What's new
What's new

Looking for Brother tooling suggestions

BRIAN.T

Cast Iron
Joined
Jul 23, 2018
Location
Los Angeles
I've just purchased a 22 tool changer brother r450 pallet machine. 10k high torque dual contact spindle (16k wasn't available)

I'm planning on loading up the last 15 or so packets with my most commonly used tools. However, I've never worked with a bt30 spindle, so I'm not sure exactly how much I'm going to have to adjust. Mostly aluminum, nothing tight tolerance.

For my "large" end mill, I'm going with a 3 flute 1/2 destiny 1" length of cut. However I'm thinking I might want to look into chip breaker type end mills for general purpose. I actually think something like the kor5 might be a good choice, more flutes, faster feeds, chip breakers. Perhaps 1" loc on a 1/2 in a bt30 is tool much?

Guhring 5514 carbide drills for balax form taps. Is it worth going carbide drills without coolant thru? Speed is more important than cost, but still I'm worried about pecking with carbide.

Finally I'd live a multi purpose chamfer mill/spot type tool. Or perhaps a chamfer / backside chamfer tool. Chamfer would be the primary function for me, but a couple spots here an there would be great. Any tools you guys like that Excel in both categories?
 
Congrats! Great machine, and spindle. The High Torque is very rugged with larger steel bearings and the highest drawbar force for Brother machines. It will run 10k rpm all day long too. Those Guhring drills are amazing. You can basically run those up to about 4xD without pecking and the feedrate is crazy. About like a CTS drill. For roughing aluminum, a 1/2 inch end mill is a good choice, possibly a 5/8 in a High Torque. I like endmills with lower helix angles for roughing, around 35 to 40 degrees, versus 45 degree helix. Higher helix tries to pull out of the spindle more. My go to workhorse aluminum rougher is the Hanita TC6A0R13005. I have ran that at 1.25" Axial Depth x .300" Radial at 275 IPM on a standard Brother spindle in 6061. Day in and day out parameters I would feel comfortable at 1" x .25" x 250 IPM. I run it in a side lock end mill holder. Maritool has nice Dual Contact and very short end mill holders. They also have a really nice ER32 Dual Contact that is only 52mm gage length I like alot. I am sure you will really enjoy the new machine. For smaller parts they can typically put out about three times the work of an ordinary vmc, especially with the pallet changer.
 
For my "large" end mill, I'm going with a 3 flute 1/2 destiny 1" length of cut. However I'm thinking I might want to look into chip breaker type end mills for general purpose. I actually think something like the kor5 might be a good choice, more flutes, faster feeds, chip breakers. Perhaps 1" loc on a 1/2 in a bt30 is tool much?

No, just mind the % engagement and feed rate so you don't generate so much downforce that you pull the toolholder off the taper and get some fretting. Maybe the R450 has more drawbar pull than my Speedio, but I can pull my toolholder loose with a Destiny Diamondback going balls out.

Regards.

Mike
 
No, just mind the % engagement and feed rate so you don't generate so much downforce that you pull the toolholder off the taper and get some fretting. Maybe the R450 has more drawbar pull than my Speedio, but I can pull my toolholder loose with a Destiny Diamondback going balls out.

Regards.

Mike

Interesting. This is good to know, thanks. What's balls out for you with that tool?
 
Finally I'd live a multi purpose chamfer mill/spot type tool. Or perhaps a chamfer / backside chamfer tool. Chamfer would be the primary function for me, but a couple spots here an there would be great. Any tools you guys like that Excel in both categories?

For chamfering, I like as many flutes as possible. I also like being able to chamfer with only ~.02" of the part proud of the jaws. To that end, my regular chamfering tool is an 8-flute 3/8" Harvey double-angle cutter. For inside radii that I can't reach with a 3/8" tool, I use a 1/8" 4-flute chamfer mill.

For backchamfering, I use a variety of Harvey doube-angle cutters, down to 1/8" for back-chamfering holes and small-radius features.

Spotting is done with a dedicated tool. I like MA Ford carbide spotting drills. They make a nice spot with very small center flat.

I can't recommend a single tool that is good at chamfering and spotting.

Regards.

Mike
 
My "big" endmill in the standard Speedio loadout is .5" x 1.25" and that's with 16k spindles. You can definitely go bigger than that with a 10k high torque, and get back some of the SFM you'd get from being limited to 10k if it makes sense for your parts. 5/8 would be no problem.

I just use a 3/8" carbide drill/mill as my general purpose spot/countersink/chamfer tool. Cheap and effective. 4 Flute Carbide Drill Mill .375 Dia x 1.0 Flute Length 90deg MariTool Obviously if you have a long production run of something then use something more specialized, but for a "it's always there" part of your loadout I can't see why you'd need more.
 
Interesting. This is good to know, thanks. What's balls out for you with that tool?

In 6061 ... 16,000 rpm, 3-flute Destiny Diamondback EM,1-1/4" axial engagement, 35% radial engagement, 288 IPM. The spindle motor will handle it, but the toolholder gets shaky in the taper.

I have gone over to Maritool segmented 3-flute roughers when possible. These cut with lower spindle load and (I think) less downforce. The problem I have with the Maritool roughers is they seem a bit fragile on account of the very deep flutes leaving less backbone. I have broken a couple of them on cuts that Diamondbacks have survived miles of.

