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:

Force feed in G70


Recommended Posts

Hey everyone,

I'm fairly new to post editing, and am trying to edit my Generic Hass ST 4X lathe post so it will force a feed rate to post on my G70 canned cycle line. 

The issue I'm having is many time my student  use a roughing and finishing canned cycle to turn there part, then single point there thread, and like to come back over the thread to take off any burs that may have come up. Well when we post just the Finish canned cycle (G70) after the thread,  it doesn't post a feed after the P100 Q110 lines, leaving the tool to feed at the last feed rate, which in this case is a treading reed(F.050 IPR). 

So all need to do is force the G70 to post a feed after the PQ for the tool its using. I can get the post to output a feed but it's using the feed from the roughing cycle, not the finishing cycle. 

Any help would be appreciated.

Link to comment
Share on other sites

Thanks for the reply.

I'm aware that an * will force the output. And I've tried that. But for some reason unless the finishing is directly following the roughing cycle it doesn't post out the feed. Or when I do add the *. It post out the feed rate for the rough tool and not the finish. This is the issue I'm having.

Link to comment
Share on other sites
1 hour ago, Wayne Schwarze said:

Any help would be appreciated.

As So not a Guru said Lathes are a bit different. Not my forte either...

There is a pffr post block which forces feed output, and I can see that in the g71-73 output post blocks.

However you are trying to set the feed rate in what is essentially the subroutine call line 

N4 G71 P5 Q12 U-0.01 W0.005 D0.08 F0.01
N5 G00 X4.5
N6 G01 X3. R.25 F.005
N7 Z-1.75 R.5
N8 X1.5 R.125
N9 Z-2.25 R.125
N10 X.75 R.125
N11 Z-3.
N12 X0.73
N13 G70 P5 Q12

N13 in the above code

I found this in the  

pread_g70 postblock:

 

pbld, n$, *scclgcode, *ng70s, *ng70e, e$

You could try

pbld, n$, *scclgcode, *ng70s, *ng70e, pffr, e$

but that will only output  the current modal feed rate. So you might need to save the finish feed as a user defined variable and call it here. 

Running a trace in the debugger should show you what's happening more clearly.

Link to comment
Share on other sites
4 hours ago, nickbe10 said:

As So not a Guru said Lathes are a bit different. Not my forte either...

There is a pffr post block which forces feed output, and I can see that in the g71-73 output post blocks.

However you are trying to set the feed rate in what is essentially the subroutine call line 


N4 G71 P5 Q12 U-0.01 W0.005 D0.08 F0.01
N5 G00 X4.5
N6 G01 X3. R.25 F.005
N7 Z-1.75 R.5
N8 X1.5 R.125
N9 Z-2.25 R.125
N10 X.75 R.125
N11 Z-3.
N12 X0.73
N13 G70 P5 Q12

N13 in the above code

I found this in the  


pread_g70 postblock:

 


pbld, n$, *scclgcode, *ng70s, *ng70e, e$

You could try


pbld, n$, *scclgcode, *ng70s, *ng70e, pffr, e$

but that will only output  the current modal feed rate. So you might need to save the finish feed as a user defined variable and call it here. 

Running a trace in the debugger should show you what's happening more clearly.

Thanks for the help, but this is exactly what I've already tries and where I'm stuck. I add the pffr to the line and try and trace the debug. I add a breakpoint to the line before the g71 and the g70 to see what's going on but the post is using strings and buffers for the g71 and doesn't show a whole lot when it comes to tracing. I seems like I need to add some buffers parameters before the G70 lines to get the pffr to post the correct callout. but for the life of me I cant seem to find the correct combination to make it do it. the butter parameters look something like this.

sav_feed = feed
      sav_ipr = ipr_actv$
      feed = sav_feedcc
      ipr_actv$ = sav_iprcc
I believe this will force it to pickup the ifr_l feed output. 
Link to comment
Share on other sites
1 minute ago, Wayne Schwarze said:

Thanks for the help, but this is exactly what I've already tries and where I'm stuck

Try posting the feed rate on it's own line:

pbld, n$, *scclgcode, *ng70s, *ng70e, e$
pbld, n$, pffr, e$

The buffer is handling the gcode and the start and finish line numbers. Looks like there are some flags set up to determine the "canned turning cycle type".

Find lathecc to see list of flags.

Link to comment
Share on other sites
Thanks for all the help, after a lot of trial and error, I finally figured it out.
I ended up having to add the orange lines to the G70 routine. 
else, if lcc_compok = zero, # Profile comp on only output flag is enabled
            ]
			
	sav_iprcc = c1_ipr_actv 
        sav_feedcc = c1_fr_pos 
        feed = sav_feedcc 
        ipr_actv$ = sav_iprcc 
		   
          pbld, n$, *scclgcode, *ng70s, *ng70e,pffr, e$ 
          foundcc = one
          lfc_in_sub = one

Now it post out the G70 feed no matter where the canned cycle is in the program. 

G18
/M8
G97 S1267 M3
G00 G54 Z0.
X1.6585
G50 S4800
G96 S550
G01 X-.0712 F.005
G00 Z.1
X2.2
Z.2
G70 P100 Q110 F.006
G00 Z.2
M9
M5
G53 X0.
G53 Z0.
M30
  • Like 3
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

  • 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.

Follow us

×
×
  • Create New...