[yardbird1969]

Hello All,
Machine is Doosan PUMA 300 lathe FANUC i series
Normally I write out long hand all grooves. Just G0 and G1 F.01
I am cutting an OD groove and was going to try G75 the Doosan programming Manual shows no reference to chamfers or corner rounding in the book.
Tool is a .1875 wide cut off tool not made for turning or I would try G71
The groove is 2.35” +/-.005 wide
.69” radius deep
.06” x 45(x2) chamfers on the top
.120”rad(x2) radius in the bottom corners

G75 R
G75 X Z P Q F

Are there more variables to the G75 canned grooving cycle for chamfering and corner rounding of the groove?
Thank you
-Brent-

[Heavy_Metal]

Hi Brent,

Which Fanuc i control do you have ?
We have different controls ( 0T / 18T / 18i-TB ) but it is not possible on our lathes, not without Manual Guide i.
I use 2x G75 and G01/G02/G03 for finishing the contour.
I start with the yellow toolpath, G75 at X200mm, to remove the first step.
Then i start the second, green toolpath, also G75, now at X126mm, to remove the material between the radius.
Third step, the red toolpath is for finishing the contour.
All three steps with the same tool.
Our 18i-TB control has Manual-Guide i and according to the book G1470 and G1471 can do the job.
See my attachments.

Regards,
Heavy_Metal
The Netherlands.

[yardbird1969]

Hi Heavy_Metal,
The control is I believe is an Oi-TD and thank you for your help.

[tigerhao]

FYI

[yardbird1969]

tigerhao,
Thank you for the illustration.
-Brent-

[Heavy_Metal]

Hi Brent,

Looked today on my Doosan 18i-TB and only the Manual Guide i, G1470 option (and G1471) can do the job.
Only when you can write a proper macro G75 can be used, or what I explained in the earlier #2 post.
The Manual Guide G1470 has different options for corners (all 4) like, NOTHING/CHAMFER/RADIUS and also REPEAT (grooves).

Regards,
Heavy_Metal
The Netherlands.

[yardbird1969]

Hi Heavy_Metal,
I did the job exactly as you suggested in your earlier #2 post. Thanks again! G75 worked well for material removal. We have only had the PUMA 300 a few months. Along with all the yellow Fanuc manuals was blue & grey Doosan box that had Doosan manuals in it. On the side of the box it says control oi-TD. On the machine front panel it say Fanuc i series. When powering up the machine the CRT screen says Manual-Guide i when booting up. “Manual-Guide I according to the book G1470 and G1471 can do the job.” Can G1470 & G1471 be programed manually or is it the conversational programming side of the control?
Where do I verify what is the actual control is on this machine?
Thank you Heavy_Metal
Brent

[DouglasR]

If the machine has a Fanuc 0iT-D CNC, then it most likely is equipped with EZ-Guide i programming function, which is located under the "Custom 1" menu.

For G75 grooving cycle in conventional programming - this cycle is is ok for roughing out a groove. But it can lead to tool marks on the groove walls.

[Heavy_Metal]

Hi Brent,

I don't use the Manual Guide i option, to much functions, but maybe in the future.
On my Doosan I activate MGi with the [GRAPH] key, the [POS] key returns to normal (ISO) mode.
The groove G1470 option with CHAMFER/ARC corners create a long line/block of codes.
When you create a normale g-code (ISO) program I think you can insert a G1470 code as well.
Tomorrow I will check how to verify the actual control, maybe [SYSTEM] or [CUSTOM] key.

Regards,
Heavy_Metal.

[Heavy_Metal]

Hi Brent,
To verify the actual control on my Doosan, [SYSTEM] key, [PMCDGN] soft key.

CNC TYPE NAME: PMC-SB7 & FS-18ITB (18i-TB)

Regards,
Heavy_Metal.

[yardbird1969]

Hi DouglasR,

Yes my machine is equipped with the EZ Guide I option.
Not sure I want to mess with that or not. the old dog new tricks thing.
I will settle with a NO to my original question and leave it at that.
G75 did work well for stock removal.

Thank you DouglasR,

Brent

[yardbird1969]

Hi Brent,
To verify the actual control on my Doosan, [SYSTEM] key, [PMCDGN] soft key.

CNC TYPE NAME: PMC-SB7 & FS-18ITB (18i-TB)

Regards,
Heavy_Metal.

Hi Heavy_Metal,

Thank you! I will try to verify my actual control today as you suggested.

The answer to my original question is NO.
I really do not wish to start using a computer generated tool path. I can’t read or edit them.
When the Factory Doosan rep left after a day of training on the machine along with some training on the
conversational programming side of the control (Maybe EZ Guide I option?).
This is one of two programs that the Factory Doosan guy left in the machine when he left our factory.

%
O0001
G1900D2.L6.K0.02
G500T12.W12.R4.M11.S500.C54.H96.B9.
G1120P1.Q0.04H100.C0.015D0.002F0.01E0.01V0.01W1.U0 .05L0.1M0.1Z22.X2.Y2.N2.I0.03K100.
G1450H0.1V1.05A0.
G1451H0.1V0.K7.D0.L0.M0.T2.
G1451H0.V0.K5.C0.L0.M0.T2.
G1451H0.V0.345K3.D0.375L0.M0.T1.
G1454H-0.03V0.375C0.03T1.
G1451H-1.375V0.375K5.C-1.5L0.M0.T1.
G1455H-1.5V0.5R0.125I-1.375J0.5K2.T1.
G1451H-1.5V0.97K3.D1.L0.M0.T1.
G1454H-1.53V1.C0.03T1.
G1451H-1.55V1.K5.C-1.55L0.M0.T1.
G1451H-1.55V1.05K3.D1.05L0.M0.T2.
G1451H0.1V1.05K1.C0.1L0.M0.T2.
G1456
%


Thank you Heavy_Metal

[DouglasR]

Hi DouglasR,

Yes my machine is equipped with the EZ Guide I option.
Not sure I want to mess with that or not. the old dog new tricks thing.
I will settle with a NO to my original question and leave it at that.
G75 did work well for stock removal.

Thank you DouglasR,

Brent

Very good, Brent.
If you like I can fwd our in house manuals and reference materials to you.
All the best!