Zero to bed

[sawkerf]

How hard is it to make the switch to zeroing to the bed? I have always zeroed to the material and I was told that switching would help negate inconsistant material thickness problems. Other than setting up a spot off the table to zero on, what do I need to do to make the switch?

[myxpykalix]

I think the whole idea is to Z zero to the table and not to a place off the table so you will get an accurate reading.
Some have set up "off table" zero spots but if your table is scarred up or one section used more then others your off table zero won't accurately reflect the true table height.
Having said that i'm sure several have set it up and use it successfully possibly.

I always Zzero to material top and have had to rerun the cutout toolpath more then a few times due to thickness irregularities.

Here is the biggest reason i don't Zero to bed. Several times i set up a file to z to bed, set up my plywood on the table, spend 5 minutes clamping and screwing down only to realize i forgot to Zzero to the bed before i did all that. Had to undo it all....:mad:

All you have to do is when you are setting up your file in whatever pgm you use you choose "table surface" as your Zzero point, then C2 to the table when setting up your material.
There is no setting in the control software you have to change.

[Simops]

If using sheet goods it's better to zero to the spoilboard bed....not mandatory though but I have found I get better consistent cuts.

But like Jack I to have succumbed a many a time to forgetting to zero to the bed before screwing down my 4x 4 sheet:eek: The other problem is that if you have to do a tool change or two during the project cut it's a problem if you don't have anywhere to put your Z zero plate on the bed....below is my way if I have to do a tool change until I can find better.....

Anyhow put your Z zero plate on bed and zero your first bit the usual way.
Then I lay down my 4 x 4 sheet and screw it down
Then the first cut I do (programmed) is have a profiled hole cut out on some dead space on the sheet
Then when I have to do a tool change I put in my new tool but only hand tighten the collet nut.
Move to over the hole and lower the bit manually down into it until the bit just starts to move up the collet.
Then I zero the Z axis.
Tighten the collet. This bit is now zeroed to the bed.
Continue cutting.

Cheers

[adrianm]

Depends on the type of toolpaths you're doing. For through profile cuts it doesn't really matter (on most materials) if the first pass is starting a fraction deeper than planned but you don't want to be short on the final pass.

I use an off the table zero spot which is adjustable to whatever the spoil board height is. If I'm doing a toolpath where the depth of partial cut is critical (such as a pocket, 3D, or VCarve) then I'll zero off the material using the plate instead.

I modified my Post Processor and ShopBot files to make that process automatic so I don't have to worry about it which zero is which. The machine tells me and then does it.

[ssflyer]

I guess it depends on your machine, but I notice most people seem to put their spoilboard on in the middle cutting area of the machine. On my 96 x 60, I ran it all the way across. This has a couple of benefits, in my mind:

1) keeps chips from falling under the table
2) The machine actually has a larger cutting area than advertised, so I have room on the sides to set my Z-Zero plate.

For sheet goods, I usually cut 4' x 8' sheets, so I always have room for the plate. For 5' wide sheets, I still have room. ;)

[chunkstyle]

Kip,

I hacked off a 1 1/2" chunk of that aluminum zero plate and mounted it off table. Around 12.5,50.125 spot. Whenever the cutting file has a tool change the machine runs off table and uses that hunk of aluminum to touch off from. Cutting resumes. No fuss, no muss.
Whenever I resurface the spoil board it's usually by .02-.03". That number gets deducted from the 'block height' value in the 'my variables'. Save the settings and check the block height value just saved by touching off the plate again using a 1/2" price of drill rod in the spindle. I then lower the drill rod to the table with a z move of .014". Check the gap between table and end of drill rod with .014" feeler guage. I find it like checking motor valves in an engine. Too loose? Try the .016" feeler. Too tight? How bout the .012" feeler? Reduce, increase that difference from original z drop of .014" (+- .002") in the block height value of the 'my variables' folder. Lot of explaining but goes pretty quick and becomes routine SOP after every resurface of spoil board.
I'll run that drill rod around the table and check in several spots with that .014" feeler guage. It's pritty much right on the money around the table. Been doing this with good productive results. I cut cabs for my business as well as for other shops. Hope this made sense and helps.