VelocityMach

Sequence Numbers in Canned cycles

17 posts in this topic

I have a mori seki c-axis lathe, i am using the mpmaster post. Right now i have my sequence numbers going by 10's and only at the tool changes. I'm wondering if there is a way to get the N numbers in the canned cycles to match the sequence number plus 1. so if my facing cycle is...

 

N10 T0101

 

the canned cycle would be...

 

G71 P11 Q12 U.02 W.01 F.02

 

right now i have it posting...

 

G71 P21 Q22 U.02 W.01 F.02

 

how do i get it to reand the same sequence number as the block its posting for?

 

I have been messing with this for a while, thought its about time to ask the pros.

 

Thanks for any and all help

Share this post


Link to post
Share on other sites

"whatever your variable is" = n$

Share this post


Link to post
Share on other sites

i have it working on one canned cycle. but when i post anything else with it everything goes haywire. the next block starts at 100. like this...

 

G54

N10 T0202

G18 G99

M46

G97 S164 M03

G0 X10. Z.5 M8

G50 S2400

G96 S430

X8.074

Z.1

G71 U.5 R.1

G71 P11 Q12 U.02 W.01 F.02

N11 G0 X7.744 S430

G1 Z0.

X7.7815

G3 X7.874 Z-.0462 R.0462

G1 Z-7.2516

N12 X8.074

M9

G0 G53 X0. Z-45.

M05

M01

 

(TOOL - 12 OFFSET - 12)

(4" CORE BORE)

G54

N100 T1212

G18 G99

G97 S150 M03

G0 X0. Z.25 M8

(DRILL BORE)

G83 Z-9. R-.15 F.01

G80

M9

G0 G53 X0. Z-45.

M05

M01

 

how do i get the next block to be 20? this is how my sequence numbers are setup now.

 

pheader$ #Start of file

pheader_custom

if tseqno = 1 & omitseq$ = 1,

[

seqno$ = 10

seqinc$ = 1

n$ = seqno$

]

Share this post


Link to post
Share on other sites

Under the NC output settings branch of the control def there is another rolleyes.gif place to set them up.

Though if your not outputting them on each line you will need to create a counter type thingamabob to get it.

 

What do you want the N # to match? Is it the Q# ?

Use the debugger to find the line that outputs the Q, then at the beginning of that line in the post you need to call your new counter variable (which needs to be defined before you can use it).

 

And just before you output it, you need to say (new counter variable) = (Q's variable).

 

 

Hope I'll be here to help tomorrow, just put 85" dia. 410 SS part on the machine & it's like .800 outta flat... ugggghhhhh

 

BTW, just looking at the bit you posted at the end.... seqno I would assume to be the starting value for your N#'s, seqinc I would assume to be the increment at which it increases.

Share this post


Link to post
Share on other sites

85 inch diameter?!?!? what are ya making? sounds like you got your stainless from china...

 

i am trying to get the n number to post out in increments of 10. and the canned cycles to follow in increments of 1. like the canned cycle i posted. excpet instead of n20 t1212 posting out it gave me n100 t1212. i'll keep messing with it and post any results.

 

good luck with your part, thanks for the help.

Share this post


Link to post
Share on other sites

Ok, someone did some work to your post. I don't have that seqno stuff in the stock mpfan.

If you can pin down where your N numbers are coming from (may be different for 1st toolpath in file)

Then put this in a line above it.

seqno$ = seqno$ +1

 

then directly below the output line

 

seqno$ =seqno$ -1

 

You may have to put it inside a conditional statement if that same output line is used for other situations (non-canned cycle paths).

 

if opcode$ = (canned cycle),
 [  
 seqno$ = seqno$ +1
 ]

 

 

 

same thing with the -1 after the output line.

 

if opcode$ = (canned cycle),
 [  
 seqno$ = seqno$ +1
 ]

 

 

Let me know what you run into!!! I can help you find the opcodes or whatever else you can think of that would be unique to the path (your trigger for the conditional statement) that you want the special sequence number for.

Share this post


Link to post
Share on other sites

my canned cycles are reading from this block

 

if omitseq$ = one,

[

ng70s = n$

ng70e = n$ + 1

]

 

ng70s is for the p value and ng70e is for the q value. that part seems to be working.

 

its number the other - non canned cycle toolpaths that are giving me grief. i will keep trying new things but i thought maybe that would help you understand whats going on.

Share this post


Link to post
Share on other sites

So we are on the same page, in the code above all that is happenning is the P value gets set to whatever the sequence number variable is at that point of the post processing process, and the Q value is set to the the same as the sequence # + 1. (i.e. if n$ happens to be 700, P will be 700 and Q will be 701.)

 

I would....

