I had a gentle crash today (bent a reamer), and if you are going to have one I like the gentle ones. The problem was H00 as the tool length offset in my post. There is a setting on my Haas that checks to be sure the tool number and the offset numbers agree and I know it used to work because it has stopped simulations a few times for me with a warning.

Today it did not work and I can't figure out why. I ran the program below in simulation several times and the warning never came on. I have not changed anything in the post my CAM software outputs but obviously something has happened.

I thought one safety measure would be to put a large value in the length offset column for H00 but there is no 00 in the Haas length offset table. Viewing this fact I wonder where the Haas was going?

The real problem is, what is in my post, or what setting has changes that would disable the warning from coming on in a situation where it obviously should?

N20T7 M06 (0.15INCH DRILL, 135 INC)
N21G10 L12 G90 P7 R0.15
N22G90 G80 G40 G54
N23S800 M03
N24G43 H0
N25/M08
N26G00 X-0.625 Y-0.625 Z0.02
N27G01 Z-0.5 F14. S800
N28Z0.02
N29G00 X-14.875 Y-8.125
N30G01 Z-0.5
N31Z0.02
N32M09
N33M01
N34M30
%

I'm a bit of a slave to my CAM program so when things like this come up I'm in trouble. I thing the problem is with the Haas and I thought this was the place to find out. :)

I hope somebody jumps in to substantiate this since I don't remember for sure. I think the catch is that it's H0. Zero is the only one that will do that since there is no tool zero. H1 would cause an error.

Lemme' guess: Mastercam and you forgot to fill in all the H&T numbers in the dialog box when you setup the tool. Am I warm?

Haas Setting #15 is H and T agreement ..

A "H00" should send the tool to home..IE: tool change postion..Unless you have a G10 that is over riding it..

Did you have the Check box ticked In OneCNC to force an T and H agreement??

I'll second Donkey. Gotta be MasterCAM.

Haas will do H&T checking, but it recognizes H0 as a valid offset. I'm not sure why. I destroyed an $80 carbide countersink and an ER-16 nut/collet when I didn't catch a H0 that got posted out.

MasterCAM does this really inconsistently for me. It only occurs when I choose a tool from their default library and renumber it. When I update the operation after changing parameters (note: NOT H&T #'s), it will sometimes change to H0. I always have the box tagged to make sure H&T match.

I haven't had this problem in awhile, and I now religiously check H&T agreement, even when I just make minor changes to other tools and repost a program.

I never thought about the zero not triggering the match alarm because it's not recognized by the control. I'll change the post and try it today.

Thanks guys.

H00 has never been checked on the Haas control because many people use it to cancel the TLO. If it did then you would get an H & T code alarm for every tool. As most people Use negative TLO's this is not a problem as the TLO will cancel away from your work. The problem is when you have a large negative Z work offset (G54 etc) and all of your tools have a positive value. When the TLO is canceled and the positive value is removed from the tool, it will move the tool back down. This could be a crash. We have had many discussions on how to deal with this and all of them have their own problems. So we decided to just leave it alone for now.

I'm using the Haas probe set up and I noticed that all the Z offset numbers were way different than the ones I was getting with my old height setter. This could have something to do with the tool heading for the table rather than the tool changer position.

Vern

yes this is exactly what Apps is talking about. I made this mistake of "zeroing" the tlo values in the table of tools I wasn't using to try and make them safe, this was a mistake.
The way to make unused tool locations "safe" is to put a positive value larger than the z travel of the machine, so I always put a 20. in my vf2 for unused tools to make that location z "safe". A really big value will usually generate a z overtravel alarm and no motion which is even safer.
A zero tlo value will move the spindle DOWN to your G54, 55.... etc. z offset value which is always negative if you use a probing system to set coordinate offset Z values. Having a large value in the tlo table for tool locations that haven't been touched off, will usually prevent an accident.
joev

Good point, and I had safety values in the length table, but with the H zero I managed to find a way to circumvent my best intentions and your timely advise. :)

I get the feeling from Haas apps' post that I'm not the first person this has happened to. It is very refreshing to see that Haas is paying attention to our problems and forthcoming with answers and explanations.

Now, if I could just get them to send me their magazine.

Vern

... I made this mistake of "zeroing" the tlo values in the table of tools I wasn't using to try and make them safe, this was a mistake....

This is connected to one of my favorite pontificatory topics; which I just mentioned in a different thread for the umpteenth time: http://www.cnczone.com/forums/showthread.php?p=540372#post540372

No matter what way you set your tool offsets, or where, if it is at all possible make sure that the the plus/minus keyboard transposition makes the tool move up not down; up is a lot less solid.

My solution is to not use H00 to cancel TLO and do it with the following:

G0 G91 G28 Z0
G49
G90

With the machine in incremental and the command to Z0 it is a little safer.

My solution is to not use H00 to cancel TLO and do it with the following:

G0 G91 G28 Z0
G49
G90

With the machine in incremental and the command to Z0 it is a little safer.

Or use G53 G49 G00 Z0.0 and remove the risk that you leave your machine in incremental for the next tool. :)