[henrikm]

Hi.

Been running my diy router for about 6 months now, and it performs perfectly in most situations.

I had a guy approach me last week asking to have house numbers cut out of alu. I took the challenge and have started experimenting with light cuts in a piece of scrap.

I've been trying to do a profile cut in the full depth of the material (15mm, .6in) and there are no problems until I almost cut through (about 12mm in I guess), then I get alot of chatter and vibrations and have to shut down. It seems like it might be due to buildup of chips.

The bit is a 6mm 2 flute end mill. Running at 12000 rpm and 120mm/sec feed rate taking 0,5mm cuts. Have tried several different settings but seem to churn out the same result every time. For coolant and chip clearing I use CRC (ie. WD40) and compressed air. Not sure what spec the alu is.

Any suggestions what I might try next?

[louieatienza]

Are you sure it's 120mm/sec? That's about 280ipm?! If you're doig 120mm/min that's less than 5ipm and that's too slow.

I try to achieve a chipload of .0027" in aluminum, and usually cut 7000 cast (mic-6), 7050 and 7075, and some 6061. At 12krpm that works out to 64ipm.

If you're getting excessive chatter, and you're cleaning out the swarf and lubricating, then it could be...

- You're running too slow making too small chips, and they're rubbing against the slot wall, causing the bit to heat up

- You're machine might lack ridgidity in the Y-Z, or your bearings or screws have some slop or play

- Your Z axis is not perfectly trammed

- You could try a single-edge spiral-O-flute which will create larger chips and clear them out better

- Your collet may have excessive runout, or the collet or taper bore has debris causing runout

- If you are not using a carbide bit, do so. They are much stiffer than HSS of the same diameter and stay sharper longer. A TiN or ZrN coated bit can help. While on the same subject, try using a bit specifically designed for aluminum; they usually have a higher helix angle, better chip clearances, more polished flutes. If you have to cut 15mm, I would get an endmill that has a flute length not much longer than that.

- Make sure you are not inserting the tool past the flute fadeout into the collet.

I wrote a thread on router bits and end mills in this forum that has more info on these bits as well as links to videos showing the parameters I use... Good luck!

[louieatienza]

Another thing you can try. Set your profile cut about .02" away and cut to 12mm. Then make another profile pass at the intended cut line. This will give your endmill clearance for the deep part of the cut.

[henrikm]

Thank you very much for your thorough reply. I'll do some testing this weekend.

[msimpson99]

From what I understand, you say it does not chatter until you get to the end of your cut. That is most likely because the stock is moving. Add tabs to your cutout. You may need more/thicker tabs if you are already using tabs.

[louieatienza]

From what I understand, you say it does not chatter until you get to the end of your cut. That is most likely because the stock is moving. Add tabs to your cutout. You may need more/thicker tabs if you are already using tabs.

His material is 16mm, and the chatter starts at 12mm. If the part is moving that would have been observed from the get-go. I think the main thing is going 120mm/min when he should be about 1400mm/min or so, adjusting the depth to suit the machine ridgidity.

Another thing; if you find your bit is chattering excessively towatd the bottom you may need to clear any swarf and apply more lubricant, since if your z isn not perfectly trammed to the table, it will rub and favor one side of the kerf or another. This can happen anyway if the Z is not ridgid enough. You may have to run the job in two stages, first at half depth, then vacuum any chips and relubricate, and do the second pass to the full depth. If it was me, I'd offset the rough passes about .02" then do a final single pass at full depth removing the .02", this usually leaves a nice clean edge.

Here's some videos using a 1/8" spiral-O-flute endmill, at .032"doc and about 30-35ipm:

[ame="http://www.youtube.com/watch?v=mAsp3_uN7SY&feature=plcp"]Home Made CNC cutting aluminum clock gear 1/4" thickness Part 1 - YouTube[/ame]
[ame="http://www.youtube.com/watch?v=HhQ-NL5GGyA&feature=plcp"]Milling Harley-Davidson logo out of 1/4" aluminum, part 3 - YouTube[/ame]
[ame="http://www.youtube.com/watch?v=rOPxB6yX_SI&feature=plcp"]Home Made CNC Router Milling Aluminum, Celtic Cross Part 2: Profile! - YouTube[/ame]

[warrenb]

Did I read you right? You have a .5mm stepdown?

Add a stepover of 3mm per step down. Then one final clean up pass of about .1mm full depth.

Your cutter and the chips just don't have anywhere to go as it's getting whipped around in that deep slot. The stepover will help with that.

Hi.

Been running my diy router for about 6 months now, and it performs perfectly in most situations.

I had a guy approach me last week asking to have house numbers cut out of alu. I took the challenge and have started experimenting with light cuts in a piece of scrap.

I've been trying to do a profile cut in the full depth of the material (15mm, .6in) and there are no problems until I almost cut through (about 12mm in I guess), then I get alot of chatter and vibrations and have to shut down. It seems like it might be due to buildup of chips.

The bit is a 6mm 2 flute end mill. Running at 12000 rpm and 120mm/sec feed rate taking 0,5mm cuts. Have tried several different settings but seem to churn out the same result every time. For coolant and chip clearing I use CRC (ie. WD40) and compressed air. Not sure what spec the alu is.

Any suggestions what I might try next?