[Bodie]

Hi,
I am trying to insert an Iso sub program within an existing mazatrol program.
The problem is with the work offset and tool offset.
The Wpc has been set on the main mazatrol program (everything works ok) then when in the sub im changing to a G56 work offset - when the tool is moving to its first position it seems to be ignoring the tool length data (z) stored within the machine therefore trying to rapid through the job (its ok on the x and y axis).
So then i tried the G43 H15 command within the sub putting the tool offset length into the geometery page in position 15, but again this is having no effect and trying to go to the same position through the workpiece.
Should the iso sub still read the tool info stored within the machine or do i need to input other information ?
Thanks for your help

[psychomill]

Yes it should. But your parameters could be conflicting here. If the EIA parameter for tool length is set to read from Tool Data, you may be in effect "zeroing" you tool length by adding value from the Tool Offset page. Depending on the method of tool offsetting you do (positive offsetting or from machine zero), this could alter you Z dramatically.

The simple thing to check here for though is your G56 offset. Is the Z offset in G56 correct? You can also tell whats going on in your parameters if you omit the "H15", in MDI (with the spindle out of the way of the part), just type in "G43Z0." with T15 in the spindle. Then check your tool/spindle position relative to the part and see what is off (this is providing that your work offset is correct). If the machine parameters are set to read from Tool Data, the tool tip should be at "Z0" (therefore you don't need the "H"). If the parameters are set to read from Tool offset, the tool tip should off roughly the distance of the tool length (you'll need to use the "H"). Be careful not to travel the tool into the table. You can remove the tool from the spindle to test this. You just need to make sure you tool change to T15 so the machine knows that you're using T15 for tool length.

I do get the feeling though (only because this is the most common mistake) is that your G56 Z offset is not correct.

[joedirt]

You need to set parameters F93 and F94 to use Mazatrol tool offsets in an ISO program. If you look in the EIA/ISO programming manual under tool length offsets it will tell you what you need.

[ALEX87]

I'm having some similar problems with my VTC we changed the parameters for Z and it was F93 but is there another parameter for x? while running the EIA program it doesn't seem to pick up the mazatrol tool data for the diameter of the tool.