BT30 Spindle Capabilities

[crossthread82]

How do those work? They just use a pin for anti-rotate against the weldon flat?
Also do you remember how much the holder was?

They use a shallow taper collet that is pulled into the holder from the rear with stud on the back of the collet. Holder pulls the collet in by turning a screw on the outside similar to a hydraulic holder. The collets with pins act as a anti pullout system in conjunction with the weldon flat. Strong grip, low runout, good balance.

Overall I ended up going with the regofix Powrgrip system. Regofix has something similar to the pin system with their secuRgrip line of holders and collets; however I've never found it necessary.

From what I remember the Emuge holders are very pricey ~$400+ for a cat40 and that didn't include the collets.

 

[Finegrain]

The only reason I am copy/pasting some operations, is because I want to focus on the roughing first, since that’s the majority of the cycle time.

Really? IME roughing is minor compared to all the finishing, edge breaks, etc.

Regards.

Mike

 

[Micmac1]

How do those work? They just use a pin for anti-rotate against the weldon flat?
Also do you remember how much the holder was?

I want to say the holders are around $350ish and each size collets are $175-$200 each. NOT CHEAP STUFF. They have the side lock option for the weldon where a pin locks in but we opted for just the clamp no pin because mose of the endmills we run do not have weldon flats, and honestly with the machine we run it in, the spindle would stall long before these collets slip even without the weldon pin. We also run emuge endmills in these and i dont think theres another endmill out there that compares, they are alot 2-3x the price. General stuff we dont use them but certain applications the topcut endmill they offer, espicialy in hp alloys is unreal.

 

[DavidScott]

Not sure if they make in BT30 but the emuge FPC locking holder

They have them in both the 14mm and 20mm versions, but the projection is 82mm so way too much for a 30 taper.

For roughing in aluminum I doubt you can beat a true corn cob mill in a Maritool stub side lock holder. Don't get caught up on spindle speed, these mills like to take a heavy chipload, like .045" for 1/2" mills. They cut with less spindle load, lift, or other cutter forces than anything else I have tried, total game changers.

 

[empower]

They have them in both the 14mm and 20mm versions, but the projection is 82mm so way too much for a 30 taper.

For roughing in aluminum I doubt you can beat a true corn cob mill in a Maritool stub side lock holder. Don't get caught up on spindle speed, these mills like to take a heavy chipload, like .045" for 1/2" mills. They cut with less spindle load, lift, or other cutter forces than anything else I have tried, total game changers.

careful what you refer to as chipload. typically that means feed per tooth, in which case .045" would be astronomical. for radial load, thats pretty light.

 

[DavidScott]

careful what you refer to as chipload. typically that means feed per tooth, in which case .045" would be astronomical. for radial load, thats pretty light.

Yep, chip load. .045" per tooth is the high end of what MA Ford recommends for their 1/2" corn cob for aluminum. That is aggressive but food for thought.

 

[LOTT]

Anyone recommend 3 Flute roughers that accept side locks? The Helical ones are straight shank. Thanks

Thanks for the 3/8" EM recommendation, will look into them

Every endmill accepts a side lock if you have a diamond wheel...

I like these guys for corncob roughers, they last forever or until someone makes a mistake, whichever comes first.

Roughing End Mills — CarbideToolSource.com

www.carbidetoolsource.com

 

[empower]

Yep, chip load. .045" per tooth is the high end of what MA Ford recommends for their 1/2" corn cob for aluminum. That is aggressive but food for thought.

what the fuck...
i have a really hard time believing any tool taking that big of a chipload. not calling you a liar or anything, just seems utterly insane

 

[crossthread82]

what the fuck...
i have a really hard time believing any tool taking that big of a chipload. not calling you a liar or anything, just seems utterly insane

I had a hard time believing that at first too...until I looked it up....

 

[DavidScott]

what the fuck...
i have a really hard time believing any tool taking that big of a chipload. not calling you a liar or anything, just seems utterly insane

Yeah, playing with a good corn cob mill set up well is kind of like machining softer plastics. If you haven't played with a few then you are missing out. MA Ford and Garr are some of the free-er cutting ones while Maritool sells some that aren't quite as aggressive. I like Maritool's version when trimming off pieces because they are less likely to grab them and cause trouble.

 

[Garwood]

what the fuck...
i have a really hard time believing any tool taking that big of a chipload. not calling you a liar or anything, just seems utterly insane

Really? Don't you play with bigger machines too?

I live mostly in 10K RPM Cat50 land. I've accidently run aggressive programs with the feed override at 250% on a machine that ACTUALLY FEEDS 1000 IPM and noticed the chips look a bit thicker. Like .070" thick lol.

 

[ducesrwld]

Yeah, playing with a good corn cob mill set up well is kind of like machining softer plastics. If you haven't played with a few then you are missing out. MA Ford and Garr are some of the free-er cutting ones while Maritool sells some that aren't quite as aggressive. I like Maritool's version when trimming off pieces because they are less likely to grab them and cause trouble.

just phat fingered an extra 0 in some plastic on our router and ripped through at 1000 IPM recently on a prove out program...moral of the story never understimate what a tool can do til you've tried it or done something like above by mistake. tool held up over a 4' run...dayum!

i've been looking at the chiploads on the corn cob roughers they are in most cases a 3-4x on chip loads better order a few up and put them to the test. don't knock em til you try em.

