Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Heidenhain 530 Post Processor

ikertx0

By ikertx0,
in Post Processor Development Forum

 Share

Recommended Posts

ikertx0 Enthusiast

ikertx0

Posted
Posted 
Hello!
I use a generic heidenhain tnc 530 post processor with various modifications made. But I found a bug.
Sometimes after an FMAX it does not show the programmed advance F.
I attach a video of the machining, and the generated file.
It can be seen in T.H that after FMAX in the second hole there is no work advance

Best Regards

 

T.H

Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
Posted
41 minutes ago, ikertx0 said: 

Hello!
I use a generic heidenhain tnc 530 post processor with various modifications made. But I found a bug.
Sometimes after an FMAX it does not show the programmed advance F.

I attach a video of the machining, and the generated file.

It can be seen in T.H that after FMAX in the second hole there is no work advance

Best Regards

 

T.H

Make a up a Z2G and someone can review. Without it not much anyone can make any sense out of just looking at a Video and code.

When you reached out to the Mastercam Dealer you Purchased the Mastercam from what was their response to the issue you found?

  • Thanks 1
Link to comment
Share on other sites
ikertx0 Enthusiast

ikertx0

Posted
  • Author
Posted (edited)
On 12/4/2021 at 8:59 AM, crazy^millman said:

Make a up a Z2G and someone can review. Without it not much anyone can make any sense out of just looking at a Video and code.

When you reached out to the Mastercam Dealer you Purchased the Mastercam from what was their response to the issue you found?

Thanks 

Attached zip2go.

I still have not gotten a response from the reseller.

It is a PST that I am doing without reseller

 

Edited by gcode
deleted zip2go per poster's request
Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
Posted
2 hours ago, ikertx0 said:

Could it be a BUG?

 

I just discovered that, if the advance speed, and the penetration advance is the same value,

 

Fxxx does not appear after FMAX, while if the values are different it is postprocessed fine.

 

Captura333.JPG

Captura111.JPG

Thank you for taking the time and effort to put together a Z2G file and sharing it.

I posted the code and do get a F2000 after the FMAX on Line 13 as I see in your posted code. In both screen shots and on most machines having the feed rate one time is good enough as the feed rate stays model throughout a program until a new feedrate is called. I changed the plunge rate to 1500 and got that in the posted code also like I think you are reffering to in the information you provided.

Note to those looking for help like this. Put up a sample of code you are getting and a sample of code like you want to see it. It helps anyone trying to help you figure out exactly what your asking help on.

Not sure what is not coming out correctly for you since everything looks correct. Very old machines did need feed rates on every line, but the machine would have to be 30+ years old since that is the last time I seen a machine requiring that output. Now if you wanting feed rate forced on every line that there is a move then you will need to change the plinout and the pcirout sections of the post and use a * before pfeed like so *pfeed. Not sure just throwing out possible suggestions. 

BEGIN PGM T_1500_PLUNGE MM
;FECHA - 04-12-21 HORA - 11:48
;HEIDENHAIN MIPRE TNC 426/530/640
;FICHERO MCAM - C:\USERS\RON\APPDATA\LOCAL\TEMP\WZ1BDA\USERS\IKER\DESKTOP\PRUEBA1.MCAM
;FICHERO NC - C:\USERS\RON\DOCUMENTS\MY MASTERCAM 2020\MASTERCAM\MILL\NC\T_1500_PLUNGE.H
BLK FORM  0.1 Z X+0.000 Y+0.000 Z+0.000
BLK FORM  0.2   X+0.000 Y+0.000 Z+0.000
* - T1 = 12 FRESA TÓRICA   |  DIAM. D+12.
TOOL CALL 1 Z S4774
L Z+50.000 R0 FMAX M03
L X+1.300 Y+0.000 R0 FMAX M9
L Z+2.000 R0 FMAX
L Z-0.500 R0 F1500 <-- Plunge Feed Rate
CC X+0.000 Y+0.000
C X-1.300 DR+ R0 F2000 <--- Feed Rate
CC X+0.000 Y+0.000
C X+1.300 DR+ R0
L Z-1.000 R0 F1500 <-- Plunge Feed Rate
CC X+0.000 Y+0.000
C X-1.300 DR+ R0 F2000 <-- Faed Rate
CC X+0.000 Y+0.000
C X+1.300 DR+ R0
L Z-1.500 R0 F1500
CC X+0.000 Y+0.000
C X-1.300 DR+ R0 F2000
CC X+0.000 Y+0.000
C X+1.300 DR+ R0
L Z-2.000 R0 F1500
CC X+0.000 Y+0.000
C X-1.300 DR+ R0 F2000
CC X+0.000 Y+0.000
C X+1.300 DR+ R0
L Z-2.500 R0 F1500
CC X+0.000 Y+0.000
C X-1.300 DR+ R0 F2000
CC X+0.000 Y+0.000
C X+1.300 DR+ R0
L Z-3.000 R0 F1500
CC X+0.000 Y+0.000
C X-1.300 DR+ R0 F2000
CC X+0.000 Y+0.000
C X+1.300 DR+ R0
L Z-3.500 R0 F1500
CC X+0.000 Y+0.000
C X-1.300 DR+ R0 F2000
CC X+0.000 Y+0.000
C X+1.300 DR+ R0
L Z-4.000 R0 F1500
CC X+0.000 Y+0.000
C X-1.300 DR+ R0 F2000
CC X+0.000 Y+0.000
C X+1.300 DR+ R0
L Z-4.500 R0 F1500
CC X+0.000 Y+0.000
C X-1.300 DR+ R0 F2000
CC X+0.000 Y+0.000
C X+1.300 DR+ R0
L Z-5.000 R0 F1500
CC X+0.000 Y+0.000
C X-1.300 DR+ R0 F2000
CC X+0.000 Y+0.000
C X+1.300 DR+ R0
L Z+25.000 R0 FMAX
L X+26.300 R0 FMAX
L Z+2.000 R0 FMAX
L Z-0.500 R0 F1500
CC X+25.000 Y+0.000
C X+23.700 DR+ R0 F2000
CC X+25.000 Y+0.000
C X+26.300 DR+ R0
L Z-1.000 R0 F1500
CC X+25.000 Y+0.000
C X+23.700 DR+ R0 F2000
CC X+25.000 Y+0.000
C X+26.300 DR+ R0
L Z-1.500 R0 F1500
CC X+25.000 Y+0.000
C X+23.700 DR+ R0 F2000
CC X+25.000 Y+0.000
C X+26.300 DR+ R0 
L Z-2.000 R0 F1500 <-- Plunge Feed Rate
CC X+25.000 Y+0.000
C X+23.700 DR+ R0 F2000 <--- Feed Rate
CC X+25.000 Y+0.000
C X+26.300 DR+ R0
L Z-2.500 R0 F1500
CC X+25.000 Y+0.000
C X+23.700 DR+ R0 F2000 <--- Feed Rate
CC X+25.000 Y+0.000
C X+26.300 DR+ R0
L Z-3.000 R0 F1500
CC X+25.000 Y+0.000
C X+23.700 DR+ R0 F2000 <--- Feed Rate
CC X+25.000 Y+0.000
C X+26.300 DR+ R0
L Z-3.500 R0 F1500
CC X+25.000 Y+0.000
C X+23.700 DR+ R0 F2000
CC X+25.000 Y+0.000
C X+26.300 DR+ R0
L Z-4.000 R0 F1500
CC X+25.000 Y+0.000
C X+23.700 DR+ R0 F2000 
CC X+25.000 Y+0.000
C X+26.300 DR+ R0
L Z-4.500 R0 F1500
CC X+25.000 Y+0.000
C X+23.700 DR+ R0 F2000
CC X+25.000 Y+0.000
C X+26.300 DR+ R0
L Z-5.000 R0 F1500
CC X+25.000 Y+0.000
C X+23.700 DR+ R0 F2000
CC X+25.000 Y+0.000
C X+26.300 DR+ R0
L Z+50.000 R0 FMAX
L M9 M40
L M01
END PGM T_1500_PLUNGE MM

