H&T don't match?

[Donkey Hotey]

This is an odd one. I just had a minor crash this morning during a drill cycle. I missed one of the dialog box fields in Mastercam and didn't end up with a length offset on a drill (ouch). It didn't break the drill but it did scrap the part.

H&T checking is turned on and I've gotten the error recently on other operations (not this program). For some reason, this ran just fine, in graphics, but you can see that H&T didn't match and it predictably ran right into the part. It made some pretty nice chips too--big meaty spirals, about 0.050 thick.

Any ideas? Anybody seen this before in the Haas control?

T19 M6 G0 G90 G56 X0. Y0. S3000 M3 G43 H0 Z.2 M8 G99 G81 Z-.6127 R.2 F3. G80 M9 M01

[Geof]

I played with my simulator.

Yes, H0 does not trigger the H & T not matched alarm.

The controller carries on but the tool offset has been set to zero.

My standard practice is to leave the Z coordinate for any Work Zero at either 0.0 or a very small negative value. This means my length compensation has a large negative value so, if for some reason, the machine does not pick up the Tool Length Comp and leaves it at zero my tools just stay well above the part.

You crashed.

By any chance do you set your Work Zero Z at the table surface and then have your tool length compensation come up from there? That is the only way I can think of to get a crash with this situation.

[PBMW]

I'm not sure how you would do that Geof.
I set my tool length offsets off the table on all of my machines. Then the G54 or what ever Z value is set from there. Is that what you're talking about?

[PBMW]

Must be gettin old...double posts.

[Geof]

Originally Posted by PBMW I'm not sure how you would do that Geof. I set my tool length offsets off the table on all of my machines. Then the G54 or what ever Z value is set from there. Is that what you're talking about?

I don't know because I don't quite understand what you are doing. Or maybe I do...Your Z in the G54 is positive?

What I was getting at is that when I did the G43 H0 test it did n ot give the alarm and the tool length comp was set to zero so the tool stayed higher than it should have been.

Greg had his drill crash the part. In other words it went lower than it should have gone. The only way I can think of to get a tool to go lower than it should when the length offset is zero is if the offset is normally a positive value. And the only way offsets can be positive is if the G54 Z is a long way negative.

[PBMW]

Yea. My G54 Z values are positive

[Geof]

Originally Posted by PBMW Yea. My G54 Z values are positive

Living dangerously, eh?

I have a basic priciple when it comes to work zero coordinates or length offsets; they have to be negative.

When a value should be negative and by accident you make it positive you finish up cutting air well above the part.

When a value should be positive and by accident you make it negative what you cut or hit is much more solid than air.

[Donkey Hotey]

I have the Renishaw probing. I think the work offsets are done a little differently than without probing. I don't know. I've never used a mill without probing. (and I'm still happy that I bought that option )

In this case, zero was the top surface of the part. I'm not sure if the control adds the two offsets together (work & tool) or if it subtracts one from the other. I'm not in front of it to verify.

It doesn't really matter though. I usually get this correct. The bigger issue for me was that it missed the H&T error. It's interesting that it didn't fail on Geof's simulator either.

[Geof]

Originally Posted by Donkey Hotey .. I'm not sure if the control adds the two offsets together (work & tool) or if it subtracts one from the other. I'm not in front of it to verify. It doesn't really matter though. I usually get this correct. The bigger issue for me was that it missed the H&T error. It's interesting that it didn't fail on Geof's simulator either.

The control adds the values in the active work coordinate table, the G52 table, and the tool offset entry and moves to the resultant coordinate position in machine coordinates. The different entries can be a mix of positive and negative or all negative; they cannot be all positive.

I think the bigger issue is that when it misses the H & T error and sticks a zero in you go lower than you want to; my approach means I go higher. Less exciting maybe but easier on the old ticker.

[Donkey Hotey]

Conceptually, I agree with your logic on the tools. Your way would just throw an out-of-range alarm. I don't have a choice with the probing...or do I?

[fuzzyracing1967]

I'll have to check that out tommorow,I don't ever remember putting h0 in a program,this would be good to know! However I agree with Geof on the whole negative offsets thing,I was unlucky enough,(or lucky enough,however you look at it)to be close by when a tool holder welded itself to a part becouse of a simple - sign.

[Geof]

Originally Posted by Donkey Hotey ..... I don't have a choice with the probing...or do I?

You're asking me!!!!!???? The Luddite who uses a piece of paper for setting tool length offsets.