Post processor for the Techno CNC interface. Build #377

[Anonymous]

Hi I have an older TECHNO CNC machine with the build #377 interface (PC interface)

This is a 3 axis Mill / gantry router, it has NO tool changer.

Ive tried several of the "stock posts" for HSM & Fusion 360...

It was recommended that the ISEL.cps - Generic ISEL Intermediate be tried... it dos not work...fails at Post

Here is the failed log for ISEL.cps:

Information: Configuration: Generic ISEL Intermediate
Information: Vendor: ISEL
Information: Posting intermediate data to 'C:\Users\Mark Jackson\AppData\Local\Fusion 360 CAM\nc\techno test_001.ncp'
Error: Failed to post process. See below for details.
...
Code page changed to '1252  (ANSI - Latin I)'
Start time: Wednesday, October 05, 2016 5:34:03 PM
Code page changed to '20127 (US-ASCII)'
Post processor engine: 4.2.1 41078
Configuration path: C:\Users\Mark Jackson\AppData\Local\Autodesk\webdeploy\production\8230b364be98230257f730ec9822611826c56dfb\Applications\CAM360\Data\Posts\isel.cps
Include paths: C:\Users\Mark Jackson\AppData\Local\Autodesk\webdeploy\production\8230b364be98230257f730ec9822611826c56dfb\Applications\CAM360\Data\Posts
Configuration modification date: Thursday, June 02, 2016 7:33:37 PM
Output path: C:\Users\Mark Jackson\AppData\Local\Fusion 360 CAM\nc\techno test_001.ncp
Checksum of intermediate NC data: a6b0b3064f31b6ab97ade2ac8d67adaf
Checksum of configuration: 87e8549591838a6c8c7af44fae522e48
Vendor url: https://www.isel.com
Legal: Copyright (C) 2012-2016 by Autodesk, Inc.
Generated by: Fusion 360 CAM 2.0.2377
...
Error: Inch mode is not supported.
^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^
Error: Failed to invoke 'onOpen' in the post configuration.
Error: Failed to invoke function 'onOpen'.
Error: Failed to execute configuration.
Stop time: Wednesday, October 05, 2016 5:34:03 PM
Post processing failed.

Ive also seen another thread stating that the osia.cps - Generic OSAI  post would work for TECHNO but it dose not, it uses some Canned Cycle (G79) which I think is a Drilling or thread cycle for a Lathe that the TECHNO interface is not recognizing.

Here is the OSIA post that fails when running on the TECHNO interface (error is "Canned Cycle Not Found"  )

; TECHNO TEST_001
; TCHONO TEST_001
; T1  D=0.1875 CR=0. - ZMIN=0. - FLAT END MILL
N10 G90 G94
N11 G17
N12 G70
N13 G00 G79 G91 Z0.
N14 G90
; 2D CONTOUR1
N15 M09
N16 T1 M06
N17 S18000 M03
N18 M08
N20 G00 X9.85 Y5.2312
N21 Z0.85 h01
N22 G00 Z0.45
N23 G01 Z0.2894 F75.
N24 Z0.2687 F30.
N25 G18
N26 G02 X9.8687 Z0.25 R0.0188
N27 G01 X9.8875 F75.
N28 G17
N29 G03 X9.9062 Y5.25 R0.0187
N30 G01 Y5.8437
N31 Z0.375
N32 Y6.
N34 G03 X9.8927 Y6.1562 R0.9062
N35 G01 Z0.25 F30.
N37 G03 X9.1563 Y6.8927 R0.9063 F75.
N38 G01 Z0.375
N40 G03 X9. Y6.9062 R0.9063
N41 G01 X8.8438
N42 Z0.25 F30.
N43 X4.6563 F75.
N44 Z0.375
N45 X4.5
N47 G03 X4.3438 Y6.8927 R0.9063
N48 G01 Z0.25 F30.
N50 G03 X3.6073 Y6.1562 R0.9063 F75.
N51 G01 Z0.375
N53 G03 X3.5938 Y6. R0.9063
N54 G01 Y5.8437
N55 Z0.25 F30.
N56 Y4.6563 F75.
N57 Z0.375
N58 Y4.5
N60 G03 X3.6073 Y4.3438 R0.9063
N61 G01 Z0.25 F30.
N63 G03 X4.3438 Y3.6073 R0.9063 F75.
N64 G01 Z0.375
N66 G03 X4.5 Y3.5938 R0.9063
N67 G01 X4.6563
N68 Z0.25 F30.
N69 X8.8438 F75.
N70 Z0.375
N71 X9.
N73 G03 X9.1563 Y3.6073 R0.9063
N74 G01 Z0.25 F30.
N76 G03 X9.8927 Y4.3438 R0.9062 F75.
N77 G01 Z0.375
N79 G03 X9.9062 Y4.5 R0.9062
N80 G01 Y4.6563
N81 Z0.25 F30.
N82 Y5.25 F75.
N84 G03 X9.8875 Y5.2687 R0.0187
N85 G01 X9.8687
N86 G18
N87 G03 X9.85 Z0.2687 R0.0187
N88 G00 Z0.85
N89 G17
N90 (UAO,0)
; DRILL1
N91 M08
N92 G00 X11. Y2.
N93 Z0.85
N95 Z0.45
N96 G81 R0.45 R0.45 Z0.45 F30.
N97 X11.
N98 X10.5 Y7.5
N99 X2.5
N100 Y2.
N101 G80
N102 Z0.85
N104 (UAO,0)
N105 M09
N106 G79 G91 Z0.
N107 G79 X0. Y0.
N108 M30

