Old dogs and new tricks

[richards]

After going to the Jamboree this year and seeing what Bill Young was doing with a 1/4" cutter and after listening to the Onsrud representative talk about optimum RPM, feed speed and depth of cut, I decided to rethink my techmique on some parts. One of the things that I make every few months is a flight of airplane rocking horses. The kids love them, but they've really been a pain to put together. Usually, I've cut them out of Baltic Birch (now just birch plywood since Baltic Birch has disappeared) and then use wooden dowels for assembly. Cutting two airplanes out of a single sheet takes about 25 minutes, but drilling dowel holes along the edge of the material took about two hours. Then pounding things together, clamping and gluing took another hour. All in all, not very productive, even for a labor of love.

When it finally dawned on me that with a little creative thinking, I could cut mortise and tenon joints with corner circles so that the mortises would not have to be squared up by hand nor would the tenons have to be rounded over by hand. Then, since the holes only needed to be 0.300" in diameter, I decided to try cutting everything with a 1/4" one-flute O-spiral cutter. Then using Gabe Pari's method that he posted October 10, 2006, which can be found here (http://www.talkshopbot.com/forum/show.cgi?tpc=29&post=41367#POST41367), I made two 1/4" deep passes climb cutting and one final pass conventional. I was totally amazed at the accuracy of the cuts. With those little cuts, I was able to draw the mortises just 0.015" larger than the tenons and have everything fit together with greater precision than I'd ever had before.

What I found was:

1. By specifying the small circle def to be 0.35" in the VU command, that the little circles were round instead of elipses.

2. By using Gabe's method of combining climb cuts and conventional cuts, I could get clean edges and a tight fit.

3. By running a single-flute 1/4" O-spiral cutter at 1/4" depth per pass, 4-ips and 15,000 RPM, I was pulling less than 3A at the spindle and yet the total time to cut only increased three minutes (from 25 minutes to 28 minutes). Since it takes me that long to change cutters and re-zero the Z axis, there was actually no lost time.

4. By rethinking the entire project, I get a better product that snaps together in less than four minutes, looks better and is stronger.

All in all, not bad for an old dog who thought that learning new things was just for the young pups.

[phil_o]

Very interesting, thanks for passing on your experiences.

[waynelocke]

Mike,
Can you post a drawing of the mortise and tenon joint? I don't understand the "tenon joints with corner circles".
Wayne

[richards]

Wayne,
I'll try to post something tomorrow. Today, I'm rebuilding some large disk arrays for a computer customer about 100 miles from my shop. In the meantime, think of doggy biscuits. Since all inside corners have an arc equal to the radius of the cutter, by cutting a circle slightly past the corner you can remove that arc; however, you get a cut that resembles a doggy biscuit.

[Brady Watson]

The day we stop learning is the day we become obsolete...

-B

[paco]

Maybe it's something like that.


5239

I call it overshooting the corner(s). I use it with dados and cross assembly (like dinosaur and insects models).

I find it a little tedious to modify each corner and I have been seeking if it could be possible to make this a CAM strategy or option... sort of like tabbing; one would click the corner(s) to overshoot and it would cut slightly in the corner(s) for easing the assembly.

[Brady Watson]

Paco,
This is pretty easy to do in PW, Insignia, Pro or VCarvePro.

1. Draw your inner rectangle to the size you need.

2. Offset that rectangle to the outside 40% the corner radius that you want (EG if you want a 0.250" radius, offset part 0.100")

3. Create 4 circles .25" in diameter.

4. Use the alignment tools to set the outside edge of each circle even with each corner of the outside (offset) rectangle. (one circle per corner)

5. Delete the offset rectangle. Select all the parts & use the weld function.

It takes all of about 30 seconds to do this after you do it the 1st time.

-B

[paco]

Hey Brady!

That's what I do... or so.

quote:It takes all of about 30 seconds to do this after you do it the 1st time.

This is for each section; what if you have many?...

The previous method I used is a pre-drawn four corners with the circles then cut and paste then align as wished, remove the corner and weld the circle to the corner... about the same amount of work... but I need the snapping feature...

[Brady Watson]

To do what, locate the pocket in the part? Can't you draw one horizontal line & one vertical line & use the transform function to accurately located them...then just use the centering tools to set the pocket to the centers of each line?

I guess if you are doing a lot of files like this, you could create some custom cuts in SB3 to pop in a part anywhere you want. Along with the Offset feature this shouldn't be too bad...although personally, if I can't SEE it on the screen 1st, I don't trust it.

