[wganders]

Almost every shop I have worked in just touched the tool off the top of the part with a feeler gage (top of the part was always Z zero); job shop environment. What's the problem with that. Only one place used a gage block to set the tools and that was because they ran the same parts over and over; no real variation in Z, with all the fixtures being basically the same height.

[HuFlungDung]

What is the problem? Lack of an absolute Z plane reference for the tools. Depending on the batch of parts you have to make, you could have a .01" thickness variation even on billet aluminum. If you have any critical features, such as pocket depth, to maintain accurately, you could spoil one (or more) parts after changing out a tool if you reset to the top of a piece of stock with a different thickness than the first piece you happened to pull out of the pile. As I recounted in my story above, it can and will happen eventually, through forgetfulness.

[speeeeed]

It makes no differance what you set the tools to as long as you use the same thing to measure from to the top of the top of the part for the G54 Z work offset. Alot of people use a one inch block of varios materials, as long as it is parallel.
As far as X & Y Always use an edge finder for a square part an indicater for a round part.
Teach the correct way leave it to them to find the quick,less accurate ways later in life. Setting tools to the top of the part directly is not the way to do things for many reasons.
keeping some tools that are commonly used Loaded and set is a great way to decrease set up times (standard Tooling). This does not lend itself to setting tools to the part. Just measure from the top of your block/Standard to the top of the part and put the positive or negative number in the g54 Z work offset.

P.S.G54 is the default work offet not G51. Also there is a setting that will turn off the writing of what is in the
g54 Z work offset to the tool length offset when setting the tools. Be sure this is off.

[helix77]

i agree .... i started out being taught to use a feeler gage.... the better i got as a machinist the less comfortable with this a became.... its not that its not accurate...its just not accurate enough (for a precison toolmaker anyway if you run castings then it might not matter). i have designed and built my own tool presetter.... and let me tell you what.. once you have gotten used to a quality presetting method ..man you can set up tools lighting fast. i dont even bother leaving the same tools in the carousel. (i like to clean the tapers on the tool holders anyway).
after teaching my self the correct way...you couldnt drag me kickin and screaming back to feelergages or jo-blox (unless useing a jo block to sweep an edge)

[Donkey Hotey]

And once you've owned a probing system and tool presetter, you never want to deal with the manual methods again.

This thread has been a real eye-opener for me. Wow, am I ever glad that I got the Renishaw probing with my VF-2. Luckily, I've never had to deal with these methods on my mill. The lathe on the other hand...

[HelicopterJohn]

HI Donkey Hotey,

I ordered the Renishaw Wireless Probing System on my new HAAS TM-1P. I got a message from my dealer that is was finished last Friday. Looking forward to the machine and also the Probing System.

John

[SeymourDumore]

What's wrong with using the top of stock as Z0? As it was mentioned, many things.
One of the most important of those for a jobshop is the fact that you may have multiple setups for multiple parts, or multiple setups for the same part. There is no easy, but certainly no good way of setting your tools to all of them.
Case in point, I have 4 vises and a 4th axis on my VF4. All have a job set up on them that are running parts as they leave the EDM or the lathe. All can run simultaneously just by selecting the correct part program. All tools are picked up to the same fixed jaw, 19 tools total. Never a guesswork as to what to pick where.
Also, who says that the top of the stock has to be the programZ0? Who says the Z0 has to even be on the part?

Nope, picking tools to the stock has 0 advantages and every possible disadvantage.

Toolsetter with fixed side:
http://www.rajshreeengineers.com/z-axiszero.htm

3D taster for picking up X Y and Z
http://www.haff-schneider.de/index.p..._id=32&clang=1

[helix77]

the z0 can be wherever you want it to be...its up to you.... it is just"usually"set at the top of the part... it absolutly dose not matter if you program z pos or z neg.. the machine dosnt care. i think that the point of this topic is that the tools are set so that they are all on the same level, then you change the level of all of the tools together useing g54 z (on haas anyway)..as well as safty and accuracy during setup..
if you have fine tuned all of your vises to run simultanious then thats great..but before that has happend your tools must be set.
i personally set tools from the vise ways(if useing a vise)..then subtract the presetter thickness...then add the distance from the ways to the top of the part.
this allows me to preset from the same place every time..and if i break or dull a tool during cycle i know were to reset it. and since the first operation is usually facing the part ...the reason for setting the tools in this manner becomes clear.

