Newbie- Zero top of material or top of bed

[Action-KAT]

So I'm finally cutting some things now on my router, have a quick question regarding where is best for zero the Z.

I am mainly going to be cutting wood and maybe acrylic and possible Ali later.

Is it best to Zero on top of material or the machine bed.
may train of thought is if I cut a couple of repeat wooden parts and one wooden blank is slightly thicker then I would need to redo my Gcode to take this into account every time I cut.
Where if I go off the bed anything thicker will still end up finished the same size after routing just cutting the top lower.

I am thinking more when the wood is profile cutting I can be very accurate to a gnats gonads when Zero to the table bed but if I go off the material and I cut a couple without redoing the Gcode then I could be quite a lot out.
What are your thoughts on this
How do set your Z and why,
It might be straight forward to some but I'm new to this so always learning cheers guys

[CarveOne]

I always zero on the top surface, and now I use a zero setter plate to zero the cutter more accurately than "just eyeball accurate".

CarveOne

[Action-KAT]

Hi CarveOne
I take that's material surface,
Do you have reset you Gcode if you are cutting a repeat part where the material is slightly thicker, or how do you get around this.

[ger21]

The top is always zero.

But, what I do, is reference to the table, then set my zero a fixed distance above the table, whatever the thickness is supposed to be. For the exact reason you said, the same code works regardless of material thickness, provided it's close. My auto zero does this automatically, with the thickness entered in a DRO.

When V Carving, though, I reference off the top, as Zero needs to be exactly at the top.

[CarveOne]

Originally Posted by Action-KAT Hi CarveOne I take that's material surface, Do you have reset you Gcode if you are cutting a repeat part where the material is slightly thicker, or how do you get around this.

Yes, that's material surface, not table top. I use the zero setter for each piece I cut. It automatically compensates for the zero plate thickness and if the material is thicker or thinner it still cuts to a consistent depth. It also retracts the same distance relative to the material surface for the clearance height. It takes a lot of effort out of getting setup for each new job.

The one I'm using right now is Greolt's Aussie Zero Setter, but I'll change to ger21's Mach3 screen and the Big Tex zero setter in the near future for some extra features this combination has.

CarveOne

[RomanLini]

I always zero to the table top, with an accurate Z axis tool setter. Then use a height gauge to measure the material thickness and enter that into the software.

But most of my work is more "machining" of a finished size object like a block or a device etc (which must be referenced to table top) rather than "engraving" into the top surface of stock.

[UUU]

I always treat Z-zero as top of the work. I find it's easier to review the G code when positive Z values are clear of the work and negative are cuts.

For setting, I use a 6mm precision roller - bring the tool close to the top of the work, and retract slowly until the roller will pass underneath, then set Z to +6. This is slower than a proper Z-setting tool, but it's very cheap, and fairly foolproof.

[Cruiser]

The placement of Z zero is a preferential thing, it can be top most of matr'l or the bottom of the feature in order to match the print or drawing.
The problem is staying with one or the other within the program and keeping the reference in mind.
Most of the wizards give no option of where to place zero, it is usually on top most of part. When this is the case then just stay consistent.
When I hand program a part, I always put zero at the bottom of feature and then all cut measurements will conform to the print instead of having to convert negatives to positives and have possible error in the conversion.
Another point of reference here could be with the setup of the machine itself. All the machines that I've run in the last 30 yrs have been setup with face of spindle (no tool holders) touching table being zero. Then home the Z to switch without auto zero and read the dim and enter it into the homing function and turn on the auto. Now I can measure a tool, enter it into offsets, and mount it, then measure the part/fixture/vise etc. and enter it into WPO. Then command machine with proper entry's to a position and test it all for being proper.
Another trick I use is keeping g54 empty and unused, all programs will use another WPO. Then to quick set a tool I will call g54 (no wpo entered) and run tool to table and using a micrometer standard set it to a friction slid under tool then set tool's new offset. Until I started doing this, I ran into occasional trouble by forgetting that WPO's effect tool position when setting.
These are the basics that I use and it keeps me out of most trouble.

[Action-KAT]

Thanks guys
This all makes me think I'll Zero to the table top for most of my work
that way repeat work doesn't need the Gcode changing just needs to be close.
and top of the material if I have any engraving work to do
More than likely same way as ger21
and I will get around to setting up an auto zero tool as soon as I can.
cheers for putting my mind at rest with which way to go
KAT

[hemsworthlad]

Do the auto zero sooner rather than later. It will be the best 10mins out your life you've ever used.!

I zero using both methods depending on material and job, 95% of time referance from material top because I'm cutting Ali and don't matter but if like you need accurate finished thickness then work from ref off the bed.

[Action-KAT]

Cheers hemsworthlad

That's about where I'm at but mainly wood so the other way round for me.
I am just looking at the auto Z now,
so hopefully have it sorted sooner as you say.
cheers for the advise
KAT