Need help cutting Aluminum

[sean_adams]

Hi All,
I am having problems cutting some aluminum. It's 3/8" 6061 plate and bar stock. I started out using an Onsrud 63-622, 1/4" bit for the first file. I had talked to a rep at Onsrud about pass depth and was using their recommended settings. The first bit snapped.
Pass depth= 0.25"
Feed rate = 250 inches per min
The second bit snapped using the following settings.
Pass depth= 0.25"
Feed rate = 200 inches per min
Having run out of 63-622 bits I switched to a 63-618, 3/16" bit.I set the Pass depth at 0.1875", and the Feed rate at 100 inches per min.
After it had a chance to ramp up "Snap". My last 63-618 bit, settings, Pass depth= 0.09", Feed rate 100 inches per min.It worked, i cut two pieces. I moved on to the next part file using the same settings, and snapped the bit about 3/4 of the way through the file. I was blowing the channel out until it, re-welded itself in the last pass and a half. Obviously too much heat built up. From what i understand i should probably increase the feed rate, but it already sounds like it's at it's limit. I'm thinking a little less pass depth and increase the feed rate. Any help or advice would be appreciated.
Sean.

[wayne_walker]

Hi All,
I am having problems cutting some aluminum. It's 3/8" 6061 plate and bar stock. I started out using an Onsrud 63-622, 1/4" bit for the first file. I had talked to a rep at Onsrud about pass depth and was using their recommended settings. The first bit snapped.
Pass depth= 0.25"
Feed rate = 250 inches per min
The second bit snapped using the following settings.
Pass depth= 0.25"
Feed rate = 200 inches per min
Having run out of 63-622 bits I switched to a 63-618, 3/16" bit.I set the Pass depth at 0.1875", and the Feed rate at 100 inches per min.
After it had a chance to ramp up "Snap". My last 63-618 bit, settings, Pass depth= 0.09", Feed rate 100 inches per min.It worked, i cut two pieces. I moved on to the next part file using the same settings, and snapped the bit about 3/4 of the way through the file. I was blowing the channel out until it, re-welded itself in the last pass and a half. Obviously too much heat built up. From what i understand i should probably increase the feed rate, but it already sounds like it's at it's limit. I'm thinking a little less pass depth and increase the feed rate. Any help or advice would be appreciated.
Sean.

Sean,

I have only cut a couple pieces of aluminum. From what I experienced, and read on here, your cut depth is too deep and you speed is too fast. Also, you want to ramp into your cuts. Do a search for aluminum and I'm sure you will find a lot of very good information.

I am sure someone with much more knowledge, will chime in.

Good Luck.

Wayne

[tlempicke]

At the camp shopbot at McGrews we had a great presentation from the owner of US Router Tools (http://www.usroutertools.com/). He talked about cutting Aluminum and other metals in depth. (Pun Intended for sure)
One of his interesting suggestions was to feel the chips flying off of the bit with your hand - they should be HOT! that is the heat being removed from the cut.
He says he is willing to consult on the phone, and he apparently has extensive experience with shopbots and other makes of tools similar in nature.
If you get your problems solved don't forget to post the results here for the rest of us.

[Brady Watson]

Cutting AL has been discussed here many, many times. Do a search.

Ignore what the Onsrud guy told you...he should be thrown a beatin' for giving you those numbers.

Run 13k to 15k RPM & MS,1.2,0.7 to start. Absolutely ramp into your profile cuts. Pass depth @ .025" to .04" per pass, err on the conservative side. Using dust collection will help with cooling.

After you cut some parts, feather in more speed as necessary. Denatured or Isopropyl from a spritz bottle will help to cool when you get deep into the cut, although you probably won't need it. The parts need to be held down really well.

Keep in mind this is a light router and not a 5000# milling machine. This is why the pass depth needs to be shallow.

-B

[donek]

I cut quite a lot of aluminum. I don't bother with the Onsrud cutters. I use the acupro. They are a fair bit less expensive. I've only broken about 3 cutters and it was always my mistake. Brady has it right. I do tend to push a little bit harder though. Most cuts are done with a 1/4in cutter. You have to go easier on a 3/16.
Roughing passes: 2 in/sec 0.05in pass depth, max RPM on a PC router
finish passes: 1.2in/sec 0.05in pass depth, max RPM on a PC router

When cutting thick stock like you are cutting I will cut a maximum depth of 1/4 in and then step in and restart the cut. You can't easily clear the chips on really deep cuts so you give the cutter extra room by offsetting your tool path, cutting a partial depth and then stepping in closer to your finished shape.

[donek]

One other thing. Since you are only using 0.05in of the cutter to actually do the work, when the cutter gets dull, just grind off the end and start cutting again. I keep an extra few cutters on hand and just go to the grinder and do my best to duplicate the facets on the end of the cutter. With a little practice it only takes about 5 minutes to have an old cutter cutting as good as a new one.

[Alex Naumenko]

I cut a lot of .125 aluminum In two pass .25 single flute vortex. 110 inch per min. I do have cold air gun pointed all the time. Misting surface with lubricant before starting to cut helping with finish a lot.

[sean_adams]

Thanks guys, I was successful using a pass depth of 0.03 at 100 inches/min. I was blowing out the swarf with compressed air that was loaded with condensation. I noticed that the cut quality was very good after the tool had slowed around a corner and ran through the condensation. A little more tweaking and it will look great. I was using Vcarve Pro Shopbot edition 8, does anyone know if you can slow the feedrate down automatically when you choose a separate last pass with an offset?

[scottp55]

Been playing with "Last Pass" in VCP8, and I haven't found a way yet.
Been reverting to the old way of making 2 separate toolpaths when it's critical and need more options, and then saving both to a combined .sbp cut file(make SURE they are in the correct order in your toolpath list!).
Doesn't take long if you just "Duplicate"(right click) toolpath, change options,eliminate/add offset,rename.
Maybe I've missed something though.

[jerry_stanek]

One other thing you could do is use the shift < key to slow it down