Z Zeroing to Spoilboard Question

[WaltS]

So I've read a lot of threads about personal preference for where to Z zero. I personally like to zero to the top of the workpiece. I measure the piece with digital calipers and put the value in VCP. I was reading a recent thread about doing the same except for the profile cut, and zeroing to the spoilboard for that. That lit a lightbulb under me. My workpieces are not always perfectly flat, and I do not surface each piece, for personal reasons. So if I measure a piece at .762", it may be .765" someplace else. I usually take several measurements and use the thickest, but it doesn't always work out to the .000" and when I run the profile cute sometimes I have to go back and add an extra .02" or so to finish cutting all the way through the piece at some places. So if I zero off the spoilboard for the profile cut, I can put in a thickness number a few hundredths or so more than what I measure my piece to be, and then when I cut it it won't matter if I was off by a few hundreds, right? It will air cut a little before it gets to the piece and then cut down to the spoilboard and stop. Is my thinking right, or am I missing something in the process? I know I will have to remember to change the material thickness before calculating the profile cut, but other than that? Thanks as always.

[4DThinker]

If your spoilboard has been machined flat, then use it to zero out Z except put in a negative value of the thickness you told Vcarve your material was. Now Z zero will be exactly the height above your spoilboard that your tool paths think the material is. No matter how inconsistent the material thickness really is all profile cuts will cut through.

[highpockets]

+1

[highpockets]

Peter at CNCnutz on Youtube has a good explanation.

[WaltS]

Ok thank you. So to make sure I got it, I shouldn't do what I was thinking and change the zero datum point from top to bottom in VCP setup for the profile cut? I should change the Z zero setting in my machines control program after I zero off the spoilboard for the profile cut? And yes, my spoilbaord is surfaced and flat. Thanks. I was thinking about it wrongly it seems.

Edit - ok thanks, let me watch the video first.

Thanks for the video, John. Ok, so I did understand correctly. so if my piece is .762 - .765 I would put in -0.765 in my control software after I zero to the spoilboard. Sounds great. Excited to try.

[Adrian]

If you zero to the spoilboard and set VCarve to the same then you will always cut through the material regardless of the thickness of the material. No calculation required. I actually set the z-zero a hair lower than the spoilboard surface as that lets me produce parts that require no sanding at all. Resurfacing the spoil board every couple of weeks is a lot easier than sanding hundreds of parts.

[Leo]

There are bunches of viewpoints. I have used both methods through the years. Mind you, I am from a metal cutting world and from a manufacturing world. I have worked in 8 different companies for between 3-10 years in each one, programming Lathes, Machining centers both Vertical and horizontal. I even worked in one place on a twin spindle CR Onsrud router. Done a lot of interesting things.

Even on a lathe we could debate where to put "Z" zero and why. I'm not going to go there

Years ago when I programmed machining centers, no CAM or computers to write code, I programmed "Z" zero to top of part. The philosophy was simple. Minus "Z" numbers were cutting, and plus numbers were not. You can make the same argument on a lathe to locate "Z" on face of part. MOST swiss lathes, or bar machines are face of part.

(not a repeat)
Years ago when I programmed machining centers, no CAM or computers to write code, I programmed "Z" zero to fixture location point - (essentially, bottom of part). The philosophy was simple. All programmed numbers were from a common program zero, regardless of how the part was placed in the fixture. You can make the same argument on a lathe to locate "Z" on the chuck jaws.

Then there is tool setting, and radius compensation, and other stuff too.

Every company I worked at had strong opinion as to which way was best. They all told me to do what I felt best, but if I did something that was not to local convention - whoooeeeee - that was a disaster. Soo, I learned to follow local convention. Now, to me, it really doesn't matter where "X" - "Y" - "Z" zero is, I just roll with it.

Soooo - who is right and who is wrong. I'm not going to answer that either way. They are both right. Vectric knows this, that is why you have choices.

Here in this forum, there is no defined local convention.
What you will hear over and over is the same thing.
Top is good, because---------
Bottom is good because -------
And they are right.

