[elaganis]

Does anyone the correct way to shift the X and Z tool measurements when using a gang holder? I have a TL-1 w/an automatic 4-pos. changer. Not enough for everything I need to do. So I made gang tool holders to double my tool change capacity. Example, I have a spot drill and drill at T4. Both are programmed but the one set for offset 4 is the only one that works. When I call out a new offset, ie. T405 vs. T404, it never shifts and redrills the hole.

[jackson]

did you change the offset #5 to compesate there has to be diferences in the tool so you need to make nesessery changes to the offset

[Geof]

Does anyone the correct way to shift the X and Z tool measurements when using a gang holder? I have a TL-1 w/an automatic 4-pos. changer. Not enough for everything I need to do. So I made gang tool holders to double my tool change capacity. Example, I have a spot drill and drill at T4. Both are programmed but the one set for offset 4 is the only one that works. When I call out a new offset, ie. T405 vs. T404, it never shifts and redrills the hole.

I use gang tools on several different positions on the four place toolchanger and just number the tools T101, T111, T121; T202, T212, T222 etc.

When entering the tool offsets you just have to cursor down to the correct line in the table.

[elaganis]

I use gang tools on several different positions on the four place toolchanger and just number the tools T101, T111, T121; T202, T212, T222 etc.

When entering the tool offsets you just have to cursor down to the correct line in the table.

I did the offset Dia measure in x and Z at offset number 5.

I assume T101 is Tool 1 offset 1.
and therefore T102 is Tool 1 offset 2, T1<tool number 02<tool offset number
Yours seems to be different?

[Geof]

I did the offset Dia measure in x and Z at offset number 5.

I assume T101 is Tool 1 offset 1.
and therefore T102 is Tool 1 offset 2, T1<tool number 02<tool offset number
Yours seems to be different?

If you have three tools ganged on the toolchanger at position 1 you always need to have T1nn so the toochanger goes to position 1.

For one tool use T101 and put the offsets for this tool in line 1 of the offset table.

For the next tool use T111 and put the offsets for this tool in line 11 of the offset table.

For the next tool use T121 and put the offsets for this tool in line 21 of the offset table.

Do the same for the other locations on the toolchanger.

T202 is line 2 in the table.
T212 is line 12 in the table.
T222 is line 22 in the table.

Etc.

I find doing it this way makes it easier to identify which offset is associated with which tool in the gang. Normally I make the tool closest in 101, the next one out 111 and the furthest out 121.

We do this on all our machines; TL1, GT20, SL10, HL1 to speed up cycle times on small parts.

[elaganis]

Thanks Geof! I will try this right now.
-E

[elaganis]

It didn't work at first. (same as I've been programming it) I realized the problem was in my post which was calling out a tool offset cancel prior to the next tool offset. My bad.
thanks again for the advice!

[elaganis]

Ok just broke the tool. maybe I need the offset command? Here is the program:
(TOOL - 4 OFFSET - 5)
(LDRILL DRILL .125 DIA. INSERT - NONE)
G0T0405
G97S1000M03
G0G54X0.Z.25
Z.1
G1Z-.4F.01
G0Z2.25
T0404G96S1000
Z.1
X.1603
G1Z0.F.005
Z-.0471
G2X.1229Z-.076R.0317
X.1234Z-.0797R.0317
G1Z-.1741
X.1092Z-.167
G0X.081
Z.1
X.1703
G1Z0.
Z-.0505
G2X.1329Z-.076R.0267
X.1335Z-.0797R.0267
G1X.1334Z-.1741
X.1192Z-.167
G0X.0889
Z.1
X.1803
G1Z0.
Z-.0545
G2X.1429Z-.076R.0217
X.1434Z-.079R.0217
G1Z-.1741
X.1292Z-.167
G0X.0989
Z.02
G0X0.Z6.M05
T0400
M01

Offset 4 has a boring bar while offset 5 is a drill. It basically tries to bore with the drill. In other words the gang block never shifts.

Help?

[Geof]

I think I found your problem; it is not your offsets it is in the program and it is not really a mistake. I think your boring tool must have been shorter than your drill.

