Brother finishing pass

Houndogforever · Feb 17, 2018

I have a part, 1018 cd steel, held in a raptor dovetail clamp on a rotary axis. There is one particular dimension that I need to reach and finish mill 1.350 deep while only taking off .005-.010 from the side to be finished. I can't have any tool deflection, or at least minimal.

I was using a 3/4" carbide end mill in my old Fadal when doing this, but the BT30 spindle doesn't really like a 3/4 tool.
So my question is, to take a finishing pass 1.35deep on 1018 what diameter tool will work best in the BT30 brother spindle? 1/2" dia? 12mm? 3/8"? Also, 3 flute, 4 flute, 5 flute or more? I don't want a lot of tool pressure so I am thinking 4 flute.

But for those that have used the brother on steel, what kind of parameters are you doing to keep a nice square cut?

Thanks for all input.
Jon

dstryr · Feb 17, 2018

What kind of tool holder are you using? Can you reach it with a stub 3/4 holder from Maritool? BT3 End Mill Tool Holders - MariTool

If it was me I'd use a 1/2" in a stub holder but you mention its on a 4th so not sure if your spindle will clear? I'd use a 5fl as well

Finegrain · Feb 17, 2018

BT30 is fine running a 3/4" tool if you're only taking off .01".

You say no or minimal deflection, but what does that mean quantitatively? .001"? .0001"? Ask HSM Advisor what he gets for your parameters.

Regards.

Mike

Milland · Feb 17, 2018

I haven't used this combo myself, so just some thoughts - I agree wit dstyr, use a stub holder, 1/2" EM should work, but I'd be very tempted to keep the finish stock to .005", and use an uncoated, very sharp 3fl EM meant for Al finishing (but one without a circular land). My reasoning is that you've got a very flexible setup (rotary, knife edge clamping, 30 taper machine, etc.) and so should try to minimize load at the tool edge to prevent deflection.

Cutting forces should be low enough to allow the endmill to last a reasonable amount of time, and the small engagement force from the 3fl EM should lessen taper on the cut lenght. Adjust speed and feed to suit.

My biggest worry would be how consistent the stock is, as 1018 might be somewhat "uncontrolled" for alloy and mill processing. If using crap stock you might hit hard spots that damage the cutter and change the effective parameters.

Nerdlinger · Feb 17, 2018

Is the length of cut 1.35" or just the depth of the feature? Like Finegrain said - what's the actual tolerance?

hmmmm, I wonder if the rigidity gained from more flutes (say, 6-fluter) is offset by the greater contact area and the resulting pressure :scratchchin:

Milland · Feb 17, 2018

Nerdlinger said:
hmmmm, I wonder if the rigidity gained from more flutes (say, 6-fluter) is offset by the greater contact area and the resulting pressure

That's my take on it, and why I was thinking three flute. With only .005" being taken off there's not much bending load being put into the tool or part.

DavidScott · Feb 17, 2018

I agree with you about 3/4" shanks beign too big for BT30, and I do have the Maritool "stuby" side lock holder. IMO Maritool sidelock stubby holders end at 5/8". I would go either 1/2" or 5/8" multiflute. I was just looking through the IMCO catalog yesterday and although I haven't been a fan I must say they have some very interesting tools now. You may want to look at them. I would try 5, 7, or 9 flutes for what you need, and 1/2" because I am cheap.

adama · Feb 17, 2018

IMHO its flutes in the cut that matters not flutes on the tool, you want minimal deflection, only have one flute in the cut at any given time and you have done all you can there to minimise tool forces whilst maximising rigidity from the additional material in the cutter.

Dead easy way to find out how good - bad you have it is just run one part twice and compare it with a part ran once.

One quirk on my floppy machine i do find since switching to HSM tool paths for this kinda cut, too little radial engagement ends up like conventional cutting and the tool deflection seams to increase, i find once i drop bellow about 5% radial engagement i dont see any improvement in deflection. Seams theres a point were you go from cutting to rubbing, give it something nice to cut and it seams happier.

BROTHERFRANK · Feb 17, 2018

I have seen very good success with 5 flutes. A shop I know that runs a lot of 1018 on their brother machines, highly recommends the IMCO end mills. Here are some pics of machining Titanium with a 3/8" 5 flute with 2.5" reach. Used .015" step over with HSM to rough and then a finish pass with .010" stock. I would go with a 1/2" for your app. Possibly a neck style.

gkoenig · Feb 17, 2018

If you wanna try out a stubby Maritool 1/2" holder, I've got one and I think I've got an IMCO 5 flute 525 sitting around here somewhere. Just a quick pull-stud swap. Happy to swing by with it!

