ISO Haas ST Lathe post without C axis and without live tools

[shadwin123D]

I have tried all of the Haas lathe posts offered in the library.   I  have tried modifying posts by turning off various modals in the script,  I keep getting different outputs having sub programs, c axis code in drill cycles, M155 codes, etc.  I can remove some of the code, but usually end of with some remnant referring to a live tooling situation.   Does anybody have a clean post for Haas lathes that do not have C axis or Y axis or live tooling.   Help!!

[AchimN]

Did you try this one as well? https://cam.autodesk.com/hsmposts?p=haas_turning

[shadwin123D]

I got an error the first time.   Milling toolpath is not supported.  I will try turning off some of the variable fields.

Information: Configuration: HAAS Turning
Information: Vendor: Haas Automation
Information: Posting intermediate data to 'C:\Users\CNC Instructor\AppData\Local\Fusion 360 CAM\nc\8516.nc'
Error: Failed to post process. See below for details.
...
Code page changed to '1252 (ANSI - Latin I)'
Start time: Tuesday, September 18, 2018 5:37:34 PM
Code page changed to '20127 (US-ASCII)'
Post processor engine: 4.2.1 42089
Configuration path: C:\Users\CNC Instructor\Desktop\Haas Posts\haas turning V 42115.cps
Include paths: C:\Users\CNC Instructor\Desktop\Haas Posts
Configuration modification date: Tuesday, September 18, 2018 5:36:30 PM
Output path: C:\Users\CNC Instructor\AppData\Local\Fusion 360 CAM\nc\8516.nc
Checksum of intermediate NC data: e8c29f712d0e2753438f5dc21905fb2e
Checksum of configuration: 46d30c306b79f11010f3359bc271e259
Vendor url: https://www.haascnc.com
Legal: Copyright (C) 2012-2018 by Autodesk, Inc.
Generated by: Fusion 360 CAM 2.0.4391
...

###############################################################################
Error: Milling toolpath is not supported by the post configuration.
Failed while processing onOpen().
###############################################################################

Error: Failed to invoke 'onOpen' in the post configuration.
Error:
Error: Failed to execute configuration.
Stop time: Tuesday, September 18, 2018 5:37:34 PM
Post processing failed.

[shadwin123D]

It is a very basic Post config.  Does not have provision to set a Z home position for tool change. Unable to turn cycles on/off, turn tailstock on/off, etc.  Tried turning cycles off and still got same error report.

Here is a link to part.  We are having trouble with Setup2.  Already shorted program to bare minimum processes .

https://a360.co/2MJ5prI

I have attached the most recent post I had customized, but something changed this summer and now it is not providing me good drill codes.

[shadwin123D]

Here is a video going thru the paces.   I get the following unusable code...  

line 45 - P3018 M133

Line 50 - G0 C-72.938  (several places)

Line 54 - G83 X0.0089 C-72.938 Z-.06 R0.2 A0.0797 F0.004 (G83 is not a usuable code for Haas lathe,, shouldn't X be X0.0?

Line 74 - Not sure about G95.   It sure appears to look at my program as a mill program specifically.

https://autode.sk/2NR0edP

[ArjanDijk]

Don't touch the Haas ST posts, they are for machines with driven tools.

In your setup2 your are not drilling in the center. There is a slight offset. This is off course not possible with a 2 axis lathe. Open the sketch and adjust the midpoint. See the code below

%
O8516 (TITAN 85L DM 2OP)
N10 G98 G18
N11 G20
N12 G50 S6000
N13 M31
N14 G53 G0 X0.

(Rough Face)
N15 T101
(NPR51)
N16 G99
N17 M22
N18 G97 S1698 M3
N19 G55
N20 M8
N21 G0 X1.8 Z0.4443
N22 G50 S3000
N23 G96 S800 M3
N24 G0 Z0.004
N25 G1 X1.16 F0.008
N26 X1.
N27 X-0.0312
N28 X0.0819 Z0.0606
N29 G0 X1.8
N30 Z0.4443
N31 G97 S1698 M3
N32 M9
N33 G53 X0.

(Drill4)
N34 M1
N35 T1010
N36 G98
N37 M22
N38 G97 S3018 M3
N39 G55
N40 M8
N41 G0 X0. Z0.62
N42 G17
N43 G0 Z0.22
N44 Z0.62
N45 Z0.22
N46 G83 X0. Z-0.6 R0.2 Q0.0797 F12.0737
N47 G80
N48 Z0.62
N49 M9
N50 G53 X0.

(Drill2)
N51 M1
N52 T1111
N53 G98
N54 M22
N55 G97 S1630 M3
N56 G55
N57 M8
N58 G0 X0. Z1.22
N59 G17
N60 G0 Z0.22
N61 Z1.22
N62 Z0.22
N63 G84 X0. Z-0.269 R0.2 P0 F101.875
N64 G80
N65 Z1.22

N66 M9
N67 G53 X0.
N68 G53 Z0.
N69 M30
%

[shadwin123D · Accepted solution]

Thanks, I reviewed my students model and see where he missed the origin of the hole location.  I used the haas lathe post you recommended and got rid of the Caxis movements and the subprogram calls.  I lost my canned drill cycles and now have tailstock and chip conveyor code showing up.   I no longer have a variable field to turn on/off tailstock or chip conveyor.   I can still have them manually remove those commands, but would be nice to not have to worry about it.

[ArjanDijk]

Glad to be of help. Please accept my reply as a solution.

Regarding your options. I understand the issue. Previously millturn posts had an option to disable C axis, but thats not there in the last Haas post. Maybe request a Haas ST turning only post on the post idea forum. Would not be too much work

[Anonymous · Accepted solution]

For future troubleshooting, check in your Drill's tool definition dialogue box. On the General tab where you define the tool and offset numbers as well as coolant, there is a check box for Live tool. If you do not want C axis output, ensure that this option is unchecked. 

[derekfriedrichs]

That fix didnt help me, I have a left hand thread, and the error says that counterclockwise rotation is not supported

I have a 2020 Haas ST-35 Standard

Thanks

[derekfriedrichs]

Doest do a bit of a difference, still posts out the 155 code.  I dont have a c axis, this post processor sucks ass