[Joe S.]

Tool Length Offset Register:
Hi All,
Our shop has a HAAS TM3 which I use daily, I own a FADAL TM also.

When using the Fadal, I can use different H offsets for any given tool For instance Tool 3 I can use H3 or H10 and it will use the offset listed in the called H ofset register.

I have NOT figured how to accomplish this with the Haas, if I call T3 AND THEN G43 H6 in my program it faults when trying to load the program.

This ability would enable me to use the same tool on multiple fixture offsets in a single program.

It has a 10 tool changer, can I call tool 3 tool 13 and use H13 and do this?
Am I failing to see some simple way to do this?

[daleman]

you would have to turn the h and t match setting off before you could give a tool a different height offset hit the settings button and scroll down till you find the h and t must match setting think it is setting 15

[Machineit]

As daleman said, go into "Setting Graphics" and turn off H and T match.

I must say though that I would only use it with extreme caution, as it is crash city ready to happen. I would turn it off for a specific jobs, then turn it back on.

Mike

[Geof]

......This ability would enable me to use the same tool on multiple fixture offsets in a single program......

We do this using G52 Z. If you are not familiar with G52 read about it in the manual. It is a method to create a secondary work zero, I think the manual calls them daughter work zeroes.

The way we use it for multiple fixtures is to set the tool offsets to a reference point on the machine and then the program for each fixture has a G52 Z value that shifts the tool offsets the correct amount for that fixture.

As Machineit says turning off H and T match is a high risk procedure because you have to remember to turn it back on. In the case of G52 any values are set to zero when the program hits the M30 (or you hit Reset) so they cannot carry over when another program is run.

[txcncman]

I totally get why someone would need to do this since setting tool length offsets is so difficult on Haas mills.

[Matt@RFR]

I totally get why someone would need to do this since setting tool length offsets is so difficult on Haas mills.

For the OP's situation, I use G52 like Geof. But I also use non-matching H and D numbers quite a lot. Different D numbers for tight tolerance, differing size features with different flute length engagement needs different D offsets. And fussy work where two or more tools need to match perfectly in Z, and in several different locations with different floor thickness and other part geometry or fixturing support. And don't forget using two H numbers for double angle cutters for chamfering the top and bottom of a part so the chamfers can be adjusted independently.

So no, I wouldn't write this method off just because it might be a little risky.

[Machineit]

For the OP's situation, I use G52 like Geof. But I also use non-matching H and D numbers quite a lot. Different D numbers for tight tolerance, differing size features with different flute length engagement needs different D offsets. And fussy work where two or more tools need to match perfectly in Z, and in several different locations with different floor thickness and other part geometry or fixturing support. And don't forget using two H numbers for double angle cutters for chamfering the top and bottom of a part so the chamfers can be adjusted independently.

So no, I wouldn't write this method off just because it might be a little risky.

I promise and agree to label it as "a little risky", if those who use it report back to us on the crashes they experience using it.

Have Fun--Mike

[Matt@RFR]

I promise and agree to label it as "a little risky", if those who use it report back to us on the crashes they experience using it.

Have Fun--Mike

Been doing it this way for years with zero crashes because of it. There were a couple almost-crashes that got caught, but that is what a slow walk through of the first part is for. I really don't see the problem. As a matter of fact, I never have H&T agreement set and always catch potential isssues when Mastercam decides to post something funky.

[txcncman]

Tool Length Offset Register:
Hi All,
Our shop has a HAAS TM3 which I use daily, I own a FADAL TM also.

When using the Fadal, I can use different H offsets for any given tool For instance Tool 3 I can use H3 or H10 and it will use the offset listed in the called H ofset register.

I have NOT figured how to accomplish this with the Haas, if I call T3 AND THEN G43 H6 in my program it faults when trying to load the program.

This ability would enable me to use the same tool on multiple fixture offsets in a single program.

It has a 10 tool changer, can I call tool 3 tool 13 and use H13 and do this?
Am I failing to see some simple way to do this?

I totally get why someone would need to do this since setting tool length offsets is so difficult on Haas mills.

[glovebox20]

Tool Length Offset Register:
Hi All,
Our shop has a HAAS TM3 which I use daily, I own a FADAL TM also.

When using the Fadal, I can use different H offsets for any given tool For instance Tool 3 I can use H3 or H10 and it will use the offset listed in the called H ofset register.

I have NOT figured how to accomplish this with the Haas, if I call T3 AND THEN G43 H6 in my program it faults when trying to load the program.

This ability would enable me to use the same tool on multiple fixture offsets in a single program.

It has a 10 tool changer, can I call tool 3 tool 13 and use H13 and do this?
Am I failing to see some simple way to do this?

Isn't this what workoffset are used for? If you break a tool and only update the tool length for one fixture, you many be in for a big surprise. I'm sure you use workoffsets for x and y, why not use z as well? But I guess they are more than one way to eat an Oreo.

