Results 1 to 9 of 9

Thread: Fire in the hole!

  1. #1
    Join Date
    Sep 2015
    Location
    Buford, GA
    Posts
    29

    Default Fire in the hole!

    So I piggybacked this off another thread, but thought I'd start a new one.

    I've had my router spontaneously combust a few times. The first time I was plunging holes with a compression bit, which I didn't know you shouldn't do.

    This last time is a mystery. I was cutting 3/4" pine plywood with a 1/4" straight-flute (2-flute) carbide bit (Freud), and had probably cut about 8 or 9 sheets. It may have been beginning to dull a little, but I've had different bits cutting that were much more dull. I can tell the dullness by how much the edges "fray" instead of clean cut.

    Anyway, I didn't even notice I had a problem until the machine finished cutting the program and shut off. That prompted me to return to the machine from across the shop, where I noticed a stream of white smoke coming up through the plywood. Well, I dumped a bunch of water on it, which did the trick. The flame seemed to stay between the material and the spoilboard, burning both, but not getting through either.

    The location of "ground zero" (image attached) was obvious, but the machine continued to cut out the material (bottom to top) until the sheet was done. The pieces cut out after the fire started were fine (if a bit singed).

    My only assumption is that there was a knot buried in the plywood that was either particularly hard, or has a high dried sap content, which combusted from the heat.

    Any ideas?
    Attached Images Attached Images

  2. #2
    Join Date
    Jun 2004
    Location
    Springfield Mo
    Posts
    839

    Default Fire & Bot rescue chief Andy

    Sounds like a lot of plywood work for a 1/4 inch bit of any kind. I would guess use at least a 3 flute 3/8th bit of some kind. Vacuum hold down can spread a fire pretty quickly.

    The bit people can tell you exactly what to use and the speed and feeds. An up-cut bit will pull the chips out of the wood and avoid compression heating. A bit should just be warm when finished not HOT which means it is dull or working too hard.

    Many times it is best just to use the Bot to mark the hole locations and finish them with a regular drill as drilling is hard on the router which is made to cut sideways.

    And of course never leave the Bot unattended for any reason... at least until you have posted a few thousand times. Hang in there !
    The decimal point seems to be the most important on the z axis... x & y not so much....
    ShopBot... Where even the scraps and things you mess up and throw away are cool....

  3. #3
    Join Date
    Sep 2015
    Location
    Buford, GA
    Posts
    29

    Default

    Is it? I've been cutting plywood with these bits now for 6 years, with mostly success. I suppose I could upgrade to a 3/8" bit.

    I do also use upcut spiral bits often, but they require more sanding on the top surface. Maybe I'm being a cheap ass, but the straight flute bits are $15 each, vs. $44 each and they seem to last the same amount of time.

  4. #4
    Join Date
    Dec 2011
    Location
    Piedmont, SD
    Posts
    715

    Default

    I suppose I could upgrade to a 3/8" bit.
    Yes, I highly recommend it. Like you, I used .25 bits to cut 1/2 and 3/4" plys for many years. A few years ago, I gleaned through some posts that perhaps I should go to 3/8, and tried it. Never went back. Bit pricing is first thing you need to get over, especially if you're used to $15 budget. Best I've used for a 3/8 compression is Onsrud 60-123MW , $60. second favorite: Centurian Tools 38CR21.03FEM200-HP. Almost identical bit, similar results and longevity, but half the cost. Both of these are extended wear (Max Wear Onsrud) (High Performance Centurian), meaning composition/coatings are higher quality so you retain a decent level of sharpness all the longer.
    While you may dismiss based on expense, you should seriously consider.
    Here's why: (assuming you're running 3 pass cutouts with the .25)

    - Less passes for cutouts x a dozen or two sheets can really add up. At two passes vs 3, you're spinning 4 motors 50% more time as you log cutout time.
    = machine runs longer = more energy spent ($)
    = Next sheet goes on all the quicker ($)
    = Mass of larger bit = more stable run, smoother kerf
    = Compression will almost eliminate any sanding of up-torn fibers still clinging ($)
    = Less wear on your CNC, especially the expendable pinion gears($)

    Go ahead and try , even with a cheaper straight bit to start, just to see time savings and likely a minor cut quality improvement. I've basically concluded, You're not really burning that much extra cash, if any, once all parts of the equation are factored. Why not be done sooner with a better finish and less machine wear?

    Give it a shot. I'm betting you wont go back to 1/4" bits for anything thicker than 1/4" ply.
    I haven't.
    FWIW

    Jeff

  5. #5
    Join Date
    Sep 2015
    Location
    Buford, GA
    Posts
    29

    Default

    Thanks for the thoughtful response. I really do appreciate it. I do use a compression bit for certain applications. However, I'm currently running an OLD 4'x8' PRT (Circa 2003?) with the Porter Cable router. Since I plunge drill a lot of 1/4" holes, I can't have the compression bit in for that, which would mean two tool changes every program. Total pain in the butt. That said, I've just agreed to buy a lightly used, 2016 PRSAlpha with the automatic tool changer and 5hp spindle. So, I'll probably have to rethink all my existing programs, but at least I could process all the internal pocketing and hole drilling with one tool, and all the cut-outs with the compression bit with minimal tool-change time. The reason I do a lot of plunging is that I'm making "boxes" that get assembled sort-of IKEA-style. I have a horizontal boring machine and I "drill" the hose in the sheet good to line up with the edge holes.

    Given what I've read about plunging using the spindle and the damage that can do, I'm probably going to invest the $2000 into the air drill attachment.

