It's begun....

[JAZZCNC]

After zeroing you can go on to MDI, raise the tool up obviously, type G0 X2.5 Y2.5 and zero the axes again. Assuming you zeroed both in the positive direction, the machine is now zeroed.

Even easier way than that if your using the default 1024 screen set. First set the Safe Z in Config (which you really should do for safety reasons regardless) and make sure it works in Work coordinates.
Then all you have to do is type the offset (-2.5 in your case) direct into the X,Y DRO by clicking on each DRO (Must press Enter to apply it) then simply clicking GOTO ZERO button just below DRO's.
You will still need to have the Z axis Zero set equal to the top or above material. The Z axis will retract first to Machine Zero coords because of SAFE Z then move the X,Y axis then return Z axis to Zero work coords.

[Washout]

Perfect - thanks for that - more like Excel/Word rather than Lotus123/Wordperfect :-)

Chris

[Washout]

Thanks for that,

The new interface is much cleaner and I especially like the new jog tab rather than the old one hiding most of the DROs.

I've now had the machine cut the holes to attach its bed extrusions to the frame and it did that really well apart from on mishap where for some reason the mchine decided it was going to rapid and ramp to the first drilling spot. It made a nice gouge in the extrusion before I realised what was happening and hit my e-stop (which worked perfectly). I didn't snap the tool which is a blessing and I guess the 5mm carbide end mill went into the material by about 4mm before I caught it. A quick reset and zero and all was well , so not quite sure what happened as it had just cut the countbores on a seperate G-Code job before hand.

Anyway after resetting and cutting a bunch of holes to finish the bed without mishap, I have just "air cut" my first 3D part and it seemed to work OK. I do have another question though:

I'm using GWizard to help with feeds and speeds and for the drilling operations and counterbores the 18,000rpm, 750mm/min feed and 515 plunge rate GWizard suggested seemed to work really well. For the 3D roughing operation I'm about to try I'm using an 8mm Carbide End mill (3flute) and it is suggesting 13,000rpm, 2,000 mm/min and 750 plunge - does this sound right guys, as it seems to be very aggressive?

If there is ever a UK CNC meet up, I am going to owe you guys a small brewery.....

Cheers


Chris

[JAZZCNC]

Anyway after resetting and cutting a bunch of holes to finish the bed without mishap, I have just "air cut" my first 3D part and it seemed to work OK. I do have another question though:

I'm using GWizard to help with feeds and speeds and for the drilling operations and counterbores the 18,000rpm, 750mm/min feed and 515 plunge rate GWizard suggested seemed to work really well. For the 3D roughing operation I'm about to try I'm using an 8mm Carbide End mill (3flute) and it is suggesting 13,000rpm, 2,000 mm/min and 750 plunge - does this sound right guys, as it seems to be very aggressive?

Can't answer really without knowing material, DOC.

Warning thou regards G-wizzard.? The calcs are based on using a milling machine which is much stronger than what you'll probably be using so I'd always knock a bit off to account for this.! How much mostly depends on your machine but 25% would be a good safe start.

[Washout]

Ah yes DOC - I tried a 1mm and 3mm DOC and its 6082 T651 Ali

[JAZZCNC]

Ah yes DOC - I tried a 1mm and 3mm DOC and its 6082 T651 Ali

You'll need a very strong machine with powerful spindle to cut at 3mm DOC and those feed rates Gwiz suggested with 8mm cutter.

Try 1mm @ 800mm/min 10,000rpm and take it from there.!!. . . . I cut @2.5-3mm Doc @800mm/min 9-10,000 rpm 8mm 3 flute ripper using blown air.
Each machine is different so you'll need to play with settings to find the sweet spot for yours. If you push too hard to start with you'll just cause premature wear and possible damage machine so start off easy with DOC and Feed rate then use the Feed override to change feed rate on the fly while cutting, also play with spindle rpm has well.
By doing this you'll find the sweet spot quicker and get the best finish and tool wear.

[Washout]

Thanks,

I thought that was a little aggressive - I'm not too fussed about the length of the job (or at least won't be once I have my mist working and don't have to stand there puffing WD40 at the tool and brushing chips away for hours). I'll report back with results and must get some pics or video up.

Cheers


Chris

[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.

[Washout]

Thanks for the feedback Jonathan,

I went a bit shy on the DOC on the 8mm, after breaking the 6mm earlier and you're right it was 3 flute. I have the other mounting bracket to do tomorrow, so I'll pluck up the courage to up the feed rate, but I'm a bit wary of the sturdiness of my machine until I get that 2nd ballscrew on, so maybe a lighter DOC than 1.5mm (that and get an order in for more end mills ;-) ).

Another thing I need to figure out is an estop for the spindle/VFD and two pole that into the big red button for the control box.

For these pieces I'm not fussed about the chatter marks, they were quite light anyway, but a finishing pass will be in order for the other parts I'm making.

Solved my locking nut problem by binning the supplied M4 grub screws and chopping some M4 button head bolts to size (they had hardly any "hex" on the head and seemed to be made of silly putty). Ah yes Oldham Couplings - will go find some now.

Cheers


Chris