Feed speed for cutting mdf

[eklug]

I am the CNC programmer in my shop and I have two operators that run our shopbots. We carve the ends and sides out of corner blocks for fascias. When I used to run the shopbots I rarely ran it faster than 3in/sec. Now I find they have been cranking the thing up to 8 in/sec. In my opinion this is much too fast. It is way too hard on the router (we also have a spindle that can probably handle it). Some depths we cut range from .25" all the way to 1" in a single pass. Our maintence man says that a fast feed speed is fine as long as the router doesnt sound like it is bogging down. Well I know at 1" deep anything above a 2 in/sec and it bogs down.

Can I get everyones opinion on feed speed for cutting mdf? How fast do you run and what are the consequences for running it faster than it perhaps should?

thanks
emily

p.s I need some ammunition for my meeting about the cncs with production and the plant manager.

[richards]

Emily, the chipload calculator on the SB3 tools menu shows that you need fast feed speed to keep from burning up your cutters. I cut MDF at 12,000 RPM at a feed rate of 8-ips with a 2-flute downcut spiral 3/8-inch cutter. That gives me a chipload of 0.020, which is about what I want with MDF. Using a 1-flute cutter, I normally run at 5-ips at 15,000 RPM to get the same chipload. My vacuum system keeps me from cutting all of the way through the MDF, but I normally cut -0.730" on 0.750" material.

Before I got a spindle, I made multiple passes with the PC-7518 router. My typical approach was to use a 1-flute straight cutter at 19,000 RPM and a feed rate from 5 to 6-ips. The depth of cut was determined by sound. If the router bogged down, I took a shallower cut.

As long as the router/spindle is spinning at the desired rate, the chipload will give you the best possible cut and the longest possible life for the cutter. Spinning too fast and moving too slow creates too much heat. Spinning too slow and moving too fast will give a rough cut and will probably cause the Shopbot to either stall or miss steps (depending on how 'too fast' you're running).

My work is almost always long straight cuts where ramping is not a major factor. If I were cutting arcs and circles or if the line segments were short such that ramping kept the speed down, I would use a 1-flute cutter so that I could use a low feed speed. However, I would always try to keep the ratio between the feedspeed and the spindle RPM balanced to give me a 0.020 chipload. Since the power on my 3-hp spindle is constant between 12,000 RPM and 18,000 RPM, that means I would need the feed speed to be between 4-ips and 6-ips with a 1-flute cutter.

One great advantage with a Colombo spindle is that I can watch the Amps being used by the spindle. Normally I like to baby my machine and keep the Amp reading less than 8A, which is about 2-1/2 hp. (746 watts = 1 hp, 8A X 240 Volts = 1920 watts, 1920 watts / 746 = 2,57 hp.)

[eklug]

Im not concerned about the spindle bc i know it can handle higher loads than our regular router. But we need to have the two machines running in unison bc they both carve out areas of the same block and pass them back and forth. So the spindle is limited to what the router can do. We cant make multiple passes on the same cut bc of the time involved. The areas we cut are usually small (about 4" or 5" long and about 1"-2" wide with depths anywhere from .25 up to 1") and have a few curves usually. I have slowed the ramping speeds down a little to give a smoother cut in those corners and curves but the machine still seems to jerk quite a bit. Using the chipload calculator i come up with .05 for a speed of 8ips @ 18000rpm. Im not sure what you are using to measure your chipload but when i plug in your speed of 8ips @ 12000rpm into the shopbot calculator i come up with .07 for a chipload.

[Brady Watson]

Emily,
Your tool will never reach 8IPS when doing those small moves that you mentioned (IE 5" long). Try dropping the move speed to 4 or 5 IPS and reducing slow corner speed to 35 or 40. I think that you will find those speeds more reasonable and experience an increase in smoothness of the tool. Cranking it up to 8IPS when do small moves will introduce shock loads to the pinions and cause them to prematurely wear. The tool should not be 'banging'...your intuition was correct. The tool is pretty idiot-proof, but it's like asking your car to go from 0 to 100 to 0 in the parking lot...Even if this could be done, the ride sure wouldn't be very smooth.

So...if production time is important, your operator should be aking himself what is a realistic speed for the tool to move in a given situation. When small or intricate moves are needed, there isn't a whole lot you can do to speed things up. Some shapes and designs just take some time to cut.

-B

[richards]

Emily,
Sorry that it took so long to get back with you. I just took a whirl-wind trip to L.A. to check on some stepper drivers and other related electronics.

I'm not able to duplicate your chipload figures using the SB3 Chipload Calculator. 8ips @18,000 with 2-flutes gives me 0.0133. 8ips @ 12,000 with 2-flutes still gives me 0.020 (unless I set the flutes to 0.57 - then I get 0.07).

Brady is correct in describing how to deal with short moves. Trying to find a way to speed things up might be difficult given the limitations that you've described.

[eklug]

I must not have your same chipload calculator. Mine doesnt give me the option of different flutes. Mine is RPM chipload calculator version 1.0.00. It came with the first version of SB control software. Weve since upgraded to a newer version on the computers that run the cncs but i dont have that on mine. Ill check out the chipload calc thats on those machines and see if i get the same results.

[richards]

The chipload formula, if you're entering feed speed in inches-per-second, is:

Chipload = (Feed Speed X 60) / (RPM * Flutes).

Feed Speed in IPS = (RPM * Flutes * Chip Load) / 60

RPM = (Feed Speed * 60) / Chip Load / Flutes

[tvonschimo]

Shouldn't the diameter of the bit be taken into account in the calculations?

[richards]

I thought the same thing the first time I saw the chipload formula. But someone explained to me that basically what is going on would be comparable to peeling an apple. The size of the knife is not important in most cases. A very small apple might require a small knife and a very large apple might make you wish you had a large knife, but the thickness of the peel doesn't depend of the size of the knife.

In my own experience, using cutters from 1/4-inch diameter to 1/2-inch diameter, the formula works very well. Others have said that small cutters (1/8-inch and smaller) require adjustment.

There are other formulas that take the diameter of the cutter into consideration, for instance the SFM formula (surface feet per minute).