[chipsahoy]

I have a question on the drilling cycle for the 10T control.

If I wan to peck drill a hole what is the proper code.

Do I use a G74 , G83 or what.

I tried the G74 and the machine didnt go any where.

Or is this an option and my control doesn't have it..

Also what is the length of the buffer memory in these machines.. Mine is a 1986 10t Fanuc..

thanks Chips

[stevo1]

Post your code so we can take a look at it.

It will depend on which G-code system you are using (A,B,C). It has been a while on this control but G83 should be peck drilling no matter what system you are using. I don’t recall if you can do a G73 for high speed peck or not. You can tell what G-code system you are using by looking at parameter 2400 bit 7&6 (I think that’s the parameter).
00XXXXXX=systemA
01XXXXXX=systemB
10XXXXXX=systemC

Yes the canned cycles are an on the control. You will know if the option is not active because it would alarm out with “improper G-code”. You didn’t mention that so I ass u me it is active. If not PM me your 9100 parameters and I will take a look at them.

IIRC in the 10,11,12 series the buffer length is 10 characters.

Stevo

[sinha_nsit]

I have heard that the canned drilling cycles would be available only with live tooling. On a simple lathe, G74 can be used. Make sure that the syntax is correct. See the attachment for details. This, of course, is for 0i series.

[stevo1]

Chips….I got your PM and I am posting here so anyone can chime in.

G0G90X0Z3.
G83Z-1.5R.1Q.1F3.
M30

The Z3. Is the “initial” plane. The Z-1.5 is drill depth. R.1 is the “return” plane. Q.1 is the peck size. Now you can use G98 or G99 in the G83 line depending on if you want to return to the “initial” plane or the “return” plane when drilling is complete. IIRC most fanucs will be default G98 so if that is what you want then you do not need to insert that code.

Stevo

[dcoupar]

I'm assuming your feedrate (F3.) is in inches per minute?

I doubt that G83 is available unless you have live tooling, so I suggest using G74. According to the 10TA manual G74 uses the following format:

G74 X__ Z(W)__ I__ K__ F__ D__

You can use Z to specify the absolute depth from Z0, or W to specify the incremental depth from the starting point.

I and D are not used for straight peck drilling, and you most likely position to X0 Z0.1 before calling the cycle.

G97 S500 M03 (START SPINDLE AT 500 RPM)
G00 G99 X0 Z0.1 (MOVE TO START POINT, SET IPR MODE)
G74 Z-1.5 K0.1 F0.01 (PECK 1.5 DEEP, WITH 0.1 DEEP PECK)
G00 G28 U0. W0. (RETURN X AND Z TO HOME)

As for "buffer memory" do you mean program storage capacity? It seems to me that the 10T was available with 20, 40, or 80 meters of "tape storage". Not a lot, but usually sufficient for a 2-axis lathe.