Need Help!- Cutter comps

[johny0407]

We have a GE Fanuc Series 18-M controller at work. I've noticed that this controller does NOT have any place to put the cutter radius comp in. Say if I have a tool which is undersized, how do I tell the controller by how much its undersized? It only has a place to put the tool lengths in, but also we use only tool slots 11 through 18. (even though we only have 8 tool slots) And in the controller we could (even though we don't) put values (tool lenghts) for tools 1 through 10. Our programs have 'H' values for tool lengths.
Whats the syntax (in the program) in order to have tool radius comp be effective in this machine? And where do I input the tool radius comp at?
Example code: Using tool in slot 5, notice tool length is on H15
T15 M06
( .750 EM FLAT )
( TOOL - 15 DIA. OFF. - 15 LEN. - 15 DIA. - .75 )
( .750 EM FLAT )
G43 H15 Z3.
G54 G0 X0 Y0 S8000 M03
M20
Z3.
M70
X.1251 Y-.4 Z1.25
G1 Z.9125 F50.
Y3.625 F300.

I know these are a lot of questions but this issue is starting to cause us some problems.

Thanks guys!

[christinandavid]

Hi,

Would have thought that H, D and associated wear offsets would be on the same page (Tool Offset Table). Someone on here should know whether this option is enabled/disabled by modifying a system parameter.

To invoke it in the program you simply put a D15 in the program and use G41/G42 when you approach contour, G40 to cancel compensation when you depart.

DP

[johny0407]

Yeah, i know when and where to put the 'D' codes... but where do I input the 'D' offset values!!! I've heard that I'm supposed to use the number of the H code minus 10 (T15>>>H15>>>D5) OR (T11>>>H11>>>D1)
But i'm not sure how truthful this is...

[dcoupar]

Sounds like your control is set for Tool Offset Memory A. The 18M-B came standard with 32 offsets, which can be used either for length offsets or cutter radius offsets. They offered additional offsets (64, 99, 200, 400, 499, and 999).

You can use any offset for length and any offset for CRC. Some programmers use the same number as the tool for the H offset, and then add 20 or 50 to that for the D offset,
i.e. T10, H10, D60

In your case, maybe T10, H10, D1 should work. So store the length comp in offset 10, and the radius in offset 1.

[John_B]

I've found it to work best to go the plus direction, versus using T10 / H10 / D1 then using T1 and having to use the field that I was going to use for D1 and having to find somewhere else to store the D offset (and change the program).

For example, I have a Mori Seiki with a 20 tool changer, and it has a 64 offset memory. I use 1-20 for T1-T20 length offsets (H1-H20), and then use 21-40 for D21-D40 (T1 corresponding to D21 and so on).

Another machine I have has a 10 tool changer and 32 offset memory, so I use 1-10 for T1-T10 length offsets (H1-H10), and 11-20 for D11-D20 (T1 corresponding to D11...).

Whatever works best for you, but I have several operators that have to understand what I've programmed. I also wanted to make it easy on myself - so I picked a system that was simple to remember.

Regards,
John