Small diameter (.125") double compression router bits?

[stevespo]

Has anyone seen a small diameter "double compression" (upcut & downcut) spiral router bit? Sizes from 1/4" to 1"+ are easy to find, but I have not found anything smaller.

Like this, just in a 1/8" diameter:

http://www.toolstoday.com/p-5638-cnc...e-2-flute.aspx

I'm cutting lots of small shapes in baltic birch plywood and it's very fuzzy using an upcut only bit. So, my strategy has been to run the toolpath one time with a downcut bit, and then complete the cuts with an upcut bit. This works nicely, but requires pausing the program, changing tools, resetting Z zero, etc.

I'm also wondering if a bit this small can be used to take a full depth cut in a piece of 1/4" plywood? I generally cut in 3 passes of about .085", at speeds of 80-120 IPM. I would assume that I can make a deeper cut provided I slow down my feedrate accordingly. I'm not trying to improve my cut times, just avoid the tool change.

Thanks!

Steve

[Big-tex]

I have never seen 1/8 compression. One way you can do is create tool path with say tool #1 (downspiral) profile starting at z 0 down to .25 depth and second tool path with tool #2 ( upspiral) starting .25 down to .5 .
Another words 2 tool paths for 2 separate tools.

[stevespo]

Big-tex, that has been my technique, and it works quite well. Just requires a pause and a tool change - which I'd like to avoid.

Depending on the geometry, I've been getting pretty good results with an 1/8" downcut bit. A little bit of fuzz on the bottom, but not too bad. My 1/8" upcuts have been miserable, so I probably need some better geometry for this application.

I did finally find a .125" double compression bit. It's single flute, so lower feed rate but I'm going to give it a try. Expensive at $40, but the time savings on just a job or two may well be worth it. I'll report back after I run some parts.

http://www.toolsxp.com/Onsrud-Cutter...s-60-100SE.asp

Steve

[Big-tex]

Ok 1/4 baltic ply I would not cut 1 shot with 1/8 dia. tool. You can give it a try worst you break a bit. With 1 flute bit your feed rate would be lower comparing to 2 flute but what I worry about is stress put on small tooling. That is why I would recommend .125 passes. Just kind of curious what machine you got and whit kinda stuff is it cutting.

[stevespo]

Generally, I don't use a DOC more than the diameter of the tool. Most of the time, I'll use 1/2 to 1/4 of the tool diameter and take many light passes (so, 3 passes with a .125" cutter in .250 plywood). I've been doing this at 120 IPM with a pretty standard downcut spiral bit - with good results and no breakage.

I expect that trying to cut full depth in one pass will require a significant slowdown in feed rate. Onsrud seems to recommend .010" chip load for that particular tool geometry. So, .125" tool, single flute, .010" chip load, 24K RPM = 240 IPM. That's for 1xDOC, so using their 25% reduction for 2xDOC, I could (should?) expect to run at 180 IPM.

Maybe, maybe not. I figure I'll start slow and bring it up as I feel more confident. Worst case, I break a $40 tool. Not something I'm looking forward to, but it happens from time to time.

BTW, I have an aluminum DIY machine. Linear rails, ballscrews and a 2.2kW spindle. I'm running 425 oz-in steppers (Gecko 203V @ 72VDC), but in the process of moving over to servos. My build thread:

In progress - 8020, linear rails, ball screws, steppers

Steve

[ger21]

I expect that trying to cut full depth in one pass will require a significant slowdown in feed rate. Onsrud seems to recommend .010" chip load for that particular tool geometry. So, .125" tool, single flute, .010" chip load, 24K RPM = 240 IPM. That's for 1xDOC, so using their 25% reduction for 2xDOC, I could (should?) expect to run at 180 IPM.

Maybe, maybe not. I figure I'll start slow and bring it up as I feel more confident. Worst case, I break a $40 tool.

Onsrud recommends .012-.018 for that tool. https://www.onsrud.com/xdoc/ChipHPlyWood

The middle of that range gives you 360ipm - 90 = 270ipm @ 24K

I've never used a 1/8" compression bit, but as a guess, I'd start at 18,000 rpm and 125ipm, which is close to the recommended feedrate with .012 chipload and 18,000 rpm.

Unless your cutting at 300ipm, you don't need to spin an 1/8" bit that fast.

[stevespo]

Gerry, that's really helpful. I just realized I was looking at the MDF table when I saw the .010" chip load number. .012-.018 is recommended for hard plywood.

I know these numbers are based on engineering, experience, real world testing, etc - but I always have a hard time (mentally) running the tools at the speeds they're designed for. Slow feedrates are no good for the tool, but some sort of safety margin is comforting to me.

I'm expecting the tool in a few days, so I'll definitely report back my findings.

Steve

[Big-tex]

Yeah Onsrud catalog and chip loads are always good to look up. I deal with them at work and have to adjust stuff based on new materials/tools used.

[ger21]

I know these numbers are based on engineering, experience, real world testing, etc - but I always have a hard time (mentally) running the tools at the speeds they're designed for. Slow feedrates are no good for the tool, but some sort of safety margin is comforting to me.

At work, I recently realized I'd been running the RPM much too high for a long time. I used to program at 16K RPM and 300-400ipm with 1/2" tools. A few months ago I turned the spindle override all the way down, and it actually cuts better. I don't know the actual rpm, but I'm guessing around 10K-12K? You can hear that it's doing a lot more work, and getting some really big chips, especially in plywood. But I've found that the tooling lasts about 50% longer.

From what I've seen, it's easier to break bits by going too slow and generating a lot of heat, then going too fast and exceeding the bits capabilities. I know that shops that do cabinet nesting cut 3/4" material at 1000ipm with 1/4" compression bits, so you shouldn't have any problems.

Let us know how it goes.

[Big-tex]

At work, I recently realized I'd been running the RPM much too high for a long time. I used to program at 16K RPM and 300-400ipm with 1/2" tools. A few months ago I turned the spindle override all the way down, and it actually cuts better. I don't know the actual rpm, but I'm guessing around 10K-12K? You can hear that it's doing a lot more work, and getting some really big chips, especially in plywood. But I've found that the tooling lasts about 50% longer.

From what I've seen, it's easier to break bits by going too slow and generating a lot of heat, then going too fast and exceeding the bits capabilities. I know that shops that do cabinet nesting cut 3/4" material at 1000ipm with 1/4" compression bits, so you shouldn't have any problems.

Let us know how it goes.

My expeience is same w/ one exeption, I do not allow operator to mess with feeds or RPMs.
When job calls for new type of bit I adjust it all myself by manufacturers specs first and further down by touching bit by hand and making sure there isn't heat any build up.
Same goes for variation in density/hardness on materials cut. Routers are air cooled unileke mills with coolant. Heat= tool wear especialy on resharpened tooling.

[stevespo]

Do you have a rule of thumb for the Z feed rate? BobCAD/CAM doesn't support ramping for profile operations, so I'm doing a straight plunge at 1/3 the cutting feedrate. Is that reasonable?

Steve

[Big-tex]

Based on tooling I do plunging at 50-60% feed rate.If I do have an option I ramp that will save on tooling wear.
It worked for me so far............