-B

[paco]

5240

[Brady Watson]

LOL!!!


5241

[evan]

SheetCAM (http://www.sheetcam.com/) has this as a toolpath strategy. It's a great inexpensive 2-1/2D CAM program.

[paco]

Evan,

can you show us?

Thanks in advance.

PS: I'm the one with the green saber... jumping all around real cranked.

[richards]

Paco has understood my method. It's really very simple. I generate some rectangles that represent the mortises or tenons, offset those rectangles a little (2.3mm in this instance), place some circles and then cut the file in three parts: 1. Circles; 2. Rectangles; 3. Perimeter

Here's a JPG of an AutoCAD LT drawing that shows a little of what I do:


5242

The green cicles with cross-hairs show the placement of the midpoint of one side of the rectangle. The blue circles represent the small 0.300" circles. The red rectanges represent the mortises. The black profile represents the parameter of the part.

It takes a little work, but on a job that will be run many times, the little bit of time spent in AutoCAD LT greatly reduces the total amount of time required to do the entire job.

[evan]

Paco,

Sorry to have to email this to you but I was having problems uploading a screen shot.
When you start a profile cut (inside, outside, or along vector) this dialog box opens , under the "Cut path" tab there is a box to check now called "Overcut corners" (on the PDF it's called "Sharpen corners", it has since been changed to be clearer.) This causes the bit to overrun the corner by a small percent (10% I think) of the radius of the bit, creating a sharp out side corner. I hope this makes sense. You can down load a free trial copy to check it out. I have no financial interest in the software SheetCAM. I do own a copy and use it frequently.

PS. I don't have a lightsaber, don't hurt me.

[paco]

Thanks Evan!


5243

Does it overcut all corners?... or can select the ones you need the overcut?

[evan]

All the corners of the profile selected. He's real good about upgrading the software and if asked and enough people think it's worth while he'll add features in. A very responsive company kinda like the Vectric guys... I think he's out of Jolly Ol' England also.

[Brady Watson]

Les is a really helpful & good guy, in my experience.

-B

[richards]

You guys must have parts that need lots of holes! My little airplane/rocking horse has 48 holes and it takes about 8 minutes to change the size of all the mortises and tenons to fit - depending on the thickness of that batch of material.

I just have a spreadsheet set up with the length of each mortise/tenon. When I enter a thickness of the material, the software generates a spreadsheet that I print out. Then I just make a bunch of rectangles, offset the rectangle and pop in the circles. In all reality, it takes as long to describe the process as it does to actually do it.

Now, if I were to design one-offs, perhaps I would use some kind of software to help out; but, probably not. I don't like drilling any hole larger than 5mm with my spindle. All of these circles are cut using the CC command so that I can ramp into the cut. It's quick and easy, both on me and on the equipment. A side benefit to using the CC command is that even when I cut the profiles, a hole already exists, so I don't even have to drill down on those cuts.

[jseiler]

what I like to do is cut the mortise so it has "ears" only in the long direction, then cut a shallow groove between the ears to allow for seating of a shouldered tenon. Of course, when you 'bot a shouldered tenon, you end up with a radiused inside cut and that's what the cut between the ears is for.

For example, crosspiece cross section is 1"x3", shouldered tenon is 1"x2" (taking a half inch on either side to make the shoulder), 1/4" bit. I would cut the mortise so it is 1"wide exactly, 2.25" accross "ear to ear" and 2.01" between the flats. I would then cut a groove between the ears .125"deep, 1"x2.25". If you do this, it won't cut the sides of the mortise, just the ends between the ears to accomodate the radius of the shouldered tenon. Fits great, lots of glue area, hides the edges of the overshoot needed to accomodate a square corner. Essentially just like mike does it, just with the ears poking out the ends, not on the sides where its harder to hide. Usually the way I draw this is to draw the square mortise (1"x2"), copy it twice, make one copy .25" longer for the shallow groove(1x2.25), make one narrower by .25 (.75x2"). center the .25" circles on the corners of the narrower rectangle. Weld the circles and mortise rectangle. Cut that using conventional and climb like Mike posted. Cut the shallow groove from the long rectangle .125 (you can use a little less, but 1/2 the bit diameter works).

For this to work, the shoulder must be at least 1/2 a bit diameter, although I usually go one bit diameter to make sure I completely cover the "ears" in my mortise and don't provide a place for glue to blow out.

In practice, I usually allow 10 thou for glue.

John

[handh]

Hey guys, if you visit Thermwood's web site they are doing a joint simalar with there CNC nesting. Click on there newsletter to the right of the screen to read about the joint. This might give you more ideas.


