Haas Tool offset table

Hello
I own a Haas TM1P with the next gen controls.
I have a question regarding setting up my tool table.
My machine has a 10 position ATC. I have around 40 toolholders.
I would like to add all the tools with their offset to the table.
But I'm not sure how to do it.

I can setup and call 10 tools.
But when I order a M6 T11 it says the toolnumber is out of range.
It doesn't know in which pocket of the ATC tool 11 is. So how can I specify this?
There is no pocket information in the offset table to specify this.

And I can't imagine I have to measure offset each time I need to use a different tool (a different one than the 10 in the atc).
Because I can't change toolnumbers.
Besides I already lost 1 space to my 3d taster. I can't set it up as tool 50, because it needs to be in the ATC

Or I need to write down the offsets for all my tools.
Load up the atc and manually input the offsets if I want to swap tools.

First set of 10 tools would be T1-T10, H1-H10.
Second set of 10 would also be T1-T10 except use H11-H20.
Third set use H21-H30, etc.

ie (first set of ten)
T1M6
G54...
G43 H1 Z.25 M8


(second set of ten)
T1M6
G54...
G43 H11 Z.25 M8

You will need to keep the tool tagged as to which set of ten, or which TLO it is assigned to.

You will also have to turn off H and T code agreement. (on settings page)

I have a TM1, too. I have about 40 holders, most of which are used for standard tools, like a spot drill, tap drills, roughing end mills. On the machine I keep tool pocket 10 free. I'll program T1-10, but use H## and D## to reflect the tool either already loaded in the carousel, or if I use T10, I'll load that manually with the tool I've designated in the program. I have each holder marked with paint as to what number I'm using for H and D. Much care has to be taken when first setting up the machine to make sure that H & D agree with the T I'm using. I also have turned off the parameter for T and H agreement.

Ah makes sense, thanks for the quick reply
Not very user friendly though. Would be easier to have an option to select pockets Haas does this for the other type of toolchanger

On the umbrella style magazine, the tool always goes back in the same slot it came out of.
On the side mount magazine, the tool goes into the pot that the next tool called came out of.
So even if you set all pockets to match tool no.s, after your first time thru the program the tools wouldn't match the pocket they are in anyway.
Pocket no.s aren't used in programming either.
The only time I've ever need to know about the pockets is if I'm using a large tool (facemill) where the 2 adjacent pockets need to be empty, or if I want to call up that tool in pocket 7 but don't know the tool no. I can do P7 ATC fwd.

Ok

One more question.


I'm busy setting up my tools to cut some air for a test haha.
Tools are loaded in the ATC

There is lots of information to find about how to set the tool and work offsets. Should be very easy. But somehow I'm not able to do it.

I use a precision block on the table where I touch of my tools.
Load a tool -> touch off -> press 'measure tool height'. And the value is saved in the table (machine coords)
Repeat for all tools.

Next step is to set zero for my workpiece.

I load a tool (tool 1) and toolheight
G0 G54 G90
M6 T1
G43 H1

I touch of my tool to the top of the workpiece -> offsets -> work offsets -> press the 'part zero set' button.
Value is saved for the Z axis in the G54 work offset table.

When I compare the work and machine coords everything is ok.

Now I want to load up tool 2. To make sure the z height is ok.

M6 T2
G43 H2

Tool changes and I jog to the top of the workpiece. But the offset isn't loaded.
It still has the length of tool 1.

What I'm doing wrong?

I also generated a simple part in my CAD software.
And when I run the file it stops with an error, that it exceeds z as travel.

It fails on "G43 H1 Z15"


So something is going wrong with loading the offsets. Wrong values?


My offsets are for example
T1: -350mm
T2: -310mm

These are absolute coords. I just did a test and when I make them smaller (when I manually input -20mm) the code runs.
But this isn't a workable solution.

It seems the negative absolute coords that the machine adds to the table (once set tool length is pressed) gives problems?

Edit:

I read something about setting 64. It uses the work system offset to set tool lengths. But that means when the Z zero changes for the G54 and I want to add another tool. The offsets are all wrong.

Not exactly sure because I set TLO and WCS different, but you may need to make a Z move.
T2M6
G54 G00
G43 H2 Z25.4

should put you 1" above workpiece.

Also, using your method, the Z in G54 is going to be the difference between your touch-off block and the top of your part.
If your part is higher that the touch-off block your G54 Z value will be positive.

You are correct about setting 64. There are a couple of ways around this.
1) You initially set all tools with G54 Z set to zero. You could change it back to 0, touch your new tool off the block, and hit "Tool Offset Measure". That will automatically zap it in to the length offset. Then change G54 Z back to its real value.

2) Leave G54 Z value as-is, touch the new tool off the block and manually key in the machine absolute Z position as you new tool offset. That is what you're measuring when G54 Z is at 0 anyway.

3) Set your G54 Z value before touching ANY tools off at the beginning of your setup.
Now with setting 64 ON and G54 active, when you touch off your block, the tool lengths will all be based off the G54 Z value and you can add additional tools at will.


If you want to know an alternate way to set TLO and WCS I could walk you thru that also.
It's more logical (I think) and the way every shop I've ever worked at does it.

Not exactly sure because I set TLO and WCS different, but you may need to make a Z move.

Click to expand...

Yes I tried, but it returns an error that it exceeds z travel.


I'm thinking how I did this on my old machine.
I had a electronic toolsetter and I made a macro for it.
It set a WCS (one that I didn't use) exactly the same as the absolute CS.
It would probe and save the negative value on the tooltabel.

I think this is the same method you mention as option 1?

