box joint problems

This forum is for general discussion regarding VCarve Pro
Post Reply
bobowo
Posts: 3
Joined: Sun Jan 19, 2014 10:31 pm
Model of CNC Machine: router, plasma cutter

box joint problems

Post by bobowo »

Hello folks, I've been a Vcarve user for awhile- since 6.0- mostly doing signs and one offs that don't require super tolerances in their dimensions. Now I'm trying to make some box joints and am having some problems getting the fingers and slots to match. I have drawn my slots slightly wider than my fingers (.503" vs .497") to allow for gluing, but when actual measurements are taken my slots are .53" or there abouts. I'm using Mach 3 and have set my steps so that a 5" movement in both x and y axis is exactly 5". My son the machinist says it has to be lost motion somewhere but I'm not so sure. I'm using a .25" upcut bit (brand new) which actually measures .246" in diameter. By experimentation I found that if I set the diameter of this bit at .22" in the tool table, I'm getting mighty close to the results I'm after. One other thing I changed was the file format that I'm saving my Vcarve drawings in: I had been saving as ".tap" files but changed to the "Mach2/3.txt." files figuring maybe some kind of translation error was going on. Still on the fence about that though. If anyone here could shed a little light on this subject I would be grateful. Thanks.

User avatar
Adrian
Vectric Archimage
Posts: 11113
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: box joint problems

Post by Adrian »

There can be many factors which affect the fit of parts. A 1/4" bit will flex and different types of cut (climb/conventional) will produce different sized parts as well. There's always flex/movement in everything apart from the big end "heavy iron" machines too.

I always use the allowance offset feature to adjust the toolpath for a perfect fit after cutting a trial piece.

4DThinker
Vectric Wizard
Posts: 1416
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro, Probotix Meteor 25" x 50"

Re: box joint problems

Post by 4DThinker »

The only brand of bits I've come to trust is Onsrud. I've got a whiteside 3/16" bit that measures .1905. I had a Freud 1/16" bit that was off-centered and made holes nearly 3/32" diameter when it simply plunged. If the bit measures .246 but still didn't cut a .246 wide slot then that .246 may not be centered relative to the 1/4" shaft.

If a bit is making a full width pass if may deflect more than when it is only cutting a stepover pass using 30-40% of its width. This is one reason the latest versions of Vcarve have a last pass feature.

I make mostly joinery on our CNCs rather than signs or simple profile cutouts. I have gotten different results using the same tool path g-code file by just using different manufacturer's bits. In making tool paths for finger/box joints I typically use the same vectors for both sides of the joint. I then use the allowance feature with a negative value (-.002" usually) to build in a little glue room. This is only after I've measure the bit I want to use and verified what it will cut before telling Vcarve/Aspire what its true diameter is.

4D

4DThinker
Vectric Wizard
Posts: 1416
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro, Probotix Meteor 25" x 50"

Re: box joint problems

Post by 4DThinker »

The best reason for using the same vectors for both side of a box joint is that any error between what you've told VCarve the bit size is will be the same on both sides of the cut. You can then tune the fit by changing the allowance value for one or both sides.
Male Side.jpg
Female Side.jpg
4D
Attachments
4 inch wide half inch thick.crv
(270.5 KiB) Downloaded 76 times

User avatar
zeeway
Vectric Wizard
Posts: 3157
Joined: Thu Feb 11, 2010 9:24 pm
Model of CNC Machine: Self-built
Location: SC, USA

Re: box joint problems

Post by zeeway »

The other big factor in slot size is the actual wood you are using, and whether you are cutting with the grain or across the grain. The only way to know the size of the slot you will get, is to test cut the actual material and measure.

ger21
Vectric Wizard
Posts: 1576
Joined: Sun Sep 16, 2007 2:59 pm
Model of CNC Machine: Custom DIY
Location: Shelby Township, MI, USA
Contact:

Re: box joint problems

Post by ger21 »

You may also find that the size will vary depending on whether you're climb cutting or conventional cutting.
There are a lot of variables that can affect the fit of joints like this. It's a good idea to take good notes and make sure you do the same thing every time.
Gerry - http://www.thecncwoodworker.com

User avatar
Mark's Wood Chips
Vectric Craftsman
Posts: 201
Joined: Thu Mar 19, 2015 12:36 pm
Model of CNC Machine: ShopSabre 23 with Rotary
Location: Hubertus, WI 53033
Contact:

Re: box joint problems

Post by Mark's Wood Chips »

A lot of good information in this discussion. There are so many variables affecting accuracy regarding cutters, substrates and technique. The obvious place to start is taking a hard look at the mechanics - calibration, couplings, backlash and rigidity. Once those parameters are addressed, the software numbers can be tweaked for the job at hand. I find it interesting that the more accurate you can measure something, the harder it becomes to make a part.

bobowo
Posts: 3
Joined: Sun Jan 19, 2014 10:31 pm
Model of CNC Machine: router, plasma cutter

Re: box joint problems

Post by bobowo »

OP here- thanks for all the insight. It seems there are many factors coming into play from variations in bit sizes, wood types (I'm using mill finish #1 southern yellow pine, milling the end grain by supporting it vertically in the machine) and machine rigidity/backlash. I haven't tried the allowance offset feature- I'll look into that. I'm using Whiteside upcut spiral bits, cutting .20 inches deep per pass with a step over about 40%. Slot size is .50 wide x .77 deep. My results are acceptable for this project as I'm making shallow boxes (3.5" x 17" x 21") to hold machine shop tools, endmills, taps ,etc. for my son's machine shop (formerly my woodshop- oh well). My son is assisting me in determining backlash and repeatability issues and hope to get that worked out over the next few weeks. He's used to dealing with "half a thousandth" on Bridgeport type mills at work and looks at me like I'm a crazy man when I say a 32nd (.033") is good enough. He calls my work "farmer tech" and laughs but is gradually seeing that "close enough is good enough" for alot of things that need to be done when woodworking. Once again thanks to all who responded.

Post Reply