[alank2]

Hi,

I hope this is the right forum to ask. I'm going to cut my first fixture using a microcarve MV3. I've got a cheap HF router on it (28K rpm) with a 1/8" carbide spiral bit. I will be cutting 1/2" plywood in multiple layers (0.1" at a time).

The main square is to hold a plastic enclosure. The top and bottom squares are finger grooves for case removal. The left and right pecks and to mount toggle clamps, and the corner holes are for a 1/4-20 bolt to mount it to the table.

Any recommendation on the feed rate and plunge rate? Is 0.1" per pass a good number to use?



Thanks,

Alan

[spoiledbrat]

Alan, as for the feed/speed, I stand ready to be educated along side you. I would currently run that at 0.0625 depth per cut, 150 ipm.

I would advise you to completely pocket the 1/4-20 clearance holes if there is a remnant left inside, otherwise, looks good.

So, anyone have that feed/speed recommendation?

Rob

[ger21]

.1" per pass is fine for a 1/8" tool in plywood. However, I'd probably start at .0625 first to get a feel for the machine.
28K rpm is really far higher than you need, and taking shallower cuts will also keep the tool cooler.

Your spindle and machine rigidity will typically be the limiting factor when it comes to feedrate. If the machine is up to it, you can cut up to 300ipm if you have a good, sharp bit.

I'd use 15,000 rpm and 125ipm as a starting point.

[alank2]

Hi Gerry,

I'm limited to 28K right now, but I have a SuperPID on the way and when it arrives I can slow the router down.

I had my mach3 driver speed set at 45K and was getting a wierd lockup where the steppers would stop with a loud noise during high speed movement. I set it back to 25K and it seems to have solved that - any ideas why?

Thanks,

Alan

[louieatienza]

Alan, as for the feed/speed, I stand ready to be educated along side you. I would currently run that at 0.0625 depth per cut, 150 ipm.

I would advise you to completely pocket the 1/4-20 clearance holes if there is a remnant left inside, otherwise, looks good.

So, anyone have that feed/speed recommendation?

Rob

I would agree that the slug in the rectangular pocket may bind and cause your bit to break, unless you either pocket it out (looks small enough) or affix it to you spoilboard (via screw on center) or raise the work and allow the slug to drop down.

Rob, I think your beast of a machine can make quick work of this, with at least .125"doc...

Alan, I'd make test cuts starting at .063", though 125ipm sounds a bit fast for the microcarve screws, unless you have multi-start scrwes (most I've seen have single start screws). Anyway, make test cuts at the highest speed that yields a clean edge, then make more test cuts in .016" increments till the cut quality suffers or you break your bit! Then back off about .016". The bit woll heat up regardless of cut depth since it will be "rubbing" in the kerf walls as you go down, which will heat it up and cause it to wear faster. Pocketing the hole out may make it easier on your bit and router; also ramp into the work if you can rather than plunge.

[alank2]

Hi,

I would agree that the slug in the rectangular pocket may bind and cause your bit to break, unless you either pocket it out (looks small enough) or affix it to you spoilboard (via screw on center) or raise the work and allow the slug to drop down.

I've cut a few squares for testing and so far I haven't had any binding issues even when the item in the center breaks free. I think my router cuts clockwise and I have been cutting in a clockwise direction - not sure if that matters. Can it really bind and break? Why wouldn't it just cut anything that runs into it? This is a 1/8" spiral bit...

Thanks,

Alan

[louieatienza]

Hi,



I've cut a few squares for testing and so far I haven't had any binding issues even when the item in the center breaks free. I think my router cuts clockwise and I have been cutting in a clockwise direction - not sure if that matters. Can it really bind and break? Why wouldn't it just cut anything that runs into it? This is a 1/8" spiral bit...

Thanks,

Alan

I ask that question everytime I look into a pile of 1/4", 3/8" and even 1/2" solid carbide bits and endmills that have broken, snapped off, etc. I use spiral bits as well. The bit can potentially "catch" the grain on the slug, rotating or pulling it as the axes move, causing the bit to bind, potentially stalling the router, and with the mechanical advantage of the leadscrews, actually snap the bit. At the very least, the "kickback" from the bit into the slug can "bend" the bit into the pocket wall, putting a "divot" there. I've had a wall outlet MELT because a bit got jammed from a slug (OK it was G10, very hard and abrasive) and the router was fighting it to the bitter end (I hit the stop button).

[ger21]

I ask that question everytime I look into a pile of 1/4", 3/8" and even 1/2" solid carbide bits and endmills that have broken, snapped off, etc

I on the other hand, can count on one hand the bit's I've broken in 15 years of cutting wood.

Not counting, of course, accidentally cutting into hardened steel at 400ipm.

I've never had a "slug" break a bit, and I never pocket when I just need a hole. But, I don't use 1/8" bits all that often.

The bit will heat up regardless of cut depth since it will be "rubbing" in the kerf walls as you go down, which will heat it up and cause it to wear faster

I don't really buy that "rubbing" theory. With small tools, deeper cuts will leave far more chips packed into the cut, which creates a ton of heat. Especially at 28K. Shallow cuts will cut much cooler.

[louieatienza]

I on the other hand, can count on one hand the bit's I've broken in 15 years of cutting wood.

Not counting, of course, accidentally cutting into hardened steel at 400ipm.

I've never had a "slug" break a bit, and I never pocket when I just need a hole. But, I don't use 1/8" bits all that often.


I don't really buy that "rubbing" theory. With small tools, deeper cuts will leave far more chips packed into the cut, which creates a ton of heat. Especially at 28K. Shallow cuts will cut much cooler.

Knock on... er...

Granted it's not a huge pile. And I've cut everything from aluminum to mild steel to G10 Garolite from 3/8" to 1-1/4". Four bits were from the same manufacturer, same bit; one broke at the fadeout, on another the cutting edges just shattered... using the manufacturer's recommended chipload and SFM. I was fortunate that the manufacturer actually replaced ALL FOUR bits - at a retail value of $2480! Most of the broken ones were from running into nails in my spoilboard (I stopped pinning my stuff down because of this), clamps, screws, running through a screw or nail at 750ipm... dumb things one does at 3AM, which seems to be the only free time I have to run my machine.

As for the deeper cuts, I've been using single edge spiral-O bits whenever possible for 1/8" and 1/16" profile cuts. From my observations, unless you blow the kerf out with air, taking too shallow a cut just makes finer dust which packs into the bottom of the kerf anyway, whereas the "larger" chips seem to get thrown out of the kerf more or less. I do use dust collection which helps somewhat, but even then I'll blow air into the kerf to clear it as my dust shield allows this.

On some pieces where I don't have a second chance, I've even created multiple offsets a small distance like .02" or so equal to the number of steps down, and start from the furthest from the cut line and manually increase the doc toward the last pass, so I'm stepping down AND in to the cut line. I believe MasterCAM can do this automatically.

[BanduraMaker]

I on the other hand, can count on one hand the bit's I've broken in 15 years of cutting wood.

Hmmm... two in one year for me. That means I've only got three left for the next 14...assuming no table saw accidents!