problems with offsets on MC3VA with OSP 500 M-G

[XLVACP]

I'm a rookie with regards to CNC so this problem may be the result of something I'm not doing correctly.
After changing out a 5/8 mill and replacing it with a 3/4 mill i began experiencing incorrect tool position in Z.
I did reset the tool length offset and reposted my program after changing the cutter.
When I run the program the tool is high in Z but the Actual Position screen shows it is where it should be. As soon as I hit reset to stop the spindle the Z axis position immediately changes to reflect the true position of the tool.
Here are the procedures that i've been using for setting offsets.
·To set tool length offset :
1.MDI
2.G15 H0 ; Write ; Cycle Start (Look for C0 indication on Current Position page)
3.Tool Data
4.Tool Length Offset
5.Tool #
6.Cal (4. If using indicator tool setter)
7.Write

·To set work offset in Z :
1.Tool setter on top of work piece
2.Zero Set
3.Cal (4. If using indicator tool setter)
4.Write


Would be most grateful for any advice someone might be able to give.
Thanks.

Similar Threads:

• Need Help!- Problems on VM17 192 error and problems finding home.
• Need Help!- TLO Tool Offsets Zeroed and Fixture Offsets Lost on Power Down DX-32 Torq-Cut 30
• Need Help!- HAMAI MC3VA WITH FANUC15MA PARAMETER LOST
• Need Help!- Toolpath display and soft-limit problems when using offsets
• Help understanding work offsets and extended work offsets

[deadlykitten]

hy here may be the problem :

As soon as I hit reset to stop the spindle the Z axis position immediately changes to reflect the true position of the tool

Z axis after cnc reset should not reflect the "position of the tool", but the "position of the axis"

"position of the axis" + "tool offset"="position of the tool"

cnc reset disables all tool corections, thus all tool offsets

after that line i stopped reading your post ! ... pls make sure that is clear until now kindly !

[XLVACP]

hy here may be the problem :



Z axis after cnc reset should not reflect the "position of the tool", but the "position of the axis"

"position of the axis" + "tool offset"="position of the tool"

cnc reset disables all tool corections, thus all tool offsets

after that line i stopped reading your post ! ... pls make sure that is clear until now kindly !

OK,that makes sense.Perhaps my setting procedure (listed in the first posting) is incorrect then.
Thanks

[deadlykitten]

OK,that makes sense.Perhaps my setting procedure (listed in the first posting) is incorrect then.
Thanks

i can not say if your procedure is corect/incorrect, but i can suggest comparing offset value for bought tools :

... lets say that bought tools are in the same toolholder
... lets say that tool 1 sticks out of the holder with 50mm; thus there are 50mm between tool nose and holder face
... lets say that tool 2 sticks out of the holder with 65mm

after offset procedure, the difference between offsets must be cca15 ( 60-15 );+15 or -15 ... however, in absolute value, offset difference is equal with real distance



if tools are in different holders, than you have to find another fix point to compare, like the flange of the holder; you are talking about a mill i suppose, thus holders have taper+flange; kindly !

[OkumaWiz]

You are missing a step in your touch off.

When you hit reset, the tool offset goes away, but fixture offset remains.

So if you are using your G15 H0 to clear the fixture offset and then touch off the tool to the table, then when you want to establish your fixture offset, the tool would need to have the tool offset active.

If you do the G56 H5 (for tool offset 5) and then touch off the work offset, it will take the active offset into account.

What most people do is to use the spindle face (no offset needed) to establish the work offset and once that is established, then touch off the tool with the work offset active using the CAL feature. That way, even a reset will not throw things off and your tool offsets make sense in that they will reflect the length of the tool from the spindle face. So when you look at a tool in the spindle and it appears to stick out 5 inches, when you check the offset, it will reflect a value of about 5 inches. When you switch from work offset to work offset, just empty the spindle and touch off your new z to the spindle face again with your sensor on the top of the Z0 location.

Best regards,