Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Post with Subroutines

23 REPLIES 23
SOLVED
Reply
Message 1 of 24
Big_Mak
4284 Views, 23 Replies

Post with Subroutines

For multi part posts, it would be a good option to post with sub programs so the main program calls the WCS then calls the applicable operations sub program.

 

Secondly I'd like to see the option when posts to multiple WCS' that you can return to G28 Z0, or just to the Clearance plane so save some motion.

23 REPLIES 23
Message 2 of 24
al.whatmough
in reply to: Big_Mak

What post are you using?

 

We have a Fanuc post that will post with Sub-Programs.  Each sub-Program being a seperate file.

fanuc.png

 

The Haas post allows Sub-programs as well. Each sub-program will just be lower down in the code.

 

haas with sub programs.png

 

 

---------
AL Whatmough
Director Product Management - Manufacturing

Note, I love to engage on the forums. However, I spend a lot of time in meetings trying to help clear the path for our amazing team of Developers working on Manufacturing at Autodesk. So, if I don't respond immediately, it's not that I don't care.
Message 3 of 24
Big_Mak
in reply to: al.whatmough

I'm using a haas post that has been modified for tapping in feed per rev.
Message 4 of 24
al.whatmough
in reply to: Big_Mak

If it was derived from the Stock post is shoud have the "useSubroutines" Option.

---------
AL Whatmough
Director Product Management - Manufacturing

Note, I love to engage on the forums. However, I spend a lot of time in meetings trying to help clear the path for our amazing team of Developers working on Manufacturing at Autodesk. So, if I don't respond immediately, it's not that I don't care.
Message 5 of 24
Big_Mak
in reply to: al.whatmough

I'll mess with it to see if I can get it to output what I want.

Thanks.
Message 6 of 24
Big_Mak
in reply to: al.whatmough

I messed with it and it output the subs!  Great!  I'm a happy camper!

Message 7 of 24
scottmoyse
in reply to: Big_Mak


@Big_Mak wrote:

I messed with it and it output the subs!  Great!  I'm a happy camper!


@Big_Mak how do you make use of the subs? Since all it does by default is push the bulk of the code to the end of the nc file, calling it up in the simpler code at the top. Are you doing something beyond that with it?


Scott Moyse
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.


EESignature


Design & Manufacturing Technical Services Manager at Cadpro New Zealand

Co-founder of the Grumpy Sloth full aluminium billet mechanical keyboard project

Message 8 of 24
Big_Mak
in reply to: scottmoyse

I use this subprogram option if I'm machining the same setup, but many parts.  This way the main program set's the work coordinates, and calls the subs.  The subs then drive the tools around the parts cutting metal.

Message 9 of 24
scottmoyse
in reply to: Big_Mak

Yeah but how are you setting the new coordinates for each iteration of the subprogram.

Scott Moyse
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.


EESignature


Design & Manufacturing Technical Services Manager at Cadpro New Zealand

Co-founder of the Grumpy Sloth full aluminium billet mechanical keyboard project

Message 10 of 24
Big_Mak
in reply to: scottmoyse

The main program would look like this:

 

%
O01001 (Top)

N10 G90 G94 G17
N11 G21
N12 G28 G91 Z0.
N13 G90

(Face1)
N14 T1 M6 ( Ally Killer )
N15 S3000 M3
N16 G54
N17 /M8
N20 G0 X149.53 Y0.
N21 G43 Z15.15 H1
N22 T6
N23 M98 P01002 (Face1)
N32 G28 G91 Z0.
N33 G90

(Face1)
N34 G55
N36 G17
N37 G0 X149.53 Y0.
N38 G43 Z15.15 H1
N39 M98 P01003 (Face1)
N48 G28 G91 Z0.
N49 G90

(Face1)
N50 G56
N52 G17
N53 G0 X149.53 Y0.
N54 G43 Z15.15 H1
N55 M98 P01004 (Face1)
N64 G28 G91 Z0.
N65 G90

(Face1)
N66 G57
N68 G17
N69 G0 X149.53 Y0.
N70 G43 Z15.15 H1
N71 M98 P01005 (Face1)
N80 M5
N81 G28 G91 Z0.
N82 G90

(Drill1)
N83 M9
N84 M1
N85 T6 M6 ( 1/4" Spot Drill )
N86 S3500 M3
N87 G54
N88 /M8
N90 G17
N91 G0 X-80. Y0.
N92 G43 Z15.15 H6
N93 T7
N94 M98 P01006 (Drill1)
N102 G28 G91 Z0.
N103 G90

Message 11 of 24
scottmoyse
in reply to: Big_Mak

Perfect thanks. so how are you getting it to post out one coordinate system per section? Manual NC?

