats basically the same thing but beefier and well, older and running a Yasnac control.(4000rpm max both machines)

I have had pretty decent success with programming with Surfcam.

The issue I am coming across is that we cannot do Z plunge roughing. (we only have 2 axis on the surfcam.) I have been roughing using the standard tool information processes and pathing.My boss thinks, and I agree that the TM1 isn't tough enough for Z plunge roughing anyway.(Its probably not tough enough for our purposes anyway to begin with, but thats another story.)

It seems from what I've been reading that there are few different philosophies on roughing out material. IE ; Z plunge roughing, using roughing endmill's and just foregoing rougher's and just using standard endmill's.

And like I said using Z plunge is pretty much out.

So I've been dulling the bottom 1/8 of a lot of rougher's and snapping quite a few too over the last 2 years.I'm trying to establish a chart of speeds and feeds and my bosses would like me to speed things up, so just turning the feed override down isn't really the answer I'm looking for.

We generally cut 4140, O-1, A-2 and other misc tool steels.

I guess what I'm asking is ; Does anyone have any tips?

Or maybe just answer how do you do things at your shop.

I'm another "alone on an Island under a bus" guy here

Thanks in advance.

(Repost from Haas Forum, I though I might get more views here).

[-Chris-]

Hi, I'm not sure what process your doing such as pocketing or outside contureing But a good option for your machine and cam package would be to drill an entry hole in your pocket to the bottom to plunge a two fluted insert cutter like an Ingersol with .03 radius's on the inserts run it at 2500 rpm and at 20 inches a minute. Use lots of air no coolent with depth cuts about .1 deep. works good for me -Chris-

[little bubba]

We have one decent mill and couple of older floppier lower horse mills in the shop. First thing, don't skimp on your tools, even on a 2hp CNC'd knee mill, I run carbide variable flutes/helix endmills. More up front cost, but it pays itself back very quickly(usually about 10 minutes) in tool life and time saved.

On the burning up the bottom 1/8", think of ways to use the whole endmill, deep and narrow cuts. Several benefits, more life out of the tool since you are using the whole thing, and you have chip thinning on your side, so you can up your feeds and move a whole lot more metal for a given rpm and chip thickness. It also seems to help on floppier machines by twisting it up in one direction, seems to keep it from bouncing around too much.

On the plunge roughing, that is probably the direction in which your machine is the stiffest. Not that hard to hand code it. A quick little sub and you're off and running.

[LeeWay]

I haven't cut anything near that hard yet nor is my machine all that rigid, but I find that ramping down in pockets and profiles takes it easy on everything.
I don't usually take more than .025" DOC on softer steels. I run about 3000 RPM and feed about 20 IPM to 25 depending on how soft the material is.
This doesn't stress any parts of my machine or tools. I could likely take a little heavier cut, but then I start snapping tools.
I use cheap tooling for all my production stuff and only use good tools when I need nicer parts. All my production stuff gets powder coated, so nice looking parts aren't critical.

[lostkoss]

Thanks for the tips guys, I appreciate the input.

If I do not have time to respond to everyone individually.I still value your opinions and advice! Just trying to get some work done too !

I'm going to try and figure out how to post screenshots and such over this weekend and maybe I will have some more specific questions in the future.

Right now I'm just trying to help pull this shop out of the 70's and the information on these forums so far has been very useful !

Thanks again.

[ALLtra Mach]

Axial and radial chip thinning. Reduce radial D.O.C. by 75% and increase feed rate 200 - 300%.
For roughing a pocket, use a ball end mill with a thin axial cut. The ball end transfers the radial load axially where your machine is strongest and you can get a much higher material removal rate.
And good mills with geometry and coatings that match the material.

As far as your software not having z-axis. If it'll program a drill pattern, then you can use that as a plunging cycle.

[lostkoss]

Originally Posted by ALLtra Mach As far as your software not having z-axis. If it'll program a drill pattern, then you can use that as a plunging cycle.

You know...I never quite thought of it that way.

A very interesting set of thoughts just occurred when that light bulb went on just now.

Thanks for the tip !

[5axisguy]

Plunge milling with a drilling cycle is a no-no, sounds like it would work but your tool would only last a few plunges, the high end cam systems that strictly do plunge milling actually back the tool away from the material on the way up, all the plunging tools work only on the bottom, dragging it back up the wall will take the inserts out in a hurry. Plunge milling is more scientific than just dropping a tool down where it will fit. Also like mentioned earlier, you need a very robust machine, preferablly a horizontal for the chips to fall without a ton of air blast, we rough 4140PH. on our machines with either Diejet or Hitachi high feed mills, on our kuraki we run a 3.00 dia tool at .05 depth of cut at 175" per min, feed, it will run for hours roughing out moldbase pockets like that.

[ALLtra Mach]

Never thought of that.
Though I have run plunging off of drilling cycles, I don't get too carried away with it!
Out of curiosity, how do you start a plunging cycle on a closed feature?

[5axisguy]

Honestly I have never done it, I program with powermill by delcam, and they have a deticated plunge milling strategy, which works fine, but, they advised me against using it on our 5x machine, it's way way too whimpy for that, they infact went thru several spindles in their development stages writing the software, I can only assume you have to helix a hole with some other type of tool before plunging into a cavity, or drop into a drilled hole, the plunge milling is a very powerfull strategy and you have many options but I have not looked into it much. I only know the basic do's and dont's. That's why I mention not using the drilling option, they did, and they failed miserably. Perhaps in very isolated cases it would be fine. It's just one more thing to worry about because there is a significant ammount of flex when chopping down with those plungers. I actually "back in the day" did alot of plunge roughing on just a manual bridgeport with great success, like for enlongating holes or doing slots for example. Its a very efficient way to remove material, in some situations.

[DSL PWR]

On my TM-1 I run a 3/4" Mitsubishi AQX Mill drill. It runs at 3055 rpm, and 18"/min. I go .1(4140)-.15(1018) deep in steel. The TM-1 isn't stout enough to plunge this in (it will go, but it doesn't like it) so I do a helical entry. I bought an Ingersol hi feed mill and if you have the right job it works not too bad, but again it would be better in a stronger machine.

[lostkoss]

Hey everyone thanks for the advice ! Keep it coming.

I agree that avoiding plunge roughing except in an unusual circumstance is best.
But its nice to have a idea how to pull it off if needed.

I have been working with some of the recommendations both in this thread and other threads and so far things are progressing nicely.

I'm getting good results by going with carbide bull and ball mills for roughing and doing away with the old school rougher's unless I absolutely need them.I might even be able to get them to budget me in some more expensive tooling and carbide indexable's if I can prove the value outweighs the cost.

I'm sure as I keep trying different things out I'll have more specific questions in the future.

Thanks CNC-Zone !