I set up my TL1, the first picture shows a shot of the graphics display from the program the second picture with a jiggling camera shows the tools. I was using a 1/8" endmill as a boring tool. The third picture shows the offset table for your program with the drill being offset 4 and the boring tool offset 5. I machine a piece of brass successfully.

However I did get a scare and I was lucky I did not break a tool. The reason I did not was because my boring tool was slightly longer than the drill. Here is a section of your program showing the place I think your breakage occurred.
I have put comments on the relevant lines.

%
O00000
(TOOL - 4 OFFSET - 5)
(LDRILL DRILL .125 DIA. INSERT - NONE)
G00 T405 This line sets offset 5; in my case Z is -20.6882
G97 S1000 M03
G00 G54 X0. Z0.25
Z0.1
G01 Z-0.4 F0.01
G00 Z2.25
T404 G96 S1000 This line sets offset 4; in my case Z is -20.6062
Z0.1 This is the guilty line. The offset is now set for the boring tool but the drill
is still in position. This line only move Z to Z0.1 using offset 4 but it
does not move X so the drill stays in position. In my case offset 4 is
0.082 more positive than offset five so the drill stops 0.182" away from
the work.
If the boring tool had been shorter then offset 4 would have been
closer and at this move the drill would have rammed into the work.

The solution is to put the X move before the Z move so that the correct tool is in place.

Below is how I would do the offsets and this is also shown in the fourth picture. Instead of using 4 and 5 I use 4 and 14. The first tool to do anything, the drill in this case, I make Tool 404 using offset 4 and the next tool is Tool 414 using offset 14.

%
O00000
(TOOL - 4 OFFSET - 4 AND 14)
(DRILL .125 DIA. OFFSET 04)
(BORING TOOL OFFSET 14)
G00 T404
G97 S1000 M03
G00 G54 X0. Z0.25
Z0.1
G01 Z-0.4 F0.01
G00 Z2.25
T414 G96 S1000
Z0.1
X0.1603
G01 Z0. F0.005
Z-0.0471
G02 X0.1229 Z-0.076 R0.0317
X0.1234 Z-0.0797 R0.0317
G01 Z-0.1741
X0.1092 Z-0.167
G00
Z0.1
X0.1703
G01 Z0.
Z-0.0505
G02 X0.1329 Z-0.076 R0.0267
X0.1335 Z-0.0797 R0.0267
G01 X0.1334 Z-0.1741
X0.1192 Z-0.167
G00
Z0.1
X0.1803
G01 Z0.
Z-0.0545
G02 X0.1429 Z-0.076 R0.0217
X0.1434 Z-0.079 R0.0217
G01 Z-0.1741
X0.1292 Z-0.167
G00
Z0.02
G00 X0. Z6. M05
T400
M01
%


And if your boring tool was not shorter than your drill I don't know what went wrong.

[elaganis]

Once again Geof, thank you.
However, I did get it working before I read this by adding G0 G54 X0. Z1. right before the new offset call out of T414. The Z plane at 1" was my check. How does this differ from what you had? I'm assuming the X move did the trick since the command was modal?

[Geof]

Once again Geof, thank you.
However, I did get it working before I read this by adding G0 G54 X0. Z1. right before the new offset call out of T414. The Z plane at 1" was my check. How does this differ from what you had? I'm assuming the X move did the trick since the command was modal?

I would have to look at it on the machine to say exactly what it did. I think probably it was that you moved 1 inch further away and also moved your X to a different location.

[tobyaxis]

Geof is it safe to assume that a Haas Lathe will cancel the last offset like this:

G0G40G80G99M5
G28U0W0M9
G50S2000M41
T0100M8<<<<<<<<<<<Tool Index
G96S750M3
G0X1.25Z.1T0101>>>>>>>>>Tool 1 Offset 1
G41G1Z0F.025
X0F.006
Z.075
G40G0Z1.5
T0100>>>>>>>>>>>Cancel Offset
G0X1.25Z.1T0121>>>>>>>>>>>Tool 1 Offset 21
G71P10Q20U.01W.008D500F.01
N10G41G0X.4
G1Z0F.006
X.5Z-.05
Z-1.0
N20X1.25

G40G0 Z1.5M9
T0100>>>>>>>>>>>>Cancel Tool Offsets
G28U0W0
etc.
etc.

