Noob question - roughing

[sndsa]

Hi guys,

What is the best/quickest way to rough? I've had a quick look around the site but have not really come across anything yet.

I spoke to some guys yesterday who say they use a ballnose (carbide tips) - say 16mm and taking say 5mm cuts?

If possible can you assist with the following:
1) tool
2) Speeds and Feed
3) Cut increments

Any tips will be much appreciated as we have very little experience in milling

We have 2 x Haas VF2's,and use the machines for our own tool making (rubber moulding).We have edgecam if it means anything.

thanks
darren

[Machineit]

What you are asking fills books, literally!

In order to determine what you ask one would have to know what material you are roughing, how it is being held, how much is to be removed, is it internal external, a pocket, a mold, if internal does it go through the material so the chips can clear, and on and on.

Whenever you start a job, start by determining the material to be cut. From that you can use tables or books to find the speed (SFPM) for that particular material, the recommended chip load per tooth of the cutter. If you are doing general roughing for pockets for example and you were using that 16mm cutter you would generally take 8mm cuts (half of the tool diameter). The depth of the cut mainly depends on the material, the machines capabilities, such as HP, available RPM, the coolant system on the machine and so forth.

Unless you are doing a mold cavity I don't think many would rough with a ball endmill. Too much engagement and they can tend to make noise/chatter. The surface speed on a ball endmill varies from almost nothing at the tip to very high on the OD of the tool and that is not good.

Depending on what you are cutting, for example doing a simple pocket on a 12mm piece of aluminum then a finish cut, most would just use a standard endmill and rough and finish with the same tool.

If you have a lot of roughing to do, I would use a roughing endmill with serrated flutes for any type of steel. They make smaller more easy to manage chips and use less power, generally they are made for roughing. For aluminum, most would still use a standard flute carbide endmill and crank up the rpm and speed and watch the chips fly. It's fun!

If you can post an example of what you are working on you will get answers to how to do the roughing. Without that we really can't help. Heck, even with that you will still get 15 different ways to do it

Good luck and good learning.

Mike

[WallyL7]

Like Mike said, we probably need a LOT more info here. Books are written on the subject.

But, to answer your list of questions...

If possible can you assist with the following:
1) tool
You will need the correct tool for whatever material you are cutting...
2) Speeds and Feed
You will also need to have the correct speed and feed for the tool that you are using for that specific material...
3) Cut increments
Finally, you will need to use proper cut increments for the given tool you are using for the specific material you are cutting...


You can see where this is going right?

Give us some examples of what you are needing to rough ( what material, and rough idea of what you are doing to it) and that may help us give you a better idea of how to do it. Mastercam is what I use and it has a ton of slick toolpath options for roughing material. Are you really familiar with edgecam? Are you really familiar with machining and the Vf-2's capabilities? How solid is the workholding? That also dictates how quickly you can rough out material (as well as how you should go about the roughing process...)


The most simple answer to that is the new highspeed troichodial toolpaths are probably the quickest at removing material at a break-neck rate of speed. But like we said, there is a little more to it than that normally.

[Geof]

Originally Posted by sndsa ......What is the best/quickest way to rough?.....darren

Highest rpm sensible for the material and cutter.

Deepest cut, largest stepover and highest feed without either stalling the machine or breaking the cutter.

[sndsa]

Thanks for the feedback guys,

sorry about the lack of info.

Ok 99% of the time we will us mild steel for our tooling. stock is generally quite chunky So we fix it with clamps, bed clamps or in our hydraulic vice.
Mainly cavity machining or pocket (most likely contoured walls etc)

For example, the last job was a block - about 250x250x180High, from here we took out a pocket about 190x190x16mm deep. Call it a plus sign on either side.

The job before that - stock about 300mm x 200mm x 100mm High. From here we took out two pockets about 100x50x50mm deep. Contours on each wall and radius on the bottom. I will upload a picture of a mould as an example.

Our next job will be about a 300x250x100mm thick stock - from here we will be machining four say 100diameter tapered holes, depth about 70mm.

So in a nut shell yes mainly cavities.

@wally - we purchased the advanced milling package from edgecam (due to their support here in SA) and have just completed about 2 weeks of training. so to answer you question, I have learnt or say at least seen alot the theory, with little practice or at least have good support if I need the guys to help with some functions.
With the simulator you can at least play around to find more efficient routes etc.

Knowing nothing, we were sold a 16mm high speed cutter from Iscar, with inserts. When getting the specs, I think it was 0.5mm depth at something like 2700rpm - 1000 feedrate, going by memory here so could be wrong.