[Donkey Hotey]

the z0 can be wherever you want it to be...its up to you.... it is just"usually"set at the top of the part...

I'm really curious about this method because that's what they told us in the Haas class. What I still don't get is how the 'top of the part' will ever give you control of your part thickness. If I machine from the 'top of the part' then flip it over and machine from the 'top of the part' again, I have no idea how thick the part is.

I've got the Renishaw probing but I still face the same problems. If using a vise, I set a workstop for my X face, then I drop in a 123 block. I use the back jaw as Y zero, the workstop on the left as X zero and the top of the 123 block as Z zero. When I'm done picking off the faces, I subtract the thickness of the 123 block from the Z offset (1") making the top of the parallels, step jaw or whatever, the Z-zero plane.

All of my Z's are now positive and I control part dimensions from three positive, repeatable planes on the vise. If running multiple stations (vises), each gets a similar work offset of its own and I call them from the program.

Doing this without probing would be the same except you'd use edge finders and a height presetter. It all makes sense to me but I have to wonder if I missed something since so many people talk about using the 'top of the part' for Z zero.

[djr76]

Doing this without probing would be the same except you'd use edge finders and a height presetter. It all makes sense to me but I have to wonder if I missed something since so many people talk about using the 'top of the part' for Z zero.

I wouldnt think so, its more of a preference thing. I set all my tools on top of the part, but 99.99% of the time, my first tool is a face mill where I face the part to establish a set Z plane. There is nothing wrong with the way you are doing it.

[Baketech]

Very interesting thread...

I tend to use different methods depending upon the type of job and machine. It's good to be flexible here, and use the best strategy for the job at hand.

Many of the fixtures I've built include a spot for setting X,Y & Z. This just seems to work for many of the reasons already pointed out in the thread...

For piece-work, it often becomes the top of the part just out of convenience...

[helix77]

donkey hot key.... you are doing it exactly right.. its just that when you substract your 1-2-3 block thickness this is where 'you' are done... the rest of the people useing the top of the part method simply add the part thickness back (with the exeption of the stock to be faced away).
this top of the part method is usually op 1 for me.. because it dosnt matter how much is faced off (usually .01-.03).. because the finished thickness will be machined and maintained on op 2

[maxine]

The short of it is, on the mill, that your workoffsets become active in all 3 axis as soon as the program reads the G54 (or whichever one you are using). So, the Z work offset has nothing to do with tool length, but everything to do with reference planes.

I feel that it is good practise to set the tools to a special gauge block (something that you and your students will reserve for this sole purpose). A vertical dial gauge called a presetter can be bought to serve as this gauge. I'd be remiss to have it in the lab for fear the students would crush it.....make that "for certainly they would crush it" But, any thing can serve the purpose so long as everyone agrees that the object would be the setting gauge. Such a device should at minimum have carefully faced and parallel ends. A 2-4-6 block would work.

So touch all the tools off this gauge block. This way, if you need to add more tools, or change out a broken tool, you'll have something you can quickly set on the table to touch the new tool off of.

Now, there will be some random difference in height between this gauge and the actual top of the workpiece. This difference is, of course, the same for all the tools in the set that you have installed and measured, and so the Z component of the current workoffset serves exactly as a method of compensating for this distance.

In jog mode, switch your Position display to the operator screen. Usually your last tool will be sitting on the gauge block because you just finished measuring the last tool length offset. So, if the tool is touching the gauge, and the Z axis component of the screen display is flashing (because that is the active jogging axis), press Origin to zero the Z axis display. Now jog away from the gauge, and over to the workpiece. Touch the workpiece. The jogged value in the Z axis display will be the measured distance between the gauge and the work. You'll have to key this value into the Z work offset register of your choice, you cannot teach this position in with a single button push.

I'd advise that your setting gauge be 'tall', that is higher than your typical workpiece when clamped in the vise. The gauge should sit on the table and not on the vise. If you follow this convention, then your Z work offset component will be negative in value. If your student forgets to type in the correct sign, the ensuing accident takes place up in the air In contrast, if you pick a setting gauge that is 'sometimes higher, sometimes lower' than the work, then you run the danger, almost with 100% certainty, of having a serious crash.

