1/4" or 3/8" compression

[john_hartman]

I have recently finished the ecabinets class and preparing to start ALL cabinet fabrication through this software and the link. I will be adding a couple air drills to my spindle and was wondering how those with a single spindle are getting along.

I have been using a .25 compression, but for a lot of reasons would like to use a .375 compression. However, I am torn because I can still see where a .25 would be useful. So what is the consensus on this? Thanks!

[Gary Campbell]

John...
It's almost universally accepted that the 3/8 bit is better for a number of reasons. I wont get into them. What I will do is give you the reasons that a smaller (either 1/4 or 5mm) bit it used instead of the 3/8.

The most likely is to match the predominate boring size for the file and eliminate a bit change.
In many cases machine move/power requires the smaller bit.

If you add drills, then the first doesnt apply to you.
If you have an Alpha, then the second doesnt apply either.

If you use dado or blind dado construction, then you may want to consider a mortise compression for a single bit strategy. It will allow you to cut dados deeper than .2 +/- without chipping the surface. They do not thru cut as fast as a compression, but are a great single bit. Prior to my ATC, this was the setup I used for nearly all cabinets.

[nat_wheatley]

John,

I prefer a 1/4" bit for these reasons:

-It matches the size of the dado for my backs, so there's no bit change.

-Smaller bit=less sideways force against the parts, so I get better hold down with my minimal vacuum.

-Less sawdust than with a 3/8" bit.

That said, I think my cut quality was better when I used a 3/8" bit, though with a cleanup pass, the end difference between the 2 was negligible.

Nat

[dlcw]

John,

I use eCabs and SBLink as well. An important thing to learn about with eCabs and SBLink is sizing joinery right to minimize bit changes. This might include changing mortise width from say 60% to another number that works better with the bits you have.

I use a 3/8" for all of my outline cutting on 3/4" and thicker material (two pass cut, climb on first pass - leave a 1/32" skin, conventional on second pass - thru cut).

On 5/8" baltic birch used for drawer boxes I use a 1/4" to help reduce the waste a little.

For mortise and tenon joinery I stray a little from what Gary does and I use a 1/4" down spiral to make sure I have clean cuts.

For 3/4" and thicker material I only have to do 1 manual bit change from the 1/4" spiral to the 3/8" mortise compression.

On 5/8" baltic birch I don't have to do any bit changes because the 1/4" mortise compression will do all my mortise and tenon joints and cutout.

My air drill punches all my shelf pin holes (currently 1/4"). This has worked well for me having only one spindle and one air drill.

[john_hartman]

These are all valid reasons. Ideally I continue to use both bits. I was hoping to eliminate the bit change though. Is a manual bit change through the link a pain or is it set-up to do so? If you are zeroing from the table surface and you have material on top then I suppose this would be an issue, right. So what the solution; some how set-up an "off-table" zero surface? How is this done?

The main reason I like the .25 bit is for the same reason Nat mentioned; backs. A lot of the time I use .25 backs but other times I use .5. What I don't think ecabinets can do, or I should say I don't now how to do, is make a .375 rabbit in the back of the cabinet and have it use .25 material. This would certainly solve this issue of using a .25 bit.

Nat- with regards to your "hold-down" statement; are you using a couple of Fien vacs. That's what I'm using and have not considered if the switch to a .375 bit will have adverse hold down issues.

[wberminio]

John

I initially used .25" mc bit. -3 passes
I have been using .375" mc bit -2 passes/ 1st onion skin 2nd cut through
My backs are all .5"-I find it saves time for me-no need for extra hanger
I have an air drill 5mm hole 32 mm spacing.
I zero to table with an offset block

I have found that cut quality has improved.
Btw I'm running a PRS Standard with 16+hp blower for hold down


Experiment-You'll find what works best for your setup/method

[Gary Campbell]

John...
A manual bit change takes some getting used to, but there are a good number of users doing it. I did hundreds of them when developing and testing the Custom (MTC) files for use with the SB Link.

Many SB Link users use an "off surface" zero block. This is simply a conductive surface off to the side or end of the spoilboard with a single wire going to the INPUT 1 terminal on the CNC board, same as the zero plate. The location of that block and its height relative to the current spoilboard are stored in the my_variables file similar to the Zzeroplate thickness.

You can "trick" ecabs into placing a .375 dado at the back of your cabinets and then have it cut .25 material for the back. You MUST be zeroing to bed for this to work or you will leave some major tracks in the spoilboard.

Notes for vac hold down....
That melamine and PF plywood are much more slippery than unfinished ply so they have more friction. Due to sealed surface they may develop more vacuum. Finding the sweet spot takes experimentation.

[nat_wheatley]

John,

I have 4 Amtek motors mounted directly to the underside of my table. These work surprisingly well and are fine for 95% of what I do. I typically lack hold down when I'm cutting small/partial sheets. I do mask the exposed areas of the spoilboard, but ocassionally have the smaller material slip when I'm doing my first/skin pass. I'll occassionally lose a stretcher(s) if its near the outside of the spoilboard also.

Nat

[john_hartman]

[QUOTE=islaww;104891]John...

