Cutting a 3/16" groove in melamine. What bit and feeds?

[ed_lang]

I have a job pending that seems quite easy. I need to cut a 3/16" groove, 3/16" deep offset in from the outside by 2.5" on 47 doors.

I have never cut melamine and hope to get some samples to try before cutting the real job.

What bit should I get and what feeds would be good for starting?

[richards]

I use a down-cut spiral to minimize chipout. Be sure to drill, not ramp, into the cut. Ramping in melamine causes chipping. Drilling melamine is hard on cutters, so be prepared to replace cutters more often than you would have to if you could plunge to depth off the sheet and then move into the cut from the side instead of drilling. I've had good results using White Side cutters - which are normally available locally. Freud and CMT cutters tend to scream too much. Onsrud are my first choice, but they're not always in stock locally.

I don't cut many 3/16-inch grooves, but when I cut 1/4-inch grooves for drawer bottoms, I use about 8-ips on the x & y axes and about 0.75-ips on the z-axis. Spindle speed is determined by chip load, but I usually run somewhere around 13,000 rpm and then change the speed until the cutter sounds right and the chips feel right.

[paco]

Yes,

downcut for this kind of groove or straight edge carbide tipped (real sharp)... but I prefer compression (2 flutes) for cutting out (both sides perfect) in two pass for 1/4" CED or single for 3/8" and 1/2" CED. Mortising compression have a 3/16" high up cut length...

I'd say test straight edge carbide tipped first to see if it meet your needs; they're cheaper, readily available and do the job until they get dull.

3/16" CED tool; you'll be at max cutting length (generaly 3/4" CEL) from most model available...

Maybe you can figure those "special" grooves with the hand help router (JIG and 3/16 down cut bit)... while the Bot cut your part with a more appropriate "production" tool bit...?

[richards]

Ed, I assumed that you were cutting a 3/16-inch deep groove in 3/4-inch thick material when I suggested a spiral down cutter.

If cutting all the way through the material in one pass, follow Paco's suggestion and use a compression cutter. However, if you're cutting all the way through thin material, you'll be cutting deep into the spoil board if you want the transition point of the up/down cutter centered in the material.

[ed_lang]

The customer has doors and drawers for a total of 47 pcs. He wants the groove cut 2 or 2.5" in from the edge, 3/16" wide and 3/16" deep to break up the solid surface. These are mounted and have been in use for a few years. He will pay to unmount and remove all hardware. I'll get just doors and drawer fronts.

I spoke with him today and he is OK for me to "test" on the back of the door in case it gets some chip out.

I told him $10 per part. Door or drawer it didn't matter. He was OK with that. I must have been too cheap.

I have 4 3/16" 1/4" shank straight single flute cutters on order so I'll try them out.

[ed_lang]

I did try the 3/16" straight single flute cutters and didn't like the little chip here and there. I am going to try the down spiral cutters next.

I am glad this guy is in no hurry.

[ed_lang]

The 3/16" down spiral bits did a perfect job!

1600 rpm on the router and 3 ips.

[gerald_d]

Maybe 16000?

[ed_lang]

Yes, 16K not 1.6K.

Can you tell I was happy to get a good cut?

[gerald_d]

Yep, down-spirals are excellent for this application.

[odulfst]

is 10$ too cheap? what is some standard pricing? has there been a thred about what people normally charge for man/bot hours?

[pierre_wessels]

Located in Vancouver BC,
I use $60/hr + material cost. Minimum 1 hour charge and I have never been told that it was unreasonable. I use the same rate for both cutting and programing. I actually feel that I could probably charge more without resistance. I do have a good day job so I have the luxury of turning away things that I am not interested in doing.
Pierre