To Z Zero on top or bottom...that is the question.

[nick]

I have been struggleing for some time now with not having a vacuum hold down...I've been screwing things to the base...and I have been Z Zeroing on the material surface...

For one off's it has worked fine...but now that I'm getting busy, my work is getting more complex and involved...

And this method on top isn't working...

Should I be Z-Zeroing on my table base...this makes sence to me but I wanted to see what others use...and with or without a vacuum table.

Thanks again

[Gary Campbell]

Nick...
When we process multiple panels, we zero to a jig that is a known thickness. (.740) ( http://www.youtube.com/watch?v=b7M1mMhOvr0&feature=channel_page )
I wrote a custom file that zeros the X & Y on the index pins, zeros the Z, and writes the drill offsets to the my_variables file.
all of our thru cuts are .750 depth. No mater what the actual plywood thickness is, our cuts and hole depths remain the same.

To cut multiples of the same part you should not have to rezero between parts. Zero on the first.. either to the part or the table, and then run your parts. They will all be the same.
Gary

[nick]

Gary...I forgot to mention that this is only a problem with 3D cutting...

Sorry for the lack of info.

[tmerrill]

Nick,

For my 3D work I normally pick an area that isn't going to get machined and do all my Z-zero's there on the surface.

If the entire surface is going to be machined, you can try this: Measure the thickness of the material as accurately as you can with a digital caliper or similar tool. Z-zero to the table surface, then manually raise the Z to the measured thickness and use the ZZ command to reset Z to zero.

Tim

[beacon14]

Unless I am V-carving or doing a similar cut that does not go all the way through the material I always zero to the table. As Gary says that way the material thickness can vary slightly but my cut always goes the same depth into the spoilboard.

If you can describe your problem in more detail it may turn out not to be the zeroing location. For intricate 3D work using multiple bits the lack of a vacuum holddown may be contributing to the problem if the part is warping or moving as material is being removed.

[bleeth]

Nick: I generally like top zeroing for the following reasons:
1. If the actual part is not the same thickness as I programmed for I still go down into the surface exactly the amount I want. So if there is a relief that I offset the artwork down .03 to be sure I cut it all it doesn't matter if my object piece is right at the designed .75 or not.
2. For box parts I get controlled depth of hinge and shelf holes.
3. For multiple parts I have found that thicknesses of substrate can vary from spec.

Exceptions:
1. For Lithophanes I like to zero from the bottom so I have control of the thinnest part for transparency.
2. If not using vacuum and cutting parts out of a sheet and relying on a skin to hold parts together I have control over that better so it is easier to leave a thinner skin.
3. Zeroing from the bottom tends to result in longer cycle times betwwen spoilboard resurfacing.

If your reliefs are being cut in controlled thickness material such as Corian than table zeroing should be fine. If you are toolpathing the relief after you have perfectly verified the thickness of the material than table zero should be fine. I have had guys who were so used to table zero that top zero seemed ridiculous to them and vice-versa.
The other thing is the thickness of your z-zero plate. I am still using the SB plate that came with my machine 4 years ago. Just now, for the first time, I actually put a digital caliper on it. It varied by a few thousandths. By now it probably isn't perfectly flat either. The quality of the plate and accuracy of the number in your z-zero file can be extremely critical when maching particularly sensitive parts or doing more shallow engraving. (New plate in my near future!!!)
So the real answer to your question is: As long as the parameters of your toolpathing take into account the necessary ingredients implied by your zeroing routine you should have no problem with table zeroing. One advantage of that is if you zero from the table and have a file zero at the top then at least you won't dive into your spoilboard as would happen if the reverse occured!!!
So really there is no definitive answer for this and from the posts that came in while I was replying you can see that once you are used to the system you primarily use it will work for almost all circumstances.

[nick]

Dave,

For the most part they all will be a controlled thickness...but their's always that one...and that stuff drives me crazy when you spend sooo much time in the design and cutting to see high spots and low spots.

For now I will control the thickness the best I can...and the more and more I think about...the more and more I would like to Z off the table and have a vacuum hold dowm so I know my table and material are parallel.

[nat_wheatley]

All of this is mentioned above. Because material thickness will vary, here's my take on it:

If the critical measurement is the depth of cut (face of material to bottom of cut) zero to the top of material. If the critical measurement is thickness of material remaining (bottom of cut to material back), zero to the table surface.

Through cutting falls in the second category, where the thickness of material remaining can be either 0, or negative (cutting into the spoilboard).

[harryball]

If you alternate a lot it can be confusing. Try zeroing to the material top and running a zero to table file. :-) Time to break out the bondo... not that I've ever done that of course ;-)

One solution is to create a readme.txt file in your project cutfiles folder. I put facts in that file I'm so sure I will remember that I forget them the next day.

Sample readme...
ZZero table
1/4 bit mortise comp
XY zero = project center
Run outer profile last

etc...

If it is a single file I might try to add info to the file name...

PanryShelf-14bit_zt.sbp
BathShelf-38bit_zt.sbp
VText-60dV_zm.sbp

zt = zero to table
zm = zero to material.
14bit = 1/4" bit
60dV = 60 degree V bit

I try to keep it simple but the over all goal is to stop from carving up my table and/or breaking bits. These little things can make you look like a genius when you are demo'ing your machine.

/RB

[bcondon]

In my very short time with the machine, I was advised to surface anything that is important for accuracy and then you can always zero from the top of the work. It has worked for me in the last 3 months. I am just starting 3D using aspire

[hespj]

If I'm doing 3D stuff I zero to the table base. Apart from anything else it's more natural to draw a 3D object with zero at the base. Also after the first cutting operation the top face might not be there any more.

For stuff where the table isn't accessible (8x4 sheets) and where the top surface remains intact I zero to the top surface.