Regards.

Mike
 
I run a lot of the Maritool standard 3 flute cutters and have had vary good luck with them ,, I tryed there roughers and also found they snap if you push them hard ,, I went back to running the TAZ roughers from lakeshore ,, one nice thing about the Taz cutters is you you get to Z depth super fast with them ,, I program most parts at a 30* down feed slope and have gone as hi as 45* ... I have NEVER had one weld up.
 
For chamfering, I like as many flutes as possible. I also like being able to chamfer with only ~.02" of the part proud of the jaws. To that end, my regular chamfering tool is an 8-flute 3/8" Harvey double-angle cutter. For inside radii that I can't reach with a 3/8" tool, I use a 1/8" 4-flute chamfer mill.

For backchamfering, I use a variety of Harvey doube-angle cutters, down to 1/8" for back-chamfering holes and small-radius features.

Spotting is done with a dedicated tool. I like MA Ford carbide spotting drills. They make a nice spot with very small center flat.

I can't recommend a single tool that is good at chamfering and spotting.

Regards.

Mike

Yeah I can't seem to find a tool I like that's good at both spotting and chamfering. I think you're right about using a double angle cutter. The one drawback for me is not being able to chamfer small holes or slots as I could with a standard chamfer mill. Someone should make a double angle cutter that comes to a point. That would a handy tool.
 
My "big" endmill in the standard Speedio loadout is .5" x 1.25" and that's with 16k spindles. You can definitely go bigger than that with a 10k high torque, and get back some of the SFM you'd get from being limited to 10k if it makes sense for your parts. 5/8 would be no problem.

I just use a 3/8" carbide drill/mill as my general purpose spot/countersink/chamfer tool. Cheap and effective. 4 Flute Carbide Drill Mill .375 Dia x 1.0 Flute Length 90deg MariTool Obviously if you have a long production run of something then use something more specialized, but for a "it's always there" part of your loadout I can't see why you'd need more.

That's great to hear, those specs are my go to end mill for almost everything. Can't go wrong!

As for the drill mill, that's what we use now, well internal tool's version. They are great for chamfering, not quite as good for spotting. I tend to rip up the tips faster than I'd like. Perhaps mari's are superior. Maybe I'll give them a shot.
 
Yeah I can't seem to find a tool I like that's good at both spotting and chamfering. I think you're right about using a double angle cutter. The one drawback for me is not being able to chamfer small holes or slots as I could with a standard chamfer mill. Someone should make a double angle cutter that comes to a point. That would a handy tool.

Make a drawing. Submit it here: Custom Tool Request from Midwest Industrial Tool Grinding | MITGI

They'll make it and coat it, and it'll cost you about the same as an off the shelf standard tool.

No affiliation, just a happy customer.
 
Another recommendation. Typically you want the shortest tool holders and tools. I have an exception to that to make your life a little easier. When acquiring small Diameter (ER16 and under) holders, get a little longer gage length (around 80mm, no less than 60mm) to give yourself something to hold when loading in the 14, 21 or 22 Tool magazines. Especially holding drills or taps, a little extra length won't be a big performance difference, but you will be glad when you are loading the tools!
 
Last edited:
Someone should make a double angle cutter that comes to a point.

That would defeat a lot of the benefit of a double-angle cutter -- being able to chamfer an edge that has limited Z clearance due to vise jaws or other part features. Yes, you can chamfer with the first .02" of a 90* chamfer mill, but it's like using a .04" cutter - you have to go real slow to get a nice chamfer. With a regular 3/8" double-angle cutter, you can be .01" up on the flutes and you are cutting with a .27" diameter tool. Also, many 4-flute chamfer mills have only 2 effective flutes at the tip, as 2 of the 4 flues are relieved at the tip.

Regards.

Mike
 
As far as aluminum roughing I have been using the same Maritool 1/2" 3 flute corn cob rougher in my old brother since I got it. Always in the super short Maritool side lock holder and high strength pull studs.

One thing I would like to see is more 5/6/7 flute alu finishers. The only company I see making them is Swift Carb. The flute count really limits speed in these machines.

And very important! Torque the pull studs to recommended torque- NO MORE! Over tightening deforms the tool holder.
 
One thing I would like to see is more 5/6/7 flute alu finishers. The only company I see making them is Swift Carb. The flute count really limits speed in these machines.

Those are really nice when you need them. Fullerton with make you 6 flute end mills with their aluminum geometry, but you've got to order about 10 for it to get to a good price. I've got 7 on my desk that are ready to test.
 
Not sure what you mean by a "good" spotting / chamfering tool, but we use these -

https://www.mscdirect.com/product/details/06298541

The tip diameter is about .005" so they work well if programmed exact diameter for spotting (IE .08 deep will give you about .163-.166" diameter), and chamfering works well enough. Of course we aren't trying to run anything wide open/absolute min cycle time...
 
BTW, you have 22 tools and lightning-fast tool changes -- why fret about saving a tool pocket or tool change?

Regards.

Mike

Because when you need 23 or 24 tools..

Our older Haas machines only have 20 pockets, and it gets to be a PITA when you have a job that needs 21 or 22 tools...
 








 
Back
Top