Where to zero Z

[mikejohn]

The answer to this may be in the Forum somewhere, but I've carried out a search and can not find it.
Is there a convention when you zero z at the table, and when you zero z at the top surface of the material?
As one method gives negative Z in the .sbp file and the other positive, this must be important.
I can see where either way might be preferable.
If you had two lengths of material of on even thickness, you create a perfect lap joint by cutting one down to a known height above the table, the other the same known height down from the top of the material. You do not need to know the exact thickness of the material, your joint will be perfect.
So, is there a simple convention for this?
.........Mike

[billp]

Mike,
One case where zeroing off of the table comes in handy is when you want to cut out part files of different thicknesses. If you zero off the table you just have to make sure you start your bit ABOVE the surface of the material(s), and then whether it's 1 inch or .25" you will cut the same patterns. Of course you need to be aware of the cutting length of your bit when doing this, but it means the same file can be used in multiple applications.

[gerald_d]

Mike, a digital caliper (http://images.google.com/images?sourceid=navclient&ie=UTF-8&rls=GGLD%2CGGLD:2005-07%2CGGLD:en&q=digital%2Bcaliper) is one our most useful tools. We then know the thickness of stock, depth of cut grooves, etc. Our preference is top surface of stock at zero, but we are not religious about that - sometimes it makes more sense to zero the table, or on a ledge in the part. Generally we know that the "minus" depths actually cut something - as deep as the minus number.

[mikejohn]

Bill, Gerald
So its a case of judging the prefered method when making the cutting file?
The digital calipers look a lot better than the ones I have now (squint and use a magnifying glass!!) And not very expensive. I guess they all go imperial or metric?
How does hole drilling work best? If I want a 6mm (1/4inch) hole do I plunge with a 6mm bit, or make 6mm circles with a 4mm bit (in 6mm Birch ply)?
..........Mike

[billp]

Mike,
In reality I think you can make almost ANY size circle ( as long as it is smaller than the ultimate size you are looking for) as most programs will use the center of the bit as their "guide" when generating the toolpath. So if you drew 1mm holes and used a 6mm bit your final hole would turn out to be 6mm.....
And Gerald's point about using digital calipers is REALLY important. Probably more so these days than ever, as lumber distributors look for more ways to "economize". That's why they sell "plywood router bit sets" KNOWING that the true thickness of what you buy is no longer as advertised.

[Brady Watson]

Mike,
If you search around you can find a digital caliper for $40 accurate to .001". If you wait until Christmas time...Harbor Freight has them for $15!


Another important thing to check is the thickness of your z-zero plate & the &ZBot variable value in the zzero.sbp file in SBParts. There should not be a dicrepancy between the 2 values...if there is, then all of you parts will be off (or table will be gouged) by the difference. Mine was out a full .01".

While you can tell the machine where zero is anywhere, every toolpathing program I have ever encountered defines zero at the top of the block. By doing it that way, there won't be confusion when talking to other CNC operators regarding zero position.

One advantage to zeroing off of the table is that you can create a custom part file that will run to the zero (table surface) regardless of material thickness. In other words, you could run material that is .23, .25, .28" thick without the need to re-zero each sheet in a production run. You do however need to make sure that you have a safe-Z height high enough to clear the material...

-Brady

[Ken Brisk (Unregistered Guest)]

Great information! I have had my machine for five years and I have always zeroed off the material and set the depth of cut in my file. I never thought to zero on the table. This forum is the second best tool in my shop. Of course the Shopbot is first.

[gerald_d]

Those calipers shown in that Google search above are practically all identical in shape. Why? Because there are many "Chinese" copies of a good original Japanese design. The original is from Mitutoyo, which is much higher quality and price.

A display with 0.001" resolution can mislead one into thinking it is that accurate (especially with the copy brands). The slightest change of thumb pressure, or temperature, or position of the object in the jaw, makes the reading go all over the show.

[mikejohn]

Gerald
You are from the dark side, a metalworker

I believe such people as you need to work to very tight tolerances.
In your opinion, what is a reasonable tolerance to expect from the ShopBot cutting softwood,MDF or birch ply?
.....Mike

[gerald_d]

Mike, you started this thread under the pretense of asking "Where to zero z" - since it is your thread, you can probably go anywhere you want with it.......

Without compensating for anything, taking a first cut, we will probably get within 0.5mm for x&y. Then, by by tuning for deflection caused by flex, runout, bluntness, etc, we can easily get down to the 0.1mm or 0.05mm ranges. The z direction is always more accurate (less flex and run out) - 0.05mm is pretty typical.