"Many SB Link users use an "off surface" zero block. This is simply a conductive surface off to the side or end of the spoilboard with a single wire going to the INPUT 1 terminal on the CNC board, same as the zero plate. The location of that block and its height relative to the current spoilboard are stored in the my_variables file similar to the Zzeroplate thickness."

So I use the same wire from the exisitng z-zero plate and solder it to a fixed nut and bolt, adjusting the bolt as the table gets resurfaced. How is everyone doing this?

"You can "trick" ecabs into placing a .375 dado at the back of your cabinets and then have it cut .25 material for the back. You MUST be zeroing to bed for this to work or you will leave some major tracks in the spoilboard."

So we're cutting a .375 rabit/dado with a .375 MC bit and using a .25 back material. From what I tell the width of the cut matches to the thickness of the material, so how do you trick it into using thinner material?

[Gary Campbell]

John...
personally I use a sanded aliminum plate, tapped for a machine screw and fasten a wire to it that way. I do not interfere with the OEM zzero plate wiring. In my case the stored variable is adjusted as the spoilboard is surfaced. I have custom files that 1) read and store that difference, 2) adjust it from within my surfacer routine as I surface.

Trying to adjust a bolt to the table surface will return unsatisfactory results.

Tell the software that the back is a 3/8 with zero inset. Throw a 1/4 on the table and cut it. As long as you zero to bed, all is good. Trade offs, but it will work.

[englert]

John,

As I recall your back material is applied to the the back of the cabinet, though inset in a rabbet (full dado). As Gary indicated, you should use a 3/8" material instead of 1/4" when you design the cabinet. Since you're using 3/8" in your design, the resulting full dado or rabbet will be 3/8". If you use 1/2" material, it'll be 1/2". The machine does not know what material you layout on the table, so when it comes time to cut the backs, you just put a 1/4" on the table instead of 3/8".

If you'll recall, I suggested that you should create a material and name it so that you know to load 1/4" material instead of the 3/8" or 1/2", that we discussed. Since the material has a different name, it will nest all the parts made with the same named material.

With regards to setting up zero. If there are no dados or other joinery in the back, then setting up z-zero to the table surface is not necessary. They are all thru-cuts, so the retracted height is a little higher than necessary, but that's okay. It's not deeper!

You've probably already figured this out, but if not.

Happy New Year to all,


Dennis L. Englert

[ken_rychlik]

Dennis,

I don't follow you on the not cutting into the spoil board.

If the program thinks you are cutting 1/2 inch material and you zero to the top of a piece of 1/4 inch, then you will be cutting into the spoilboard 1/4 inch.

If you use a piece of 1/2 inch to zero the bit to the top of the material, then place the 1/4 inch in for cutting, that would work as you described.

The easiest way is just to zero to the bed and you don't have to worry about how thick the material is.

[englert]

Gary may need to kick in here, but we use a ZSHIFT memory variable that I believe also is used with the ShopBot Link. The ZSHIFT variable contains the material thickness from eCabinets and essentially shifts the Z0 up by that amount.

Now that I think about it Gary's original statement is correct. I'm probably still in a fog from the holidays and the almost two week vacation.

Anyway, set Z-zero to the surface of the table, then the ZSHIFT variable adjusts Z0 up. So while you may be using 1/4" material, but chose 1/2" material in the design, Z0 will be set 1/2" off of the table.

Sorry for the confusion. Thanks for re-posting the question Ken. Perhaps, I'll get the brain started again in the New Year.

Dennis

[Gary Campbell]

Kenneth...

I think I can add a little to the above. You are both correct. The difference between zero to top of mtl and Zero the bed IS the material thickness or ZSHIFT variable.

Therefore if you zero to top of material and cut thru your depth is: negative(mtl thk + cut thru depth). I.e. bit is never deeper than cut thru depth. Zshift variable is NOT used as a Z offset.

If you zero to bed, your depth is shifted UP the mtl thk (ZSHIFT) and then cut depth of mtl thk (same) and into the spoilboard by the cut thru depth. Again, same depth as above. Zshift IS applied as an offset(positve) to the Z axis. Same cutting depth as above.

In my scenario above, and as Dennis confirms, with zero to bed AND outline only cuts, it doesnt matter what material thickness is on the table. The machine will cut as per its settings to a depth of the "Cut Thru Depth" setting.

Using zero to top of mtl will cause the cut depth to be either too deep or shallow by the amout of the design vs actual thickness. This only applies to a condition setup by me above where a sheet thickness was used that was different than that input into eCabs.

Remember: If its hardware, it made to be maintained. If its software, its made to be tricked.

[erniek]

Another consideration when chosing a router bit is the number of flutes.

For myself I have found that I can cut faster with a single fluted compression spiral bit than a double fluted one. Probably because I have a PRT standard which has limited cutting force. With a single fluted 1/4" cutter I can cut at 5 IPS and with a double I have to slow it down to 3.5 IPS.

[john_hartman]

Well at the moment all this z-zero and z-shift is confusing. I'm sure it will make more sense when I actually start up the link.. :) Thanks the feedback everyone!