here is the TECHNO CNC Interface (Build#377)...

Here is an example G-CODE that dose work but is posted from AutoCAD to Gcode Lisp...(lisp run in AutoCAD)

(GP1508_GP1518_GP2508_GP2518 GO7-Vulcan7.nc)
(65998811026 5	GP1508	SystemPod Pre-Cut for Simrad GO7 / B&G Vulcan 7 and space on left, for 9.5" wide guard)
(65998811027 2	GP1518	SystemPod Pre-Cut for Simrad GO7 / B&G Vulcan 7 and one instrument (3.6" hole) for 9.5" wide guard)
(65998811030 2	GP2508	SystemPod Pre-Cut for Simrad GO7 / B&G Vulcan 7 and space on left, for 12" wide guard)
(65998811031 9	GP2518	SystemPod Pre-Cut for Simrad GO7 / B&G Vulcan 7 and one instrument (3.6" hole) for 12" wide guard)
(USE .1875 END MILL CUTTER)
(MDJ 06-30-2015)

N1 G17 G20 G90 G40 G80 G64 G49 G0 
N2 G8 P1
N3 G90 
N4 M3
N5 G0 Z1.00000
N6 G0 X-4.38120 Y18.13877 Z1.00000
N7 G1 X-4.38120 Y18.13877 Z-0.50000 F50
N8 G2 X-4.15062 Y17.90819 Z-0.50000 I0.00000 J-0.23058 F50
N9 G1 X-4.15062 Y11.68685 Z-0.50000
N10 G2 X-4.38120 Y11.45627 Z-0.50000 I-0.23058 J0.00000
N11 G1 X-5.70827 Y11.45627 Z-0.50000
N12 G1 X-5.70827 Y11.34060 Z-0.50000
N13 G1 X-7.03546 Y11.34060 Z-0.50000
N14 G1 X-7.03546 Y11.45627 Z-0.50000
N15 G1 X-8.36254 Y11.45627 Z-0.50000
N16 G2 X-8.59312 Y11.68685 Z-0.50000 I0.00000 J0.23058
N17 G1 X-8.59312 Y17.90819 Z-0.50000
N18 G2 X-8.36254 Y18.13877 Z-0.50000 I0.23058 J0.00000
N19 G1 X-7.03546 Y18.13877 Z-0.50000
N20 G1 X-7.03546 Y18.25444 Z-0.50000
N21 G1 X-5.70827 Y18.25444 Z-0.50000
N22 G1 X-5.70827 Y18.13877 Z-0.50000
N23 G1 X-4.38120 Y18.13877 Z-0.50000
N24 G0 X-4.38120 Y18.13877 Z1.00000
N25 G0 X-4.38120 Y18.16877 Z1.00000
N26 G1 X-4.38120 Y18.16877 Z-0.50000 F50
N27 G2 X-4.12062 Y17.90819 Z-0.50000 I0.00000 J-0.26058 F50
N28 G1 X-4.12062 Y11.68685 Z-0.50000
N29 G2 X-4.38120 Y11.42627 Z-0.50000 I-0.26058 J0.00000
N30 G1 X-5.67827 Y11.42627 Z-0.50000
N31 G1 X-5.67827 Y11.31060 Z-0.50000
N32 G1 X-7.06546 Y11.31060 Z-0.50000
N33 G1 X-7.06546 Y11.42627 Z-0.50000
N34 G1 X-8.36254 Y11.42627 Z-0.50000
N35 G2 X-8.62312 Y11.68685 Z-0.50000 I0.00000 J0.26058
N36 G1 X-8.62312 Y17.90819 Z-0.50000
N37 G2 X-8.36254 Y18.16877 Z-0.50000 I0.26058 J0.00000
N38 G1 X-7.06546 Y18.16877 Z-0.50000
