It's begun....

[Washout]

Update:

I finished cutting my first part today after a bit of trial and a fair bit of error.

The part was a replacement gantry mounting bracket, which I had hand cut originally and thought I would get something a little more precise on the machine. I am using 15mm thick 6082 T651 Ali.

Firstly I quickly ran up the part on Vectric's Cut 2D and placed 8x5mm through holes to fix to the bearing blocks and 4x6mm holes with 4mm deep and 11.5mm dia counterbores, which fix to the bottom of the gantry. The previous mishap when drilling holes in extrusion meant I was out of 5mm carbide end mills, so opted for a 4mm carbide 3 flute which was running at 18,000 rpm 0.5mm DOC, 750m/min feed and 515m/min plunge (these were suggested by GWizard). The cuts were inside edge profiles, so spiral cutting.

This operation ran fine with no mishaps.

Then I modelled an outside profile cut to cut the part from the plate, using a 6mm end mill and tried 10,000 rpm, 0.8mm DOC, 750 m/min feed, 515 m/min plunge.

This ran fine until it got to ~10mm into the material and then the tool bogged down (probably on chips), went a little hysterical where it was stuck and before I could hit the estop. Once I had bought the spindle to a rest I figured it was another stepper/driver glitch and looking at the tool it appeared to be fine with no gummed up ali on it. So I rewound the job and started again. This time, once the job had reached material it ran fine for a couple of cycles and then again bogged down, and jammed, then snapped the tool.

I was using WD40 every so often and also using my airbrush to try and clear the chips, which was only partially successful and looking back on it I reckon the tool got bogged down in chips in the slot and this caused the jam/snapped tool.

So I figured I would tone stuff down and with Jazz's advice on feeds and speeds in previous posts, tried again with an 8mm end mill and this time used the airbrush exclusively, with some coolant to act as a mister. I also reran GWizard and with this time tried 12165 rpm, 0.2mm DOC, a 750m/min feed and 250m/mm plunge (although this time I opted for a ramp rather than stright plunge). I found the conservative/aggressive slider this time in GWizard and went for the former.

This time the job completed without mishap, but I do need to do a few things in the future and the first of those is to rig up the airbrush/mister so its on constantly rather than me chasing the tool around and trying not to tangle the airline from the compressor.

I do have chatter lines on the sides of the job, so I think I will have to bite the bullet and retro-fit a second ballscrew on the x axis, which should help with this.

I did a quick check over of the machine when I was done and the X and Y locking nuts had come loose. Not sure the set screws/grub screws are man enough for the job. so will have to think about solving that as I don't want one of the ballscrews breaking free or breaking the coupler. I was thinking about replacing the helical cut ones with the interlocking kind (don't know the name for them but have seen them on various sites).

Also my PC is far enough away from the machine that its a pain to have to keep going backwards and forwards if I want to feedhold and restart, but I'll likely live with it until I move home in the next week or so.

Once I have got a better hang of feeds and speeds and the new ballscrew in I think I'll have a go at cutting some gantry sides out of plate as well, although I'm eager to have a crack at something not fo rthe machine itself....

More to come...


Chris

[Jonathan]

0.2mm DOC is disappointing. 12165rpm sounds a bit fast for an 8mm carbide cutter in aluminium. I use around 9800rpm (600mm/min, 1.5 DOC,8mm single flute). Looks like that was a 3 flute cutter since you've set the plunge to a third of feedrate which is what Gwizard suggests? If so then 750mm/min is slow, you wont be getting a big enough chipload. Use more like 1800mm/min if it's 3 flute.

If you want a quick way of guessing the feeds and speeds then scale it proportionately off one you know works. For instance I know that 9800rpm, 600mm/min, 1.5 DOC works well with the 8mm single flute, so if I used a 2 flute cutter I would just use twice the feedrate (1200mm/min), as its got twice the number of flutes and maybe decrease the depth of cut to reduce the force on the cutter. Using that logic, your 4mm 3fl should be run at 19600rpm and 1800mm/min...clearly this isn't the most accurate way to determine the settings, but it's a good start.

Sounds like you're describing and oldham coupling. They're pretty good, but you should be able to mount the motor accurately enough to use a solid coupling.

You could try using a finishing pass to eliminate the chatter marks - just take off 0.1-0.2mm at full depth.