We not phased if we don't run the machine at 100% as its not production work. As noobies we will also run the machine a little more conservative until we get more experience. I would however prefer to decrease roughing time and spend it on finishing.

If you guys tell me 1/2 of the diameter, I will most likely use a 1/3 to get going. Anything is better than freekin 0.5mm! I will try post a link to its specs.

I like the idea of a standard endmill, I'm sure you are talking about one with inserts?


90% of the time we have to ramp or helicoil into the job.
lucky edgecam makes this quite easy, occasionally we can go in from a bore that has already been machined but that doesn't happen often

We have another VF2 machine which we will eventually be use for production work, but lets cross that bridge when we get there.


thanks again for the feedback!

[sndsa]

Like you guys say, speeds, feed and increments depend on the tool.

here is an image of a mould we have done, if I'm not mistaken the pockets were about 100long x 50 wide about 60mm deep


Perhaps if you can give me some examples of your best roughing method for cavities, I can purchase a similar tool then get the suppliers suggestions, then run it past you guys.

If it helps we have high speed machining as for cooling: standard + directional attachment.

[double a-ron]

I have a low power machine (7hp MiniMill 2) so I stay away from "high speed machining" or HSM. I simply can't make it work with only 6k rpm and 7hp. I'm betting you won't be able to make it work either with only 7.5k rpm. Alas, I have discovered a miracle called "high feed machining". It's the polar opposite of HSM. In HSM you run full depth, say 1" deep, with a .5" coated solid carbide end mill running at 12K rpm dry and take light radial cuts. Like no more than 10% of the tool. The problem with this is two fold. 1: the chips created are a nightmare to remove from deep pockets. 2: unless EdgeCam has algorithms for generating tool paths that tightly control radial engagement of the cutter, creating the tool path can take allot of time. You can imagine what would happen if the cutter went to do a full slot (180 deg of cutter engagement) at 800ipm. SNAP! I have GibbsCam and they want me to drop 3 grand on volumill to have that kind of control of the tool path.

High feed machining or HFM is the opposite. You take a special HFM indexable end mill, almost everyone makes them now. Tungaloy, Iscar, Ingersol, we got ours from Seco. The Idea is simple, normal old school offsetting tool path. 40%
step over, largest tool possible. They typically run 2 or 3 inserts at .05 ipt (not a typo) with a .04" step down and normal spindle speeds. Example feeds and speeds for a 1.5" 3 flute cutter: 2037 rpm, 305 ipm. On my machine that's a %100 load on the spindle with no spikes. Your machine would be like %60. The chips are small flakes instead of HSM's 1" long spaghetti noodles. The best part is, for deep pocketing, I 've used our .75" cutter to do a 3.5" deep pocket. Try that with HSM. ChAtTeR. This is possible because the load in HFM is directed toward the machine's spindle as oposed to HSM were it is directed toward the side of the cutter. Also when the inserts wear out you just index them to a fresh side. Beats the hell out of buying a whole new end mill.

Like they said, books....

[Ydna]

For steel milling very irregular pockets, especially those with non-straight walls (tapered etc) I like the high-feed machining route. I use either an index mill like he said above, or a bullnose endmill depending on how deep the pocket is and how large of a tool you can fit in there. The toolpaths have relatively small step-down amounts but the feedrates are fast. After the roughing is complete you might not need to do a semi-finish pass since the small step-down sometimes does it in one fell swoop. Depends on the surface finish you want.

I don't do a lot of steel milling that calls for high-feed milling but it seems pretty effective if the part geometry is acceptable for it. But there are many other ways too, depending on how much cash you want to throw at tooling

[sndsa]

thanks guys,

I really appreciate the help, no wonder there are so many books about this!

@ double a-ron, I have iscar coming over tomorrow, i will ask them what tools can handle HFM.
Let me find out exactly how they rate the tools we have bought.
@Ydna - like you say as big as what you can fit. I think I need to buy a good ballnose and index mills. (unless Iscar can show us how stupid we have been)

I will get him to demonstrate his 'high speed cutter' which they convinced us to buy. I have a job in there waiting to be machined.

I'm looking at another mould at the moment. I will have say 6 x 100mm dia bores say 55mm deep, straight sides and flat bottom.

I will also play around with some strategies on edgecam.

I will keep you posted as to what these guys say tomorrow,

cheers
darren

[sndsa]

Ok so Iscar was here this morning (unfortunately I wasn't there to talk directly)

The 16mm High speed end mill we have can apparently work at the following:

3000rpm
2000feed
0.5mm cuts
This should improve times but not as good as going with some of you other options