It can get confusing because there "SEEMS" to be nobody making a strong case for what to do. That's cause any way is going to work well, and you have 10 choices.

Again - it's all about personal preference. My preference is Top - Center I have all my reasons and if I had employees they would do it MY way. I DO deviate sometimes depending on the situation. Top Center does not work for tileing.

Lots of people do it lower left bottom. That philosophy is - all numbers are positive and any negative numbers "could" be a potential problem.

Notice - in my philosophies, most of the reasoning is in the sign of the numbers in the program. Let me ask, do we read the g-code any more? If not, does the sign of the numbers matter? For me, at home and with Vectric I don't really care about the numbers, and I am a g-code guy. I am still actively programming long have professionally. At work I program mostly lathes and I program "Z" zero to face of part.

[LittleGreyMan]

Soooo - who is right and who is wrong. I'm not going to answer that either way. They are both right. Vectric knows this, that is why you have choices.

+1

We generally work like Adrian, but not always. Depends o, the part, the job and the way you hold the part: directly on the table, on a spoilboard, with vacuum…

If you are simply engraving a perfectly flat material, why bother with its thickness? In this case I zero on the top.

The important thing is the way you asked your questions: it demonstrates you understood the principles. So don't be shy, it's up to you to make the better choice for the job you're running!

[WaltS]

Thanks for all the wonderful, helpful, and informative posts, as always, I learned more than just what I was asking. Love this forum. Best people ever IMHO.

Just to note, I mostly do flat, rectangular signs, some are just that, simple rectangles, where they are cut to size before I carve them so thickness of material "usually" doesn't even matter. That's why I pretty much zero to the top of the material. The ones that aren't just plain rectangles and have a somewhat curvy profile are the ones I'm now rethinking, and that is what my original question was about. I don't mass produce anything, and so far have limited business, but at least I'm getting business, which is exciting. But the point is, I don't mind taking an extra minute or two to do something right now, and I'd rather spend that time on the piece instead of resurfacing my spoilboard (it's a pretty complex SP and after I run out of resurfacing options I somewhat dread making a new one). I understand the other way around, also. Both make sense. I've always zeroed X and Y to the bottom left, it makes sense and works for me. I have fences attached to my SP for that purpose and it's just so easy for me to slap a piece into that corner, clamp it, Z zero and go. I still don't see the need, for me, to go from center, but I may some day. But at least now I see a clear reason to Z zero off the spoilboard for a profile cut. I read these forums everyday, and it's exciting to put into practice something I wondered "why do it that way" about. Thanks All!!!

[Leo]

Walt,

I love to explain things to you. You are excited to learn, so that helps me to get excited to teach. I am still working and part of my job is teaching. I currently have several young apprentices under me. One in particular is a 25 year old girl, with no machining background at all except for a 12 week program for people without a trade and unemployed and at the end of their benefits. One year ago she was working in a daycare facility. One of the local schools, where I earned my BSME degree is running the program. We donated machinery and technology to the program. In turn we get the cream of the crop. My 25 year old girl is apprenticing on a $500,000 grinder and working to 20 millionths accuracy. This stuff gets me all excited.

Yeah - I like top center. Mostly I will eyeball the orientation to the slots on the table to get the sides parallel to axis of machine. Takes me maybe 30 seconds or less. I draw a line across the corners to intersect in center. I will eyeball the cutter to the center mark "X" & "Y". I can get that really close - again 15-30 seconds. Takes longer to tighten the clamps.

I load a cutter in the spindle and touch to top - again, 15-30 seconds.

MOST of the time I cut the periphery, so perfect alignment really does not matter.

As to thickness - that really doesn't matter either. When I use HDU, that is consistent. When I mill or make thickness on anything else, I don't bother with standardizing. I don't get hung up on standard 3/4 thick - at least not on a single piece item. Making a cabinet, sure - making a plaque, nah.

Soo, all in all - I can throw something on the machine and have it totally setup and ready to cut in - errr - 1-2 minutes?

