Overall Problem: Tabs aren’t coming out the correct size.
Hi All, first post on the forum , probably should have made it a lot sooner.
I have an X50 journeyman that still seems to be fighting me on my initial setup of it. I have a design that uses tabs, so trying to do some CNC joinery, but when I went to make it, I could not get my tabs to slot together. .
I’ve reduced it to a simplified design, as seen below
When I cut them out, I can’t get them together, and when I measure the cutouts with my calipers, I’m getting the width of the tabs at .7650", and the width of the slots at .7350", with the whole block being 3.7575".
I’m not really sure where to from here, I’ve had the same results with 2 different cam softwares (Carveco and Fusion), and welcome any input I can get from here.
Thanks!
I just combed through my 2D Contour setup on Fusion, I’m pretty confident that I don’t have it setup to leave stock behind, but I welcome help making sure it’s not something as simple as that.
Looks like I’m clear on that in Carveco as well.
(but again, I’m new to this, so I’m certainly not going to bet the farm that I have it right, but I will say that I think it would be impressive to make the same error in two different CAM options)
It’s a very nearly new mill from Bits N Bits, other than a V Groove bit that I accidentally plunged into the Z sensor block, I haven’t had a chance to really mess up a bit yet. I appreciate the thought though!
On my Journeyman, I’ve found that I have to specify a small negative “stock to leave” when I need to machine a feature to a dead-accurate dimension. Usually -0.003" to -0.004", depending on the cutting direction, material, bit condition, and depth of cut. And that’s on a finishing pass where there’s only maybe 0.010" of material left to remove.
It takes some contact pressure to force the cutting edge of a bit into the material, which means that the material is generally pushing the bit away from the cut. And as nothing is perfectly rigid, this will cause some deflection of the bit and/or machine. Adjusting the “stock to leave” is an easy way to compensate for this effect.
I’ll give that a try, I had been using MDF for the diagnostics to try to give it it’s best chance for the best best cuts (I thought it would be sort of be the most neutral thing it would carve. I’ll see if a negative will get me to where I want things to be.
I’ve had pretty good luck making similar joints. My method:
Use Node Edit (VCarve) to shrink/expand everything on one side by .010 inch to provide clearance. That usually gives me a “hammer fit”. .020 gives me a sliding clearance. It’s a pain to draw on a large joint, but you should be able to create an array to make it easier. When you’re done drawing it, move the two parts together and check that clearance on the first and last fingers.
Specify a .010 finish pass.
Make sure to use gentle ramps at the start of each cut.
I appreciate you clarifying, I did misunderstand what you meant initially. I checked with my calipers and it’s the quarter inch end mill I expect it to be.
So I’ve confirmed that I didn’t have it set to leave any stock behind in fusion, I’ll set it to -0.004 and see if that solves my issue. I appreciate everyone’s insight on this, hopefully I guess to report back that this has solved my issue!
That test seems to have been successful, I’m going to try a few more things tomorrow to make sure I can actually call this problem solved, but it sure looks like it is!
Thanks again to everyone who provided input.
Based on a detailed email exchange with Cody Elkins of Cadence Manufacturing who make the Jenny bits I learned something about how CNC bits are made. The bits starts as 0.25 inch diameter carbide blanks which the flutes are milled out of. The tolerance on the blanks is plus 0.0000 minus 0.0002 inches. As a result of this tolerance and the need to remove carbide during milling to get a sharp edge on the flutes, 1/4 inch CNC bits will always be smaller than 0.25 inches in diameter. I measured my bits from 4 different US manufacturers and found that the diameters ranged from 0.247 to 0.249 inches. I always use the same bit for cutting finger joints projects and add an allowance for the under size bit.
