Question on easily milling to a finished thickness

[Mark Bolton]

Im guessing this is a simple answer but I cant seem to get my head around it.

We have been opting to use the CNC as a jointer/planer as of late for flattening and surfacing glue ups as well as slabs for customers. Im trying to refine the process mainly on the second side but here is what Im doing....

I setup the code to mill say .030 per pass to a depth of lets say an inch (we will never go that deep). The cutter is set to the .030 max per pass so the file will run some 30+ passes. I have an M0 after each pass. The thought is on the first side of a slab or panel glue up it will run a pass at .030, pause, if we dont get a full clean up, we hit enter and go again.

On the second side, Im wondering how would we do something similar to what machinists do and look for our high spot visually, touch off, and then machine down to a fixed thickness off the table say using .030 passes (the last pass would be whatever is needed)? I can go into Vcarve and setup a toolpath with Z zero on the table and machine to .8125 but I have to set a start height which means I may be cutting air for several passes.

[James Biddle]

I'm interested as well. I've got some big slab flattening coming up where the slabs won't fit entirely on the bed. My thought was to use my Bosch cross line laser to quickly spot the high point and then go there for the touch off. My bed is level so I'm thinking that should work. I've also got to figure out how to rotate the slab and re-align it.

[Jim Becker]

My impression from Gary's (impressive) teaching these past two days is that you more or less have the right idea cleaning up one side (I'd do the intended bottom first), flipping and then cutting to your desired end-thickness. If you work from the table as your known height, it may require less machine resetting and you could just save a new copy of the tool path that is adjusted for a starting height that is appropriate for the second face. For surfacing operations, cutting a little air may very well be part of the job, depending on the nature of the slab you're working. Some of the videos I've watched of this kind of thing clearly indicated that might be the case. That's for slabs that you have less control over since they can be very variable in thickness as well as "straight/flat/twist", etc. For glued up panels, you have a better idea of what to expect and should be able to setup a more pre-programmed approach for each side.

[Mark Bolton]

James,
We've done the large slab thing a few times where we had to flip. We did one a bit back that was 11' long (our table is 100" long). The way we did it was to put the slab on the table and wedge it up off the table by an inch or so using hardwood wedges. This allows for any non-flat bottoms and twist. We used welding jacks like these https://www.zoro.com/sumner-v-head-p...IaAjbYEALw_wcB to support the end off the end of the of the table.

We then setup our rotary laser and got the top face of the slab close to level with the laser. We surfaced in the area of the slab that was on the table checking with the laser to make sure we were deep enough to guarantee a full cleanup on the end we couldnt surface. We then just documented the dimensions from the surfaced face to the laser, then rotated the slab 180, and using the jacks and the wedges got the surfaced area back to dead on the laser dimension and just milled the other end to that height.

After that it was just flip the slab over, laying it directly on the table this time and we put the welding jacks under the unsupported end and hooked our tapes on the under side of the slab and made sure we had the end off the table at the same height as the table with the laser. Surface, spin, surface.

It worked well.

[Mark Bolton]

My impression from Gary's (impressive) teaching these past two days is that you more or less have the right idea cleaning up one side (I'd do the intended bottom first), flipping and then cutting to your desired end-thickness. If you work from the table as your known height, it may require less machine resetting and you could just save a new copy of the tool path that is adjusted for a starting height that is appropriate for the second face. For surfacing operations, cutting a little air may very well be part of the job, depending on the nature of the slab you're working. Some of the videos I've watched of this kind of thing clearly indicated that might be the case. That's for slabs that you have less control over since they can be very variable in thickness as well as "straight/flat/twist", etc. For glued up panels, you have a better idea of what to expect and should be able to setup a more pre-programmed approach for each side.

Jim,
Cutting a bunch of air on the first pass, or maybe two if they are way out, is unavoidable. My hope though was to find a way to perhaps have a program/tool path where you could say "from what ever starting point I choose, I want to cut to a distance of .8125 above the spoil board) so to speak. So let say you have a slab or a glue up that has a big hump in it. You dont know how tall this hump is (nor to you care) but you want to start the spindle, come down in Z until you touch off, and then say "GO". Go means start surfacing at this Z height down to .8125".

I can do all this manually, I can Z zero off the spoil board, put my work on the table, start the spindle, come down in Z to touch off, look at Z height in wincnc, and then go into Vcarve, set up my job with that being the material thickness, and setup a pocket toolpath to take me down to .8125". I was trying to see if there was a way to simply avoid a few steps.

If we have a really funky slab that is very thick or thin on one end, we will just setup a couple different jobs and mill off the high spots with tool paths that just take in those high areas until we get down to a point where we are hitting more wood than air.

Its a bit frustrating to watch a toolpath that covers a large slab and the cutter is only hitting at one end or one corner when youve got a long way to go or are having to take light passes so I will just break it up into as many smaller zones as needed. Usually I can be toolpathing the next zone while one is running.

[Brad Shipton]

I see what you are getting at. You want to minimize the pocket dimensions in the various planes of the board based on the amount of material you need to remove at that level. If you can create a reasonable 3D model of the actual shape, you could use rest machining to optimize this. Without a 3D model you are beat. You basically need a contour map of the board faces. Then you could simply offset those contours to create your tool path at those levels. A fancy probe setup would make this easy, but I suspect you might find the manual method just as fast because the standard routines they use would measure too many points. I recall watching a 3D VCarve video where they showed how to get the program to calculate the leftover areas and then they selected those areas for secondary cuts. That might work. The software I use can do this fairly easily, but I do not do so too often. I also dropped most of the 3D stuff for it because of the maintenance costs.

I mocked up an example 3D model. This is a slab where the center is humped up by 0.5". I am not sure if you could do this in sketchup or not. I inserted two planes and found the intersection curve at each level (highlighted lines in image). If I were to tool path this to save I would simply draw the shape outside those lines at each level and create my toolpath. Will that save any time? Maybe with a large enough slab.

SLAB-Q.jpg

I have taken off as much as 0.125" in a single pass, but I slow down a bit and reduce my stepover.

You can see the problem in this first slab image. This was a slab someone bought and it was not dried correctly. I flattened it for them and cut out their sink holes. This was the first run and you can see where the cutter was removing stock at the two ends, but in between it was still missing. I spent a bit of time that day watching the spindle cut air.

Slab-02.jpg
SLAB.jpg

[Jim Becker]

I'm wondering if it's worth doing multiple area tool paths for this since you can be doing other things nearby while it does what it needs to do based on a reasonable starting point above the table, pocketing down to flat and then flipping to run an identical pocket tool path that starts a whisker above your preliminary stopping point. Yea...there's "air cutting", but if I recall, you have a big, fast machine so the whole operation should be much faster overall because you can trot that cutter along.

You could also knock a few of the high spots off with the uber-fancy hand plane before running the board on the CNC.

[Mark Bolton]

I hear ya but cutting air is just wasted time and wear and tear on the machine. With a large uneven surface there is always going to be a little air. When you get your machine and start seeing that small changes in cut strategy can double your cut time or halve it. I usually like to have the machine producing when its running.

My issue with zoning is a rare one. I was more so trying to solve the touch off and cut to a fixed thickness issue but I guess Im seeing my way through it, sorta, lol.