I found that Canceling the last offset has fewer problems than calling a new one. Provided that the tool is in a safe position to cancel the last offset (at least 3 times the nose radius away from the work piece).

[lathe guy]

Try using a G50 X and Z instead of geometry offsets. The only difference
will be that you must start your program from the same positon each time. If your machine is small it is a good idea to start from the G28 home position for each tool.

[Geof]

Geof is it safe to assume that a Haas Lathe will cancel the last offset like this:...

You have caught me here. I don't know because I never bother cancelling offsets. I suppose to be picky I should and if I missed setting the offset for a new tool it could give me a crunch. However, on the lathe the offset call is in the tool change command Tn0n so it is difficult to miss. I suppose on the mill it would be easier to miss because it is a separate G43 H0n command but so far I have been lucky.

[elaganis]

Try using a G50 X and Z instead of geometry offsets. The only difference
will be that you must start your program from the same positon each time. If your machine is small it is a good idea to start from the G28 home position for each tool.

The TL1 is a small machine but using the G28 for the tool change, which as far as I know cancels tool offsets, is painfully slow. The rapids on the TL1 crawl at 100% and worse yet the 4-position tool changers has the worlds slowest automatic tool change. Which is why I took the time to make custom gang tool holders for part quantity over 50. And with the G0 I move the changer just far back enough to clear prior to a Tool change.

As far as G50, I'm not sure. I've only used it to set Max spindle speed.

[Geof]

The TL1 is a small machine but using the G28 for the tool change, which as far as I know cancels tool offsets, is painfully slow. The rapids on the TL1 crawl at 100% and worse yet the 4-position tool changers has the worlds slowest automatic tool change. Which is why I took the time to make custom gang tool holders for part quantity over 50. And with the G0 I move the changer just far back enough to clear prior to a Tool change.

As far as G50, I'm not sure. I've only used it to set Max spindle speed.

Painfully slow is TOO mild .

Regarding G50 when I read the manual I get the understanding that in Fanuc Mode G50 sets Machine Coordinates not Tool Offsets. In Yasnac Mode G50 is used to set and cancel Tool Offsets.

[lathe guy]

Take a look at your parameter setting make sure that how your tool offsets are read by the controll will allow you to use the same tool geometry with different wear offsets. IE: T01 = tool 1 and geometry 01 and the trailing 01 is just the wear offset. This will allow you to put the difference between the tool postions in the wear offset. Some machines such as Hitachi you need to use an offset value of 50 or more for gang loaded tool on the same tool post.

[Geof]

Take a look at your parameter setting make sure that how your tool offsets are read by the controll will allow you to use the same tool geometry with different wear offsets. IE: T01 = tool 1 and geometry 01 and the trailing 01 is just the wear offset. This will allow you to put the difference between the tool postions in the wear offset. Some machines such as Hitachi you need to use an offset value of 50 or more for gang loaded tool on the same tool post.

You don't need to worry about this.

If you have three tools at position 1:

T101 gives you tool 1, position 1 using geometry offset 1 and wear 1
T111 gives you tool 1, position 2 using geometry offset 11 and wear 11
T121 gives you tool 1, position 3 using geometry offset 21 and wear 21

[jackson]

You don't need to worry about this.

If you have three tools at position 1:

T101 gives you tool 1, position 1 using geometry offset 1 and wear 1
T111 gives you tool 1, position 2 using geometry offset 11 and wear 11
T121 gives you tool 1, position 3 using geometry offset 21 and wear 21

I have a Lynx 220m lathe and it has a 24 station turret makes life alot easer

[Geof]

I have a Lynx 220m lathe and it has a 24 station turret makes life alot easer

This is nothing to do with having more tools it is ganging the tools when possible to reduce time on tool changes. It doesn't matter how fast your machine can do a tool change it will be faster just moving an inch or so to another tool ganged at the same turret position.