Anyway, we dont make an issue of final dimension, but we do often make an issue of final fit. We can consistently produce dowel holes that are tap_once_with_a_mallet. Customers ask us sometimes to make looser joints because they want space for glue or paint. The ShopBot will spit out 100's of parts for you with identical fits, though you may have to tune the first few samples.

[mikejohn]

Gerald
One of the problems I find with the Forum is the wander factor. I'm inclined to look on it as a multi-person conversation.
Many times, a reply then directs me to a question which veers off track slightly.
Three answers later, and I've moved many places sideways.

So whats the more correct forum protocol? To start a new thread with the new question, perhaps pointing towards the old thread, or allow for thread drift?
Your precision I find impressive. Maybe in the weeks to come I will find my precision impressive

......Mike

[fleinbach]

I prefer Zeroing off the material surface. Not to say that in some isolated circumstance I may find it desirable to Zero else ware. To me it boils down to consistency. If I consistently Zero to the surface it is easier to maintain a mind set that all my cuts are a negative value.

[gerald_d]

My take on thread drift is that the person who started the the thread is the one to be satisfied with the direction of the thread. If someone starts a thread with a question, then it is rude for someone else to hi-jack that thread until it is clear that the original question is not being discussed any further. However, the fact that the conversation is reserved for the person that starts the thread places a high obligation on the thread starter to do his homework and to acknowledge that someone is taking the trouble to reply to him/her. If the thread starter is not really taking part in their own thread, then I have no problem in causing some drift.

That precision is not impressive to the folk who believe the last digits displayed on their SB screens or their measuring tools - but it is realistic day to day stuff.

[bill.young]

My philosophy on z-axis zeroing is that if the CUT is the feature that's important...such as when you're v-carving or need to drill holes that are 1/4" deep...then you're better off zeroing at the material surface. But if the material that's left is the important part...if you want to leave a 1/4" thick tongue on a part or .03" uncut for instance...then you're better off zeroing at the table surface.

If both are important (like scarfs when both the cut and material left are important) then just pick one that makes sense to you and measure your material thickness accurately. I default to the table surface because when I'm just cutting out pieces and there are no thickness or cut features that are critical, I don't have to measure each sheet of ply to keep from cutting up my vacuum table surface.

Bill

[mikejohn]

Bill
I think you have hit the nail on the head.
if the cut is the feature that's important, then you're better off zeroing at the material surface.If the material that's left is the important part,you're better off zeroing at the table surface.
It's easy to understand when your drawing what you want of the piece.
I do take Franks point, and Geralds earlier, that negative values show you are cutting.
I guess its horses for courses, the way that best suits you is the right way.
Gerald, I take your point about hijacking, and will try and stick to that principle
.........Mike

[simon]

Because materials are often warped, bulging, or imprecisely manufactured, I now zero onto the table surface, then JZ to the nominal thickness of the material, and zz there.

I have, however, forgotten to do this last bit on a couple of occasions, however, and made a mess of the vacuum bed, broken bits, etc. I am now going to rewrite my zero routine to ask for the material thickness before zeroing to its surface.

Simon

[billp]

Simon,
I think I am missing something in your explanation; if you are going to "JZ to the nominal thickness of the material,and zz here" WHY do you zero onto the table surface to begin with? It seems like the two steps are where you are having your problem,no?

[richards]

Bill,

If I've read correctly, Simon mentioned "nominal" thickness of material that may be "warped, bulging, or imprecisely manufactured". I've had that problem when milling rough lumber.

Because I'm still relatively new to the shopbot, I always measure from the top of the material to keep confusion to a minimum. (Younger minds may not face the "confusion factor" -- yet.). However, almost everything I cut has consistant thickness (MDF, partical board, baltic birch).

-Mike

[jay]

"Younger minds may not face the "confusion factor" -- yet.)"

Over the last couple of months I have been writing a pause feature at the beginning of my files to ensure that I have zero'd on the correct surface. I find I need to do this as I have been practising Bill Youngs principal on cutting and can easily forget where I zero'd when I wrote the file a month or so ago.

[beacon14]

Bill,

Simon is using the table as a reference surface, then offsetting the zero point by the "theoretical" thickness of the material.

This way he gets the advantages of precise material thickness below the cut, and the ease of knowing that all negative z moves are cutting moves. It sounds like a great system.

Since I rarely do tabbing or skins, I just zero to the top of the material. It's much easier to reset zero after bit changes or for any reason, especially if you are cutting a full sheet, and don't want to have to move the sheet to zero the next bit to the table.