Cutting Aluminum Plates

[renegade]

Hello all-


After breaking and burning a couple of standard 1/4" end mills, I thought I should reach out for some wisdom. I need to cut some holes in 1/8" aluminum plate. They are 24mm flanked by a pair of 3.2mm holes. I'll be making these one at a time for the next month or so, but if successful, I'll be making several a day. I was planning on using an Amana 51471 and cutting dry. I watched the Todaytool video where they dry-cut 1/4" plate with this bit and it looked like the way to go. I was thinking I could plunge the 3.2mm holes and profile cut the 24mm. Will this work? Do I need any kind of mister or air cooling? 


Thanks-

Chris

[chuck26287]

Jan 7, 2018 21:14:13 GMT -5 renegade said:

Hello all-


After breaking and burning a couple of standard 1/4" end mills, I thought I should reach out for some wisdom. I need to cut some holes in 1/8" aluminum plate. They are 24mm flanked by a pair of 3.2mm holes. I'll be making these one at a time for the next month or so, but if successful, I'll be making several a day. I was planning on using an Amana 51471 and cutting dry. I watched the Todaytool video where they dry-cut 1/4" plate with this bit and it looked like the way to go. I was thinking I could plunge the 3.2mm holes and profile cut the 24mm. Will this work? Do I need any kind of mister or air cooling? 


Thanks-

Chris

I've used the Amana 51482 for cutting through 1/2" plate 6061 Aluminum. It's worked dry, but I always feel better doing something to help lubricate the bit. I've used a pump spray bottle to manually mist rubbing alcohol on the bit for cooling. I've also used 3-in-1 oil as the bit was cutting. I would place a drop in the cut channel in a few placed along the path so the bit travelled through the oil and was lubed. Sometimes have to use compressed air to keep a channel cleared of chips, or the oil holds them. For repetitive work, I'd invest in a dedicated mister.



I've attached screen shots of the speeds & feeds for the 51482, from G-Wizard Calculator. These are for 0.003 & 0.004 chip loads. The larger chip (higher/faster IPM) can help keep the bit cooler as it carries away more heat. These both keep the RPM at the Amana recommended 18000, and keep tool deflection below 0.001". Keep in mind, though, that's for a bit with 5/8" of cutting height, so it has longer stick-out, and will be running at a lower IPM than the 51471 you mentioned, to keep the tool deflection below that 0.001".

Attachments:

[renegade]

Chuck-

Thanks so much for this. I downloaded the Gwizard app and was having some trouble setting it up to try out.

I will only be working with 1/8” (16 ga?) plate. Do you think the 51471 would be the best bit for that? From the RPM and feed rates you mentioned for the 51482, would I want to increase the feed rate or the cut depth to get the desired chip load?

Lastly, do you think simply plunging the 1/8” holes will work or should I bore those with an actual drill bit? They’re clearance holes for a screw to pass through. They’re not going to be tapped, so if there’s a shade of runout, that’s totally okay for the application. My main concern is bit life.

Thanks again!

[chuck26287]

Jan 8, 2018 8:02:17 GMT -5 renegade said:

Chuck-

Thanks so much for this. I downloaded the Gwizard app and was having some trouble setting it up to try out.

I will only be working with 1/8” (16 ga?) plate. Do you think the 51471 would be the best bit for that? From the RPM and feed rates you mentioned for the 51482, would I want to increase the feed rate or the cut depth to get the desired chip load?

Lastly, do you think simply plunging the 1/8” holes will work or should I bore those with an actual drill bit? They’re clearance holes for a screw to pass through. They’re not going to be tapped, so if there’s a shade of runout, that’s totally okay for the application. My main concern is bit life.

Thanks again!

The best bit would be the one that is just long enough to make the desired cut.  The less stick-out the bit has, the more rigid it is (less deflection) at a given set of speeds & feeds.  The 51471 would be better if you are not going to need to cut anything thicker.  If you're drilling holes, I would use a good drill bit, not the 51471.  It's an "O"-Flute bit, and while it might work, drilling holes is not the forte of its design.  That's what drill bits are for... right tool for the right job always works better.
Since the 51471 is shorter, you could run a little more depth of cut, since there is less deflection, but I don't know how much deeper without inputting that tool in my tool crib in G-Wizard Calculator and running the S&F.  Keeping the same RPM and IPM should give you the same chip load as in the screen shots.  Generalized chip load formula is IPT (chip load in Inches Per Tooth) = IPM/(RPM X # of flutes), so you can see changing depth of cut doesn't theoretically change your chip load.

[Deleted]

The point of a fog buster or mister is not so much for cooling as to get the cut chips out of the way so you aren't recutting chips which is terrible for your cutter and the finish. The lubricant also helps reduce built-up edge, that is it keeps the aluminum from sticking to the tool which will also be bad for the finish and the tool. Aluminum is very sticky, even your 6061 which is a good machining type. Since it's fairly thin stock make sure your holding method is rigid because if the sheet stock moves that will also break your tool. A drill would be best for the holes or spiral cuts with an endmill at 10-15 degrees. Since your stock is thin, chip removal isn't as big a problem as for thicker stock so you may want a down cut bit if you can't hold the workpiece firmly so you have added support. If you batch them out with many at a time you could drill the two small holes and a starter hole for the large one in all your pieces then switch to an endmill to pocket the large hole to size. Then you could use a 1/4" bit for enlarging the 25mm hole so it would go faster and you wouldn't have to worry about plunging full depth into the pilot hole.

