Zero to table top or top of work?

[gene]

What is the advantage to zeroing the bit to the table top as to the top of the work?
If you zero to the table top and cut 3/4 materials what do you do differently as to the bit clearances so the bit dont hit the work while jogging to position?

[myxpykalix]

This is something that always concerns me. I alway zero to the top of material but occasionally you get a file that is created with the zero to top of table.

Sometimes you don't know that and it took me several tries when it would "top out" to figure out that the Z was to the table and the default Z travel height was too high and the combo of those factors caused the "topping out".

Also I would think if you zero your x,y and not the z but move your carriage but then try to do a JH you will certainly run into something (ask me how i know).
I haven't run into an occassion where I thought it was better to zero to table. If you zero to material you have the bit above the material plus your set default above Z travel height.

[beacon14]

Many people who mostly carve into the top surface of their workpieces zero to the top of the material routinely, however most people who do a lot of through cutting seem to zero to the table.

The advantage of the latter is control over how deep the bit goes into the spoilboard. The advantage of the former is control over how deep the bit goes into the surface of the material such as for V-carving. Most people swear by one way or the other because they are used to it, and have to be very careful when doing whichever way they are not used to.

[knight_toolworks]

I use both but when cutting plywood and such it is nice to zero on the table. but this is harder to setup the toolpath if you don't want to cut all the way through or all the way in one pass. vcarve will do it in one pass unless you tell it not to cut all the way. stepdown does not work on table zero for the most part.
so both work well depending on what you are doing.

[ed_lang]

Gene,
I zero both ways, depends on the job. Here are two examples.

If I want to V-carve into material, I will zero the Z at the surface of the material. I want the v-carving to go into the material exact distances.
Yesterday I was cutting some Corian signs. I was able to zero the Z to the top of the material and V-carve as well as cut out the shapes. My Corian was 0.5" and it didn't change thickness much across the material. (unlike plywood)

When I am cutting cabinet parts or other items where I will be cutting dados and rabbits I zero to the table. Reason being... the material will vary across a sheet of plywood in thickness. If I have to hold a tight outside finished size the depth from the top of the material for the dado is not as important as the amount of material left from the bottom of the dado to the table. Also when the material you are cutting is not the same thickness across the sheet, how will you cut out the parts cleanly? Some places you will be cutting deeper than needed and some places you may not cut through. Zero to the table and cut clean parts.

I use both methods to zero but if you decide to use both in one project, be sure to keep straight what tool path was created using which zero point. When you mix up the methods, PartWorks and V-Carve PRO will not be able to simulate you entire project.

To help me keep straight on what tool path was created at what zero point I name my tool paths like this....

90deg Ztop lettering --- This is cut with a 90 degree V bit with the Z zeroed to the top and it cuts the letters on the sign.

0.25EM Zbed cutout --- This is cut with a 0.25" end mill that has been zeroed to the bed of the machine and will cut the profile of the sign.


Make a little sawdust and try both methods. Then mix up the methods and see how that works. Find out what works best for you and your jobs.

If I have not been clear in this post, please let me know.

[donchapman]

By always zeroing to the top of the material I don't have to rely on my memory as to which I chose "this time".

If I need to make a through cut I measure the material with a digital caliper and usually leave .02" skin on the bottom of the material so my vacuum hold down will securely hold the material.

I could just as correctly have chosen to always zero to the table, but the important factor for me is consistency, since I know myself well enough to realize that if I were always swithching back and forth I would eventually screw up a $375 sheet of HDU, or worse.

[harryball]

What Ed said... I use both methods as well. For files I use often I put a popup message in the file that says something like "Set RPM's to 15k and Zzero to the TOP of the material"

It reminds me when I come back and run the file again. When I'm running bat house kits I zero to the top of the material to cut all the grooves and to the table when I do my cut throughs.

Robert

[myxpykalix]

See you learn something everyday! Since i don't cut cabinets i've never thought to zero to the bed (or why i should do it that way) but now I do. So thanks Ed you're still teaching me stuff a year later.

[Gary Campbell]

Gene..
Another reason to possibly zero to the bed could be in the case of dado's. If you have 3/4" plywood (normally varies +/- .030) you can set the mtl. thickness to .75, your dado depth to .25 and no matter how much the materials vary, you will always be left with .50 in the dado area. Until we switched to Columbia Pure Bond plywoods, we always did it that way. Now with all the sheets we have measured falling between .743 and .749 we just zero to the top and it makes our cutting, drilling and dadoing easier to keep track of as Ed alludes to above.
Gary

[dubliner]

I saw these the other day & thought they would be a neat way of Zeroing in a hurry if you needed to, what do you think? You could reverse the prong.

7902

[hespj]

I zero to the table unless cutting full size sheets when I zero to the top of material (the table is inaccessible with a full size sheet in position).

