Tool Dia. Offsets

[stang5197]

I am trying to find some information on how the dia. offset function works on the Haas mills.

I understand how the tool height offset works, but sometimes after several parts I need to change the tool diameter.

On the offset screen there is an option for diameter compensation but I can't seem to figure out how it works (also is there a setting that needs to be turned on)?

We are using cam software for programming and the machine is a '01 VF0E

[axis]

do you have tool offset diamiter set in you cam program you ned to have the g code in the program for it to work

[stang5197]

We can set the diameter in the cam, but after say 50 or 75 parts we need to make the a tool diameter offset, say 0.001" smaller to compensate for wear.

On the Heller machines you can simply make a tool diameter offset at the controller to compensate for wear. The Haas appears to have that function but can't find any information on it (in the manual).

[axis]

you need to set it in the program a g41 or g42 it is in the manual under ofsets it is not easy to figure out they also have some info in cnc maganzine about three issue ago if you go to the haas website you can find the old issues

[Geof]

You make the wear compensation in the Offset Page under DIAMETER WEAR.

[jimzin15754]

You have to assign a D command in your programming, I usually put it in the same line where I pick up the tool height ie: G43G0M8H1D1Z.1;
Remember when doing this tool diameter compensation must start in a linear move and not an arc ie: G41G1Y1.0 or G42G1Y1.0 are working examples of picking up the tool diameter. The exception being G13 or G14 when the tool arcs in and out of a circular pocket ie: G13I.5D1 will work just fine. Hope this helps. Hope this helps

[GlenBA]

We can set the diameter in the cam,

Make sure you set compensation to "Wear", for contour and that same for the final pass in pockets. That is for MC. This will put in a G41/G42 and corresponding D value for the tool.

The Haas appears to have that function but can't find any information on it (in the manual).

Look under "CUTTER COMPENSATION". On the tool offset page set the wear for the diameter or radius, depending on setting 40, of the tool. Note that If diameter is specified, the cutter compensation shift amount is half of the value entered.

[drewmeister]

make sure that you know what kind of cutter comp your cam is outputting. I know in mastercam you have several choices. the easiest to use is cutter comp wear. where you input nothing in the diameter registry until you want to comp the tool .001 or what ever you want. When mastercam posts your file, it will automatically comp the tool for you but still give you a g42 of g43 and a g40 at the end of the cut. If you are inputing radius or diameter in the registry, it is just as easy to change. type in -10 then enter and the control will comp .001. Or you can just type in -.001 or a positive value if you want.