I also don't like machining in the same place on the machine. I like to spread the wear pattern around the machine. Using the method I use - I can be anywhere on the machine.

[WaltS]

If you zero to the spoilboard and set VCarve to the same then you will always cut through the material regardless of the thickness of the material. No calculation required. I actually set the z-zero a hair lower than the spoilboard surface as that lets me produce parts that require no sanding at all. Resurfacing the spoil board every couple of weeks is a lot easier than sanding hundreds of parts.

So are you then doing the way I was originally thinking, setting the Z zero to bottom in VCP? Instead of the way it was suggested here to set it using a negative number in the control software? I'm just curious as to what the differences are? Either way you still have to know the thickness of the material. Just curious.

Leo, thanks for the wonderful information. One thing I have learned since starting all this is there are a number of different ways to do the same thing, and personal preference can be the main reason. Sometimes it's just easier to understand one way over another, but like I said, I learn so much just reading here, even when I don't have a question.

[highpockets]

In Aspire or VCP I set Z Zero Position to top (Material Surface) and XY Datum Position to center, it just works better for me.

I set all tools to Z Zero off the Material Surface. The exception is any toolpath that goes all the way through the material. Then I set Z Zero to Spoilboard minus the thickness of the material (as described earlier). I don't get upset when I mark up the spoilboard, I just don't see the need to cut into it all the time. Again my personal preference.

Walt, you're right there are lots of ways to skin the cat it's all down to figuring out what way works best for you.

[WaltS]

Thanks John. I don't mind marking up the spoilboard, that's what it's there for. Plus some of the marks are fun reminders of projects I've done, like that circle for my daughter's ring bowl. But if I can keep it intact the longer the better that's one less thing I need to remake sometime down the road. Hoping someday to be too busy to worry about having to make a new spoilboard.

[IslaWW]

Now that all the answers and opinions are in, let me chime in with some food for thought. My personal use is similar to Leo's work setups, at least one of them. I use a mill with vises, so my XY datum is top left due to fixed vise jaws. I have tools mounted in holders and change with an Erickson QC system. They are pre-measured and numbered and zeroed to the bottom of the vise jaws, at two levels. All irrelevant, just like Leo notes above, it doesn't matter.

Top of material, bottom of material, the machine doesn't know or care. Click Vectric button on top or bottom for the Z and Vectric doesn't care. Negative code for top zero and positive for bottom. The math is always exactly the same. From a machining or designing standpoint there is absolutely no difference to the design software or the machine operation with either scenario.

Everyone has a preference, maybe even an opinion, but the real question may be in the WHY. Why do some folks do better when Z is zeroed to the top? What about the bottom? Which is more accurate? The answer is that assuming you have flat material that can be measured accurately, there is absolutely no difference. I will assume the worst, your material is not flat and you cant measure it correctly.

If you are doing top critical operations like vcarving or dados, top zero works better, but your cut thru is sometimes short, sometimes too deep. The other case is that your zero is to the bottom and dados or vcarving comes out at funky depths. There are numerous posts where users post about these issues and the number of workarounds they use or are proposed by others is infinite. Dual datum files, bump this, etc, etc. The real solution is to use flat material or surface it with the machine and learn to measure it accurately.

If you follow the numerous threads regarding this topic you may notice that zeroing the Z to material top with a portable, conductive Z setting device is the odds on favorite. FYI: this is the single least accurate method available to those with adequate eyesight. The forum doesn't have enough whitespace to list all the things wrong with that combo.

Just food for thought.

[redwood]

"If you follow the numerous threads regarding this topic you may notice that zeroing the Z to material top with a portable, conductive Z setting device is the odds on favorite. FYI: this is the single least accurate method available to those with adequate eyesight. The forum doesn't have enough whitespace to list all the things wrong with that combo."

Oh, but I want to hear at least a little more about that. Now, I may be one of those without the adequate eyesight (essentially blind in one eye and other little issues), but I would still like to hear the reasoning.