Many guys will set all the tools directly off the workpiece. This is okay, but then your Z work offset component is left as zero all the time. You'll also need to redo the whole set of tool offset measurements whenever you change workpiece height. There is a potential pitfall to setting the tools off of a workpiece, especially if it has no good reference surfaces on it, or if a series of rough cut bars will be machined and they vary somewhat in height. If you set the tools on a rough reference, then face it, the reference is gone and is not recoverable. Setting up a new tool to a new reference plane while leaving the rest of the set of tools unchanged can easily result in a spoiled part.

CNC newbie here trying to follow these instructions. When you say "switch the display to the operator screen" how do I do that? I couldn't find it or more accurately I am learning and just don't know which screen is which. I appreciate the help !

[Geof]

CNC newbie here trying to follow these instructions. When you say "switch the display to the operator screen" how do I do that? I couldn't find it or more accurately I am learning and just don't know which screen is which. I appreciate the help !

When you push POSIT several times you step through all the various screens. One shows all the coordinate positions; Machine, Work, Dist to go and Operator at the same time. You can step through them individually by pushing POSIT and looking for the name at the top of the screen.

Did you have alook at the thread I started on setting tool offsets? Here is the link:

http://www.cnczone.com/forums/showthread.php?t=41641

This procedure is equivalent to the one Hu describes but I think mine is a bit simpler.

[maxine]

When you push POSIT several times you step through all the various screens. One shows all the coordinate positions; Machine, Work, Dist to go and Operator at the same time. You can step through them individually by pushing POSIT and looking for the name at the top of the screen.

Did you have alook at the thread I started on setting tool offsets? Here is the link:

http://www.cnczone.com/forums/showthread.php?t=41641

This procedure is equivalent to the one Hu describes but I think mine is a bit simpler.

Thanks for the help. I will go read that thread and then head to the shop and page through the POSIT like you suggest. Sorry for rookie questions but I want to make doubly sure I am doing the offsets right. This is my first move from manual to a CNC machine and I don't want to crash my new machine right out of the box.

One other question if I may? My machine had a couple of minor problems when it arrived with some parameters set wrong. Selway came through for me by figuring out the problem and fixing it. But when he did that he downloaded some stuff from a memory stick he had with him onto my machine (diagnostic stuff maybe, I am not sure?). After he was done with the repair he deleted all the programs that were stored in memory. Before leaving he reloaded the spindle run in program and the spindle warm up program, but I noticed yesterday that Visual Quick Code and Quick Code are also gone. Plus I don't know what else was in there that got deleted. I only know the quick code stuff was there because I had looked at it a bit while I was waiting a week for the repair work. So how do I get those programs back and what else should be there that I should be looking for?

Thanks again for the help, sites like this are a gold mine for a beginner like me.

[Geof]

...... I only know the quick code stuff was there because I had looked at it a bit while I was waiting a week for the repair work. So how do I get those programs back and what else should be there that I should be looking for?

Thanks again for the help, sites like this are a gold mine for a beginner like me.

I think you are going to have to chase your service guy to reinstall them.

[Geof]

Thanks for the help. I will go read that thread and then head to the shop and page through the POSIT like you suggest........

Thanks again for the help, sites like this are a gold mine for a beginner like me.

You might have already found out your gold mine is filled with iron pyrite...that is fool's gold .

Don't page through using POSIT; POSIT pushed once brings up the position page and cursor Up or Down pages through the various displays. Sorry about that.

[maxine]

OK thanks I did figure that out and found the operator screen yesterday. Once I did that I followed the posted directions and the the tool offsets worked fine.

Also today I looked at the memory stick that came with the machine for the first time. There are a whole bunch of programs on it so I am hoping that quick code, visual quick code and anything else that was deleted is there. I just need to figure out what the program names mean.

Yeah it may be fools gold I bought but I am having fun learning it

Thanks again for the help!

[Geof]

....Also today I looked at the memory stick that came with the machine for the first time. There are a whole bunch of programs on it so I am hoping that quick code, visual quick code and anything else that was deleted is there. I just need to figure out what the program names mean......

Coincidentally I looked at a floppy that came with one of my older machines and found all those files. There is also a README.txt which identifies everything.

[maxine]

That's great news. I didn't notice a readme file but I wasn't looking for one either. It must be there. I'll check when I can get over to the shop tomorrow. Thanks for the heads up.