What's new
What's new

Ideal BT30 Aluminum Finisher?

Is that such a claim to fame though?

With the exception of coatings discoloring, every tool I run only in aluminum still looks pretty new.
No, but this tool was taking big, fast cuts all day every day for a long time and it looked new. The person I was quoting said that he hasn't had the YG-1 Alu-Power hold up for him. Or something to that affect. I don't understand why.
Damn near every end mill designed for aluminum has held up for me unless it was a programming error on my part. But since I never make mistakes..... :sulk:
 
How confident are you that it isn't a material related?

I am fairly ignorant with aluminum (i'll be posting a slew of questions this week to demonstrate) but I did a job a couple years ago, high surface finish requirement, parts came out beautiful. Last year customer wanted another batch. Same everything, material was even from the same supplier, but had a murky/milky finish to it. We wound up having to tumble the parts to give them a uniform finish.
It's quite suspect. I'm told the issue started showing up around the time the material vendor was changed on us through covid. We were super busy then, and running through tools as well as material, so it could have been anything. We used to run Kaiser Select 6061, but they sent us Service Center branded bars. We had those on the shelf for quite a while, but they're gone now and were running the Kaiser with extremely similar results. I dug a bit, and found a mystery piece that had no markings. We ran it side by side, and it was clearly better, but not great like it used to be. The thing that makes me question the material is how rough the cut is off the saw. I have old OP1's for this part, and you can still see the saw finish on the carrier is pretty good.
 
Weird. I've only gotten a murky finish on aluminum when there was either buildup on the cutter due to insufficient lubrication or chips were getting recut. Or on a lathe if a bird's nest rubs against the finished surface.

But, it sounds like the OP's problem is "mild chatter" rather than smearing.

It's absolutely not smearing. It appears to be chatter, but it's a silent cut that's running damn slow. We spent far too much time trying to dial this finish in, when this issue first came up. The toolpath we settled on worked OK, but I wasn't happy with it, and we didn't touch it since. The problematic profile is a spline, and its made up of a boatload of line segments. The Speedios handle it fairly well, and it shouldn't randomly change, but this may be a factor.

It is only finishing on the wall too, its pulled way off the floor.

I'll see if I can find some good examples of the saw cut stock to share.
 
  • Like
Reactions: pcd
It's absolutely not smearing. It appears to be chatter, but it's a silent cut that's running damn slow. We spent far too much time trying to dial this finish in, when this issue first came up. The toolpath we settled on worked OK, but I wasn't happy with it, and we didn't touch it since. The problematic profile is a spline, and its made up of a boatload of line segments. The Speedios handle it fairly well, and it shouldn't randomly change, but this may be a factor.

It is only finishing on the wall too, its pulled way off the floor.

I'll see if I can find some good examples of the saw cut stock to share.
'running damn slow'
that could be your issue, slow isn't always the cure for chatter.

Actually anymore I notice the opposite to be the cure.
 
It appears to be chatter, but it's a silent cut that's running damn slow.
'running damn slow'
that could be your issue, slow isn't always the cure for chatter.

Actually anymore I notice the opposite to be the cure.
Slow RPM or slow feed?

Houdini is correct, either reducing your rpm or increasing your feed in this situation.

I've found even small adjustments can alter the harmonics enough to improve. A part I was having surface finish issues with had vibration issues at .002 cpt, and bumping it up to .0025 brought it down to near nothing, .003 cpt eliminated it. Another I was able to drop the cpt down to .001 to get the surface finish needed, but my SFM was painfully slow. Like 50 sfm!
 
Slow RPM or slow feed?

Houdini is correct, either reducing your rpm or increasing your feed in this situation.

I've found even small adjustments can alter the harmonics enough to improve. A part I was having surface finish issues with had vibration issues at .002 cpt, and bumping it up to .0025 brought it down to near nothing, .003 cpt eliminated it. Another I was able to drop the cpt down to .001 to get the surface finish needed, but my SFM was painfully slow. Like 50 sfm!
In 6061 I have had a lot of 5xd finish passes lately , the system did not like the ole standard - 'slow rpm higher feed rate.'
More often than not have to increase rpm, increase feed rate, and increase WOC.
 
This was a year or two ago now, but I believe we tried from ~0.0004"/flute to 0.0045" on that finish pass. We ended up at I believe 0.001"/fl and 16k. I can get a good finish by adding a minute onto the cycle, but that's not possible to accommodate without more machines. That same tool is used as a rougher and finisher, it runs 0.0065"/fl when roughing, spindle flat out at 16k. We load it up to 0.012"/fl on some toolpaths to settle it down, but it always runs 16k. Most of the toolpaths are absolutely sent on this part, many of them were dialed in by increasing chipload until rapid edge failure, dialed in over months of runtime. Process reliability has been exceptional. The finisher gets demoted to the rougher after a preset runtime, and edge failures in production just about don't happen. Generally adding more load to the tool has helped kill chatter on these Speedios.

The very same tool gets a killer finish at the same speeds on the inside of the part, and it USED to be the same on the outside. Nothing changed, I think, and it's crummy on the outside. IDK. That new tool was supposed to show up today, but it's looking like tomorrow.
 
Not in my experience. I have a 3/4 necked 3 flue Alu-Power that has roughed a ton of 7075 aluminum at full flute length and about a 30% stepover, just ripping that material off. Still looks brand new after 3 months of cutting.
I'm talking about small ones. 3/16" and 1/8". The Destiny's will take twice the cut. I'm sure the bigger ones are fine but I have roughers, Destiny and Swiftcarb for those.
 
