Zeroing off using your machine bed

[cusoak]

I watch a lot of videos and never see anyone use the machine bed to set the Z zero.
If you used your spoil board to set the Z would that eliminate cutting in to it when cutting a part out.
Or is there some other reason it is not used.
Jeff

[tomgardiner]

I've never made a video but almost always zero at the spoilboard. I still manage to cut into my spoilboard. I have a tool z setting arrangement that references to the spoilboard so it would be more work to touch off the work surface. I haven't seen any drawback to zeroing to the spoilboard.

[Adrian]

I always zero off the machine bed. I have an adjustable zero point just off the bed which I reset each time I plane the spoilboard down. When I do a tool change the machine automatically touches off there.

My toolpaths are set to cut 0.25mm into the spoilboard as that gives me parts that require no sanding. The time spent once a month resurfacing the spoilboard is massively less than that which I would spend sanding without that overcut.

[Mobius]

I do a bit of both. If it is a through cut or I'm using the CNC to surface a piece, then I zero off of the spoilboard. If I'm doing a engraving/v-carve where it is more important to know where the top side of the piece is, or cutting a piece where it wasn't previously surfaced by the CNC, I zero off of the top.

Can get confusing though. More than once I've screwed up and buried a bit into the material or spoilboard. I now add a note to the start of each G-code file stating where the zero is (ie: Bottom Right Spoilboard OR Bottom Left Top Surface, etc.)

[garylmast]

Although I zero from the material, I actually touch the spoilboard first then put a negative number (the thickness of the material at setup) in the Zero Z box. That does two things, when I hit “Go To Zero”, it doesn’t drive the mill through the material getting back to the spoilboard. Also, if in my setup, I call the material thickness for an example 0.75” and my material is actually a few thousandths thinner, then even though it’s not touching the material it will still cut as intended.

Gary

[mtylerfl]

Hi Gary,

Your method will work for cutouts, no problem.

However, not for creating pockets of an accurate depth from the material surface nor for Raster 3D carves.

If you enter a negative 0.75” as a material thickness after spoilboard touch, and your material is thinner than that amount, your pocket depths would be shy by the difference between 0.75” and the actual thickness of material. Same for rasters - you’ll end up with “flat spots” and any material allowance between Roughing and finishing will be incorrect (areas near the surface of the material)

I’m also puzzled why your machine is not lifting to a safe Z Height before moving to your XY zero position after spoilboard touchdown? (if you don’t enter the negative Z)

[garylmast]

If you enter a negative 0.75” as a material thickness after spoilboard touch, and your material is thinner than that amount, your pocket depths would be shy by the difference between 0.75” and the actual thickness of material. Same for rasters - you’ll end up with “flat spots” and any material allowance between Roughing and finishing will be incorrect (areas near the surface of the material)

I’m also puzzled why your machine is not lifting to a safe Z Height before moving to your XY zero position after spoilboard touchdown? (if you don’t enter the negative Z)

Michael,

After all said and done, It's best not to be lazy and measure the material before setup, but for fun, go measure the thickness of a board at different places and I bet you'll be off a few thousandth at the different places.

You're right if I'm doing pockets and that's the exception where the pocket won't be as deep, however "most times" the material difference is only a couple thousandths, so unless you're doing inlays, that's really not big a problem. However, the majority of time I will measure the material before setup and if the material is the same as my setup, there won't be an exception.

The majority of my projects over the past year or so has been Double-sided models, so I am less concerned about what I've cut or not cut above the model as long as the model turns out the right measurement. Correct setup matters, but if the material is thinner than my setup, my model will be off if I zero to the lower height, especially notable in thinner areas of the model. As far as roughing and finishing, I don't see the problem. The finishing will just take less material, but the outcome should be the same (I usually leave material higher and lower than the model at setup, so flat areas are not a problem). So to clarify, I'm only talking a few thousandths here and there.

My machine does lift to a safe Z Height, however, since I do not have an automatic tool changer, I move the spindle to the front of the machine so I can easily change mills, then bottom it to the spoilboard, put a negative height as mentioned, raise the spindle higher than the material and hit the "Go to Zero". My reasoning is I don't want it to drive through the material finding zero.

Gary

[cusoak]

Well that is all great info. But I think that where I am in the learning process I will stay at using the material top to set my zero.
I would need to see a video on how it is done on a Shapeoko xxl cnc
Thanks.Jeff

[Adrian]

On the machine side of things it's done the same as zeroing to the top of the material. You just zero to the top of the spoil board instead.

