hi Guys,

i have a question whats your tool feed m/min for nesting plywood and MDF and what size and type of cutter you using?

Thanks

More information is needed to make any sense of the responses. Feed rates for an industrial cnc would be a problem for a lighter machine.
As for cutters, I use a 3/8" compression bit from FS Tool. 15000 rpm @ 450 in/min. My machine is a light industrial 4 x 8 FMT.

3/8 compression spiral 800 IPM @ 18K 18mm baltic birch

Dropout, are you using a 2 or 3 flute tool?

2 flute.

16000rpm, 600"/min 3/4"mdf or mel. 2 flute compression, heavy machine. Bits seem to be happy since they don't run hot.

You must first determine the maximum rpm of the tool being used and make certain you don’t exceed it. After you have made that determination there are several factors to understand. Heat is generated during the machining process. The proper size chip removes heat from the tooling surface, extending the tool life and quality of cut. I’ve provided a link to a standard chip load chart that should help you determine rpm based on your feed rate and the recommended chip load. You may have noticed I mentioned determining rpm not determining feed rate. There are characteristics about your machine that dictate what the feed rate should be for various parts and materials. If you know your optimal feed rate and chip load, then you can determine the spindle rpm. Consider the following when determining feed rate
1. What is the max linear cutting speed of your CNC? You’re not going to be able to cut in a line faster then your machine allows and unless you’re only cutting in a straight line without corners or arcs, you’re not going to want to program in the max linear feed rate for your machine.
2. CNCs have to decelerate then accelerate when going around corners and cutting arcs. Machines are not created equal and some require a longer distance to decelerate and a longer distance to accelerate back to the programmed feed rate when going around a corner. For sake of argument let’s say your cutting out a 10-inch square at the maximum feed rate your machine can cut in a linear line. In this example we’ll say that feed rate is 900 ipm and you’ve matched the rpm of the spindle to the recommended chip load for the material being cut when the CNC is at 900 ipm. Let’s also say your CNC has to travel around corners at a rate of 100 ipm and your machine requires 3 inches of travel to decelerate and 3 inches of travel to accelerate. That would mean on each of the 4 sides you would be traveling 6 inches at a slower feed rate then programmed. Conversely, you’re only traveling 4 inches on each side at the programmed feed rate. That would mean your only removing the proper size chips from the part 40% of the time. The heat generated during the deceleration/acceleration will result in excessive heat on your tool and dull the tool prematurely leading to poor quality cuts and a possible fire from the excessive heat if allowed to cut under those conditions for too long.
It’s important to know and understand your CNC’s characteristics and the optimal feed rate. This will assist you in selecting the proper tool and proper spindle rpm.

https://nutekmachinery.com/chip-load-.html