Try setting up a new variable for the canned cycle sequence numbers (i.e. ncan$)

Just search for and find all the formatting/initializing for the n$ variable & copy it right below but replace n$ with ncan$

Then change all the calls for n$ (only for the canned cycles) to your new variable.

 

 

But honestly.....

Something like this I would generally send to whomever did the original post mods.

You never know what kinda stuff they did and where it all is.

Share this post


Link to post
Share on other sites

i kind of wanted to avoid making any new variables. i have done something similar to what you are saying and had it working but was scared of the unknowns. your right, you never know whats all hidden in these things. especially when you start getting into live tooling posts. seems they have you jumping all over the place. if i do come up with some solution i will post it. thanks, your input def helped.

Share this post


Link to post
Share on other sites

i kind of wanted to avoid making any new variables. i have done something similar to what you are saying and had it working but was scared of the unknowns.

 

I was also scared, then I grew some ...... ball.gif

harhar.gif

 

J/K, Good luck & let me know if I can help.

1 person likes this

Share this post


Link to post
Share on other sites

Hi,

 

I have done this. I have my post outputting a block number at the start of every tool change sequence increasing by +1, then changed the sequence Numbers to start with N1000 and start to increase +1 on every can-cycle I produce then going back to the original sequence. You will need to create a new variable to accomplish this. The trick to this is create a new variable to store the current n$, that will allow you to maniplulate the n$ to what you desire, then recall the new variable to reastablish the n$ to the original value. What I used as a variable was "sav_numb". If you like more info on this just asked.

 

Jerry

Share this post


Link to post
Share on other sites

Hi Jerry

that looks like what i would like to do on a mplmaster lathe post do you have any code i could look at to complete this with the least amount of edits. this is a X6 mplmaster post running on a Fanuc control .

TIA :coffee:

Share this post


Link to post
Share on other sites

CADCAM3D5AXIS,

 

Do you omit sequance numbering, meaning you only post block numbers at the start of every tool change not on every line?

 

Jerry

Share this post


Link to post
Share on other sites

Hi CADCAM3D5AXIS,

 

 

First make sure you

 

 

post-19209-0-87082100-1336574654_thumb.gif

 

click on image to enlarge

 

 

Then start at the list at General user variables list this should be at line 482 in your post (+/- dependending if you have other modification within your post, just look for the comment line). At the end of this list add the variable you wish to use (use something that makes sense, like “sav_numb”). Now if you like to use N1000 and so on for can-cycles and keep that number increasing each time you do another roughing operation insert two variables. Remember variables are case sensitive. After I set a variable search the entire post to see if that variable is being used (use the find case sensitive). If you only find it once you are alset to continue.

 

 

#General user variables
xia         : 0     #Formated absolute value for X
yia         : 0     #Formated absolute value for Y
zia         : 0     #Formated absolute value for Z
cia         : 0     #Formated absolute value for C
“          “ “     #Formated 
“          “ “     #Formated 
“          “ “     #Formated 
“          “ “     #Formated 
rslt_plc    : 0     #Return value from plcval
rslt_upd    : 0     #Return value from updstr
sav_numb    : 0     #Used to save number sequence before can-cycle
pnumb       : 0     #Used to save can-cycle number 

 

Ok after that search the program down around line 3884 for prcc_call_end$ add the lines marked >>>

 

prcc_call_end$   #Rough canned cycle end
     # Restore cc_1013 to the value it held prior to the rough  # 1/17/03
     # groove canned cycle. cc_1013 was changed in ptoolend.    # 1/17/03
     if tool_op$ = 208 | tool_op$ = 62, cc_1013$ = sav_cc_1013     # 1/17/03