Yep, same as option 1 but use a WCS that you aren't currently using (ie G120) and leave 0 in as the Z which makes it the same as absolute machine zero.
Activate G120 in MDI then touch your tools off the block.

Ah thanks!
Will try tomorrow

I tried some things today but no results so far.
It refuses to load offsets.

G120
set G120 Z axis zero the same as absolute Z axis zero
Touch off tools to a precision block and hit 'measure tool offset'
Then I switch to G54
Set zero on top of a test part.
Switch to another tool (tool 2).
And it still has tooloffset 1.

I made sure I did a M6 T2 H2.
Current commands also shows that T2 is loaded with offset H2.


Next thing:

What I did was enable setting 64.
set all offsets to 0.

Activate G120
Load Tool 1
Jog to precision block, Hit 'part zero set' for Z G120
Measure tooloffset for tool 1. This is 0
I load Tool 2, touch off and press button to measure tooloffsets. This is -40.mm

I load G54
Set 0 on top of part with Tool 1
I load tool 2 and it's offsets. But it still doesn't apply the offset for tool 2.


3th try:

Setting64 off (also tried it 'on')

G54
M6 T1 H1
Touch off to workpiece to set G54 Z zero
M6 T1 H1
touch off to block, press 'measure tool offset'
M6 T2 H2
Touch off to block 'measure tool offset'

And it still doesn't load the tool length offset.
Difference between tool 1 and 2 is 40mm. In the table you can see the difference
tool1: - 30
tool2: - 70

aaaah...I know what I'm doing wrong.
I was so used to my old controls.
When there was a toolchange it will auto load/adjust the offsets in the G54 screen.

On the Haas under the G54 screen it shows -385 (if the offset is -385) for example. That's 0. On my old machine it would just show 0 and not the offset.
I think the Operator screen under jog mode is the same way as my old machine. I need to check what it does.
The whole time I was thinking the offset wasn't loaded because the G54 screen didn't change. But it's just a different method
When I command a G43 H1 Z0. it works and tools zero at the top of the block.

The G54 Z value will be the difference between my precision block and workpiece.


Edit:

I have put setting 64 'on'.
I used G120 to set zero at the top of my precision block/toolsetter.
Next step is to set all tools and press measure tool length offset.

Go back to G54 and use my 3d taster to set zero of the workpiece. Hit 'set part zero' and done!

This way I don't have to manually calculate the difference between workpiece and toolsetter.

tcncj said:

aaaah...I know what I'm doing wrong.
I was so used to my old controls.
When there was a toolchange it will auto load/adjust the offsets in the G54 screen.

On the Haas under the G54 screen it shows -385 (if the offset is -385) for example. That's 0. On my old machine it would just show 0 and not the offset.
I think the Operator screen under jog mode is the same way as my old machine. I need to check what it does.
The whole time I was thinking the offset wasn't loaded because the G54 screen didn't change. But it's just a different method
When I command a G43 H1 Z0. it works and tools zero at the top of the block.

The G54 Z value will be the difference between my precision block and workpiece.


Edit:

I have put setting 64 'on'.
I used G120 to set zero at the top of my precision block/toolsetter.
Next step is to set all tools and press measure tool length offset.

Go back to G54 and use my 3d taster to set zero of the workpiece. Hit 'set part zero' and done!

This way I don't have to manually calculate the difference between workpiece and toolsetter.

Click to expand...

For tools greater than T 10 you can edit your program to be

T 20 M00 (manually load tool 20)
Use H and D 20.

On the older machines you will have to have go to the hand jog. To swap tools the new machines you don't.

Here is a sample of my program I use with tools greater than 10 and Changing in the middle of a program.


M09
M05
G53Z0.
M01
T 20 M00
M01
G54
S5000 m03
G00 x... Y... Z... H20
Z...


And then put the D in just the same as you would normally on your cutter comp programs.

You just have to make sure you put the correct too back in the slot before it does an m06 tool change or it will lead to a wreck







Sent from my KYOCERA-E6820 using Tapatalk

shawnshop said:

For tools greater than T 10 you can edit your program to be

T 20 M00 (manually load tool 20)
Use H and D 20.

On the older machines you will have to have go to the hand jog. To swap tools the new machines you don't.

Here is a sample of my program I use with tools greater than 10 and Changing in the middle of a program.


M09
M05
G53Z0.
M01
T 20 M00
M01
G54
S5000 m03
G00 x... Y... Z... H20
Z...


And then put the D in just the same as you would normally on your cutter comp programs.

You just have to make sure you put the correct too back in the slot before it does an m06 tool change or it will lead to a wreck



As far as setting your Z height when you are setting tools of your master block when u have set your last tool. Hit the position button so you can origin your operator Z to make it read Z0. And then use that too to touch the top of your part. Then just type that reading in your G54 Z offset.





Sent from my KYOCERA-E6820 using Tapatalk

Click to expand...

Sent from my KYOCERA-E6820 using Tapatalk

Ah didn't knew that thanks, very helpful

tcncj said:

Ah didn't knew that thanks, very helpful

Click to expand...

Yes it took me a long time to figure it out. The haas service guys didn't even know how to manage it... Just wanted to sell us macros so we could write some fancy code to do just this. The biggest thing is keeping track of having the correct tool in the correct location at all times.

Sent from my KYOCERA-E6820 using Tapatalk

Yep that's a bit of a pita.
I use an excel sheet to keep track of my offsets/tools. But there comes a time I forget to edit the file. That's why I always use an optional stop function after a toolchange when I first run the program. To make sure I didn't made a mistake.

It would be so easy if you could just select which tool is loaded (1 to 200) instead of calling a T6 H150 for example.