[diacd]

Hello,
i'm sure this has been asked numerous times here, i've been scouring the internet and read several threads here and various technical articles and tool manufacturer tables and data but i find lots of conflicting information about what would be the proper speed and feed for our tool/machine to have decent speeds and tool life/quality and i'm facing some challenges.

This is the hard data:
Tool is 10mm 2-flute compression clockwise rotation (i have from several manufacturers, coated, uncoated, etc), we'll be cutting mainly 18mm MDF/chipboard laminated on both sides in one pass, vacuum hold with spoilboard.
Cuts are done at the same spacing as the tool diameter
Cutting direction is CCW.
We want to cut at a speed no less than 15m/min

Machine software is... not good, the only tool entry method is a linear ramp and i can only configure the length and the descent speed of the tool itself.



Challenges and what i've found so far:

1) On several places i've seen mentioned that for MDF the chipload should be ~0.3 to 0.5, which nets a 15m/min and 15K rpm feedrate, but then reading more tool tables like onsrud's shows a range from 0.35 to 0.58(depending on the model) and says that for 2xD(near enough for 10mm bit on 18mm material) i should lower ~25%, which means the calculated feedrate would be between 8990mm/min(0.29 load post 20% reduction) to 14260mm/min (0.46 load) at 15500rpm.
Then i checked Amana tools and their tool data for vectric and it only shows a paltry 5m/min advance at 18k rpm

Curently i'm running at 15m/15.5K

The first bit we installed we ran at 18K RPM and 16m/min advance and it lasted for ~130 boards cut(4 days of work at the most), but it showed signs of significant heat damage with crusted carbonized deposits so i'm wary of running the new one at 18k rpm as well.

I also don't want to go much higher on the feed as it leads to small piece shift due to increased shear force and the level of vacuum the machine has, it's already happened several times.

2) i'm also encountering chipping at the entry point on both sides of the entry point, currently by default machine is set for a 70mm long ramp at the default plunge of 2000 mm/min, i've changed to 3000 and it made no noticeable difference.
I've been suggested to set the plunge to 2xD and the speed to equal the feedrate in facebook, is that correct?


any input is appreciated.

[Todd Zuercher]

I've been setting up milling tool paths for nested MDF sheet milling for 20yrs and what I've found doesn't really conflict with anything you've stated above. Choosing feed rates and chip loads is always going to be a compromise. With faster higher chiploads giving better tool life at the expense of finish quality and on the flip side slower smaller chip loads generally giving better finish results at the expense of shorter tool life. The chip loads in the manufacturer's charts are guidelines to be used as starting points for experimentation.

Pushing the upper limits of chiploads are also going to risk tool breakage. This is especially true for deeper cuts. (Hence Onsrude's recommendation of a 25% reduction for 2x depth) You do seem to be trying to push the upper limits of chip load. Your 15m/m@15krpm is right at the upper edge of Onsrude's recomendation. However if you are not having trouble with edge finish, tool breakage, or work holding, go for it and maybe even push it further.

As to your tool life results, they seem like about what I would expect. MDF is extremely abrasive and wears out carbide tools very fast. We typically mill 3/4" MDF with either a 1/4" 2 flute carbide down spiral (single pass, 200ipm@17krpm) or a 1/2" PCD compression single flute (single pass, 300ipm@16krpm).

The 1/4" bits only last for about 500m of linear cutting, but they give us much less wasted material, and allow us to cut out very small items without moving by packing the dust into the milled slot. I can mill out objects with surface areas of only a few square inches without worry of them flying off the table, so long as there is at least about a 1/2" wide frame of scrap material surrounding them. Pieces larger than about 16 square inches need no surrounding framework, and can be milled with overlapping tool paths for maximum yield.

The half inch PCD diamond compression bits, will last us for about 4 months of running 24 hr shifts 5 days a week (vs about one shift for the 1/4" tool.) They don't cut as nice as a fresh new carbide tool, but they are as good or better than a carbide tool that has made a couple of runs. The big down side to the larger PCD tool is that it requires much stronger work holding to prevent part movement, because of higher cutting loads. Typically pieces must have surface areas greater than about 2feet to be able to reliably hold them.

Is your 10mm tool an up spiral or down spiral? An up spiral will typically give about double (or better) the life of a down spiral tool, when milling on a fall board, because of the lack of chip evacuation. However it can be much more difficult to hold parts down. An up spiral will have trouble with chipping the top edge when it is getting dull. Where as the down spiral will struggle with chipping the bottom edge, but have far fewer problems with part hold down.

Chipping at bottom at only the ramp in point will be exacerbated by a badly worn fall board. It is best to have the tool set to only just cut through the material and barely leave a mark. A problem I struggle with is as the tool gets too dull it stops cutting all of the way through, and pushes a skin down into the fall board. Well the machine operators see this and automatically think the tool depth needs lowered instead of replacing the worn tool. When they lower the tool it cuts a deeper groove in the fall board, and soon the skin comes back and leads to chipping on the bottom edge.

[routalot]

If the laminate on the faces of the sheet is melamine,the spoilboard needs to have a good surface.An aggressive feed rate on a grooved and worn spoilboard is likely to lead to a small patch of melamine over a groove breaking out.PCD will last much longer than TCT and I haven't found a huge improvement with compression cutters compared to sharp straight equivalents.

[ger21]

The first bit we installed we ran at 18K RPM and 16m/min advance and it lasted for ~130 boards cut(4 days of work at the most), but it showed signs of significant heat damage with crusted carbonized deposits so i'm wary of running the new one at 18k rpm as well.

I would consider this to be completely normal. Router bits are consumables, and their cost should be figured into your product. At 130 sheets, that's less then $1 per sheet. If you get the bits sharpened, the cost goes even lower. You should be able to get a 10mm tool sharpened 1-2 times, if it doesn't get too worn. I've found MDF to dull tools quickly, but it does not damage the tool nearly as much as particle board does.
We use larger, 1/2" tools (12mm), and cut at 25m/min at 17,000 rpm.

Machine software is... not good, the only tool entry method is a linear ramp and i can only configure the length and the descent speed of the tool itself

With this limitation, you are going to have a difficult time avoiding chipping during entry. You really need to ramp in away from the part, or the upcut portion of the compression bit will always chip during entry. I';d also recommend leaving a slightly larger gap between parts, or the climb cut side may cause chipping when cutting adjacent parts. With a little extra gap (even 1-1.5mm), most if not all of this chipping will be removed.

[routalot]

I tend to use no more that 12 metres/minute on melamine faced chipboard with a 10mm tool as a nested sheet often contains small components that might move with a more aggressive rate and the alternative of adding tabs,then cleaning them off takes longer than 3-4 extra minutes per sheet.The gap that works for me is 2mm and the inclusions are very real-screw heads,staples,stones and more have turned up.

[ger21]

For smaller parts, we make a rough onion skin pass, then a finish pass cutting all the way through, with the small parts cut out first. This keeps them from moving around.

[diacd]

Sorry for the delay i've had a lot of issues logging in to this forum.

I've changed our parameters and tools too since my last post:

Tool is 10mm 3-flute straight cut bit, speed is 20m/min at 18K for a CF of .37
Ramp is 40mm long

EGGER recommended us to lower the CF to .3 which resulted in carbonized deposits on the bit and very low durability.

I've also tested a 10mm 2 flute straight PCD cutter at 14m/18k rpm but both tips chipped in a short while and the body exhibits lots of carbonized deposits.

I've seen some tool tables that indicate ridiculously low CF for PCD bits, for example onsrud recommends only .009" for one of their straight pcd models (only .23 in metric)