 

[empower]

Yeah, playing with a good corn cob mill set up well is kind of like machining softer plastics. If you haven't played with a few then you are missing out. MA Ford and Garr are some of the free-er cutting ones while Maritool sells some that aren't quite as aggressive. I like Maritool's version when trimming off pieces because they are less likely to grab them and cause trouble.

i've played with plenty corn cob roughers, just never at .045" FPT.
100cubes/min using fraisa serrated rougher at 1.25" axial, .3 radial and 275 IPM. but thats nowhere near .045" fpt

 

[empower]

just phat fingered an extra 0 in some plastic on our router and ripped through at 1000 IPM recently on a prove out program...moral of the story never understimate what a tool can do til you've tried it or done something like above by mistake. tool held up over a 4' run...dayum!

i've been looking at the chiploads on the corn cob roughers they are in most cases a 3-4x on chip loads better order a few up and put them to the test. don't knock em til you try em.

i have to ask, 1000 ipm - what machine was this on?

 

[macgyver]

i have to ask, 1000 ipm - what machine was this on?

Not duces, but I had a fixed bridge CR Onsrud at my old job, it was new in '07. I ran a bunch of 3/4" plastic plate/sheet that I cut slots in that were 3/4" wide 1/2" deep and 8ft long. I was able to reliably cut at 1,300 ipm at 20,000 with a 2 flute brazed carbide router bit. It would probably have cut faster if I had some pins, blocks, or screws in it to keep it from sliding around, but I honestly didn't need any extra and at that feedrate I could just use vacuum and not worry about it.
That machine would do a max feed of 3,000 ipm if you had some reason to need it. I was at IWF a few years later and they had a new one that they had rapids at 6,000 ipm. When it parked the table, it would make you step back just as a reaction. Probably get used to it at some point, but it was fast.

 

[Vancbiker]

i have to ask, 1000 ipm - what machine was this on?

The Makino MAG where I used to work used 27K RPM with a 3/4" tool at 1000IPM for a standard roughing cut condition.

 

[Nagol]

Here to throw Gorilla Mill in the pot. I love these tools. Agree with others that if that proves to be too much for the tool you were using a dedicated rougher could help.

1/2" Diameter 45˚ Chamfered End (3FSKRI) | Gorilla Mill

Based in Milwaukee, WI – Gorilla Mill has over 30 years experience manufacturing the best carbide drills, end mills and cutting tools in the industry.

gorillamill.com

Might be able to run the same parameters just a more free cutting tool. Awesome chips too.

 

[Nagol]

Those crazy speeds are probably at like 3% engagement, not like you could slot like that. Some books really suck. I like when they give 1 answer for a given scenario and maybe I adjust from there. New Gorilla book has feedrates for slotting, 1/2xD deep, 1xD deep and 2xd profiling at 5%, 10%, 20%,30%,50% engagement. on most of the tools in there. Makes it nice when you don't need to guess in some massive range what parameters to run at.

2022 Gorilla Mill v2

DCatalog offers digital catalog publishing solutions that help to transform your content into stunning flip catalogs, magazines, brochures, annual reports, training materials and more. Increase brand awareness by simply integrating your shoppable catalog with your eCommerce platform.

gorilla-mill.dcatalog.com

Just got done running a job in 7075 Alum with one of these in 5/8 Dia and 2" LOC. I was profiling with it 0.875 deep at 1500SFM and 0.015 IPR.
Another guy ran a wrong program on one part and the thing slotted through the 2" thick part at those speeds. Blew me away

 

[BT Fabrication]

We are taking delivery of a Haas DT2 in a few weeks. The plan is to use the DT2 to produce 2 parts that had been running on the VF2SS, since its better suited for them and we need to make a lot of them. I am working on the CAM for the DT2, and have be referencing the VF2SS CAM that was used for these 2 parts. I know that BT30 machines are quite capable, but having never made a cut on one, I am a bit hesitant to just copy and paste the VF2 CAM onto the DT2, mainly the roughing operations. The rest of the operations are small drills, lots of chamfers, small taps, and smaller end mills 1/4" or smaller.

The DT2 has the 15k spindle, and HSM options. It is a dedicated machine for only machining Aluminum 6061-T.
As mentioned, my main concern is the roughing for these parts.

Here is my current roughing parameters from the VF2SS, and the tool holder I plan on using on the DT2. Do these sound fine for the DT2? To fast, too slow? Any input is greatly appreciated.

Holder: BT30 SK16-60mm
Tool: Helical 3 Flute Chip Breaker 45deg ZRN 1/2" x 1.25" LOC, 0.06" Corner Radius
Length Below holder: 1.375"
Cutting Parameters: 0.050-0.075" DOC X 1.10" LOC @ 15k rpm, 360-405ipm (0.008-0.009" chip load)

Id be in the 0.040-0.050 width of cut at that depth as the sideways forces are what rip tool holders out and compared to a vf2 and a DT2 that is lighter and much less rigid is the limiting factor.
guessing you are cutting aluminum? the DT seems to excell in the drilling and tapping and not so much in the sideways milling forces especially when 2-3X Depth over width. 5-10% radial engagement is a good spot to start. 30% radial engagement is pushing it at 1X Depth.

 

[Chips Everywhere]

16k RPM all day long, it's OK.

I run the hell out of this tool, lasts for a really long time: Maritool 1/2" x 1-1/4" rougher

Destiny Diamondback is good too, but louder, more spindle load, and more pull-out force than the Maritool EM.

Regards.

Mike

Ordering some holders and end mills today.

I just had a quick question. I'm assuming that I should be ordering the 3/8 EM holder 1.1" gauge length (almost flush with the face of the tool holder flange)? Is going with the 1.75" gauge length a problem? 1 of the 2 parts is kinda flat, so reaching it maybe a problem since I am holding the parts on pallets.

I'm going to order both 3/8 and 1/2 holders and end mills and give them a go.

EDIT:

Well, after checking my CAD model, I have no choice but to go with the 1.75" gauge length and tool 1.25" below holder or I wont be able to reach the part.