G68.2 Shift

[Anonymous]

I am running a DMU50 Gen 2 with Fanuc controls. We use HSMworks for programming. I am trying to shift the work coordinate in xyz to a selected point after each orientation movement (B,C) in G68.2. From what I understand, I am suppose to select that in the first box under tool orientation. When I do that my triad moves but there is nothing different in the posted code. I am using the generic Fanuc post for the time being. Anybody else having this problem??

Thanks,

Chris

[bob.schultz · Accepted solution]

This behavior is by design.  The post engine handles the translation of the work plane origin for each operation rather than leaving it up to the post processor to handle.  You can change this behavior and output the origin values in the G68.2 block by making the following changes to the post.  Add the following line towards the top of the file (spacing is very important for this variable, so please add it exactly as shown).

allowHelicalMoves = true;
allowedCircularPlanes = undefined; // allow any circular motion
mapWorkOrigin = false;

Now make the following change in the setWorkPlane function.

writeBlock(gFormat.format(68.2), "X" + xyzFormat.format(currentSection.workOrigin.x), "Y" + xyzFormat.format(currentSection.workOrigin.y), "Z" + xyzFormat.format(currentSection.workOrigin.z), "I" + abcFormat.format(abc.x), "J" + abcFormat.format(abc.y), "K" + abcFormat.format(abc.z)); // set frame

You will notice that the output coordinates are changed to match the new origin.

[Anonymous]

This worked great
Thank you!