5244

[handh]

Also, Heres a idea that works, A guy had a special bit made to do the joints so that material thickness doesn't come into play. Check this out. Its called tenoncam. There website seems to be down right now, but hear is a link to google's cached search. You can go back later when the site is up.

http://72.14.209.104/search?q=cache:noNeUUtY3EwJ:www.1goal.net/tenoncam.html+tenoncam&hl=en&ct=clnk&cd=1&gl=us (http://72.14.209.104/search?q=cache:noNeUUtY3EwJ:www.1goal.net/tenoncam.html+tenoncam&hl=en&ct=clnk&cd=1&gl=us)

the regular address is www.1goal.net/tenoncam (http://www.1goal.net/tenoncam)

[bill.young]

I think this joint is along the lines of John's above...it has a lot of strength for something like a drawer box. The groove can be stopped at the ends if you don't want it to show when the joint is assembled.


5245


5246

[richards]

Bill,
I like that joint. If I get a chance, I'll play with that concept later today. With proper dimensioning, it looks like it would be both mechanically strong as well as having lots of surface area for gluing.

[richards]

John,
I apologize for not crediting your idea for the joint. When I saw Bill's photos, I just skimmed the text and concentrated on the photos. Then, after spending some time in AutoCAD LT drawing it up, I sat here wishing that Bill had given some basic dimensions so that my first test would be close. That's when I re-read his post and then re-read your post and saw that you had given all the needed data.

[richards]

I spent a few hours today (finally) cutting the joint in the photos that Bill posted and John described futher up in this thread. It's really a sweet joint. Alignment was perfect. Lots of glue area. Relatively fast.

After getting that joint to work properly, I cut another variation with a rabbet on the backside 0.10" deep (on the piece with the tenons). The rabbet was cut at the router table. It gives a shoulder on both sides of the groove, but I don't think that it adds much, and, it requires an extra operation away from the Shopbot.

[richards]

Here's an image with some dimensions to show one way to use John and Bill's joint.


5247

You'll note that the MDF was 0.762" thick.

The groove for the mortise piece is 0.130" deep, while the shoulder on the tenon is 0.125" deep. The extra allows the tenon piece to seat fully into the mortise piece.

The mortise depth from the surface of the piece, is 0.55" and the total height of the tenon is 0.50" allowing a little room at the bottom of the mortise.

The groove for the mortise is 0.392" from the edge of the material; however the groove is just 0.375" wide. Adding those two figures together shows that I have a 0.005" lip. I've found it much easier to trim an edge back with a sander or router than it is to flush sand the entire side.

The 1.625" tenon fits the 2.0" mortise snuggly with about 1/64" of lateral movement.

I used a 1/4" O-flute cutter to cut the parts. Everything matched and mated together perfectly without anything more than a gentle tap with a dead-blow mallet to align the parts.

[bill.young]

Hey Mike,

Looks good. This is really the kind of thing that CNC machines were made for...doing things that would be a pain to do any other way without a lot of fussing.

I wrote an overly-complicated parametric program a couple of years ago that cut that joint for drawer boxes. It has every possible dimension as either an input or a setting...all the depths and clearances and tolerances! I ended up hiding most of them in an "advanced settings" menu just to make life simpler for the guy that's using it...and there's still too way much stuff!

The toolpath itself can be pretty simple though, especially if you cut it with a bit that's half the nominal thickness of your material. The mortices and dado can just be straight line cuts, and just be moved in and out from the edge to compensate for variations in material thickness. The tenons can get cut down to the proper thickness with a CR command with pocketing turned on, and the outline cuts of the tenons are just straight line moves with the bit radius making the rounded corners and ends (though a tiny inside radius may make turning the corners a little smoother?)


Bill

[richards]

Bill,
I totally agree with you. The drawing is just to give someone some numbers so that they can try out the joint.

Normally, I use a much simpler approach, much like the one that you described. My cutter of choice is a 3/8" downcut spiral single flute. It would handle the mortises 4X faster than the 1/4" cutter that I used for the test as well as cutting the perimeter in two passes rather than three (one climb cut to -0.50" and one conventional cut to material thickness -0.025" so that the parts stay in place).

This particular joint will probably end up as a subroutine which will only require me to specify the thickness of the material, as a response to a prompt at the start of the program, before computing everything else automatically 'behind the scenes'.

Anyway, it started me thinking of other ways to do common things - and that is where the fun comes in.