     if tool_op$ <> 208,
       [
       omitseq$ = sav_omitsq
       if omitseq$ = no$ & cc_seqno, n$ = sav_cc_st_seq     #reset start of canned cycle sequence number
       #Close the ext file
       result = fclose (sbufname3$)
       #Open the ext file as a buffer
       #Use the size to determine the start and end sequence
       subout$ = sav_subout
       size3 = rbuf(three, zero)
       if omitseq$ = one,
         [
>>>>      sav_numb = n$
>>>>      if pnumb = 0, pnumb = 1000  #This set-up the first block number of a can cycle to N1000
>>>>      n$ = pnumb
         ng70s = n$
         ng70e = n$ + 1
         ]
       else,
         [
         if old_new_sw = zero, ng70s = n$ + seqinc$
         else, ng70s = n$ + (seqinc$ * two)
         ng70e = ng70s + (seqinc$ * (size3 - one))
         ]
       pwrite_g70
       ]
     #Setup the stock and clearance directions
     g73x = vsub (lcc_xcst,lcc_xcend)
     if old_new_sw = zero, g73x = g73x * pl_ax_m0x
     else, g73x = g73x * dia_mult
     g73z = g73z * pl_ax_m0z
     xstckcc =  xstckcc * dia_mult * lccdirx
     zstckcc =  zstckcc * lccdirz * pl_ax_m0z
     clearcc =  clearcc * lccdirz * pl_ax_m0z
     #Write the cycle definition
     sav_feed = feed
     sav_ipr = ipr_actv$
     feed = sav_feedcc
     ipr_actv$ = sav_iprcc
     if lathecc = three,
       [
       #Setup the previous position for inc. in G74/G75 cycle
       sav_xa = vequ(xabs) #Save the cycle end
       copy_x = vequ(lcc_xcst) #The cycle start raw
       pshft_map_xa
       pxyzcout  ##The cycle start in machine terms
       ps_inc_calc #Recalculate incremental
       pe_inc_calc #Update previous at start
       xabs = vequ(sav_xa) #Restore the cycle end
       ps_inc_calc #Recalculate incremental
       ]
     if old_new_sw = zero,
       [
       if gcodecc < three, pg71old
       if gcodecc = three, pg73old
       if gcodecc > three, pg74old
       ]
     else,
       [
       if gcodecc < three, pg71new
       if gcodecc = three, pg73new
       if gcodecc > three, pg74new
       ]
     if lathecc = three,
       [
       #Set the cycle end position at the original start
       copy_x = vequ(lcc_xcst) #The cycle start raw
       pshft_map_xa
       pxyzcout  ##The cycle start in machine terms
       ps_inc_calc #Position at start
       pe_inc_calc #Update previous
       ps_inc_calc #Recalculate incremental
       ]
     feed = sav_feed
     ipr_actv$ = sav_ipr
     if tool_op$ <> 208,
       [
       #Bug2 is off to prevent execution crashes with long strings
       bug2$ = zero
       #Write the cycle profile, sequence are written now
       rc3 = one
       while rc3 <= size3,
         [
         sav_eob = eob$           #save out eob character as it's getting lost
         eob$ = 32                #save out eob character as it's getting lost
         prv_eob$ = 32            #save out eob character as it's getting lost   
         #Write the lathe canned cycle profile
         string3 = rbuf (three, rc3)
         if rc3 = two,
           [
           #Add the finish spindle speed to the first move
           speed = n1_ss
           #Mastercam is reporting 0 and 2 backwards for parameter 10124
           #Note that G71 type 1 and 3 are never allowed (can't change Z dir)
           if g71type = 2 | g71type = 3, pbld, *n$, *string3, *speed, e$
           if g71type = 1 | g71type = 0, pbld, *n$, *string3, *speed, "W0.", e$
           ]
         else,
           [
           if omitseq$ = one & rc3 = size3 + one, pbld, *n$, *string3, e$
           else, pbld, n$, *string3, e$
           ]
         eob$ = sav_eob          #save out eob character as it's getting lost     
         canneddone = one
         ]
       #Close the buffer
       result = fclose (three)
       #Remove the ext file
       result = remove (sbufname3$)
       bug2$ = sav_bug2
       ]
     sav_seq = n$
>>>   if omitseq$ = one,
>>>       [
>>>       pnumb =n$  + 1
>>>       if sav_numb > 0, n$ = sav_numb
>>>       ]

 

now your first can cycle number will be P1000 to Q1001 the next can cyle will be P1002 Q1003

 

 

Jerry

 

PS if you have any trouble or need more info just ask.

Share this post


Link to post
Share on other sites

Thanks Jerry when i get a chance i will update the post as above!

TIA

:thumbsup:

Share this post


Link to post
Share on other sites

Yes i only have it post at the start right now ie N1 = T0101

CADCAM3D5AXIS,

 

Do you omit sequance numbering, meaning you only post block numbers at the start of every tool change not on every line?

 

Jerry

Share this post


Link to post
Share on other sites

I took a post that didn't have a any variables for "n numbers" and I couldn't get her to go.... I could manipulate some of the numbers like start with N10 (instead of N1000) and stat with 11 and inc x 1 in the output something like that. Anyway I had to...

 

if g71type = 2 | g71type = 3, pbld, *n$, *string3, *speed, e$ if g71type = 1 | g71type = 0, pbld, *n$, *string3, *speed, "W0.", e$ ] else, [

 

if omitseq$ = one & rc3 = size3 + one, pbld, *n$, *string3, e$ else, pbld, n$, *string3, e$

 

I remove the (multiply) *n$ to-----> n$ (in these three strings)

 

And she goes.....

 

Way kuhl. :ice:

 

I really miss being a full time programmer..... :book:

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!


Register a new account

Sign in

Already have an account? Sign in here.


Sign In Now

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