N39 G1 X-7.06546 Y18.28444 Z-0.50000
N40 G1 X-5.67827 Y18.28444 Z-0.50000
N41 G1 X-5.67827 Y18.16877 Z-0.50000
N42 G1 X-4.38120 Y18.16877 Z-0.50000
N43 G0 X-4.38120 Y18.16877 Z1.00000
N44 G0 X-3.93413 Y11.25073 Z1.00000
N45 F50
N46 G83 X-3.93413 Y11.25073 Z-0.50000 R0.25000 Q0.50000
N47 G0 X-3.93413 Y11.25073 Z1.00000
N48 G0 X-8.81602 Y11.25073 Z1.00000
N49 F50
N50 G83 X-8.81602 Y11.25073 Z-0.50000 R0.25000 Q0.50000
N51 G0 X-8.81602 Y11.25073 Z1.00000
N52 G0 X-8.81602 Y18.33735 Z1.00000
N53 F50
N54 G83 X-8.81602 Y18.33735 Z-0.50000 R0.25000 Q0.50000
N55 G0 X-8.81602 Y18.33735 Z1.00000
N56 G0 X-3.93413 Y18.33735 Z1.00000
N57 F50
N58 G83 X-3.93413 Y18.33735 Z-0.50000 R0.25000 Q0.50000
N59 G0 X-3.93413 Y18.33735 Z1.00000
N60 G0 X-6.37187 Y9.80317 Z1.00000
N61 G1 X-6.37187 Y9.80317 Z-0.50000 F50
N62 G2 X-4.68486 Y8.11616 Z-0.50000 I0.00000 J-1.68701 F50
N63 G2 X-6.37187 Y6.42916 Z-0.50000 I-1.68701 J0.00000
N64 G2 X-8.05888 Y8.11616 Z-0.50000 I0.00000 J1.68701
N65 G2 X-6.37187 Y9.80317 Z-0.50000 I1.68701 J0.00000
N66 G0 X-6.37187 Y9.80317 Z1.00000
N67 G0 X-6.37187 Y9.83317 Z1.00000
N68 G1 X-6.37187 Y9.83317 Z-0.50000 F50
N69 G2 X-4.65486 Y8.11616 Z-0.50000 I0.00000 J-1.71701 F50
N70 G2 X-6.37187 Y6.39916 Z-0.50000 I-1.71701 J0.00000
N71 G2 X-8.08888 Y8.11616 Z-0.50000 I0.00000 J1.71701
N72 G2 X-6.37187 Y9.83317 Z-0.50000 I1.71701 J0.00000
N73 G0 X-6.37187 Y9.83317 Z1.00000
N74 G0
N75 G90 G49 M05
N76 M5
N77 M30

dose anyone have any other suggestions on getting this to work form HSM / Fusion360...on the TECHNO #377 interface

Thanks

[matthew.nichols]

hi @Anonymous,

I had this minimal milling post that you can try.  this is a generic one that i have for machines like this.  Let me know how it goes?  If you need any other modifications to it then there are lots of people on here or i can put you in touch with someone to make modifications.

Thank you,

[Anonymous]

Thanks Matt still isn't quite what I need

Sent from my iPhone

[xander.luciano]

Ah shoot I used to have a perfect TechnoCNC post a few years back but I have no idea where it is anymore. I'll do some searching and see if I can find it.