Scott Moyse
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.


EESignature


Design & Manufacturing Technical Services Manager at Cadpro New Zealand

Co-founder of the Grumpy Sloth full aluminium billet mechanical keyboard project

Message 12 of 24
Big_Mak
in reply to: scottmoyse

Have a look at the Machine WCS section in the attached picture.

 

Check Multiple WCS Offsets and you should be good to go with a compatible post

Message 13 of 24
scottmoyse
in reply to: Big_Mak

Ah ha. Thanks. I feel silly now. I've just never done it before.

Scott Moyse
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.


EESignature


Design & Manufacturing Technical Services Manager at Cadpro New Zealand

Co-founder of the Grumpy Sloth full aluminium billet mechanical keyboard project

Message 14 of 24
Steinwerks
in reply to: scottmoyse


@scottmoyse wrote:
Ah ha. Thanks. I feel silly now. I've just never done it before.

I've used it to work in a macro to let the operator choose how many work offsets to use, which I intend to use more often (IE a couple parts and one vise on the table or many parts and two vises, etc.). The macro only requires that the program be posted with one WCS but using subs. I can send it to you if you're interested (it's for Haas but would probably work in any Macro B machine).

Neal Stein



New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
Message 15 of 24
scottmoyse
in reply to: Steinwerks

That would be great thanks. Also that's only the second time Macro B has come up in my world, all within 24 hours. I've had a bit of a look online but I'm not seeing anything that clearly explains what it is. Do you have any resources I can read about it?

Scott Moyse
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.


EESignature


Design & Manufacturing Technical Services Manager at Cadpro New Zealand

Co-founder of the Grumpy Sloth full aluminium billet mechanical keyboard project

Message 16 of 24
Steinwerks
in reply to: scottmoyse

You can do just about anything with macros of course, so there's a lot to read and understand. I've only begun to scratch the surface, and most of my interest lies with making setups faster and automating tool adjustments with Renishaw Inspection Plus (included with Haas probing), and not actually cutting with macro programs. Here's a good place to start: http://www.practicalmachinist.com/vb/cnc-machining/macro-programming-fundamentals-167395/

I'll send you an email via your website later with all the Haas specific probing and macros information I have.
Neal Stein



New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
Message 17 of 24
scottmoyse
in reply to: Steinwerks


@atomkinder67 wrote:
You can do just about anything with macros of course, so there's a lot to read and understand. I've only begun to scratch the surface, and most of my interest lies with making setups faster and automating tool adjustments with Renishaw Inspection Plus (included with Haas probing), and not actually cutting with macro programs. Here's a good place to start: http://www.practicalmachinist.com/vb/cnc-machining/macro-programming-fundamentals-167395/

I'll send you an email via your website later with all the Haas specific probing and macros information I have.

Legend! I figured Macro B was a specific standard or syntax. 


Scott Moyse
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.


EESignature


Design & Manufacturing Technical Services Manager at Cadpro New Zealand

Co-founder of the Grumpy Sloth full aluminium billet mechanical keyboard project

Message 18 of 24
dlutz1966
in reply to: Steinwerks

Hi Neil,

 

Any chance I can get a copy of your macro for work offset subs too please.

From your post:

(I've used it to work in a macro to let the operator choose how many work offsets to use, which I intend to use more often (IE a couple parts and one vise on the table or many parts and two vises, etc.). The macro only requires that the program be posted with one WCS but using subs. I can send it to you if you're interested (it's for Haas but would probably work in any Macro B machine).

 

Thanks, Dan

Message 19 of 24
Steinwerks
in reply to: dlutz1966

@dlutz1966

 

I'll have to look for it, as this was two years ago now and I didn't wind up implementing this like I thought I would.

Neal Stein



New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
Message 20 of 24
dlutz1966
in reply to: Steinwerks

Okay I would really appreciate it. Seems like it would be nice to have.
We use an old software that we create them with now and are replacing the PC and not sure I can get it to run on a new one.
Thanks, Dan

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report