[SBC Cycle]

Isn't this what workoffset are used for? If you break a tool and only update the tool length for one fixture, you many be in for a big surprise. I'm sure you use workoffsets for x and y, why not use z as well? But I guess they are more than one way to eat an Oreo.

I'm missing something too. I use matching T and H (set in the control) and just call different work offsets. The Z value in the work offset does the adjustment. There is no reason to run multiple H values. I also have Fadals and aside from one oddball situation I've never used an alternate H value. D values a lot but never H.

Am I the one doing it wrong?

[haastec]

I'm missing something too. I use matching T and H (set in the control) and just call different work offsets. The Z value in the work offset does the adjustment. There is no reason to run multiple H values. I also have Fadals and aside from one oddball situation I've never used an alternate H value. D values a lot but never H.

Am I the one doing it wrong?

It's just a different way, or tool, to get the job done. The flexibility is there for those who choose to use the features. If you don't like or agree with the purpose of whatever feature, then don't use them. If you do, then have at it!

Besides, if you were not allowed to use different H and T values, then there would most certainly be a thread discussing why it's not allowed.

[SBC Cycle]

It's just a different way, or tool, to get the job done. The flexibility is there for those who choose to use the features. If you don't like or agree with the purpose of whatever feature, then don't use them. If you do, then have at it!

Besides, if you were not allowed to use different H and T values, then there would most certainly be a thread discussing why it's not allowed.

LOL, you're right. I would be one complaining even though I don't use it. Like I said, I found one use for it years ago and it was the only workaround to my problem, I would have been hosed without the ability to mismatch the T and H.

[Joe S.]

Hi guys,
First chance to revisit the forum, since posting . . . Thank You all for your comments.
1. RE: G52, G54 ... Offsets, I see how to implement there . . . I normally use a 1.000 setup block and have the Z offset set to -1.000 I see how you could make the difference there, long as you are observant and remember to always set you tool to the higher part.

2.txcncman . . . "I totally get why someone would need to do this since setting tool length offsets is so difficult on Haas mills"
Sarcasm? I do not fully grasp what you are implying here (twice) . . . I want to do this, so as to run 2 jobs on 2 vises all in 1 program, so hit run it
OPs 2 parts, open the doors move one replace 1 and repeat. The parts are not fixed at the same level (z).
3. The TLO table goes from 1 to hellandgone , so I ask what would happen if using our 10 tool changer, I set tool 3 to the height of vise 1 and tool 13 to vise #2 and called those respective tools in my program?
I have not had time to try this, it seems it should work using tool 3 as T3 & T13.
Yes / No ?

[Geof]

....1. RE: G52, G54 ... Offsets, I see how to implement there . . .

I am not quite sure you do see how to implement there....

G52 is not an offset like G54.

G52 creates a new offset based on the G54 offset (or any other offset G55, 56 etc).

Let us say for a particular job you set your tool offsets to your setup block and enter your Z-1.000, then you have a second job that is at a different level. You could adjust the Z offset for the new level or you can use a different tool offset for the different level. However I think the simplest way is to use G52 because if you know the second job is 0.500" higher than the first one you simply put G52 Z0.5 at the head of the program and all your Z positions are moved up 0.500".

I suggested in Post #4 that you read up on G52 and the fact that you write; "1. RE: G52, G54 ... Offsets, I see how to implement there" suggests to me you have not gone and read the manual about G52; It is not an offset the same as G54 etc.

[behindpropeller]

For the OP's situation, I use G52 like Geof. But I also use non-matching H and D numbers quite a lot. Different D numbers for tight tolerance, differing size features with different flute length engagement needs different D offsets. And fussy work where two or more tools need to match perfectly in Z, and in several different locations with different floor thickness and other part geometry or fixturing support. And don't forget using two H numbers for double angle cutters for chamfering the top and bottom of a part so the chamfers can be adjusted independently.

So no, I wouldn't write this method off just because it might be a little risky.

Matt,

Why not use the wear function?

[Matt@RFR]

Why not use the wear function?

I program in wear, so that's all I use. Still won't get you two or more 'fine tuning' offsets for one tool. I tend to work with small tools with giant L/D ratios and flimsy parts, so using more than one offset (both H and D) for one tool is a huge advantage for me.

EDIT: One thing I just thought of to make this whole thing safer, if you are really concerned about it, is to set all unused length offsets to a larger value than the machines' Z travel, so even if you screw up and call the wrong H offset, all it will do is give you an overtravel alarm.

[haastec]

3. The TLO table goes from 1 to hellandgone , so I ask what would happen if using our 10 tool changer, I set tool 3 to the height of vise 1 and tool 13 to vise #2 and called those respective tools in my program?
I have not had time to try this, it seems it should work using tool 3 as T3 & T13.
Yes / No ?

You are close! For your example, you will want to use T3 for both programs to call up the same physical tool, but you will use H3 for one program and H13 for the other to call up the correct tool length offset.

[Joe S.]

You are close! For your example, you will want to use T3 for both programs to call up the same physical tool, but you will use H3 for one program and H13 for the other to call up the correct tool length offset.

Thanks, I will give that a try.
Joe