FEEDRATE F0.

[mayday]

Running with inverse time and I get random F0. Program is 260,000 lines long so no hand edits

 

got an idea why it does it?

[gcode]

are the preceeding and following feedrates F999.

 

If so, change the format from F999 to F9999

 

 

 

I've seen some gen5X posts with a default qusetion

If feedrate = 0 then output ( your value here )

[gcode]

from the X5 gen5x post

 

 

 

fix_fr : 1 #If feedrate is zero, apply these values

deffeedpm : 1. #Default for zero feed in inch/min

deffeedpm_m : 25. #Default for zero feed in mm/min

deffrinv : 500. #Default for zero feed inverse time

 

 

 

If you set fix_fr 0 nothing is done

set to 1 the following values are applied..

[mayday]

MPMaster dosnt have that. I looked at the generic x5 and see it, think I can copy it into the MP pst?

[gcode]

I doubt it.. the meat of it is probably buried in the binary where you can't get at it

 

 

try setting it to output 4 digits on the Feed Rate axis motion page of the machine def

 

It defaults to 1000.... try changing it to 9999

[Colin Gilchrist]

MPMaster dosnt have that. I looked at the generic x5 and see it, think I can copy it into the MP pst?

 

That would be a big no Wes. Those are just variable initializations and a switch variable. Just adding that portion will not actually do anything inside MPMaster.

[Chris McIntosh]

What's the tool path you are running? Chances are the calculated line length is zero, so when doing the math things break. Are you getting an error when posting out saying dividing by zero or not?

[mayday]

Morgh between to curves on an airfoil that has leading and trailing edges with about a .005 radius. very small moves when rolling. Normally do these on an Integrax but offloading to a Mazak matrix 4 axis

[Chris McIntosh]

if you shoot me a z2g I can look at the issue, but really going to be post/mcx specific.

[gcode]

I used to have this problem with an SNK 5X gantry .

 

The post was a gen5X post not mpmaster, but changing minimum output from F999. to F9999. solved the problem

[mayday]

Z2G is to big for email. I'll try what TTom said. It doea appear it happens on very small moves around the edges

 

Y-.5057 Z.3168 A311.338 F10000.

Y-.51 Z.3098 A310.548 F10000.

Y-.514 Z.303 A309.79 F10000.

Y-.5153 Z.3008 A309.542 F0.

Y-.5201 Z.2924 A308.608 F10000.

Y-.5248 Z.2839 A307.675 F10000.

Y-.5291 Z.2755 A306.768 F10000.

 

I just do a global replace with F10000.

[Chris McIntosh]

This is a bit of a cheat, but you can always just output the 10000 if the calculated feed is 0.

 

In pfclc_deg_inv:

 

       if cuttype = three, cldelta = sqrt((x$-prv_x$)^2+(y$-prv_y$)^2+(z$-prv_z$)^2)
       if inversefeed$ = 0, frinv = fr_pos$/cldelta  # 1/min
       else, frinv = fr_pos$/(60*cldelta)  # 1/sec
       if frinv = 0, frinv = 10000 <-- ADD THIS LINE
       if rot_feed & opcode$ <> 3 & opcode$ <> 16,
         [
         if frinv > maxfrinv, frinv = maxfrinv
         if frinv < minfrinv, frinv = minfrinv
         feed = frinv
         ]

[mayday]

cheating has always worked for me

thanks

[Rstewart]

Know this is an old thread, but I could really Use some help!

 

I'm Using a Mpmaster Post and when In G93 (Inverse) I'm not Getting a F. call at All on some lines! So this alarms the machine beacause G93 isn't modal on Haas anyways...

 

I applied the^^^ "cheat" in my post, But it doesn't see this Like the F0. problem. Any Ideas???

[Rstewart]

Figured it out! Gotta switch to a smaller tool or increase the size or your geo...