[renegade]

Thanks for the replies, fellas. I'm ordering a mister today, even if it's just to blow the chips out of the way, as you say, fean. This brings up several questions. Thanks in advance for your patience and help.

For the drill, I'm guessing I can put a 1/8" bit into a 1/8" collet and go for it. Is that correct?
Should I go pure carbide for the drill bit?
What RPM should I use?

If I move away from the 51471 and opt for a 1/4" bit (or larger?) for the 24mm holes, will I be able to cut them more quickly and with less wear on the tool?

Chuck, do I need to do the advanced setup on GWizard or is the basic fine? I set it up yesterday, but there were several parameters I was unsure about and couldn't find anything on the Axiom site.

Thanks again for all the help. I owe you both a beer if you're ever in Atlanta.

[chuck26287]

Jan 8, 2018 16:18:36 GMT -5 renegade said:

Chuck, do I need to do the advanced setup on GWizard or is the basic fine? I set it up yesterday, but there were several parameters I was unsure about and couldn't find anything on the Axiom site.

You'll get more accurate returns from G-Wizard Calculator if you give it the full data set on your Axiom system.  I've attached a screen shot of the setup screen as I entered the data for my AR8 Pro.  Just modify the data specific to your model, if it's not an AR8 Pro.

Then, you also need to take the time to enter your bits in a custom Tool Crib as accurately as possible.  Pay particular attention to the stick-out length you enter.  That's the distance from the bottom of the tool holder to the bottom of the tool bit, PROVIDED it's a constant diameter from shank to the cutting diameter.  For step-down bits, like the 51482, that has a 1/4" shank, and steps down to a 1/8" cutting diameter bit, the stick-out is measured from where the smaller cutting diameter shank starts.  These bits are sometimes referred to as Micro-Milling bits at about 1/8" cutting diameter and smaller.  Correct entry of the stick-out distance has a LOT to do with the accuracy of the data returned, particularly the depth of cut you can achieve while staying under your tool deflection specification.

[renegade]

Thanks again. I have an AR8+ so this is perfect.

Any thoughts on the 1/8" twist drill bit? Also, any thoughts on the best bit for cutting the 24mm holes?

[seanathan]

I'm looking forward to seeing the update with the aluminum cutting. I've had mixed luck but was cutting without lubricant and running a relatively high DOC. The failure mode was the Bit gumming up in both cases.

[Deleted]

Jan 8, 2018 18:08:33 GMT -5 renegade said:

Thanks again. I have an AR8+ so this is perfect.

Any thoughts on the 1/8" twist drill bit? Also, any thoughts on the best bit for cutting the 24mm holes?

A standard HSS 1/8" bit will fit in the collet even if it's slightly off, I've used one that was 0.123" without a problem as the collets are designed for a small range of shanks. The important thing is to make sure the bit is properly sharpened, that is relief angle, and equal side lengths so both edges are cutting evenly. If you use the 1/8" drill for a starter clearance hole then a 1/4" bit should be fine for enlarging the hole out to 24mm even with a straight in plunge cut assuming it's centered on your starter hole.

[Deleted]

Jan 8, 2018 21:56:17 GMT -5 seanathan said:

I'm looking forward to seeing the update with the aluminum cutting. I've had mixed luck but was cutting without lubricant and running a relatively high DOC. The failure mode was the Bit gumming up in both cases.

That's common for aluminum without coolant and chip removal even with the proper speeds and feeds.

[renegade]

Alright...I think I'm getting there. I'm now using a pure carbide 1/4" 2 flute end mill. And I now have a blower / mister setup. I was going to tap into my router mount to mount the mister, but I figured out a way to do it reversibly. Will attach pix later. I have a denatured alcohol mist and first results are great. But it brought up a couple more questions.

I was having so much trouble with the profile cut, that I changed to pocket. This worked well but the chips I could find were almost as fine as hair. Very small and cylindrical This tells me that the DOC is too small. I had it on .02". I've seen several folks cutting profiles in aluminum with a 1/4" EM at 1/16" DOC. I'm going to give that a go.

Also, is the RPM set in the MMG file or do I need to set that with the VFD control on the front?

Lastly, if I want to stop a cut because it looks like it isn't going well, what's the best way to do that? I've done it a couple times and it kills me that I have to tell it to delete the stop before I can address the Z axis. Meanwhile the bit spins down still in contact with the material. What's the best procedure there?

[Deleted]

The chip load, a function of tool diameter, the material, number of teeth, RPM and feed rate, will define the size of the chips in addition to your DOC. The chip size will determine how much heat is removed from the workpiece and your tool life and is limited by your spindle HP, your machine and clamping rigidity as well as your whole motion control system.