Tool Touch off with G92 and Fanuc Tool Patch

More
30 Mar 2013 08:36 #32074 by LAIR82
Here is how we perform a tool change and touch off currently on our Milacron 10" and 15" machines with the AXIS UI. Each machine has 7 OD tools 1-7 and 7 ID tools 11-17. We have the Fanuc style tool patch applied to both machines to have fixed offsets for the tools and "wear" offsets that are applied for fine tuning, worn inserts, etc. Tool changes are done by calling for example T0101, without the need for the M6. The first 2 numbers call tool 1 and the second 2 numbers apply offset 1. Tool 1 is usually our default 80 degree OD turning tool, that is always used and in the turret.

1. With tool 1 loaded, perform tool change in MDI T0101, come up to part in the Z, touch the face, face off part. Issue G92 z0.000 to set at 0.
2. Again with tool 1, in the X come down to part, make light OD cut to clean up, stop spindle measure diameter, say it's 1.500 and issue a G92 X 1.500.
3. Load tool 2 into turret, perform MDI of T0202 to change to tool 2, come up to part in the Z, touch the face, click "Touch Off" and enter 0, click ok.
4.Again with tool 2, in the X come down to part, touch the tool to the piece, stop spindle measure diameter, say it's 1.500, click "Touch Off" and enter 1.500, click ok.
5. And so on for every tool in the turret.

Then when we go to a different part, we change to tool 1, come over in the Z, touch the face, take a clean up cut, and then perform an MDI G92 Z 0.000. the go thru the same routine in the X on tool 1, come down to part, make light OD cut to clean up, stop spindle measure diameter, say it's 3.000 and issue a G92 X 3.000.

When we do the G92 on tool 1, all of the other tools follow tool 1, so you only have to touch off one tool everytime you setup on another part.

Hopefully this makes sense, as I am not actually an operator, just the guy performing/configuring the retrofit's on our machines. This is apprently how Fanuc, Mazak, Fagor (which we have at least 1 of each), and others perform tool changes and work with offsets. SRT (my boss) posted some pics of our current project, which is just days from being turned over to production, the thread is, "Hardware"-"CNC Machines"-"2nd Cinci Up and Running".

Thanks

Rick

Please Log in or Create an account to join the conversation.

More
30 Mar 2013 23:04 #32098 by SRT
To try and clear this up using G92 Z 0 is just a way to change the origin so all of our tool offset values are taken from that corodinate position change. We really never use G92 for the X axis except the main tool that never has any offset valuse entered in the tool table, although using the Fanuc style patch allows us to make fine adjustments for wear or cutting conditions using the wear offset feature (the second two numbers of the tool number EX: T0101). On a Lathe the X axis never changes so we just change the Z when we move from job to job unless the main tol has to be removed from the Turret for some reason which is rare because an 80 deg tool is a staple on our turrets.

Please Log in or Create an account to join the conversation.

More
31 Mar 2013 02:21 #32109 by andypugh

1. With tool 1 loaded, perform tool change in MDI T0101, come up to part in the Z, touch the face, face off part. Issue G92 z0.000 to set at 0.
2. Again with tool 1, in the X come down to part, make light OD cut to clean up, stop spindle measure diameter, say it's 1.500 and issue a G92 X 1.500.
3. Load tool 2 into turret, perform MDI of T0202 to change to tool 2, come up to part in the Z, touch the face, click "Touch Off" and enter 0, click ok.
4.Again with tool 2, in the X come down to part, touch the tool to the piece, stop spindle measure diameter, say it's 1.500, click "Touch Off" and enter 1.500, click ok.
5. And so on for every tool in the turret.


This is exactly how I do it, with one subtle difference. I use the touch-off buttons. These basically do a G10, either G10 L10 P1 to set the tool table for any tool other than 1, or G10 L20 P1 to set the G54 coordinate system origin.
This is basically exactly the same as your way, except that the possibility exists to use G55, G56 etc to store alternative offset origins.

I only just noticed the G10 L11 version, that allows you to store a probe position, which sounds potentially useful.

I confess to frequently touching-off into the tool table for tool 1, or into the coordinate system for other tools.

Please Log in or Create an account to join the conversation.

Time to create page: 0.059 seconds
Powered by Kunena Forum