I'm talking about small ones. 3/16" and 1/8". The Destiny's will take twice the cut. I'm sure the bigger ones are fine but I have roughers, Destiny and Swiftcarb for those.
Can you expand on this further for me? By twice the cut you mean life? Or radial? or?

I've got a job I'm quoting that I'll be using down to 1/16, and have been looking at brands to try.
 
Can you expand on this further for me? By twice the cut you mean life? Or radial? or?

I've got a job I'm quoting that I'll be using down to 1/16, and have been looking at brands to try.
Actually I would like to see it actually done,
I run production on 7075 small parts making batches of hundreds at a time, and thousands in a year, using 3/16 and 5/32 end mills.

I do full slotting with them at 3xD+ and I have ran multiple different brands, and they have all been the same.

The difference that I notice is in the helix angle, not the brand, decent carbide is decent carbide IMHO.
 
Can you expand on this further for me? By twice the cut you mean life? Or radial? or?

I've got a job I'm quoting that I'll be using down to 1/16, and have been looking at brands to try.
For smaller end mills in aluminum, 1/4" and down, I think Harvey is hard to beat for "toughness". Destiny gives a better finish but I can push Harveys harder and the difference in finish is very minor. Their 5 fluters work really well too, and the core stiffness is amazing on longer doc cuts.
 
For smaller end mills in aluminum, 1/4" and down, I think Harvey is hard to beat for "toughness". Destiny gives a better finish but I can push Harveys harder and the difference in finish is very minor. Their 5 fluters work really well too, and the core stiffness is amazing on longer doc cuts.
speaking of rigid core wall finisher,
I tried this at the tune of $250,
what a waste of money!

I have tried various 5 flute supposedly Aluminum end mills, they all under performed a 3 flute tool, too much engagement, not enough chip clearance.

I guess context to peoples opinions also:
I built mostly 7075 injection molds for 15 years, worked a shop of 90% Aluminum for 20 years, after the fire, I took some of the customers and do 95% Aluminum now also.
All production, so longer runs 100 minimum usually. repeat monthly.
4000-5000lbs of Aluminum a month.
"What's in your wallet"

Everyone needs to mention if their talking a 30° 35° 37° 40° 45° 60°....
 
Last edited:
speaking of rigid core wall finisher,
I tried this at the tune of $250,
what a waste of money!

I have tried various 5 flute supposedly Aluminum end mills, they all under performed a 3 flute tool, too much engagement, not enough chip clearance.

I guess context to peoples opinions also:
I built mostly 7075 injection molds for 15 years, worked a shop of 90% Aluminum for 20 years, after the fire, I took some of the customers and do 95% Aluminum now also.
All production, so longer runs 100 minimum usually. repeat monthly.
4000-5000lbs of Aluminum a month.
I have been amazed at how large a radial cut the Harvey 5 fluters will take, even burying them in a corner. I have tried breaking them many times with too large a cut without issue, but they don't slot. Granted I only have tried 1/4" to .047" and the .047" mill was not nearly as "robust" as the larger tools. I find they don't leave a noticeably better finish than the 3 flute Destiny Vipers at the same speeds and IPM feeds but are much stiffer when doing long doc. They are not worlds better than a 3 fluter as long as the 3 fluter can handle the doc you're asking of it, but when the 3 fluter starts complaining the 5 fluter will still be solid.
 
Thanks both of you for your input.

I'll be posting another thread here eventually discussing this further. Two of my questions are related to the 38 vs 45 helix and ZRN vs DLC.

The job I am quoting is several hundred parts a month, and I'm stressing over quoting the tooling. With the tolerances and the sizes, I tend to quote tooling high, which with this part very well could make or break the quote.
 
Thanks both of you for your input.

I'll be posting another thread here eventually discussing this further. Two of my questions are related to the 38 vs 45 helix and ZRN vs DLC.

The job I am quoting is several hundred parts a month, and I'm stressing over quoting the tooling. With the tolerances and the sizes, I tend to quote tooling high, which with this part very well could make or break the quote.
For Aluminum most like uncoated, at full slotting I have had a ZRN coating add value, keeping the hot Aluminum from sticking, but a non-coated end mill is sharper, lives longer, and leaves a better finish.

Low helix (Helical 35°, YG1 37°)end mills definitely out perform high helix(45°) for roughing, higher helix is better for a finish unless you need a long skinny tool, then the lower helix gives less engagement and reduces chatter probability.

I personally just call it all balanced and I use Helical for everything except tiny tools, and Harvey for tiny tools. done and done.
35-37° for rough, and finish if I don't care, and 45° for a finish if it really matters, unless long and noodly.

Buy some cheap Garrs also if you want to test the waters, cheaper, and not too different, I don't buy them because the pricing is low enough for Helical, and Aluminum tooling especially if you use a separate finisher lasts for thousands of parts.
espeshly if you know how to program shit correctly, not Titan style.
If your buying micro tools(smaller than 1/8") then dont buy Garr or cheap, they will break, I use Harvey for sub 1/8"

If parts are large, I use a 1.5" 3 flute indexable ripper for all my roughing, it is slower slightly but cheaper.
We chew 1,000lbs a week with these dudes.
 
Last edited:








 
Back
Top