[jmcglynn]

Hi,

I'm making this part out of steel (standard A36 hot rolled with the mill scale cleaned off), using carbide cutters.

In this picture you can see the finishing operation, done with a 4 flute .75" ball cutter. I'm using a Z-level pattern, stepping down .025" per pass.

The speed/feed I get using machinist's toolbox is 33ipm at 3500rpm. Given that I'm taking a small cut (.025" step down with .010" material left on the surface plus the .030" steps from roughing) I think I should be able to move the cutter faster. I'd like to take a smaller step down for a better finish, but at 33ipm this operation is killing me.

Any words of wisdom on adjusting from book feeds for different situations like high speed machining?

I don't want to experiment and toast a $150 cutter if I can help it.

[dannystooblue]

Well, it can be challenging at times to get good advise on what your doing, but I will offer my opinion for what its worth. Part of it will depend on the machines capability, then the cutter, and then the geometry. I tend to prefer 2-flute ball mills for more aggressive cutting, the 4-flute tend not to get the chip out as well. The part in your picture seems to have more vertical walls and less horizontal ones. While machining vertical walls with the side of the cutter you will be limited to a slower speed, with a nice ALTIN coated carbide ball you should be able to run 750 to 800 sfm (the cutter will live longer back at 650 though) If you can keep the chip load per tooth at 0.006 to 0.008 at these speeds in your machine you should be fine. If your machine will not machine that fast (feed rate calculated), then slow the spindle to extend the life of the cutter, you can rub the cutting edges right off a new ball mill pretty fast if its not cutting something. Then when you get closer to the tip of the ball you can speed up the cutter speed, this can be figured using the effective diameter of the ball in the cut. How much stock is left on the part? 0.0075 would be a good place to have the stock for this cutter, we also rough with the ball endmills quite often or with a bullnose... square endmills just don't keep their corners well.

We tend to not use solid carbide in applications like this over 1/2" unless 100% necessary, a 1/2 coated 2-flute is less than 1/2 the price of the 3/4. If you don't need to stickout more than 2.5-3" a 1/2 will work fine as well.


Like I said, this is just my opinion, as long as you don't try to spin it too fast you should have no problems. This part doesn't appear to have any "keyhole" type situations where the cutter is in contact for more than any given 90°, in those situations where the cutter will "bark" in a corner it can cause trouble, just for future reference.



Danny

[kuyohtay]

In my opinion, use the source of the tool manufacture to define the SFM for the application. These fine people have way more knowledge than any one person can accumulate in a career AND they know their product. I try to stay away from "industrial catalogue" tooling b/c you don't KNOW what you are getting.

Call the big tooling manufactures (Kennametal, Sandvik Coromant, Iscar etc.) and they will direct you to the local distributor who usually have a technical representative available. Quite often they will let you try (FREE) their latest and greatest in hope that you become a repeat customer. They want you to be successful!

Pick the tool supplier with the best tech support locally and stick to them. They will certainly reward your loyalty.

Kuyohtay,
Sr Apps Engineer at HARDINGE

[tomr]

as danny stated we also avoid using solid carbide on jobs like this. On similar jobs we prefer to use a copy type end mill with 6mm dia inserts. We have both Carboly and Kennametal and both will run fine with a chip load of .005 per tooth @ 1100 SFM. If this type of tool is available you can run from 58 to 95 IPM. Surface finish, machine capability and set-up are all factors as you know. The other good thing about indexables is if the inserts wear or break down they can be indexed on the machine with no worry about a blend in.
tomr

[jmcglynn]

A copy mill makes perfect sense, especially for roughing this part out. I wonder if I could rough and finish with the same tool?

[WILDMAN2]

TRY THIS WEB SIGHT
WWW.ENDMILL.COM/PAGES/TRAINING/SPDFEED.HTML

[big_mak]

My $.02.

while the tool tech reps will give you great starting info, every component in the machine system will affect how fast you can go, and also what your surface finish requirement it as well.

Your endmill, the holder, the condition of your spindle, how rigid you are clamped, how much backlash is in the machine, don't forget to make concessions for the lunar cycle as well. This all has a bearing on how fast you will be able to go, well everything except for the Lunar cycle anyway. The other thing that will control how fast you are able to go even if the machine has the HSM option, is how the code is being generated. If your cut tolerance is too fine, the amount of code coming through the controll may choke off the machines movement and leave dwell makes in the part.

So as you can see there are 1,000,001 things that will impact exactly how fast you can machine this part! Maybe 1,000,002 things if you include the Lunar Cycle!!

[MikeOD]

My advice is to bring the cutter diameter down, and thus the RPM up to match the SFM, this allows you to bring the feed up. I am from the "new school" I guess, so I push SFM and ONLY use quality carbide tooling (I've never used a single HSS tool in a CNC save for maybe a countersink) and I've surfaced all sorts of materials. Quality carbides (with coolant when surfacing) can take the SFM (600-700 if not 800+ depending on the coating and substrate and metal removal rate), then you bring the cutter diameter down, bring the chip load DOWN too, and you'll get a quality surface finish. I try to avoid going higher than a 0.004" chip load when surfacing (higher if I HAVE to based on the material, but I prefer not to) and when I need a smooth surface finish I'll bring the stepover down to something along the lines of 0.004" as well if necessary...but you probably don't need an Ra of 12 microinches (which is very very achievable).

