code output needed

[tnevy]

I have a Partner machine that need R and Z output for each hole I spot or drill. I was wondering how to do this in the post. I use pfout for X and Y but need help with Z and R.

Thanks,

[BernieT]

Hi tnevy, welcome to the forum!!

 

You need to give more information:

 

what ver of Mastercam are you using, what should the code look like, what does the code look like now. Is it a Miltronics control and what version.

 

Also, it's Friday night, you may not get much help until Monday.

 

[tnevy]

MasterCam X4 software.

It is a Miltronics control.

The first G81 line is correct it has XYZ, R and feed rate. It's the second hole that has only an X or Y move as needed to get to the second hole. Machine only pauses then goes to the third hole location. At which point it gouged the part by literally moving to Y1.5Z-.11 and staying down and gouging to hole #4

 

G81 X-4.75 Y-1.5 Z-.1 R0.3 F10.

X4.75

Y1.5 Z-.11

X-4.75

G80

I need an R and Z at each hole even if it hasn't changed.

Thanks for any help you can offer to force output.

[BernieT]

Sorry, I don't have X4

 

 

Do a search (search is right under the 'New Poll' button above) for "forced output" and read about the various changes to the post processor.

 

You will need to add a f or * at the prout and pzout lines in the post. Hopefully someone can chime in with better information.

 

ALWAYS SAVE A COPY OF YOUR POST BEFORE MAKING CHANGES !!!!

 

hth

[tnevy]

I have the X Y and Z output at each line now, also the F rate just in case. Still having trouble getting the R value to output when the value hasn't

changed. I was able to fix the values I needed to be output in the

# Additional Holes

pdrill_2$ #Canned Drill Cycle, additional points

by adding an f or * to pxout, pyout, pzout

but it didn't help prdrlout

So I could still use some help to output an R value at each hole.

 

Thanks,

Tnevy

[bet338]

I don't know anything about Miltronics control,

but don't you need a G98 or G99 in your first line with the G81?

[John Summers]

You could add 'n' to the FMT statement for R. You may have to add another FS line and number just for the R value. Just copy the FS line that R refers to now, and give it a new number, and add the 'n'(without the quotes). 'n' means non-modal.

[tnevy]

A G98 or G99 with G81 doesn't help. I have all values now except R. Not really sure how to use John's advice but I will give it a try soon.

Thanks,

Tnevy

[Rob @ Target Machine]

quote:

---

but it didn't help prdrlout

So I could still use some help to output an R value at each hole.

---

If your prdlout postblock looks anything like this, you're in luck.

 

code:

---

prdrlout        #R drill position

if absinc$ = zero, refht_a, !refht_i

else, refht_i, !refht_a

---

Just add the force output modifier "*" to the variables that output the "R".

 

Like this:

code:

---

prdrlout        #R drill position

if absinc$ = zero, *refht_a, !refht_i

else, *refht_i, !refht_a

---

HTH

[Jim Evans from CNC Software]

You can NOT force out a postblock with a *. pxout, pyout, pzout and prdrlout are all postblocks and adding a * to them (pxout) will NOT work. You need to go into the postblocks themseleves and find the appropriate output variables and add the * to them. In our Mastercam posts there are also specific postblocks used to force XYZ which are pfxout, pfyout and pfzout so replacing pxout with pfxout would work for them but no such postblock exists for prdrlout.

 

John's suggestion would also work for the refht but you have to be careful to make sure NO other variables are formatted with the nonmodal format statement or they too will be forced out.

[tnevy]

I'll try Rob's suggestion of adding the *'s in the pdrlout #R drill position

It will be the easiest to change fix. I don't know where or how to use FMT and FS.

I'll let you all know how it works.

Thanks,

Tim Nevinger

K.D.M. Die Co.

[tnevy]

Everything is working great! Thanks for all the help everyone. And to Rob @ R & D Engineering that was a great and simple fix. It was great to see the exact place to add the *'s

Thanks again,

Tnevy

[Rob @ Target Machine]