Aluminum cutting and tabs

Cutting 6061 3.175 mm (1/8th inch) aluminum sheet. Making parts rather than carving things… Some posts here say cut really fast like 1250 mm/min (50 inches/min) and doc of .25 mm (.010 inches). Really aggressive. Does work. Less chatter. Pathways stay clearer. Others say start at more like 1/2 that speed and 1/2 that doc. Say they are getting consistent results. Could be more reliable. Its a bit confusing, so interested in hearing again what everyone has experienced.

But my question is really about tabs. Not much discussion that I can find here on tabs.

With all my plastic cutting I steered clear of tabs. Haven’t had a cut where it was really needed. But with aluminum, and the bit moving at these speeds, I keep breaking carbide bits because a cutout will come loose, and get in the way of the bit, which at that speed, shatters it.

So now I am experimenting with tabs to keep the cutouts from causing this problem. Of course tabs generate additional work. You have to cut the piece out, and then grind the remainder of the tab off.
I would like to minimize that work. Does anyone have any advice on the thickness, length and frequency of tabs in 6061 to hold the cutouts in place? I am trying .5mm thick and 5mm long, seems to work, but sometimes a tab isn’t cut for some reason. Maybe due to the flatness of the bed…

Also a note on cut depth. I am using VCarve Pro to generate my g-code. I found that setting the cut depth the same as the material thickness often left sections that are not completely cut through. Definitely a problem in metal, not such a big deal in plastic… This would be due to the X-carve not being completely flat and true… What I have worked out in VCarve, is if I set the cut depth a small amount (.375 mm) greater than the thickness, then it will do a couple extra passes, which insures that the entire piece is cut through. But this also seems to negate the tabs. Seems like you have to add this extra to the tab thickness, like VCarve is calculating the tab thickness based on the cut depth rather than the material thickness… Does that sound true?

Anyone have a tried and true combination of tabs and 6061 sheet cutting?

On the parts I cut out, if there are internal holes in the parts I cut the holes first then secure the piece with screws into the wasteboard so no tabs are needed. If your parts allow that I recommend it.

1 Like

In general you want to aim for a certain chip thickness per tooth.
You control that by three factors, RPM, Feed rate and number of teeth.

For a 1/8" bit (1F) you could try to aim for:
18k RPM and 450mm/min per flute (=> 2 flute = about 900mm/min etc)
Try a depth per cut = 0.5mm

The weak link with aluminium cutting is machine rigidity.

Tabs, how large are your pieces?
I have machined a fair bit of aluminium using only maskin tape/CA glue which work surprisingly well.
But how viable that is decend on the size of the part (surface area).

Eriks suggestion is a good one.

Consider setting your Z axis using your wasteboard as a reference on through cuts. If your gcode is set to cut 12.7mm deep, set your wasteboard at -12.71mm.

1 Like

If you are setting your depth extra adjust tab thickness accordingly.
Best practice is to place your material on a leveled waste board.
All good advise above.

Cutting the tabs and cleaning up the edges is a pain in the butt with aluminum.

I do a fair amount of work with 1/8 and 1/4 inch aluminum plate. I prefer to use the masking tape / cyanocrylate glue method, but I adhere the aluminum to a piece of 1/8 inch MDF cut to the same dimensions as the aluminum plate and then clamp that to the wasteboard. Easy peasey, no tabs needed.

Good advice.
I do the same for through cuts, establish surface height and then jog up to a known distance, say 13mm for 12,7mm material I simply make the carve 13mm deep.

With a little attention I can carve through one of the masking tape layers and leave the bottom layer intact :wink:

1 Like

Thanks all! Great help on all points. I did not know about the masking tape/super glue technique. Much better idea than using tabs! Going to give that a shot. Really appreciate everyone’s help!

1 Like