HSM PRO CAM - Post Processing TURN 270 PRO

Anything to do with configuring CAM systems and Post Processors to run on different CNC machines

Moderators: Mr Magoo, Martin, bradders, Steve

Post Reply
jscheminger
Posts: 5
Joined: Thu 21 May , 2015 12:35 pm
Hardware/Software: Turn 270 Pro
Router 2600 Pro
Universal Laser VLS4.6

HSM PRO CAM - Post Processing TURN 270 PRO

Post by jscheminger » Wed 11 Apr , 2018 18:33 pm

Hoping to find a post that will let me use AUtodesk Inventor/HSMPro to my new TURN 270 Pro with tool change.
Any thoughts on a compatible machine? I can output to FANUC, HAAs, Heidenhain, proLIGHT, ProtoTRAK, Tormach, Siemens, OKUMA, FAGOR, GSK.
Also can adjust the configuration on any of these...
Thanks.
Jeff

Martin
CNC Guru
CNC Guru
Posts: 1605
Joined: Fri 24 Feb , 2006 17:09 pm
Location: Brighouse

Re: HSM PRO CAM - Post Processing TURN 270 PRO

Post by Martin » Thu 12 Apr , 2018 7:32 am

Hi Jeff

Try using the Fanuc output. It's just standard G & M codes.

jscheminger
Posts: 5
Joined: Thu 21 May , 2015 12:35 pm
Hardware/Software: Turn 270 Pro
Router 2600 Pro
Universal Laser VLS4.6

Re: HSM PRO CAM - Post Processing TURN 270 PRO

Post by jscheminger » Thu 12 Apr , 2018 19:49 pm

Martin wrote:Hi Jeff

Try using the Fanuc output. It's just standard G & M codes.
Hi Martin -

Posted with FANUC (and HAAS) and have been fighting through some errors.
Is there a list of G-Codes that are good to use? I'm thinking that the post uses some G commands that are not supported.
Here are the first few lines as an example.

(FANUC POST)
O1001
G98 G18
G21
G50 S6000
G28 U0.
(GROOVE2)
T0707
G54
G99
G50 S3000
G96 S200 M3
G0 X39.05 Z5.
G0 Z-9.158
X23.05
G1 X19.05 F1.
X17.319
X23.05
G0 Z-10.152
G1 X19.05 F1.
X17.164
X19.035
X19.05
X22.521
G0 X23.05
Z-11.145
G1 X19.05 F1.
X18.397
X19.05
X23.05

I am in process of creating a part with the Denford software & post and same part with HSM post to see how the G-code matches up.

Thanks,
Jeff

Martin
CNC Guru
CNC Guru
Posts: 1605
Joined: Fri 24 Feb , 2006 17:09 pm
Location: Brighouse

Re: HSM PRO CAM - Post Processing TURN 270 PRO

Post by Martin » Fri 13 Apr , 2018 7:49 am

List of G & M codes out of the VRTurning Manual

GØØ (Rapid Positioning / Traverse).

GØ1 (Linear Interpolation).

GØ2 / GØ3 (Circular Interpolation).

GØ4 (Dwell).

G2Ø / G21(Inch/Metric Data Input).

G28 (Reference Point Return).

G4Ø / G41 / G42 (Tool Nose Radius Compensation).

G5Ø (Multiple Command Functions).

G7Ø (Finishing Cycle).

G71 (Stock Removal in X Axis).

G72 (Stock Removal in Facing).

G73 (Pattern Repeating).

G74 (End Face Peck Drilling Cycle).

G75 (Outer / Internal Dia. Drilling & Grooving Cycle).

G76 (Multiple Thread Cutting Cycle).

G81 (Deep Hole Drilling Cycle).

G9Ø (Outer / Internal Dia. Cutting Cycle).

G92 (Thread Cutting Cycle).

G94 (End/Taper Face Turning Cycle).

G96 (Constant Surface Speed Control).

G97 (Spindle Speed in Rev/Minute).

G98 (Per Minute Feed).

G99 (Per Revolution Feed).


MØØ (Program Stop).

MØ1 (Optional Stop).

MØ2 (End of Program).

MØ3 (Spindle Forward).

MØ4 (Spindle Reverse).

MØ5 (Spindle Stop).

MØ6 (Automatic Tool Change).

MØ8 (Coolant On).

MØ9 (Coolant Off).

M1Ø (Chuck Open).

M11 (Chuck Close).

M13 (Spindle Forward and Coolant On).

M14 (Spindle Reverse and Coolant On).

M25 (Tailstock Quill Extend).

M26 (Tailstock Quill Retract).

M3Ø (Program Stop and Reset).

M4Ø (Parts Catcher Extend).

M41 (Parts Catcher Retract).

M62 / M63 / M64 / M65 / M66 / M76 / M77 (Auxiliary Output Functions).

M98 (Sub Program Call).

M99 (Sub Program End and Return).

jscheminger
Posts: 5
Joined: Thu 21 May , 2015 12:35 pm
Hardware/Software: Turn 270 Pro
Router 2600 Pro
Universal Laser VLS4.6

Re: HSM PRO CAM - Post Processing TURN 270 PRO

Post by jscheminger » Fri 13 Apr , 2018 14:10 pm

Thanks Martin - very helpful.

I'm comparing g-code outputs now from HSM vs. VRTurn for part reproduced in both.

Jeff

jscheminger
Posts: 5
Joined: Thu 21 May , 2015 12:35 pm
Hardware/Software: Turn 270 Pro
Router 2600 Pro
Universal Laser VLS4.6

Re: HSM PRO CAM - Post Processing TURN 270 PRO

Post by jscheminger » Fri 13 Apr , 2018 19:51 pm

Final follow-up -

Was able to get FANUC g-code working with a couple of minor modifications - codes G18 and G54 are generated but appear unnecessary; and the output code does not include a tool change command in front of the tool number string.

Thanks again for the list of used codes - it proved very useful to get this figured out.

Jeff

Post Reply