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

[JAZZCNC]

What sort (if any) lube/coolant do you use on aluminium? I have enough parts in now to build a pressurised fog-less system but just wondering what people put in them :)

I use WD40 type lube but oil/parafin mix will work.

Back to the CAM, shapes like the odd shaped internal part on my drawing, I have roughed out the bulk with a 5mm tool, that leaves of course 2.5mm rads in all the corners, are you saying to finish cut that with the 2mm tool in one pass?

Yes will be ok in this case because your now side cutting and the tiny amount left won't hurt anything. However it's not recommended to use same size tool as the radius. ie: 2mm Rad use use 1.9mm or smaller Dia tool. This means the tool won't be cutting on two sides in the corner so won't chatter or snag and break the tool. Which can happen on really small tools. Larger tools just usually leave mark in corners and make horrible noise.

Do lead-ins and outs feature or forget them for the minute?

Well they are all part the process really so should happen anyway. For instance you'll ramp into pockets for roughing to safe tool wear but radius arc into the Finish pass if enough room for better finish. If cam program allows I always let the lead out go slightly past the lean In point as well to remove cross over point.

[Davek0974]

Thanks, lead ins and outs pretty much like the plasma then.

Radius makes sense, already use the different rad rule on the Bridgeport as that can get a bit vocal when it wants to;)

Will apply to this as well, I was going 5mm rough and 2mm finish which fits ok i think, don't really want to go below 2mm unless really needed, but there are some features that are 2mm on the job so can't use bigger.

Been researching fluids and seems pretty much anything goes, even Methylated spirits, but paraffin and oil mix seems popular - pretty much WD40 without the waxy residue ;)

New power supply arrived today, will test it out tonight ;)

[JAZZCNC]

Will apply to this as well, I was going 5mm rough and 2mm finish which fits ok i think, don't really want to go below 2mm unless really needed, but there are some features that are 2mm on the job so can't use bigger.

Unless Rad is critical then it's worth changing rad in Cad just 0.1mm makes difference to small tools and in most cases doesn't make jot difference to part. When designing I nearly always make my none critical rad's 0.1mm over size for this reason because most tools I'm using are round numbers.

[Davek0974]

Good point, thanks

[Davek0974]

On the left side of my part in the OP, there are three slotted holes on the diagonal face.

After roughing the outside with a 5mm tool, these will obviously not be cut, but with my plan to finish-pass the outside with the 2mm tool in one pass, this will mean the 2mm tool taking the full depth cut on these features.

Calculator shows speed for finish pass as 996mm/min as it's only taking 0.1mm off but here it shows speed as 380mm/min as full depth slotting cut.

Options -
run all outside at the slower rate,
run outside as multiple pass contouring at the higher rate,
try and get jiggy with path rules / action points in sheet-cam to slow down in that area,
something else??

[Ger21]

Rough cut the 3 slots in multiple passes before making your full depth perimeter cut.

[Davek0974]

But how to just rough the 3 slots?

They are 2mm wide with a 3mm loop at the base, I was going to go in with the 2mm finish tool.

Is it as simple as defining a second pre-finish pass with the 2mm tool but still leaving the same allowance after?
But then that would not fit into the slot as its 2mm tool in a 2mm slot + 2 x 0.1mm allowance.

Or are we saying go down to smaller tool?