1/2" Baltic birch drawer sides

[jonathanmahnken]

Looking for criticism/help. Im a brand new user. I have just run my first 20 drawer sides on my 4x8 warthog. it went mostly well but im totally guessing on my feed/speeds, ramp distances, number of passes, number/size of tabs ect... My machine is old and slow. Uses a PC 3.25hp router, and moves around at 340 ipm. i will attach a file of what ive done. what I noticed is that my shallow rabbets have fuzz on the inside edge, and that the perimeter cuts are fuzzed on the ends of the ply as well.

[jonathanmahnken]

I should also add that i use a 1/4" amana compression bit. any bit suggestions would be helpful

[Adrian]

Look up the chip load tables for the bit on the Amana website and then use the chip load calculations in the tool database to get as close as you can with the rpm and feed rate limitations you have.

[wilkigr]

The 1/4" compression bit that I looked at on the Amana site shows that the upcut part of the bit is 9/32" long. Looking at your file, other than the profile cut out, you are not cutting deep enough to engage the downcut part of that bit. So, you are essentially using an upcut bit and will cut tear out or fuzzies on the top surface.

I may well have looked at the wrong bit, but you can check the specs on yours, then compare that to the depth of your cuts.

[jonathanmahnken]

Thanks. Can anyone take a look at my ramp distances and tool paths to see if im making any amateur mistakes

[mrmfwilson]

To me the feed and speed seems proper for what you are cutting. Might even go to 200ipm. I have a 1.5hp spindle so the router may not be able to handle more speed. Ramps on pockets don't make much sense to me. Maybe to extend the life of the bit. One or two inches should be fine. If use it I use 1. The ramp on the profile cut can be whatever you like. Depending on the size of the project i use 1-2". I also set the plunge rate on a profile with a smooth ramp the same as the feed speed. The ramp uses the plunge rate for the ramp distance. Dropping down to 30ipm is adding a lot of time to your routing. Especially for 3 inches. You already are using a ramp, no need to slow it down. I use this mostly so the bit isn't retracting and plunging every change in depth. I moves in a smooth cut so you don't get witness marks on the sides. I usually make my tabs wide and thin. Equal in depth to the last pass. Also to try and reduce the witness marks. Also agree with wilkigr. You need to use the compression bit so that the part of the bit you want to use is the correct depth to get smooth edges on plywood. There was an excellent presentation on that in this years user group meeting. Your CNC is not that slow for a router based system. Mach 3 controller software only allows you to set the speed to 300ipm. I think running things slower is better to an extent. Hope this helps. My typical feeds and speeds for two flute down cut 1/4" bit in plywood are 1600rpm and 200ipm. I usually set the cut depth to .093. This can leave some splinters on the bottom side but not as bad as an up cut bit on the top surface because the bottom is pressed against the table. But in your case the cut depths will depend on the height of the different parts of the compression bit. My question is do you really need a compression bit? I have one but rarely use it. Most of my projects are not plywood. Most of the time, on my plywood projects, one good edge is enough. I think that you might be better off using a profile path when the pocket is less than twice the bit width.

[jonathanmahnken]

Thanks Mr Wilson. I will bump up my feed speeds. Ive been trying to do the dado and the profile cut in two passes, should I be doing a deeper first pass? No im not sure about the compression bit. I use 1/2" baltic birch for this. Because these are drawer parts they do need to be acceptable on both sides however. My rabbets are way too shallow for this type of bit it seems... maybe a straight 2 flute bit?

[mrmfwilson]

Thanks Mr Wilson. I will bump up my feed speeds. Ive been trying to do the dado and the profile cut in two passes, should I be doing a deeper first pass? No im not sure about the compression bit. I use 1/2" baltic birch for this. Because these are drawer parts they do need to be acceptable on both sides however. My rabbets are way too shallow for this type of bit it seems... maybe a straight 2 flute bit?

I would say on the rabbets that the top edge is the only one visible a 2 flute down cut would be appropriate. Most people use 1/2 the bit width as the depth as a rule of thumb. I prefer to cut shallower and go faster. But it's really a preference built with experience. I'm sure there are a lot of opinions on that subject. Really depends on the stability of the router and the material. Perhaps someone that has more experience with plywood will jump in and share their technique. Funny thing is tomorrow I am making a drawer to replace a really crappy on that fell apart in my 3 year old kitchen. Damn pressboard! Since it's just one, I'm doing it with regular saws and router table.

[dealguy11]

Something to try, if you haven't already. Whichever you are cutting, climb or conventional, try cutting the other direction. On my machine I get better cuts in plywood using conventional direction rather than climb. On plastics, just the opposite.

When I cut flat dovetails on my machine, I generally use a 1/4" downcut, and surface the spoilboard in advance to eliminate grooves on the board that encourage splinters.

[jonathanmahnken]

Thanks guys

[ger21]

Most people use 1/2 the bit width as the depth as a rule of thumb. I prefer to cut shallower and go faster.

I prefer to cut deeper and faster.
My "rule of thumb" is cut depth = bit diameter for tools 1/4" and less, and even deeper for larger bits.
1/4" deep with a 1/4" tool is not a problem at all, and still easily capable of 400+ipm if you have enough power behind it. And you'll double your tool life, by using more than 1/8" of the bit length.

[jonathanmahnken]

thanks again!