Setting Z in G54

[bloefeld]

Here's what I have done to set up my tools.

I touched them off to the flat part of my vise (not the jaws, but the bottom of the vise).

Normally on my part set-up I would add the height of my part about this point to the z-height of each tool I had touched off and then run the part.

However I was told by the HAAS guy that if I just set my Z height in G54 as the height my part is above the point I touched off my tools on, that all of the tools would self compensate for that height and I would only have to set the Z height in G54 once for each different part I made.

I am missing something here? If not, why on earth doesn't HAAS tell us new guys this little secret?

If it is correct, then the only bone-headed thing for me now is to forget to reset the Z-height and thus find a new way to crash my mill.

Cheers,

Bloefeld

[Geof]

.....If it is correct, then the only bone-headed thing for me now is to forget to reset the Z-height and thus find a new way to crash my mill.

Cheers,

Bloefeld

No, there are two bone-headed things you can do, if you insist on using the term bone-headed.

The first is forget the G54 Z value and have a (you hope) minor crash that tries to put a tool through the vise.

The second is to accidently put in a negative value and have a major crash when you try to put the tool holder and maybe also the spindle nose through the vise.

My recommendation is touch off on something higher than the highest point on your workpiece; this way the Z value in the work zero is a negative number. If you forget this Z all you do is machine air above the vise, if you put in a positive number instead of a negative number you machine air even further above the vise.

[automizer]

Think of your G54 Z as a global shift from one point to another. The benefit to this is that if you set your tool offsets to your part then machine off where you set you tools too then break a tool you can now relocate it. If you set all your tools to 1" off the top of your vise then figure out how far it is from the 1" position to the top of your material thats your G54 value. I don't mean to sound rude but what you saying here is a really basic set up method.

[bloefeld]

Hi,

Thanks for the information. I'm called a Newbie for a reason; I just purchased my mill and am not a machinist by trade or by any stretch of the imagination.

Your answer helps me to better understand what the G54 does, and how I can avoid problems that I have not yet contemplated.


Cheers,

Bloefeld

PS, Saying you don't want to appear rude, makes you appear rude. Better to just think I'm an idiot and keep it off the page. This keeps the forum helpful and not polarising

[bloefeld]

Thanks for the good advice. I have learned to run my rapids real slow on the first go and have my finger on the red button. I have all the time in the world while I learn this gizmo and I do a fair amount of 'air' machining too. I have good simulation software and a good editor that also does double duty of showing my tool-paths.

I learned this by starting out making parts out of UHMW PE. When I ran my end-mill an inch into the top of the part it didn't much care. Had I been another half-inch out, I am sure I would have cared a lot more.

Cheers,

Bloefeld

[automizer]

Glad to hear your willing to make a mistake or two to learn. If you learn well from reading I would hunt out a few books to read the help upgrade your newbie status. If you have a school close by you can take a class at its a huge help. As well you should get training with your machine, use it don't pass free teaching up.

[bloefeld]

Glad to hear your willing to make a mistake or two to learn. If you learn well from reading I would hunt out a few books to read the help upgrade your newbie status. If you have a school close by you can take a class at its a huge help. As well you should get training with your machine, use it don't pass free teaching up.

On this sort of thing I am willing to make endless mistakes. Mistakes in milling aren't as nasty as say mistakes in experiments with fluorine gas.

I am signing up for some courses at the local technical college for machining. I've also got some on-line training going on with regard to programming for the HAAS. Back when the earth was cooling and dinosaurs roamed the land, I was a pretty good programmer in Fortran (Geof will know what that is), C, Basic, C++, and APL. G-Code looks pretty simple and there is a lot of canned cycles around.

I made the mistake of cheaping out on my CAD/CAM side. I went with Alibre Design (not bad actually but it crashes a lot) and Alibre CAM. Alibre CAM is not documented and it, combined with the existence of zero knowledge on my part led to a very steep learning curve. It is now looking less like the north face of Everest and more like the side of Kilimanjaro. Gruesome, but getting easier as I get in better shape.

I am fortunate and can learn lots from reading; if you have some suggested titles I would be well pleased if you or anyone could pass them along.

