[maudib32]

So a little back story. We are currently running product and trying to find cost effective solution to the issue at hand. I've burned up a couple of bits now (they were cheap bits but they burned up) and am looking for what I need to run at for my CNC machine to get my feeds and speeds correctly. My experience with cutting is Metal, Plastic, MDF and solid wood but I seem to be struggling with plywood. I also have a second problem with my vacuum where if I am working on things I cannot cutout any of my holes or anything because well.....I end up loosing vacuum.

So here is what I'm working with:
Laguna SmartShop M
24,000 RPM Max


Problem #1:
I'm currently running 1/4" and 3/8" bits but I'm pretty sure that my feeds and speeds are just wrong. Mainly because I burned up one bit in a matter of about 20 boards (granted it was a cheap Redline Tools 1/4" Bit) but I am running into a few issues.

So I'm currently running:

Redline Tools RE10916Z 4 Flute Spiral Endmill
Tool: Ø1/4" - 4 Flute - Spiral Bit - Carbide
RPM: 16,000
Feed: 185.6 IPM
Feed/Tooth: .0029
Step Down: 0.125
Step Over: 0.125

Amana Tool 46420 SC Spiral Plunge
Tool: Ø3/8 - 2 Flute - Spiral - Carbide
RPM: 22,000
Feed: 250 IPM
Feed/Tooth: .0057
Step Down: 0.250
Step Over: 0.1875

Amana Tool 45708 Carbide Tipped V Groove 90 Degree
Tool: Ø1/2" - 45 Degree - 2 Flute - Carbide
RPM: 18,000
Feed: 200 IPM
Feed/Tooth: .0056
Step Down: 0.125
Step Over: 0.0625

That is my current setting. But I'm both looking at different cutters for longevity or upgrading the cutters but then I need to run feeds and speeds adjustments for my programs. We are trying to run times for efficiency and right now with these settings I am sitting around 7 hours to cut 8 boards. Just looking for both cutter advice and feed and speeds advice as I'm trying to find efficiency with this.

Problem #2:
Vacuum issue where if I finish cut any part to completion it looses vacuum.

I am looking at the composite brad nails as a solution for this. Having a quick run program that scores the top of the board so you can get the composite nails into place correctly on the parts before final cutting and just final cutting everything this way. Don't know if I'm barking up the right tree or not but it's what I am looking at. Does anyone else have any suggestions for keeping vacuum and parts down during cutting?

I am using a MDF spoil board that I am pulling my vacuum through.

[peteeng]

Hi Maud - The first thing to do to run fast is to get 1F bits. 1/4" at 16k is 319m/min which is the top surface speed for carbide I think so need to cut that back. I presume your cutting pine ply not hardwood ply. With a 1F tool I'd be aiming at 0.2mm/tooth (say 0.008" or bigger) 186"/min is 4700mm/min so can be faster with a 1F bit. Burning means your running the surface speed too high or the tool is rubbing. If rubbing you need to up the feed/tooth to take a bigger bite. Amana publish recommended speeds/feeds etc for their tools. Had a quick look but didn't find it. Send them a note their data sheets are very good. I've been using tools coated with DLC lately and they are really good... very clean cut and quite... Peter

[maudib32]

Peteeng

At the moment I'm cutting Birch Plywood.

Going to update the 3/8" cutter some as I'm running slow according to the chart. It's saying I should be at 230 IPM and .0064" chip load. So I'm going to update that slightly.

The recommendation on the 1/4" tool is so slow I cannot run production at that speed. So at some point I need to get some upgraded tooling to push harder. If the option is 1 flute or 2 flute then I'm going to go there. But I want to get some advice on cutting the wood before I invest in the tooling and burn it up.

The 45 degree cutter I'm just using as an engraver.

[peteeng]

Hi Maud - Also take a deeper cut. You should be able to do it in one pass? How thick is the ply? Depending on your edge finish required you can do it in one pass with some allowance then a finish cut to improve the edge? if needed ? Peter

[maudib32]

Hi Maud - Also take a deeper cut. You should be able to do it in one pass? How thick is the ply? Depending on your edge finish required you can do it in one pass with some allowance then a finish cut to improve the edge? if needed ? Peter

I am cutting 3/4" Birch Plywood. Need a good edge finish.

[routalot]

Cutting 3/4" ply in a single pass,with insufficient vacuum may well lead to the piece moving if the steppers are powerful enough.You really need to see if your vacuum system has both sufficient capacity and no leakage or blockage.Is the machine divided into vacuum zones?That has a good deal of merit if you cut smaller material than the size of the table and if not divided,a sheet of thin plastic over the exposed spoilboard may help.I have known people apply a sealer to the edge of the spoilboard,but my opinion is that it still points to insufficient vacuum capacity and doesn't make a big difference.Composite nails may be a sort of solution if the item doesn't suffer for having the nails left in place.My feeling is that trimming off the stubs in both the workpiece and the spoilboard will add some time to your operation as well as the risk of firing a new composite nail into the remnants of one that was there previously.

Was the vacuum pump ever changed from the original equipment?I would be surprised if the factory supplied item didn't generate enough holding power and if you are limiting yourself to 1/8" depth of cut on something with the surface quality of birch plywood,there has to be something awry.Is there an inline filter that may be clogged with dust?Come to that,did somebody perhaps take off the filter lid and displace a sealing ring?If the vacuum pump checks out,is it worth looking beneath the spoilboard to verify the quality of the sealing surface?As a final check,does the supply voltage to the machine match the specification on the motor plate?

Once you are certain about the sheet staying put you can fine tune the cutting parameters.The biggest gain you are going to make with your sheet processing time will come from sending the tool around the parts fewer times;holding the sheet securely will allow greater depth of cut and the times will tumble.I have seen the result of many,many passes at fine increments and one of the characteristics was a finely stepped surface on the parts as the tip of the tool was wearing far more than the next section up and the phenomenon was repeated up the whole length of the cutting edge.So you can add extra tool wear to your list of woes until a better cutting depth can be achieved.

Good luck.

[ger21]

Amana Tool 46420 SC Spiral Plunge
Tool: Ø3/8 - 2 Flute - Spiral - Carbide
RPM: 22,000
Feed: 250 IPM
Feed/Tooth: .0057
Step Down: 0.250
Step Over: 0.1875

You can run this bit 1/2" depth of cut, 17,000 rpm and 700ipm, if your machine can handle it.

Never used a 4 flute 1/4" bit, but I've run 2 flutes at 400ipm. In theory, you can go twice as fast with 4 flutes.

Plywood is very hard on bits. Depending on the specific material, expect shorter tool life.