Routing metal

[cxixer]

OK, I know it's not a good idea to cut most metal with a router. I have a few questions about it though.

A customer wants pieces cut out of up to 1/4" aluminum, up to 1/2" acrylic, and possibly 1/32" stainless.

I know my 4x4 router (PC690) could run through the acrylic. I've been cutting acrylic and polycarbonate with routers for a while before I got this CNC.

Would I need any special bit to cut the 1/4" 6061 aluminum, or could i use my normal 1/4" spiral upcut carbide bits? What is the recommended pass depth and feedrate?

Would it be possible, and what depth for 1/32" stainless steel? I've cut other sheet metals with a router, but stainless is a pretty dense metal.
Recommended pass depth and feedrate?

Thanks in advance!

[ger21]

The aluminum should cut OK, as long as the tool is sharp. not sure on the depth and feedrate though. I can't imagine that you'll be able to cut the stainless, though. If you manage to pull it off, let us know how you did it.

[Geof]

It does depend on your rpm but with a router you are probably at 20,000 plus. On the aluminum you could probably go full depth at a feed of anything up to 150 ipm....but I would start at less than half this just to get a feel. If you want to be more cautious only go 1/8" deep per pass. Coolant/Cutting Fluid is essential otherwise you are likely to get chips clogging the flutes. If you cannot use spraying coolant back off the feed down to maybe 30 or 40 ipm and just paint a line of coolant along the cut line.

Stainless? Don't spend any time trying; you will simply burn grooves in whatever cutter you use, HSS or carbide. Stainless needs slowish rpm and a good feed rate because it work hardens and you need a chip depth deep enough to get under the work hardened surface.

[blackbeard52]

For 12 years I managed a corporation that used a t690 for routing all sorts of metals, composites and the like, as a matter of fact we were tasked with finding a way to cut and test Kevlar when it was first introduced.. We used a standard straight 2 flute carbide on most materials. Three flute on some of the harder stuff. However to accomplish our end result we did take small cuts and used templates in the late 80's and mid nineties...hard to believe the Porter Cable t690 has been around that long. We manufactured tensile preparation equipment and the 690 was our spindle of choice. Having said that I dont have much faith in plunge cutting but edge cutting is certainly a possibility. I can attest to the fact that single flute is out in all cases except very soft poly. As far as I know they still use that motor today even on the CNC version I designed before I left the company in 1997....Enough rambling... I guess I made my point

[cxixer]

Originally Posted by Geof It does depend on your rpm but with a router you are probably at 20,000 plus. On the aluminum you could probably go full depth at a feed of anything up to 150 ipm....but I would start at less than half this just to get a feel. If you want to be more cautious only go 1/8" deep per pass. Coolant/Cutting Fluid is essential otherwise you are likely to get chips clogging the flutes. If you cannot use spraying coolant back off the feed down to maybe 30 or 40 ipm and just paint a line of coolant along the cut line.

1/4" Aluminum? Full Depth? 150ipm? Holy Crap!

Is there something I don't know about aluminum? MDF would crap out my router at that speed... or depth.. let alone both!

[Geof]

Originally Posted by cxixer 1/4" Aluminum? Full Depth? 150ipm? Holy Crap! Is there something I don't know about aluminum? MDF would crap out my router at that speed... or depth.. let alone both!

Well I guess I overlooked that you may not have a 20hp motor driving the cutter.

[cxixer]

Yeah my little home-depot porter cable is one of those "motion of the ocean" kinds of routers.

[dertsap]

ive had good experience on aluminum 0.05 depth at 30-50 ipm with my home setup , it's painfully slow in comparison to a cnc mill but it works
what i find works best is to always use a ramp around the profile ,this way the tool has a constant pressure on it and will have less chance of deviations due to the machine not being quite so rigid

normally i'll use a 3/8 or 1/2 " kennametal 4 flt

[Trell]

My first CNC is a POS and it will cut alum. Turn the rmp down slow so you do not get your bit hot, and use oil. I just use Pam Cooking Spray, but everybody thinks I am cooking Chicken. Cut at about .05 to .08 ipm and at .1 inch deep per pass. Use a new .25inch upcut bit It does OK but slow as s..t. As long as your not making NASA rockets it will work
If you try any faster speeds let us know

Use what you have, Not what you wish you had.......

[LeeWay]

My experience is about the same as Dertsap. 40 IPM using a PC690 and a straight 2 flute cutter for sheet or aluminum cutting end mill for thicker stuff. DOC about .05. I spray WD40.
I do think I will be doing this anymore though. I now have my mill running. I really didn't like to see those shiny little chips flying into the router motor. I didn't have any trouble with it, but kept it blown out pretty good.
Oh and she does get mighty warm doing this. I never ran it for more than about 10 minutes at a time.

[Unabiker]

I cut aluminum all day long with a router using an Onsrud single flute cutter with good results. I turn it at 17000-18000 rpm, feed at 85-90 ipm, and use Cool Mist water base coolant. Most of the time, I'm cutting through .080" 6061-T4 sheet in a single pass. I've cut 1/4" stuff in a single pass with no problem. You will need to have a sturdy machine and sturdy hold-down method.
Here's a link to the bits I use:
https://www.onsrud.com/oc/pdf/O_Flut...m_Brochure.pdf

[LeeWay]

What is the horse power of your router? I have a large older Hitachi router that is 3 1/4 HP I think. It might cut 1/4" in one pass, but I know my PC 690 ain't going there. I do cut .063 aluminum sheet with it in a single pass, but thats as deep as she can go without really bogging down. Some bogging is okay with a Universal motor, but there is a point where the torque just falls out and that is bad.