Double Compression Bit Questions (and tips?)

[BTP]

I have been cutting 1 sided prefinished 3/4" birch with 1/4" downcut.
I usually cut .79 to clean the bottom edge a little
The bottom side still gets blown to h#ll:mad:

I am moving to double sided prefinished birch 3/4"
And also double sided laminated 3/4".

So, with a double compression bit:,
Do you
Cut EXACTLY? 3/4" if you are cutting 3/4?
Or do you go a little further?

If you go exact 3/4 when cutting 3/4. Do you buy a bit that has 3/4" exact?
^ I ask that because it seems from being up & downcut together, that the way it performs better.

ALSO:
Is a double compression bit the best for this?


Thanks

[Brady Watson]

The 2-flute compression tools from Centurion Tools work very well. I would limit my over cut distance on the Z to .01-.02 - and make sure that you surface your table before doing the job so that it is flat. You will NEED to ramp into the cut using the option in the Profile toolpath fill-in sheet so that the tool never plunges straight down. Cuts can be made in multiple passes with a compression as long as the 1st stepdown is deeper than the upcut portion of the compression tool.

-B

[gene]

Please elaborate on the need to ramp into the cut . If you are using a comp cutter isnt the bottom cutting upward?

[garyc]

Alex...
For 3/4" material I would use a 3/8 plunge end compression bit. If doing shallow dados a plunge end mortise compression is best. For profiles the plain compression has a longer upshear section and removes chips better so you can cut faster.

Compression bits have an upshear end so you must plunge straight in (sorry Brady) to a depth greater than the upshear section of the bit. This is about .3" on the compression and about .23 on the mortise compression. If you ramp in the upshear section will rip the veneer face to shreds.

I usually cut thru (and beyond) the material by .015" when the spoilboard was good and .025 when not so good. Try a 2 pass method either half depth or onionskin climb/conventional at 4-6 ips depending on the power of your spindle/router and machine (std/alpha)

I have not heard of the term "double compression", but a compression IS the best bit for the job

[Brady Watson]

Please elaborate on the need to ramp into the cut . If you are using a comp cutter isnt the bottom cutting upward?

Compression bits are designed to be run full depth, although there is certainly nothing wrong doing a multi-pass profile as long as the bottom upcut portion of the bit is below the top of the material on the 1st pass - otherwise you lost the benefit of running a compression...

Plunging straight down 3/4" (and even 3/8") is really hard on tools, your spindle and you will most likely burn the part at the entry point & possibly put an entry divot on the part where the tool entered. This is why ramping in is preferred.

-B

[pkirby]

If you're worried about the tear out because of the ramping, then do the ramp on a "lead in" so that the chipout occurs on part of the waste.

[BTP]

Alex...
Try a 2 pass method either half depth or onionskin climb/conventional at 4-6 ips depending on the power of your spindle/router and machine (std/alpha)



2 pass?

I have been doing a 6 pass with a 1/4" downcut.

I have actually just realized this is why sometimes the top vaneer gets a little messed up, (1 out of 8 or so) because its only going down .1333 , and the end of the downcut bit can create a side-ways pressure on the 2nd "ply", and push the 1st ply upward.

All I cut is round table tops, so straight profile etc.


I have a STD 4x8 3.25 porter

[Brady Watson]

Alex,
You should be OK in 2 or 3 passes with a PorterCable, but this depends on your machine & how much torque it has. An older PRT without a 4G control box or newer machine would have a tough time with that much cutting force.

My recommendation (http://www.shopbotblog.com/index.php/2007/03/a-tale-of-three-bits%E2%80%A6and-the-poor-man%E2%80%99s-compression-spiral-trick/) would be to use a downcut for the first pass, .25" deep. Then change to an upcut, starting where the first pass left off, and doing 2 remaining passes at .50 and .75" deep respectively. This will give you a superior finish without the need to go to a compression bit.

-B

[BTP]

Alex,
You should be OK in 2 or 3 passes with a PorterCable, but this depends on your machine & how much torque it has. An older PRT without a 4G control box or newer machine would have a tough time with that much cutting force.

My recommendation (http://www.shopbotblog.com/index.php/2007/03/a-tale-of-three-bits%E2%80%A6and-the-poor-man%E2%80%99s-compression-spiral-trick/) would be to use a downcut for the first pass, .25" deep. Then change to an upcut, starting where the first pass left off, and doing 2 remaining passes at .50 and .75" deep respectively. This will give you a superior finish without the need to go to a compression bit.

-B
I bought my Standard 4x8 in june

I already have ordered a bit
http://routerbitworld.com/Freud-77-202-1-4-Diameter-X-7-8-Height-Double-Co-p/freud%2077-202.htm

changing bits would create a problem, since the gantry tends to move a slightly (during change) because of the force.

So, after reading your article.

Using the compression bit.

What about
3 passes
1st pass deepest
2 & 3rd is remaining split in half.
AND: running the tools feed rate slower?

[Brady Watson]

changing bits would create a problem, since the gantry tends to move a slightly (during change) because of the force.


This should not be the case. You need to adjust some things on the machine...Then pick whatever bit you want and try it for yourself and adjust speeds etc to what looks/sounds best.

Drop your X & Y motors and push them up HARD into the gear rack and tighten down the bolts. Check lower YZ car v-rollers for slop/play.

-B

[BTP]

well guys,

Glad I bought 2 bits. , and it wasnt my fault (this time)

Look what my new bit found in the center of a piece of china double sided UV birch

picture attached.