A 4 flute 3/16" cutter at 700 SFM and 0.004 IPT will require 14,260 RPM and feed at 228 IPM (as long as your Haas isn't an "SS" it will be able to follow a smooth path at that speed if you have the RPM to handle it, if it's an SS you probably don't want to push more than 150ish IPM). If you only have say a 10K spindle though, then try to only get the cutter diameter up to the point where 10K will be the SFM you desire, like say a 0.25" cutter (10,700 RPM, so run it at 10K which is like 654 SFM) now keeping the chipload the same, your feed is 160 IPM...versus that larger cutter you're running now that is crippling your feed. As the diameter goes up, the SFM remains constant, so the RPM comes down, the flutes enter the part less often, so the IPT results in a lower feedrate and a longer cut time. If you're finishing in the style I think you are (and that I'm trying to help with) then you should have done a good job roughing already, and you should only be removing say 0.015" off of the surface of the part anyways (the cusps will be taller, but the surface pressure on the cutter should still be extremely low, and you should run a semifinish pass with a slightly larger cutter, or the same size cutter with a stepover of like 0.1" or something and double the chip load...just to have a somewhat consistent surface for the finish tool) so rigidity of the cutter is a lot less of an issue (and the high RPM helps that a LOT more than you might think).

All that said...as you get closer to the bottom of the part, your SFM of your cutter is dropping (so a bull nose cutter is better than a ball mill) and only 2 of that ball mills flutes are really making contact with the part...and you will probably notice that a LOT in your parts...so may I suggest going so far as saving that ball mill for another job, and picking up a 4 or 5 or more flute bull nose flat endmill with maybe a 0.030 or 0.060 corner radius for finishing that part. The rest of my advice above still holds true (in my eyes)...I just think you'll notice a real sudden line all the way around the part where the surface finish changes dramatically with a ball mill from the lack of 2 flutes doing any work anymore as well as the drastic drop in SFM as you approach the center of the other 2 flutes (SFM comes down to effectively 0...and there's no CSS on a mill)...a corner radius on a flat tool does a SIGNIFICANTLY better job of keeping the cutting edge in the "acceptable range" for SFM...and thats REAL important when a good finish is desirable because you need to keep the material chipping instead of tearing/smearing.

[big_mak]

If you were to say use a half inch cutter, you could the use a larger Z step as opposed to using a cutter around half that diameter. The thing here is what are the surface finish requirements VS the machine time requirements, and what is the Spindle capability of the machine in question.

It's no good saying run @ 14,764 RPM if he's running a stock Haas.

That's like Jacques Villenuve or Micheal Schummacher saying you HAVE to take that corner @ 125MPH while they do it in their Ultra modern Racing machine, and you ar etrying to do it in a Pacer.

[MikeOD]

If you were to say use a half inch cutter, you could the use a larger Z step as opposed to using a cutter around half that diameter. The thing here is what are the surface finish requirements VS the machine time requirements, and what is the Spindle capability of the machine in question.

It's no good saying run @ 14,764 RPM if he's running a stock Haas.

That's like Jacques Villenuve or Micheal Schummacher saying you HAVE to take that corner @ 125MPH while they do it in their Ultra modern Racing machine, and you ar etrying to do it in a Pacer.

I agree with you...thats why I then made the 10K example...there are LOTS of 10K Haas machines out in the field...and if you only have 7500 RPM...then it still holds true. When it comes down to surfacing though, you really don't save much time trying to do it with a bigger cutter. The cusp height comes down with the larger radius cutter...but the feedrate comes down too (unless even with the larger cutter you're still at peak RPM).

I also don't feel surfacing at the machines max RPM is a bad thing. Granted you don't want to run the roughing tool all day at that RPM, but the finish pass...if the cutter is properly balanced for the RPM and the cutting parameters are appropriate for the cutter, run it up there...if you're really concerned about it, take 10% of that RPM out of where you're running it...but I still feel thats nonsense with the finish tool.

My explanation applies to just about any RPM spindle...he's at 3500...so unless it's a TM1-2-3 thats capped at 4K RPM...then he's got a LOT of RPM to go (6K or 7500 or more if he brings the cutter size down). I do this a lot, I am not trying to sound like I am the everlasting knowitall from spaceballs...but I do know how to save time surfacing in a cnc machine and achieving EXCELLENT results as well (excellent surface finishes well beyond whats "required" tools that last longer than expected, and machines that haven't needed spindle bearings or motors or drives replaced)...

[jmcglynn]

Thanks for all the input.

My machine is a new VF2 w a 10K rpm spindle.

I've got the cycle time down to 26 minutes (from just over an hour). The changes I made were:

1. Two step roughing on the outside using a 1" 3 flute indexable (carboloy power shear I think, I've had it for years and forgot it was in my box!). I'm running it at 2850rpm, 65 ipm. I rough with .125 steps, then do a second pass with .030 steps leaving .007 material on the part. The tool has a .031 corner radius so it leaves a pretty consistent thickness. The second pass I do at 100ipm.

2. Finish the outside with the same 3/4" 4 flute carbide ball mill. I'm running it like a 3/8" cutter (6111K rpm, 60ipm). I'm stepping down .008", and it's pretty happy and leaves a really nice surface finish.

3. There is a 1.75" through hole that I was drilling and then finishing with an end mill, I just pocket it with the same carboloy tool now and finish it with a 4 flute 1/2" carbide em.

I'm going to get myself a copy mill, but the local tool store didn't have one I liked.

Joe

[MikeOD]

I'm going to get myself a copy mill, but the local tool store didn't have one I liked.

That sounds like an excellent idea...but may I suggest calling your Haas salesguy and saying "hey, can you get me a tooling certificate from Kennametal or Sandvick or anyone else"...because he should be able to, and it should save you some money on cutters. I don't think I've ever bought a tool at a local tool store, always just ordered what I needed.