In the meantime, try the generic Intelitek post, I believe that is what the updated post was based off of. IIRC it would gouge the material a bit on the helical spiral entry, but that was the only issue.

I'll see if I can find it and get back with you! Let me know how the intelitek works though!

Best,

[xander.luciano]

You're (possibly) in luck today!

Good thing the old forums got migrated over and good thing google exists haha. I was able to dig up this thread from over 4 years ago! Might have something that will work for your machine.

https://forums.autodesk.com/t5/hsm-post-processor-forum/post-processor-for-intelitek-prolight-1000-c...

I also attached the post that was created for you to try out. Let me know if it works/doesn't work and I can make any necessary changes in it for you!

Best,

[Anonymous · Accepted solution]

Thanks all

I finally got back around to testing this...

It looks like the best "stock post" for the Techno  CNC interface. Build #377 is the rs274.cps

ill test some more but the rs274.cps looks to work pretty well

[xander.luciano]

Glad to hear you found something that works!

If you need anything changed, feel free to reach out to me and I'll be happy to make the change. 🙂

Happy Machining!

[Anonymous]

Hello-

I'm brand new to all this and having problems with a similar situation.  I recently bought a business that came with a CNC (older Techno Isel) router.  I have been using SolidWorks for awhile and am pretty comfortable with it.  I have HSM that operates inside SW and also recently purchased F360.  The problem is the original owner would post process to the router through ArtCam.  I am not familiar to this program and really can't afford to take the time right now with the pressure of a job I am dealing with.  ArCam post process works fine. When I use HSM, the drill or end mills first move is to the height of the stock from the WCS origin to the first hole, in my case, leaving a gouge across my material. Only having a problem with the first move, rest of the progam works as intended.  With the techno interface program you can preview the tool path and it shows the first move doing just that.  I have pulled up numerous programs that the previous owner created in ArtCam in the past and they all preview with the first move going up to the retract height before moving to the first hole.  I have tried several options listed in HSM for post processing and no matter what get the same results.  Can you help?  Thanks in advance.  

[Anonymous]

I should add, when I go to web library at http://cam.autodesk.com/posts/ for post proccessors I have found the TECHNO one but when I download it I get an error like the attached picture.   

[INNWDesign]

I work a lot with a Techno CNC machine at a guitar company. I would highly recommend that you visit the Techno site and get one of the documents that explains their NC code implementation. The Techno is very limited in its functions but you can make it work for most stuff. If your code throws any G17, G18, G43, etc. that the machine does not recognize it will NOT give desired results i.e CRASH. Only use the code that is listed in their manual. That's the best info I can give you at this point.

I am anxious to try out the new Minimal Milling.CPS file and see what the results are. I've been using the FANUC post and it got me in the ballpark most of the time

In the mean time I would also recommend you look into a program called NCPLOT. This program has saved my backside many times. It's very much worth the money and the tools are beyond fantastic. 

Three examples:

A guitar body I was designing in Fusion 360 generated the NC file and kept throwing G17 and G18 codes. No matter what options I chose, it still gave me those codes that the Techno machine has no clue what to do with and pukes. You can't just simply remove those commands as they directly related to the G2 and G3 in the code. I had to find a solution so I used NCPLOT and the Change arcs to straight lines tool worked great, problem fixed.

Need to reverse engineer a part from G code and no drawings exist? It will process that and give you a DXF file with all the layers as well. Used that Many times.

Need a part flipped in the XYZ axis, for example you need a left hand model that was design as a right handed model. It'll flip the code for you and yes, it really works.

Sorry for the ramble, just offering some solutions, suggestions and tools to help.

Thanks for the info on the Minimal Milling.CPS. I've spent countless hours searching code for stuff I knew would not run on the Techno. I sure hope this works.

And yes, I use Fusion 360 exclusively to design the guitars. The CNC function is just fantastic in my view, its right there, I don't have to switch programs.

The AutoDesk Fusion 360 team has done a terrific job. Keep up the good work.

Peace!

[AchimN]

Thanks for your feedback.

Please try the latest version of the post which is available here:

http://cam.autodesk.com/posts?p=techno_cnc_router