Compression and downcut bits

[greg_russell]

I have been searching through the forum to try and get a better understanding of the difference between a compression and a down cut bit. I cut primarily baltic birch and have had pretty good luck with downcut bits (1/4 inch mostly but I am trying 3/8 as well because it sounds like I might get better results). I am however looking for a better finished edge, and so I am curious about what a compression bit is and when I might want to use one.

Thanks for your input

Greg

[ron brown]

Greg,

A compression bit had "spiral-up" and "spiral=down" geometry. When cutting the lower portion is cutting up and the upper portion is cutting down. In theory, one gets no tearout on top or bottom.

Ron

[richards]

Compression bits work great when both portions of the cutter are in the material at the same time. If you're making shallow cuts, the compression bit might act like an up-cut bit (if only the up-cut portion is cutting) or like a down-cut bit (if the bit is extended too far into the material).

My problem with compression bits is that the Porter-Cable router doesn't have enough muscle to cut reliably in one pass at decent speeds (5-8 ips).

I've gotten the same effect by cutting the first pass with a down-cut spiral bit and then cutting the second pass with an up-cut spiral bit. Bit changing takes time, but with the Porter-cable, it at least gives fairly fast performance with little tear-out in 18mm baltic birch.

[srwtlc]

Greg,

I have used both 3/8" and 1/4" Onsrud compression spiral bits cutting 1/4" baltic birch with good clean results. The upcut portion has a cutting edge length of 3/16" so it works well for 1/4" and 3/8" material. The part number is 60-113 (1/4") and 60-123 (3/8").

[greg_russell]

Ron,

Thanks. So when using a compression bit, you would need to cut through in one pass to ensure that you are getting two clean edges? Assuming that you have a 7/8 cutting edge and you are cutting 3/4 material.

In a related question, I believe you stated in a different post that you try not to cut more than twice the diameter of your bit in one pass. In an effort to get the best finished edge, is there an advantage to using two passes, when you could make the same cut in one? Specifically in my case I am cutting out 3/4 baltic birch. With your 2x suggestion I could cut in one pass with a 3/8 bit. I would most likely use a down cut bit. Would I get better results by making two equal passes in the 3/4? I realize there are many other variables involved, but I am just trying to figure out how to minimize the amount of edge sanding that is required. The time it takes to cut out the parts is less of a concern currently.

Thanks again for your help.

Greg

[richards]

Greg,

Check other posts that describe making a rough cut at almost full depth and then a fine cut at full depth. I do that most of the time for the smoothest edge. In my case, when I'm cutting 18mm baltic birch, I cut to a depth of 15-1/2 mm on a line 2mm oversize and then make the final pass at a depth of 18.1mm at actual size. The 2mm cleanup pass removes almost all of the tool marks from the rough cut.

It's most probable that you'll need to run some tests at various feed speeds, rpms, and depths to find what works best for you in each type of material that you're cutting. For instance, I get a good edge on baltic birch at 2 ips, 16,000 rpm using a 1-flute straight 3/8-inch cutter. At 4-5 ips using a 2-flute straight 3/8-inch cutter and 16,000 - 19,000 rpm the Porter-Cable struggles and the edge is wavy. Using a 1/4-inch spiral cutting a little more than 1/2 way through the 18mm baltic birch with each pass, I get a reasonably clean edge. Using 1/4-inch spiral cutters and making two rough passes 2mm oversize as described above, I get the best finish - at the cost of three passes through the material. If the cut has large outside open curves, I don't worry too much about the edge, since it's faster to run the piece past a sander; however, if the cut has small inside curves that are too small to fit over the circular sander's spindle, making multiple passes on the Shopbot is the better method.

Mike

[ron brown]

Greg,

Michael and Scott have both given good information. Note Scott mentions the 3/8" compression spiral. That bit is rigid enough for a single pass cut in 3/4" material. Mike even states there may not be an easy path to the best finish... he is so correct.

Your best cutting bit might be a straight bit. All one can do is throw a chunk of material on the table and cut. THEN - Look at BOTH sides of the cut (see which side has the better finish), look at your chips.... think about what is happening and try another cut.

There are SO many variables to cutting and they all are related - Finish, power requirements, speed of cut, speed of part changing, hold-down requirements, dust control and noise. I've probably forgotten a couple too.

Your milage may vary (disclaimer).
Ron

[greg_russell]

Ron Mike and Scott,

Thank you very much for your help. I will continue to experiment, using your suggestions as a guide. Thanks again for taking the time to help me.

Greg

[jay_p]

Mike,

How do you set up the 2mm oversize cutting.

Jay

[Brady Watson]

Just offset the vectors to toolpath by 2mm outward. Use the offset tool in PW or do it in CAD and import it. Then only go down about 90% of the depth to do your 'roughing' pass. Trick the CAM software into thinking that the material is only 90% of your actual material thickness.

Then, create a toolpath that goes all the way down your material thickness using the original, non-offset vectors. Of course, you don't have to adhere to 2mm. In fact, I just offset the vectors by .04" or so because I work in inches. This really does create a nice clean edge because the tool doesn't have as much force on the bit, and in turn, doesn't distort or deflect.

-Brady

[richards]

Jay,

Brady gave a very good answer. I'll just add a few specific details.

In PartWizard (v.2), select the PROFILE toolpath. Change the Allowance setting to the desired amount of offset (lately, I've been using 0.020 - 0.040, depending on the material). Set/change the other perimeters and Calculate the toolpath. I usually name the oversize toolpath per_rough (perimeter rough cut). Next, set the Allowance setting to 0, set/change the other settings and Calculate the final cut, which I normally name per_fine (perimeter fine cut).

Note that the Allowance setting is not available for pocketing, drilling, etc. When I'm pocketing, I make two or more drawings in AutoCAD LT, one undersized by 0.020 - 0.040 inches for the rough cut and one at actual size for the final cut.

One other note. I get a lot more bit deflection when I do a climb cut than when I do a conventional cut; however, splitting (in lumber as opposed to plywood, MDF, partical board, etc.) is minimized. Last week I had to run 600 pocket inserts in cedar - nasty stuff. I got about 50% yield due to splitting. When I finally tried making the first pass as a climb cut at 0.25 inch depth, 19,000 rpm, 10 ips with a 3/8-inch single flute straight cutter, and the final pass as a conventional cut at 0.50 inch depth using the same bit/speeds/etc., every piece worked.

Mike