To anyone who reads this and wonders why this person got help and others haven't. They put up a Zip2Go file which means they are trying to show they are a legal customer of the software. They provided information in which someone could help them. Yes their sim number will be checked to make sure that indeed they are a legal user of the software, but they put it out there like they are. Until proven otherwise I always try to help those who put forth the effort, but it comes back as a pirated seat of software then my help stops!!!!

  • Like 2
Link to comment
Share on other sites
X_IHS Rookie

X_IHS

Posted
Posted

@ikertx0

Posts do not output feedrate if it has considered it unchanged "Modal". As you know the Heidenhain uses FMAX for rapid; fanuc ect.. G00.

Fanuc simply change between G00 and G01/G02/G03 previous used feedrate applies. Heidenhain not so much. Rons example only works because the feedrate actually changes. (plunge rate different than feedrate)

In looking at the post it is already setup for modal feed,

Search for this:

modal_feed   : yes$  #Is 'F'eedrate modal? #IKER AVANCE TODAS LINEAS

Change that to this:

modal_feed   : no$  #Is 'F'eedrate modal? #IKER AVANCE TODAS LINEAS
 

The downside is a feedrate on every interpolated line; could be corrected by setting a flag to force output only after a rapid move.

 

Link to comment
Share on other sites
ikertx0 Enthusiast

ikertx0

Posted
  • Author
Posted 
@X_IHS  @crazy^millman
Hello!

I could not answer before because I think I am a new user.

First of all, thanks for responding and helping, I am licensed until version 2021 and within January I renew the maintenance.

Secondly, in heidenhain, after FMAX an FXXX must go otherwise always work in FMAX.

I was aware of the modal_feed option, but I don't like the preview showing on all lines. 

I have created a new variable, sm_fmax, set it to fedérate output, and added to all lines after smaxrate replaced by smaxrate,sm_fmax=1

 

I am doing tests and I think I have already solved it, what do you think?

 

sm_fmax   : 0

 

pfeed           # Feedrate output

      if modal_feed = no$, *feed

      else,

        [

        if fmtrnd(feed) <> prv_feed , feed, sm_fmax=0 # Has Feedrate changed?

        else, strf0 

               if sm_fmax=1, [sm_fmax=0, *feed]                       # No, just output an 'F'

        ]

Link to comment
Share on other sites
ikertx0 Enthusiast

ikertx0

Posted
  • Author
Posted
Hace 1 minuto, X_IHS dijo:

Creo que, lamentablemente, encontrará que su lógica hace poco. La velocidad de avance en lo que respecta a mastercam nunca ha cambiado. Debe marcar cuando se haya generado el smaxrate en el bloque de publicación prapidout y luego forzar la salida en pfeed.

 

  

With that option, I have managed to make it work, and that always after an FMAX the programmed F appears
  • Like 2
Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

×
 Share
Go to topic listing

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Useful Links

Contact Info

Subscribe to eMastercam News

 

Legal

Privacy Policy

Store Terms & Conditions

Forum Guidelines

Follow us

×
×
  • Create New...