Reducing cycle time - tooling question

Hi

As I told a couple times before I'm fairly new to cnc machining. And still learning each day.
We machine 99% of the time aluminium.
Most of the parts got some inner pockets. At the moment we use a endmill to helix into the material and rough it out. Not the fastest way and we're searching for something faster.

The options we got is a indexable drill, to drill the hole which the endmill can enter.
Or getting a ripper (pro-x) mill to rough out the pockets. Which is a bit faster and will save on 2 tools in the toolchanger.
"problem" is that the 25mm pro-x mill wants around 12.000RPM. But we only have 6000RPM. would this work? And how should I adjust the feed/chipload because of the lower RPM?

Trying to search for a way to reduce cycle times

Most of the time I use smaller endmills. I find that the extra tool change wastes more time than just Helixing in. I guessing your toolchanger are pretty slow as-well if your mill maxes out at 6000rpm.

Most programs have some kind of drilling involved. You dont have to use a specific drill. Even if you are able to drill a 3/8 hole before a 1/2 endmill goes in it would be helpfull.

tcncj said:

Hi

As I told a couple times before I'm fairly new to cnc machining. And still learning each day.
We machine 99% of the time aluminium.
Most of the parts got some inner pockets. At the moment we use a endmill to helix into the material and rough it out. Not the fastest way and we're searching for something faster.

The options we got is a indexable drill, to drill the hole which the endmill can enter.
Or getting a ripper (pro-x) mill to rough out the pockets. Which is a bit faster and will save on 2 tools in the toolchanger.
"problem" is that the 25mm pro-x mill wants around 12.000RPM. But we only have 6000RPM. would this work? And how should I adjust the feed/chipload because of the lower RPM?

Trying to search for a way to reduce cycle times

Click to expand...

You offer solid options. The tendency in cnc machining is to use the least tools possible for obvious good reasons, yet with a additional rougher here and a added drill process there will make a huge difference.

another advantage with the ripper mill is that we can use it to prepare the part for some 3d contouring.
We already have a 50mm ripper mill but it's too big for some contours.

I could buy an indexable drill and drill a 20mm hole.
But the chip evacuation will be an issue I think. I don't have through tool cooling. And I have to drill 55mm deep. When I enter the 20mm hole with a 16mm endmill, the chips will be stuck in the hole pretty fast. I do have high pressure cooling but it's hard to get all the long chips out. Or I have to rough out the pocket in 2 depth of cuts. But that takes too long.

So...I think the ripper mill is the best solution. Unless someone else got some good advice and I'm overlooking something.
Only issue is I don't have 12000rpm. How should I calculate the chipload for it? should it be changed?

The "ripper mill".. I've got a 1", which I guess is pretty damn close to a 25mm..

RPM wise, I was running 7000-8500.... I don't think 6k is a problem..

Pros for pockets.. You can ramp fairly steep with the smaller ones..

You can feed the hell out of them..

The 2 fluters are NOISY!!!!!!! I hear the 3 fluters and more are a lot quieter..

I found dry to give much longer tool life than wet.. Even in 6061, seems there is a
point, even with aluminum, that the carbide/thermal shock thing starts happening..

They make a HUGE mess... I don't pull that tool out often since I have umbrella
tool changers.. The first time I ran it, it was a just a single tool run, but
when I was done, there was 2" deep of chips sitting in the carousel... Sucks
when you are 30 feet from an enclosed machine and still get a hot chip down
your shirt.

I'll link up a video I made a while back.. OLD Fadal.. The tool path sucks, but
I didn't bother changing it, I saved so much time from running solids that it
wasn't worth it, and I don't think I was pushing anywhere near as hard as I could,
at max that was about 40 cubic inches a minute (in the cut), and that's only a
5 or so HP cut. Pretty stable at depth too, that's hanging out almost 4 inches.


Curtis.. AKA Exkenna on this site sells them.. Latheinserts.com is one of his sites.
He's probably cheaper than Travers.. And he's got a lot of other good stuff too.

I already have a 50mm and 20mm (1flute) ripper mill.
The 20mm is very noisy and not optimal.
That's why I want the 2flute 25mm. The 3 flutes are not available in 25mm. And a bigger cutter won't fit the pockets.
I found a vid of Exkenna on youtube running a 1" 2f at 7500RPM. So 6000RPM max shouldn't be a problem I think

Drilling is the fastest way to remove material, but you add a Toolchange. So someone standing there watching needs to determine how much advantage there is to each. Most Tools are not run as fast as they can be run, especially Drills. You don't need to "center" and Indexable Drill, just Drill.

imho its about the machine, and you have to move matl with what you have and not what the lastest hsm program says. made a couple big (for me) mirror blanks as my 1st big job over 20 yrs ago, 12" x 12" x 3" deep. backside bunches of triangle lightweighting pockets, frontside basically a flat surface. mirrors were 3x around the periphery, and only had to leave them plus .005 and in the proper locations, they were blanks and would be finished at a diamond cutting optical place, after the mounting pads were finished there too. my gcode knowledge at the time was g1 = line, g2 and g3 a circular move of some sort, and g0 is rapid. I hired a fellow who I knew as a programming whiz, he did his thing and I ran the machine. lots of 3/8 and 1/2 carbide reduced shank endmills hanging out a mile. shit my pants at the cost of the custom tooling, and shat again when they didnt hold up well at all. something that would have worked well on the big matsuura horizontals he understood. but I only understood knee mills with 5000 rpm max, that what I had. in retrospect, he was too smart and I was too dumb, in reality the job could just not be attacked the way he saw it. tons of vibration, jammed up end mills, was even running on heavy mist coolant. after a couple weeks we punted, subbed it to a shop with a bigger Haas, still made a lil $$ but I was way late, and the product was of marginal quality. Rob said (and others have too) drilling the quickest way to move metal most of the time. if I had drilled these blanks out 100% .020 small on the dia removing 95%+ of the metal, I could have done this. but starting out, I didn't understand. and I really didn't know my machine all that well at the time. made a lil $$, lost a potential long term technical customer. key knowledge to be gained here? don't grab a big important job if you don't know what youre doing, even if the money is intoxicating. should have stopped when that 1st end mill made that huge shrieking sound, programmed a 15/32 drill to work well with the mist and the 3 hp we had to work with, set up an air blast to blow the chips out and just let it happen as fast (or slow) was it could. a couple years later, had another job I bid badly, this time 10" x 10" x 10" or so, Rc 40 steel, probably 10% of the raw matl left in the finish part. many different sort of mistakes make, but I had learned to drill 1st, rough and finish later. lost shirt, learned a lot. all good. but yes, drills are cheap compared to mills, hold up well, and are good low hp roughing strategy.

I did some cam simulations and a indexable drill is much more versatile.
Some pockets are too small to rough out with the 25mm/1" ripper mill.
But both are very useful. So I will buy them anyway.
Pre-drilling with a indexable drill saves 8 minutes on a 40min cycle time.