View Full Version : Bits burning up

06-20-2005, 06:08 AM
I had to cut MDF (3 sheets 4'x8' 8 cuts each) and went through 3 band new bits. I have a PR and was running @ .70 feed rate. One time my table was on fire. How can I stop the burning of the bits?

06-20-2005, 07:17 AM
Jimmy, we need the following info:
- Diam. of bit
- Rotation speed
- Depth of cut
- Quality of bit (solid carbide or something else?)

06-20-2005, 10:43 AM
Have you downloaded Andrew McClary's Chipload Calculator from the Forum (April 8, 2004)? His calculator will help you find the correct feed speed//RPM combination.

When I plugged in your .70 ips feed rate, 9000 RPM (the lowest possible with my PC 7518) and a 1-flute cutter, I got a chip load of 0.0047. To get a chipload of 0.011, I would have to increase the feed speed to 1.66 ips.

06-20-2005, 04:43 PM
To answer your question well, we need the information Gerald indicated. I can tell you from experience that MDF is hard on HSS bits. I won't use anything but carbide. Heat is almost always the result of too low of a chip load-- that translates to too high of cutter RPM or too slow of feed rate or BOTH.

06-20-2005, 07:16 PM

- Diam. of bit 1/4"
- Rotation speed 18000
- Depth of cut 1/4"
- Quality of bit? solid carbide 2 flute
I didn't know there was a Calculator, I'll see if I can find the post.

Thanks for all the info and help


06-21-2005, 02:11 AM
Jimmy, the dimensions/speed look safe against starting fires. I would be suspicious of those bits being true carbide as opposed to something much lesser. I once used the freebie 1/4" bit that came with a new Bosch router and also made smoke within about 5 minutes. Suggest that you try another bit supplier.

06-21-2005, 02:29 AM

Here is a link to the chip calculator.


I was not aware of it either.

Good Luck,


06-21-2005, 05:42 AM
Thanks for your reply, I'll try and find another supplier.

Thank you for the link, I think it's going to help knowing I'm close to the RPM and feed rates.

Thanks for all your help

06-21-2005, 05:52 AM
At 18,000 RPM, feed speed of .70 ips and a two-flute cutter, you're getting a chip load of about 0.001, or about 8 times smaller than the recommended minimum chip load on the chart that I use. According to the spreadsheet formula that I use, if you have to use a feed speed of 0.7 (42 inches per minute) and a 2-flute cutter, your RPM setting needs to drop to about 2,600. That's probably much slower than you can run your router. An alternative would be to run your router at about 16,000 RPM, use a 1-flute cutter, and set the feed speed to about 2-ips.

My chart lists the minimum chip load for MDF at 0.008 and the average chip load at 0.015. To get that 0.015 chip load, you'll need to slow the router to 13,000 RPM, increase the feed rate to 3 ips, and use a 1-flute bit; however, if your router is the same as mine, at 13,000 RPM it might have enough power to cut to a depth of 1/4-inch per pass.

There are always trade-offs, depending on the equipment that you have. With my alpha, I cut MDF at about 5.5 ips, 19,000 to 21,000 RPM, using a 1-flute 3/8-inch cutter. I can make a clean pass with the depth set at 0.65 inches and then a final clean-up/tabbing pass to the material's full .75 inch depth. If I had a spindle, according to the chip load calculator, I would try 16,000 RPM, 8 ips and a 2-flute cutter. Disregarding ramping, I would get a 0.015 chip. A little trial and error would show whether I needed to modify things to get both the finish and bit life that I desired.

06-21-2005, 06:49 AM
Thanks for the info Mike, I'm going to play with the speed rate and RPM's this weekend. I have a PR modified not sure how fast I can run it but I'm going to put it though the mill and see. http://www.talkshopbot.com/forum/messages/28/4132.html?1088522060


06-21-2005, 05:25 PM
Mike, I would be interested in knowing where you got your chart or over the years is it one you have developed for yourself.

Would you be interested in shareing it on the forum?

06-21-2005, 06:06 PM
I use the chart from the PDS Colombo web site, http://www.pdscolombo.com/spindle_speed.htm. There are other charts and recommendations that you can find by doing a Google search on "Chip Load". If I remember correctly, ALL of the charts have the same or very similar recommendations - usually quite broad, requiring the CNC operator to tweak things based on his machine's capabilities. (For instance, if I were cutting cabinets or other parts that have long straight segments, I would use the highest practical feed speed; however, if I were cutting parts with lots of curves and/or direction changes, I would pick a lower feed speed and lower RPM since the alpha would be in "ramp" mode more often than it would be at "speed". To quote from a Courmatt representative's post on the WoodWeb site, "I have seen the fastest machine travel at 900IPM even though it's programmed at 2000IPM." (You can find the referenced thread by doing a Google search on "baltic birch + chip load" - without the quotes.) His quote shows that ramping can play a huge part in the actual feed speed of your machine.

06-21-2005, 09:34 PM
Hey Jimmy,
I cut MDF all the time...
10,000 rpm
3.5 ips feed rate
.2-.3 step down
Either solid or carbide tipped work well.

06-21-2005, 09:41 PM
Mike, thanks for the info. I have been using the one published in the Onsrud Catalogue but find it is somewhat lacking in the actual chip load info, thanks.

What I was hoping is your chart had the ideal chip load per flute for different materials then I could just plug in the numbers for tweeking in the chip calculator link above.

06-22-2005, 09:57 AM
The chip load calculator lets you enter the number of flutes and then uses that number in its calculation.

Since I'm usually using a non-windows computer when get my greatest urge to design, I can't use Andrew's chip load calculator, so I've built a spreadsheet based on this web site: http://www.carbidespecialties.com/FAQ/Calculate.htm.

Even though a chip load calculator computes the chip load based on the number of flutes, it has no way of knowing how the cutter's design affects the chip size. A down-cut spiral packs the chips into the cut and by its very design forces the chips to be re-cut. An up-cut spiral pulls the chips out of the cut - and sometimes lifts the material right off the vacuum spoil board. A single-flute straight cutter has more gullet space per flute than a two-flute cutter, aiding chip removal (at least for the 3/8-inch single-flute Whiteside cutters that I often use).

From my reading, it seems that many CNC operators that use the "big iron" machines with auto tool changers, use a large rough cutting "hogging" cutter to remove most of the material and then use a finer cutter that gives a better surface to get to the final size, kind of like the way we all used to use a bandsaw to rough cut our material to aproximately 1/8-inch oversize before trimming the part to size with the use of a template in the pre-Shopbot days.

One last note about chip load: Again from my reading, it seems that reducing cutter heat is a primary goal of proper chip load. Using a cutter that makes chip removal more difficult, down-cut spiral for instance or multi-fluted cutters with shallow gullets, is going to restrict chip removal causing heat to be higher than desired.