-Mike

[Gary Campbell]

I know this is an older post, but is anyone out there doing any puzzle joints? Tha dado routine is pretty cut and dry, but I sure would like to implement some Bot cut joints on the face frames. Maybe with one of Bill's overly complicated input schemes!.
Thanks Gary

[mrdovey]

I've posted this link before (and tried without success to get a joinery topic going) but will offer an old web page (http://www.iedu.com/DeSoto/design.html) as one example of a "puzzle" joint suitable for face frames.

It's rack-proof and tightens with any change in humidity. It can be used either as an in-line splice or for right angle joins.

[Gary Campbell]

Morris..
That may work.. I have most of the pieces drawn up in PW to cut tests of a puzzle joint.. Hopefully by this weekend. I will get all the individual partfiles to edit.. then comes the fun with the variables.. the file editing will be my weak spot. Thanks for the info.
Maybe we can try the "joinery" thing over on Bill's WIKI there is a page waiting for us!.
Gary

[bill.young]

Hey Gary,

I was hoping someone would show an interest in that topic.

Years ago I cut a big (4x8) square for squaring up my ShopBot that used a puzzle-y joint to connect the parts together. I'll see if I can find drawings or pictures.

Bill

[Gary Campbell]

Bill..
Thanks.. I will do the trial cuts on Mon.. and see how the joint works. It is just my guess at copying the picture that Jeff Posted above.
Gary

[billp]

Gary,
I have one of Bill Y's "big squares" here. It is 71"tall, and 55" wide. The larger two "legs"are 5.5"wide...
5248
5249

[Gary Campbell]

Bills, Y & P..
That square ia awesum! Nice joint shape. I can think of many times when I wish I had one of those that I could scribe on and then replace instead of my aluminum version! I better start buttering up Bill Y.

[ed_lang]

That square looks like you need a platform under it with a trap door and a bit of rope attached to the top of the arm!

[bleeth]

It's very cute but I think I would make the "rise" 64" and the "run" 48" so I could always quickly verify it has not gotten warped.
(The first one to reply with why those numbers get's a gold star)

[jsfrost]

80

[carlcnc]

Dave

3,
4,
5 !!!

Carl

[bleeth]

A gold star for Jim Frost for the length of the hypotenuse and Carl for the rule.
When the two perpendicular legs of a right triangle are equivilent to 3 units and 4 units, the hypotenuse is equal to 5 units. Therefore the above legs will have a hypoteneuse of 5 x 16 or 80".

[bill.young]

It's been too long ago to remember why those were the measurements, but it was originally designed as an assembly and alignment tool so my guess is that on the PR tools (or could have even been the cable drive tools?) those were the measurements for something or other. Maybe the unistrut rails were 55" apart? Once you had the tool assembled you replaced the 55" leg with a 48" one to make it into an alignment square.

Turns out that the concept was better than the reality, so the last couple of ones were 4'x8' and just used to check square.

Bill

[Gary Campbell]

Dave....
How hard was it to tell the cabinetmakers from the programmers? GC

[richards]

Bill Y.,

Are the 'puzzle' joints made with through cuts or are they more of a half-lap joint?

[bill.young]

Hey Mike,

They're through cuts but I think half-laps would have been a lot better. If the joints were "just right" tight then the square stayed nice and square, but if they were just a little bit tighter then the joint would expand and bow the pieces a little when you put it together...a half-lap would have solved that problem.

Since there were 3 connections, though, I couldn't figure out a way to cut them as half-laps without having to flip one of the pieces over.

Bill

[carlcnc]

3,4,5,
Asq+Bsq = Csq
We all learned this in geometry
as a carpenter it was easier to teach the new guys yo remember 3,4,5 as the basis.
I remember laughing at a super for a large company who was so proud of his then 300$ [1972]calculator cause he could layout a square corner for a large building with the sq root function,
of course by the time he went to the office to GET his toy we had pulled a tape to 60',80'and 100' and dropped the stakes!

carl

[richards]

Bill Y.,
I'll start with two half-laps and one through cut to see how that works. (I hate flipping parts over too.) The half-lap puzzle joint - or something similar - looks like it would be an ideal joint for face frames. Either the rails or the stiles would have to be milled upside down, and overall thickness would have to be carefully watched, but those are minor consessions if the resulting joint had lots of glue area and allowed the pieces to snap together without fuss.

[bleeth]

Gary: the carpenters call angles things like 23 degrees. The cad engineers call it 22.8679342 degrees!! (I actually had this on a set of plans for a ship job!!)

[tommyr]

Or if you really want to confuse people on the job site just say use the Pythagorean Theorem.

Tom