[rscrawford]

Anyone who does production work on a big machine will nearly always leave zero at the spoil board. There are many reasons for this, but convenience is the number one reason. I can just turn my machine on, it 'homes' itself so it already knows exactly where X0Y0Z0 are (at the spoil board, front right corner). Then I simply throw a sheet on the table, turn the vacuum on, and start cutting. No measuring, jogging the spindle down, etc.

Another reason is that referencing off the spoil board gives you an exact thickness between the bottom of your dado and the bottom (outer) surface of the plywood. This is much more important than the actual depth of your dado, because this is what determines the overall dimensions of your finished cabinet.

Another reason is so that you don't cut up the spoil board too much (which decreases vacuum hold down strength).

[Mikehell]

If I'm simply cutting parts out, I zero to the bed. Anything with pockets gets zeroed to the work surface.

[IslaWW]

If I'm simply cutting parts out, I zero to the bed. Anything with pockets gets zeroed to the work surface.

In all honesty I have never figured out the logic behind this method, i.e., using two different methods to do one simple task. These CAD/CAM programs do not make math errors, neither do the machine controllers, only operators are capable of mis-measuring material or making math mistakes. Why would it be logical to introduce an opportunity for another type of error.

The conductive "Z puck" or plate is an inexpensive alternative to tool measure switches used by big iron machines, low cost, so therefore popular amongst the DIY and less costly CNC's. There are thousands of sheets cut every day in production facilities, zeroed to the bed, that cut dadoes on most every sheet. But they use Adrian's logic. Cabinet size is more important than percieved depth measured from a varying surface.

If you add to that the inconsistencies introduced by the conductive method itself... the variations are too numerous to mention. That said "Z to top" is easier to understand, and usually cheaper, so therefore will always be more popular with the lower priced machines.

[Leo]

I find as I have worked in several different companies that there is always a philosophy that goes along with the rationale as to what they choose to do.

To each chosen method the user has a full belief that what they do is the only correct way to do it, and they will tell you why.

Soo - what "I" say is just like what every one else says. That is to say that I believe the way I do it is the way it should be done.

Nah - not-really - there is no right way and there is no wrong way. It boils down to personal preference.

For my personal preference - I like to zero on TOP and in MIDDLE ----- WHY?

If ZERO in Z is on TOP - I know that Z positive numbers are ABOVE the material and Z negative numbers are cutting. I use sacrificial strips of wood under my workpiece when cutting thru. Sacrificial means I scrap that stuff as I need to - no big deal at all. I plan to cut into those strips.

With X-Y zero in middle - there are 4 quadrants -- Positive ordered pairs are in the upper right - Negative ordered pairs are lower left - upper left is (-X, +Y) Lower right is (+X, -Y). This also helps to keep everything centered especially with cutouts.

Ocasionally (5% of time) I will use lower left. I almost never set Z to the spoilboard.

BUT - this is MY personal preference. Not the right way, and not the wrong way.

All in all - you select the way that works best for YOU. -- That is what is the best way --- for you. There are more than 10 different methods - none are the right way - none are the wrong wrong way.

[Adrian]

Unless, of course, someone is following their chosen method because they completely misunderstand the process.

A few years back on Facebook I had a long and painful debate with someone who insisted you could only zero from the spoilboard/table surface if you never cut pockets or dadoes. This was because, according to him, the maths required to work out the pocket depth in the Vectric software was bound to lead to errors so it wasn't worth the risk.

I explained until I was blue in the face that it didn't make a blind bit of difference to the pocket toolpaths where the z-zero was and the figures are identical for both scenarios but this guy and ,worryingly, quite a few others kept coming up with more and more convoluted formulas to calculate pocket depths when not zeroing from the top of the material.

[Leo]

Unless, of course, someone is following their chosen method because they completely misunderstand the process.

A few years back on Facebook I had a long and painful debate with someone who insisted you could only zero from the spoilboard/table surface if you never cut pockets or dadoes. This was because, according to him, the maths required to work out the pocket depth in the Vectric software was bound to lead to errors so it wasn't worth the risk.

I explained until I was blue in the face that it didn't make a blind bit of difference to the pocket toolpaths where the z-zero was and the figures are identical for both scenarios but this guy and ,worryingly, quite a few others kept coming up with more and more convoluted formulas to calculate pocket depths when not zeroing from the top of the material.

I FULLY AGREE with you Adrian.
I find often times explaining something is at best an exercise in frustration.