Thinner tenons or wider dados?

Gene Davis · Post by **Gene Davis** » Fri, Nov 09 2007, 6:52PM

Can anyone enlighten me about how the software addresses the joint allowance parameter?

When I specify, say for a panel stock material thickness of 0.780, that the plunge depth to create a tenon is 50 percent of thickness, and that my side clearance for the joint with the mating panel is 0.020, is the slot cut to 0.390 (half of the 0.780) plus the 0.020, thus 0.410 . . .

. . . or is the slot made to 0.390, and the tenon cut down to 0.370?

And, if it is the slot width that gets the extra, which side does it go on?

The engineer-in-me makes me ask this. Sorry.

DanEpps · Post by **DanEpps** » Sat, Nov 10 2007, 7:59AM

My guess Gene (and its just that, a guess) is that the slot is enlarged with the depth a width clearances. I would say that the width clearance is made on the inside of the slot so as not to create a \"proud reveal\" on the part.

Rick Palechuk · Post by **Rick Palechuk** » Sat, Nov 10 2007, 11:45AM

My guess is that the adjustment is made in the tenon size. That would allow for a single pass for the dadoes.

Paul Ford · Post by **Paul Ford** » Sun, Nov 11 2007, 12:40PM

I think the slot would widen as when using % dado thickness, it never adjusts the tickness of the material

Rick Palechuk · Post by **Rick Palechuk** » Sun, Nov 11 2007, 4:40PM

Well CNC guys, what's the verdict.

Joe Soto · Post by **Joe Soto** » Sun, Nov 11 2007, 6:32PM

Fit Clearance is the amount that the dado slot is larger than the nominal thickness of the component that fits into it. In general, a 0.010” to 0.020” fit results in a joint that is both strong and easy to assemble.

A factor for a Full Dado construction is that you are assuming that the material that fits into the dado slot is of the proper thickness. This is seldom true. Commercial thickness tolerances can make proper assembly difficult at times. The only way to assure exact fit every time is to actually cut every mating surface. Only then do you really know its dimension. The Blind Dado joint was designed for CNC routers and requires that every mating surface be machined to a proper fit tolerance.
Joe

DanEpps · Post by **DanEpps** » Sun, Nov 11 2007, 6:50PM

Well, it looks like those of us that guessed got it half-right no matter what our guess was.

Steve Dyches · Post by **Steve Dyches** » Wed, Nov 28 2007, 1:56PM

Gene,

Just returned from machine training and I asked your question. Dado is widened on EACH side.

Steve

Rick Palechuk · Post by **Rick Palechuk** » Wed, Nov 28 2007, 11:01PM

Is it standard practice to plow a dado slot in two passes?

Bill Rutherford · Post by **Bill Rutherford** » Thu, Nov 29 2007, 6:23AM

Rick,
Yes the dado slot is always plowed in two passes. Most times by the time material thickness, and clearance settings are taken into account the dado is almost never the exact size of the bit. Add cutter comp to that so the machine has room to comp for a slighty \"off\" diameter bit and the dado is always cut with a bit smaller then the dado width, in two passes. This allows exact control over dado width

DanEpps · Post by **DanEpps** » Thu, Nov 29 2007, 7:39AM

Just like the method for assuring that a groove (as in toung & groove) is in the center of a board with a table saw...run it over the dado blade, turn it around and run it again.

Of course, these are different reasons. With the CNC, to get the dimension exact, with the table saw, to get it exactly centered.

Rick Palechuk · Post by **Rick Palechuk** » Thu, Nov 29 2007, 8:57AM

Thanks for the heads up Bill.

Steve Dyches · Post by **Steve Dyches** » Thu, Nov 29 2007, 1:52PM

By using two passes the preferred cut direction (climb vs. conventional) is what each side of the dado is getting. If the dado was cut with one pass one side would be a conventional cut and the other a climb cut.

It was also recommended to us in the class to set the dado width to 60% of material thickness. This would, for example, allow the machine to use a 3/8\" tool on .710\" thick material. If set to 50% and the material was .710\" a smaller tool would be selected for the cut.

Disclaimer: I'm a newbee so if I'm wrong you pros chime in.

Steve