Houndogforever · Feb 18, 2018

Thanks for the offer. I have the option of holding it in either a Maritool SK16 collet, stubby side lock, er25 or a Schunk Hydraulic. I don't have a particular tool right now, but since this is a repeat job, I have no concerns spending $80 or whatever for just the right cutter.

The part will have a rough facing cut on it already so the amount of radial cut is very controllable.

My gut is to go with a 1/2" tool also but was really unsure on the number of flutes thing.
thanks for all the suggestions and for the kind offer gkoenig.

edit: Oh, as to tolerance, I mill two opposing faces in the same position and they are +/-.0020 width but must be parallel within .0005 which is why I don't want any deflection down the length of the tool.

eaglemike · Feb 18, 2018

I've had the Brothers for a bit over a year. My guess would be a stub side lock would be better. Some of the stuff I tried with collets (even SK from Mari) worked ok, but worked better with the side lock. YMMV, of course. I used to think collets were always the answer.

gkoenig · Feb 19, 2018

eaglemike said:
YMMV, of course. I used to think collets were always the answer.

They Are!

... as long as those collets are RegoFix PowerGrips put together with their hydraulic dingus!

For those of us without $15k for the press, $500 for each holder, and $100 per collet, we make due.

joesimmers · Feb 20, 2018

gkoenig said:
They Are!

... as long as those collets are RegoFix PowerGrips put together with their hydraulic dingus!

For those of us without $15k for the press, $500 for each holder, and $100 per collet, we make due.

I just bought this system last year, you can get the manual press for 6k which works very well.

The holders are around 300 each, and collets around 200 each.

But it is a very nice system, it is just a burn when you first buy everything!!!!

DavidScott · Feb 20, 2018

Just putting an order of endmills together and came across exactly what you are looking for. Imco IFC Power path end mills, made just for this application. 1/2" x 2" loc, shortest for this mill, is $109 through Western but non-stock.

Rubiman14 · Feb 20, 2018

We’re also milling a similar feature on a couple of our Brother R450’s. Stainless steel and slightly different numbers though. Width +/- .0005”, .096” WOC, and .670” DOC. I’m cutting this on a .400” diameter shaft also. Doing a .090” rough cut, then a .006” finish pass.

So aside from those differences, my best results have been with a stubby Schunk Hydraulic and CGC Gorilla 7flt 1/2”. We also have Nikken SK, ER, and VC collet stuff. None of those would cut it at our speed and feeds with the mills I tried. Doing over a million a year, so time and tool life is everything. As far as mills, it would probably be easier to name what I didn’t try lol. Tool rep loved me. If I rememeber right, I ended up at 8k and 135ipm.

Orange Vise · Feb 21, 2018

If taper control is priority and you're making a lot of these parts, I'd try a screw-on-tip cutter like the Iscar Multimaster. They have a 1/2" 4-flute tip with a max DOC of 0.374", and it can be mounted to a 12mm shank.

IME repeated depth cuts with a relieved cutter is the least finicky way of controlling shoulder straightness as the cutter dulls.

rlockwood · Feb 21, 2018

i'm perplexed by the notion that a 30 taper is somehow incapable of using a 3/4" tool here..

Finegrain · Feb 21, 2018

rlockwood said:
i'm perplexed by the notion that a 30 taper is somehow incapable of using a 3/4" tool here..

Not incapable! I do it, and in fact am doing it right now with a 3/4" ball EM to finish a 3D surface. The pertinent point is you can't just run a 3/4" tool the same as you would a 1/2" or 3/8" tool for roughing or slotting, or very long engagement.

Regards.

Mike

Houndogforever · Feb 21, 2018

rlockwood said:
i'm perplexed by the notion that a 30 taper is somehow incapable of using a 3/4" tool here..

I have used a 3/4 tool for this opp before. It will work, but dropping that big tool in a tight spot is a bitch sometimes, and I was hoping to use a 1/2 em if it will work.

I actually contacted IMCO and here is what they told me to do...
M726 #69088 ½ x 1-5/8 x 3-1/2 w/.015cr.
350 SFM= 2673 RPM
.0013 IPT= 20.8 IPM
Axial- 1.350 (max)
Radial- .005-.007
Flood Coolant

These parts are in the queue so we will see how she runs in the next couple weeks.
Jon

Brother finishing pass

Hot Rolled

Diamond

Diamond

Diamond

Stainless

Diamond

Diamond

Diamond

Stainless

Titanium

Hot Rolled

Stainless

Titanium

Aluminum

Diamond

Plastic

Titanium

Stainless

Diamond

Hot Rolled

Similar threads