200 tool offset

[miller10]

24+1 toolchanger and 200 tool offset, why? please explain

[christinandavid]

Hi,

The pocket numbers do not always have to correspond to the H & D offsets you are using (although on Haas you need to turn off 'H & T code agreement' safety feature).

If your machine uses a migratory tool changer you should be able to assign whatever tool number you wish to a particular pocket when you are setting up.

Other Uses: -

You may want to keep tools set up when they are removed from the tool magazine and store the offsets somewhere in the table.

You may want to use more than one D offset with the same end-mill ie one for a roughing pass and one for a finish pass.

You may want to use more than one H offset with the same face-mill ie one for a roughing pass and one for a finish pass.

You may want to use more than one H offset with the same side & face cutter ie one for the top edge and one for the bottom edge.

There are probably machines out there with a 200 tool magazine.

DP

[miller10]

can i do toolchange in the program to a tool that does not exist in the magazine but in the tool offset?

excuse my bad English

[Geof]

Do you mean use the same tool but a different offset?

The answer to this is yes but for length offset you have to turn off Setting 15 H & T CODE AGREEMENT and just use the appropriate H number for the G43 command. For diameter offset you do not need to change any Settings just use the appropriate D number for G41 or G42.

Myself, I do not like the idea of using multiple length offsets for the same tool because then Setting 15 has to be turned off which means any offset will work with any tool. This makes it easy to enter a wrong number on the G43 line and bury a long tool into a vise or table.

[christinandavid]

Originally Posted by miller10 can i do toolchange in the program to a tool that does not exist in the magazine but in the tool offset? excuse my bad English

Try it, see what happens...

DP

[Haas__man]

I agree, there are many users who like the feature of having 200 tools available, however some do not. If you decide that you would only like 20 tools to be displayed instead of 200, then I'll find the parameter for you that alters this.

[Andre' B]

Originally Posted by Geof Myself, I do not like the idea of using multiple length offsets for the same tool because then Setting 15 has to be turned off which means any offset will work with any tool. This makes it easy to enter a wrong number on the G43 line and bury a long tool into a vise or table.

We have a lot of older programs that are still used now and then. Most all of them were programmed manually (BC, before CAM) and any cutter comps are done edge of part. Now that we are using more or even mostly CAM generated programs which for many reasons are done tool centerline I setup the CAM to offset the tool offset numbers up by 100. So with an old program tool 1 uses offset 1 and with a CAM program tool 1 uses offset 101. That way the same tools can be used in ether type of program. Works well enough until I get time to reprogram everything.

[mactec54]

miller10
Haas does make bigger machines with tool changers with 120 tools, this is one software for all machine sizes so may be they have a machine with 200 tools or just planning ahead its better to have more than not enough, not sure why this would be a problem to anyone

[gpcoe]

With the 24+1 changer you can assign any tool number to any pocket up to 200. To do this go into the offset page and press pg up untill you see the pocket assignment page. Highlight the tool number you wish to change (the one in the spindle for instance) type the number you want to assign to a pocket and press write/enter. This is very helpful for setting up multiple jobs on one machine that cylce through every month. If you have the luxury of leaving your tools set up, your offsets will never need to re-entered.

The nice part of this is if you keep multiple programs in the machine and fire off the wrong one, when the machine calls up say T100 and you don't have that tool loaded, the control will alarm out and not call up inappropriate tools. I did this very successfully with a job that required 42 tools plus probe. I ran the parts through with one tool set and then reloaded the parts with the new tool sets and ran off the second ops. This way I was able to fully prove out the part before production and not risk incorrectly entering tool offsets and screwing up the parts during production. I simply called up say T1, removed it from the spindle, reassigned the tool # for the one I was loading and inserted the new tool. Just make sure you're loading the correct tool. You can also assign a 0 to a pocket. This more or less turns that pocket off. This is necessary when loading oversized tools when you want the adjacent pockets empty for clearance.

Greg