Questions on using a moving gantry style mini-mill...

[Davek0974]

Getting near the end of my router/mini-mill build now and need to start looking at how to run jobs, i have a couple lined up already;)

I'm not new to milling - been running a Bridgeport for some years now, not new to CNC - been using a plasma table for a year now, so that should all help. I use SheetCam to produce my G-Code and I think I have it pretty much sussed for the mill now, just looking for tips.

This is the first job - pretty complex but what better way to learn;)

It's from 5mm 6061 Aluminium, has plenty of 3mm holes, slots, square features, its about 320mm long.

So far I am looking at using a 2mm carbide 2-flute cutter, mist coolant, I have figured out how to get sharp corners, also how to spiral-down to cut the holes.

Questions -

1 - I have used a calculator for feeds and got 24,000rpm, 487mm/min feed, 1mm DOC, these seem reasonable?

2 - I am unsure of DOC - this is input rather than output on the feed calculator - how do you know how much bite to take at one pass?

3 - Holding tabs to keep it together on the outside cuts, I'm guessing three or four, 0.5mm thick or less?

4 - Use the one cutter and go straight to dimension or split and do a roughing & finish passes?

5 - Use a bigger cutter for the roughing outside then switch to the 2mm for the finish?

6 - Features like the oval hole - leave it to fall out or use tabs again?

Any suggestions appreciated, I realise this is fairly adventurous but I would like to get these made in-house to increase my profit margin considerably ;)

Thanks

[Clive S]

How are you going to do the 90' corners?

[Davek0974]

How are you going to do the 90' corners?

There is a tool-path option in SheetCam that runs the cutter diagonally into the corner just enough to allow the resulting corner to accept a square cut object - a neat feature and with a 2mm cutter its barely noticeable.

[routercnc]

Hi Dave,

Taking each point in turn:

#1 Only ever used a 3mm carbide, nothing smaller. I think it would snap on my machine at those rates but possibly depends on how rigid your machine is.

#2 DOC for 3mm carbide has been about 0.3mm for me. It's quite possible I'm shortening it's life doing this but it works well but I only use it occasionally and it's still going strong.

#3 I'd use 4 holding tabs. Now in Vectric Cut2D the thickness is relative to the bottom of the cut. For that cut I would ask for 6mm total depth to make sure it went right through. Therefore 0.5mm tab would not actually hold the part and I'd need to input a tab depth of 1.5mm to get 0.5mm. I think I'd go for at least 2mm tab to make sure it did not vibrate on the last finish pass.

#4 If the part is complex (long run time, chance of an e-stop or other problem) then I'd do a roughing cut leaving 0.1mm for the outside as a finish cut.

#5 I would not attempt all that with 2mm cutter! Use 6mm or 8mm if possible to cut most of it out, then finish pass with the same bit, then go in again with the 2mm for the detail.

#6 Don't leave the oval hole as a free cut. When the cutter gets to the end the oval part will jam against the bit and mark the work, then fly across the workshop. AMHIK.
You can use tabs, but it is a pain to clean up by hand inside there, so better still is "pocket" it out (turn it all to swarf).

As a strategy I think I would:
Spot all the holes (leave finishing for the drill press)
Pocket out all the internal holes and slots (i.e. not an internal profile)
Rough profile the exterior with 6 or 8mm carbide, leaving 0.1mm
Finish profile the exterior with 6 or 8mm carbide in one full depth pass (but still use same tabs as when roughing)
Switch to 2mm cutter and profile the outside again to get the detail then profile the inside of the pockets
Cut away the tabs and tidy up the edges by hand

[Davek0974]

As a strategy I think I would:
Spot all the holes (leave finishing for the drill press)
Pocket out all the internal holes and slots (i.e. not an internal profile)
Rough profile the exterior with 6 or 8mm carbide, leaving 0.1mm
Finish profile the exterior with 6 or 8mm carbide in one full depth pass (but still use same tabs as when roughing)
Switch to 2mm cutter and profile the outside again to get the detail then profile the inside of the pockets
Cut away the tabs and tidy up the edges by hand

Thanks for that, interesting stuff, my response...

I really don't want to drill the final holes, IMHO, spiralling down should work ok, will need to test it.

Pocketing out the waste - brilliant point, probably never have thought of that one;)

Rough profile exterior - makes sense but favour a 6mm rather than going bigger.

Finish profile exterior with big cutter - if its only got 0.1mm to go, I'm not sure of the point, a 2mm solid carbide should handle that in one pass AFIK - test again.

The smaller internal shape/pocket would need a smaller roughing cutter, probably 4mm, why not go to finish on the same tool?

Tabs are the same in Sheetcam, bottom upwards. So if i have an aluminium bed, I would not want to request a 6mm cut on a 5mm sheet, I was thinking of using a sheet of stiff card or some-such between, I use a lot of 0.4mm hard card at work and that would likely work well, cut would then go to work plus 0.2mm.

I'm generally against babying cutters, on the Bridgeport I find they are happier when taking a proper cut, within the abilities of the machine, but not tickling the metal, especially with carbide which has a larger edge radius than HSS and needs to 'cut' the metal.

Some good points though, noted, thanks

[JAZZCNC]

#1 With cutters less than 3mm I work on 30% diameter DOC.

#3 Wouldn't use tabs I'd use Onion Skin of 0.1mm. This gets rid of any chance of bed damage and removes risk of lifting.

#4 Rough and Finish passes. I'd use Large tool for Pocketing and Roughing then use small tool for Finish pass and corners cleanup etc.

[CharlieRam]

Glad it helped, If you drill the holes first, then do the pockets and outer profile, m00 etc. would that reduce tool changes?

[Davek0974]

Not this time because the holes need the 2mm tool to get the sharp corners I need.

It works pretty smooth though, the 2010 tool-change routine is fantastic and a big help.


Of course, with a tool-changer........

[lucan07]

Already planning Version 2.0?

[Davek0974]

Not yet, but in the couple of years since building my first CNC plasma table, I have started to realise how cool CNC machines really are ;)

Tool-changer spindles are a bit £££££