I prefer zeroing to the table for 3D stuff because:

a).....After the first cut I probably lose the top surface of the material and no longer have anything to zero to.

b).....The 3D model is probably drawn with zero at the base, and it's natural to mimic this on the ShopBot.

I would prefer to cut sheets with zero at table too, this would allow for sheets which are a slightly different thickness, or if you want to use the same file for (say) 1/2" instead of 3/4" sheets. But as I say, with a full sheet on the table zeroing to the table becomes impossible.

[handh]

John,
You could set up your shopbot with a zero level with the table top like Ed has done here in his article. I'm going to set me up something like this on my shopbot.

http://www.shopbottools.com/getting_started.htm

Jeff

[butch]

John
I'm a new-beeie to this ShopBot CNC work, but here's what I do.
If I want to cut through the material, I zero Z to the table. But if I am carving into the material, I zero to the top of the material.
To keep me correct with a reminder, I open each file in an editor and put a print memo with a PAUSE command before the SO command to tell me where it should Z, bit size and any other information I might need to cut the file. Something like this
'My Cut File / Z=table X&Y=0 / 1/4 End Mill'
PAUSE
SO,1,1
etc.

This gives me a reminder what I need to set the SB at to run the file so I know if I am correct before the file runs. With memory defficit I need little notes all over to help me 'remember' what I meant to do!

Butch

[ed_lang]

Wow! Folks have read my articles.

Thanks Jeff.

[hespj]

Ed/Jeff - Good idea. I was thinking something like this would be a good idea, but didn't know how to implement it. I was thinking of something along these lines because I'm not convinced that the current Z Zero method is very accurate.

"if I am carving into the material, I zero to the top of the material".......Butch

Good point Butch. I haven't done much carving on my machine (much to my surprise), but one certainly needs to do this. I put info I need about the file in the file name - machining operation, tool type and size etc - maybe this could be incorporated in the file name too.

[knight_toolworks]

I just bought a cheap piece of aluminum off ebay for this job.

[bcammack]

Because our machine is configured with a clearly defined work area on the table separate from the "at rest" 0,0 point, I bonded a 2.5" square piece of unetched printed circuit board to the tabletop with contact cement, drilled a small hole through the top at the edge of the pc board, soldered a wire and passed it down through to top to the control box where I wired it in place of the original z-zero plate wire.

Then I revised the z-zero program to pick a random point within 2" of 0,0 to touch off of. It does it all without pause.

Our application is a bit different, of course, because of the way we use the ShopBot for a single purpose, cutting out sink and faucet holes in bathroom vanity tops.

[bill.young]

Here's my rule of thumb when deciding where to zero for files.

If the CUT is the most important feature...I need a .25" deep groove or am v-carving..then I create my files with the Zero point at the material surface. If the MATERIAL THAT'S LEFT is the most important part...I need a tongue that's .25" thick or want to leave .02" uncut to help with vacuum...the I zero at the table surface. This way I don't have to worry about variations in material thickness or need to accurately measure each sheet..it doesn't matter.

If neither is important (or both), then do it whichever way you prefer. I tend to zero at the table surface by default, but that's just me...pick what you're comfortable with. Whatever you do, though, make sure you add that information to the header of the file...it's good insurance.

Bill

[harryball]

I only wish I could choose the Zero method per toolpath, not for the entire file. I will often want to vcarve something onto a project which requires a bit change and rezero anyway. I will run all my regular cut throughs and tabs etc... zero'd to the table, then I want to zero to the material top and do the vcarve.

I understand the potential for confusion... but it could be no more confusing than me changing the zero method and recalculating the desired toolpaths then remembering to change back.

Robert

[gene]

Thank everyone for their replies, i had no idea it was so diverse i also liked Eds reason for the dado depth . it makes perfect sense but i never thought of it like that . The alumium rod for the table zero contact is also l sharp idea .. THANK YOU all

[knight_toolworks]

there is a way to do both methods. zero at the table raise the z to say .75 if thats the material size or where you want the zero to be then zero again.
this lets you overcome the thickness variability but it is easier to make toolpaths when you need both. so you need a .25 deep cut well just put in .25 and you have it.
I used this method when I had all of these wooden blocks that had to be all the same thickness. so with this method zero would be the thickness I wanted and I just did a pocket at zero and they were all the same and the rest of of the cuts could be done on the same toolpath file.

[Brady Watson]

Steve,
Look at Ed's write up (http://www.shopbottools.com/getting_started.htm) called How I Zero the Z to the Bed

-B

[knight_toolworks]

yes I plan on setting that up got the aluminum on hand. my method is more to make it easier to have both types of toolpaths going in vcarve.
vcarve from what I have found does not use setdowns and such when you use the surface to cut.