  6. #6
    Join Date
    Dec 2011
    Location
    Piedmont, SD
    Posts
    715

    Default

    Yeah- I've been aware of the hole drilling reducing spindle life warning. Bought a PRS Alpha new from SB with HSD 2.5HP spindle. 2-3 manual tool changes average for 3/4"cab parts (5mm holes, Dados/rabbets, cutouts). It's a drag, but just haven't found a way to condense all processes into 1 tool! Congrats on the tool changer - that's a game changer for sure.
    As for wear on spindle, I'm at 9 years with original spindle, though I'm not running the machine daily, as I'm a one person shop. That HSD is still running strong - bearings seem a little louder as years have gone by, but based on my level of use, plunging all those 5mm holes hasn't done it in. Looks like I'll easily hit 10+ years with it, but boy, I'd love to ditch the manual tool changes!

    Anyhow- just wanted to share what I've learned. Especially those bits. So many choices - what to buy? Those part numbers were given, as they have a minimal amount of up cut at the bit's tip. These both have only 3/16" length, with downcut geometry engaging at about 1/8". This is important, as others I've tried had way too much up cut, causing tear out if your first pass was too shallow.

    Again, FWIW - hope that helps.

    Good luck with your new machine - sounds like a goody!

    Jeff

  7. #7
    Join Date
    Dec 2008
    Location
    Diamond Lake, WA
    Posts
    1,691

    Default

    Quote Originally Posted by curtiss View Post
    Sounds like a lot of plywood work for a 1/4 inch bit of any kind. I would guess use at least a 3 flute 3/8th bit of some kind. Vacuum hold down can spread a fire pretty quickly.
    I've actually been using a 1/4" compression bit to cut all kinds of plywood, from 1/4" to 3/4" and 5/8" Appleply (American made baltic birch). Never had a problem. I feed at 6IPS with a spindle speed of around 14K RPM. bit is room temp after cutting a full sheet. I've got a 2009 PRS-Alpha with ATC. All my cutting and milling of plywood is done with 1/4" and smaller bits.
    Don
    Diamond Lake Custom Woodworks, LLC
    www.dlwoodworks.com
    ***********************************
    Life is not a journey to the grave with the intention of arriving safely in one pretty and well preserved piece; But to skid in broadside, thoroughly used up, worn out, bank accounts empty, credit cards maxed out, defiantly shouting "Geronimo"!

    If you make something idiot proof, all they do is create a better idiot.

  8. #8
    Join Date
    Sep 2015
    Location
    Buford, GA
    Posts
    29

    Default

    6 IPS???? Wow. What depth do you cut per pass?

    I'm probably cutting too much at a time. In 3/4" pine (0.725" actual), I cut in two passes.....basically .375" per pass, but I'm only cutting at 2.7 IPS at 19000 rpm (but using the Porter Cable router, not a spindle, so the actual rpm is probably lower).

  9. #9
    Join Date
    Dec 2008
    Location
    Diamond Lake, WA
    Posts
    1,691

    Default

    Quote Originally Posted by BoilermakerAndy View Post
    6 IPS???? Wow. What depth do you cut per pass?

    I'm probably cutting too much at a time. In 3/4" pine (0.725" actual), I cut in two passes.....basically .375" per pass, but I'm only cutting at 2.7 IPS at 19000 rpm (but using the Porter Cable router, not a spindle, so the actual rpm is probably lower).
    I cut 3/4" ply in 2 passes. Since I use compression bits, I plunge 3/16" then ramp down to 3/8". If you don't plunge first, you'll get chipout with a compression bit. I do my first two cuts with a climb cut. This pushes the bit away from the cut line. I leave a 1/32" skin and then do a final full-depth cut in a conventional direction. Puts the cut exactly on the line and makes for a REALLY clean cut. And very sharp edges on the plywood I might add.

    I cut softwoods in one pass climb cut, leaving 1/32" skin, and then second pass conventional cut. By the looks of your speeds and feeds, do you find your machine screaming when cutting? This means to slow a feed or two much RPM. The old saying goes, a screaming CNC is a hungry CNC. Faster feed or slower speed. Most softwoods I cut at 6IPS/14K RPM. Hardwoods I cut with a 1/4" depth at 6IPS/14K RPM. 14K RPM seems to be the sweet spot for MY machine when cutting material.

    When I first started using my machine I was afraid to push it to hard. I had a 2.2hp spindle at the time. As I increased my feeds the screaming went away and my results got a lot better. Don't be afraid to push your machine some. Thru trial and terror, I found out what my machine limits were. I used old bits and pushed them till they broke. I knew this was the top end of my machine. With the ATC I now have a 5hp spindle and it will very easily break bits and not bog down at all. I tried a 1/2" 3-flute down spiral and cut thru 1" of maple at 8IPS/18K RPM in one pass and it cut just fine and never bogged down the spindle. I probably could have slowed the RPM to about 16-17K. The 2.2 spindle would have really bogged down at that speed. You do need a GOOD hold down system to cut like this. LOL

    When V-carving, softwood, I run at 3-4IPS/18K RPM. Hardwood v-carve is 3-4IPS/18K RPM. The slower feed higher RPM gives me a cleaner cut with a v-carve bit.

    This is just MY observations for MY machine over 12 years of use and abuse.....

    Your mileage may vary...
    Don
    Diamond Lake Custom Woodworks, LLC
    www.dlwoodworks.com
    ***********************************
    Life is not a journey to the grave with the intention of arriving safely in one pretty and well preserved piece; But to skid in broadside, thoroughly used up, worn out, bank accounts empty, credit cards maxed out, defiantly shouting "Geronimo"!

    If you make something idiot proof, all they do is create a better idiot.

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •