cutter comp on intergrex

we have an intergrex 35y with a t-plus control, where do we put the offset value for cutter comp while milling?

Our integrex runs a fusion control, and in the tooldata page there is wearcomp in there, but with the t-plus isnt it just the described actual diameter that you would change, im not to sure though, the only t-plus machines we have are on the qt's

Mike, are you programming in Mazatrol? Then the Tool Data page should have the cutter diameter settings. Change that for comp. BTW, your control should be a MT+ control since you're on an Integrex.

that is what we were thinking. we program this thing EIA and trying to work with G41 like the rest of our machines.
thanks for your input. we need all the help we can get.

I haven't seen a MT conrol in awhile so I can't remember. Are you programming using Tool Data for offsetting or the Tool Offset page? I believe you should have both. A parameter controls which to use. If you're using Tool Data, I think you have to use centerline programming as well since tool data reflects the cutter diameter in which the control figures the radius offset from. May have to take some measured test cuts to confirm this...

OK, let me back up a little,.....

If you're using EIA (this even works in Mazatrol under Man inputs), as long as you assign a D offset to pick from, the cutter comp will be read from the Tool Offset page. If you only have a G41 and no D, I believe it will try to comp from Tool Data (Mazatrol programs). In EIA, just add the D and number, then use the tool offset page.

It's been a long time.... got me thinking now....

I run a Nexus 510, fusion 640 control. below is a page from the parameters manual regarding setup for using mazatrol tool data in an eia/iso program.

12-7 Tool Offsetting Based on MAZATROL Tool Data
Parameter selection allows you to offset both the tool length and the tool diameter using
MAZATROL tool data (tool diameter and tool length data).

12-7-1 Selecting parameters
Using the following parameters, select whether or not MAZATROL tool data is to be used:

User parameters

F92 bit 7: Tool diameter offsetting uses the MAZATROL tool data ACT-f (tool diameter data).
F93 bit 3: Tool length offsetting uses the MAZATROL tool data LENGTH (tool length data).
F94 bit 2: Tool length offsetting using the MAZATROL tool data is prevented from being
cancelled by a reference-point return command.

12-7-2 Tool length offsetting

1. Function and purpose
Even when offset data is not programmed, tool length offsetting will be performed according to the
MAZATROL tool data LENGTH that corresponds to the designated tool number.

2. Parameter setting
Set both bit 3 of parameter F93 and bit 2 of parameter F94 to 1.

3. Detailed description
1. Tool length offsetting is performed automatically, but its timing and method differ as follows:

- After a tool change command has been issued, offsetting is performed according to the
LENGTH data of the tool mounted in the spindle. (A tool change command code must be set
in the program before tool length offsetting can be done.)

- After command G43 has been set, offsetting is performed according to the LENGTH data of
the tool mounted in the spindle.

2. Tool length offsetting is cancelled in the following cases:
- When a command for tool change with some other tool is executed
- When M02 or M30 is executed
- When the reset key is pressed
- When command G49 is issued
- When a reference-point return command is executed with bit 2 of parameter F94 set to 0

3. Tool length offsetting becomes valid for the block onward that first involves Z-axis movement
after tool change.

If this applies to your machine I offer one warning.

ELIMINATE G49 COMMANDS FROM YOUR PROGRAM. A G49 will cancel your tool length immediately when using Mazatrol tool data and Crash the tool into your part as the spindle nose tries to assume the position the tip of the tool used to occupy.

Hope that helps.