[pld0vr]

Forgive me, but I am fairly new to CNC but particularly new to the HAAS control.

I have an '05 TM-1 with 10 position ATC.

Basically I have a number of setups that I run, and each requires a different group of tools to be in the tool changer.

I have noticed that there are 200 record entries available, but I am a little confused of the most efficient way to handle my tool entries and changes.


So basically let's say that setup 1 requires (trancated list for simplicity sake):

#1 0.5" roughing endmill (offset entry 1)
#2 0.5" finishing endmill (offset entry 2)
#3 0.5 ball nose (offset entry 3)
etc
etc

All of the lengths are recorded in the control.

Now I've run my parts, and the next setup/program calls for

#1 0.25" roughing endmill (offset entry 11)
#2 0.25" finishing endmill (offset entry 12)
#3 0.25 ball nose (offset entry 13)
etc
etc

which obviously have different heights...

I can't figure out how to tell the control that tool position 1, is holding offset record #11, and not offset record #1... if that makes sense. Seems like it should be possible but I can not find the details.

I don't want to do height compensation directly into my programs because if I replace a tool, obviously the height will change.

Now... I am not against running a seperate program before each setup that sets all of the tool offsets for that specific program.

For example, change all tools manually - offsets do not match actual height offsets anymore... run program - sets to measurements inside .nc file.

Not a big deal because if I replace or change a tool I can just edit the .NC file.

What do you find is the most efficient way to manage this with a HAAS control?

Thanks as always.

[Pondo]

You can turn setting 15 off and edit the program to use H11 and D11 for the second set of tools instead of H1 and D1 for tool 1. Setting 90 allows there to be up to 200 offsets on the tool page, so you could use whatever H and D offsets you'd like. The down side is that there is no "failsafe" then if the wrong tool is in there for the programmed H value. I have done this before. What I did was ink up the holders for the #2 set of tools with layout dye to avoid fockups.

There is a way to save and load tool offset page info as well, but I have never done it. I have seen Haas techs do it before though. That would be another option.

[Andre' B]

If you have macro B option you can do things like this.

Near the top of the program put a line.

(Set to 0 for offsets 1-10)
(Set to 10 for offsets 11-20)
(Set to 20 for offsets 21-30)
#100=10


Then for the H and D values each tool in the program do like this.

H[3+#100] (Would use offset 13)

D[3+#100]

This way you only have to change 1 number in the program to select which range of offsets get used.

[dertsap]

always set all of your tools from one specific point and in your program use a g52 shift from that point to your work , dead simple and saves a lot of grief


.