Feed & speeds with large bits

[richards]

I've got to cut several thousand pockets 6 - 10 inches long, 2 inches wide and 1/2-inch deep in 3/4-inch baltic birch ply. To make things simple, I'm using a Freud 1-1/2 inch bit (the same bit that I use to surface the spoil board).

The problem is feeds and speeds. I tried ramping into the cut 1/8-inch at a time at 16,000 rpm and 1-ips, making two passes, ramping another 1/8-inch and repeating until the pocket was cut. (Even at 16,000 rpm the Porter-Cable slowed significantly.) However, after fifty cuts, the first bit was fried.

Doing a little math shows that the area being removed per revolution with the 1-1/2 inch cutter is about 16 times greater than the area removed with the 3/8 inch cutters that I normally use. Since my normal cut in baltic birch is .7 inches deep at 3-ips with a 3/8 inch bit, it seems that I'll need to take some shallow passes (about .04375 inch per pass) to maintain equivalent loads on the router. Of course the goal is to cut as fast as possible without burning up a bit every 50 pockets ($0.25 per pocket for tooling at that rate).

Any suggestions?

Mike

[ron brown]

Mike,

A Her-Saf indexable bit uses an insert that is $3.35 and has four edges. The carbide is better than on brazed bits. I cut 6000 LF of soft maple on one edge and only turned it because I was doing some work on cypress and needed a better edge to cut the cypress.

Ron

Ron

[olecrafty]

Mike,

For simular cuts as you discribed I use a .5 endmill, .25 cut depth, 2.25ips, 21000rpm, and compressed air blowing on the bit. Cut from the center out to reduce loading on the bit. You may find you can cut at a faster speed in birch, this is my speed for cherry and my final cut depth is 1.125in. I use an "A" coated SGS endmill for the cuts. I change endmills after the third full day of cuts. Hope this helps

Kaiwa
olecrafty@charter.net (mailto:olecrafty@charter.net)

[richards]

Thanks for the responses.

Perhaps next time I'll try a more traditional approach and let PartWizard compute the path for me. My main problem is that the Freud bit is not a plunge cutter, so it has to be ramped into the cut. The corners require a radius of .75 inches, so using a 1-1/2 inch diameter bit seemed like a good match.

At any rate, I found that using a 2-1/2 ramp into each pass, with each pass being 0.057 inches deep, 5.5 ips and 13,000 rpm, that thnigs work quite well. I cut about 400-500 pockets today in the time that I had available.

Most cuts showed some burning when the cut direction changed, making me think that a little tweaking of the ramps might help. In any case, the pockets were accurate, repeatable and fairly fast. On the shortest piece of material (24 x 2.75 inches), I cut two 2 x 6 inch pockets 0.4 inch deep. Each piece of ply took 1 minute 42 seconds to process with 5-10 seconds to change material between cuts. Playing with the feed speed made very little difference in total cutting time - at least from 4 ips to 6 ips. Using 5.5 ips gave a decent chip size, a clean cut, and only minor loading of the router motor.

Mike

[stevem]

Mike, the cause of the burning in the corners is the radius of the bit, which is equal to the radius of the corner. This requires the router to come to a dead stop on an inside corner before changing direction. To avoid this, use a bit with a radius that is slightly smaller than the radius of the corner. The tool path will then be an arc instead of a sharp corner. The router will be able to maintain forward movement during the entire cut.

BTW, how are you holding the parts?

[richards]

Steve,

Thanks for the heads-up on the cause of the burning.

The parts are sucked down with a little $200 Rousseau vacuum pump and some platic pods that I built, similar to those that others have posted on the forum.

Kaiwa,

I tried a variation of your suggestion. This afternoon when I had to cut several hundred pockets, both 2x6 inch and 2x10 inch, in popular, I tried a 3/8-inch spiral cutter (the same that I use for most non-pocket cuts) - and was amazed. I ended up running the first cut in each pocket at 1.5 inch per second, 19,000 rpm and 0.40 depth. All the other passes in each pocket were run at 19,000 rpm, 0.40 depth and 12 ips! That's right, 12 ips. Other than the first pass which cut a 3/8-inch kerf, all other passes had a 1/8-inch overlap. There was *no* loading of the motor, and the cuts were clean, without tooling marks.

BTW, I chanced upon the feed/speed combination after I had to take off the dust skirt due to excessive splintering in the popular. Large splinters kept breaking loose due to improper cutter over-lap and then clogging the mouth of the vacuum hose. After taking the dust skirt off, I could see something wrong with the chips, leading to a little expermentation with cutter over-lap and feed speed.

At any rate, I was impressed.

Mike