As a new guy in the field I appreciate that guys like you, who have some knowledge and are willing to share it. Next time you run into a problem with composite materials or structural adhesives drop me a line, I can probably help. My field is in making stuff stick to stuff that nothing sticks to.

Cheers,

Bloefeld

[Geof]

I was a pretty good programmer in Fortran (Geof will know what that is), C, Basic, C++, and APL. G-Code looks pretty simple and there is a lot of canned cycles around.....Bloefeld

Punch cards and writing programs that would have the drum printer do an entire line of the same character and shake the building.

I only learnt Fortran far enough to do simple statistics and never touched it after 1974.

Before I started doing G-code I did learn enough about html to do my initial company website. I think these two are quite similar; G code just pushes a tool around, html pushes pixels around (loosely speaking), and both are incomprehensible until you realize that it is not necessary to understand why commands are named as they are in order to use them.

[bloefeld]

Hi Geof,

I can remember handing in my little box of punch cards to the computer techs at 8:00 AM and getting my print-out with my first syntax error at 11:00 PM.

I can also remember a language called SNOBOL that was used for simulations. I worked on a project for an entire term to try to simulate what would happen to traffic patterns if you could synchronize the lights correctly for a 5 square mile area. As I recall there was no way I could make it work so that I could get to University any faster than I was.

Your comment on G-Code is enlightening though. The syntax becomes clearer if you just focus on what the command does and not why it isn't named to do what its name implies. Good hint!

Cheers,

Bloefeld

[Geof]

Prresumably you know that originally, back in the dark ages, G and M code programming used punched paper tape. I am amused by one relic of this even now in the some definitions for a command; i.e. M30 Prog End and Rewind (Tape) in the Haas Mill Manual.

Regarding your traffic light simulation project isn't that somewhat similar to the Travelling Salesman problem which I believe is still unsolved.

[automizer]

Back when the earth was cooling and dinosaurs roamed the land, I was a pretty good programmer in Fortran (Geof will know what that is)

Sadly I was born long after this programing language died, but that still dose not leave me with out knowing In my CNC Operators class I was the only one (youngest too) to know what a punch card was and how to make/use one.
This "http://www.amazon.com/Programming-Principles-Applications-Mike-Mattson/dp/0766818888/ref=sr_1_7?ie=UTF8&s=books&qid=1219106926&sr=1-7"]book here was recommended to me and I highly recommenced it now myself.
On thing I like to remember is the machine is the ultimate lemming, you say it do. Its when you tell it the wrong thing by mis typing or the like its not the machines fault its yours it was just following orders.

[MikeOD]

I think everyone here is overcomplicating the Z offset....X and Y tell the machine where the PART zero is...why shouldn't Z as well???

Turn setting 64 on, then origin all of your tool offsets and origin all of your work Z offsets.

Now touch your spindle nose to your top of your work piece (the ground flat of the spindle in the area between the spindle dogs) with no tool in it. Highlight G54 Z in your work offsets page, and press "part zero set".

Now touch all of your tools to that same work piece and press "tool offset measure" while highlighting the correct tool offset in your tool offsets page. After you press tool offset measure once, you can press next tool and the machine will automatically rapid to tool change height, and grab the next sequential tool (even in a sidemount machine, it will sequence through tool order, not pocket order).

When you will find is your tool offsets are now a positive number, the ACTUAL gauge length of the tool from the spindle nose to the tip of the tool, and your work offset will be a large negative number (the distance from tool change height to the work).

You can crash a machine bad with any form of setting tool offsets and work offsets...the reason I advocate my method is that you have a sanity check (look at your tool offsets page and the offset numbers will actually make sense..."yeah, that tool is about 5.1 inches long"...get it?).

Your added side benefit to this now...you're all done with that part, the next one is taller or shorter, but it uses the same 20 tools...why reset all 20 tools again when there's no need to at all? Just touch the spindle nose to the new part and press "part zero set" again for G54 Z.

This will work for any work offset you want, you just need to make sure it is active before you set your tools to it...ie if you work is G57 and you want to set new tools, go to MDI and run a single line of code that just says G57...then set your new tools to that part.