x-lathe post question

[SBA]

In a converted post lathe canned rough cycles the seqence number is doubling at cycle start.

Example:

N290 T0100

N300 G0 G97 S200 M03 M42

N310 G0 Z3.245 T0101

N320 G0 X2.12 M8

N330 G50 S1600

N340 G96 S350

N680 G85 N690 U0. W0. D.2 F.01

N690 G81

If you look at line N340, the next line is N680, Double the previous line. This happens on rough turn canned cycles. At the end of the cycle after G80 the sequence number goes back to N100?

Anyone have an ides where to look for this problem.

Thanks

[Guest]

Have you tried unchecking reset sequence #'s in sub-programs in your control def, under NC output.

 

Not sure if it does canned cycles but it seems like a shot.

 

HTH

[SBA]

jmparis:

Tried that does not fix it. I only wish it was that easy but I have a feeling it is something to do with the changes from v9-v10 post. I was getting no "D" depth of cut and I finally got an answer from the Post department that resolved it and it was a post code change. I am thinking this is the same.

[DavidB]

SBA,

Im the same as you I updated my Lathe V9 posts in to X and the canned cycles have no depth of cut in them. I've been editing manualy.

What fixed this flaw in the posts to get the depth of cut outputting in the posted file?

[SBA]

DavidB:

My post is for a Okuma lathe and to fix the "D" depth of cut problem they had me change the following.

In both plinout$ and pcirout$ change the following line

if cend = 1 & rcc_flg > 0>.....

To

if (cend$ = 1 |cend$ = 3) & rcc_flg$ > 0, pbld, n$, "G80", e$

[DavidB]

SBA,

Thanks my posts where Okuma also.

Im also getting NO depth of cut on a Updated post from V9....GENERIC FANUC 2 AXIS LATHE POST WITH CANNED CYCLES.

Any ideas?

[SBA]

I am not sure but it may possibly be the same fix. I would check in the Fanuc post for the same thing change it and test.

[DavidB]

The lines you changed for the Okuma posts are not in the Fanuc post.

Anyone have an idea on on how to get the Fanuc post to out put depth of cut in a canned cycle.

 

Sorry for the Highjack SBA.

 

[Roger Martin from CNC Software]

There have been some Post Parameter Number changes from v9 -> X

 

They are documented here ->

C:mcamxdocumentationMastercamX_Post_Parameter_Ref.pdf

And look at the “V9 to X Parameter Map” section.

 

The following code segment shows the parameters used by the v9 MPLFAN.PST

code:

---

# ---------------------------------------------------------------

# Parameter information lookup tables, see pparameter

# ---------------------------------------------------------------

fprmtbl 1 5 #Rough cut parameters

10200 depthcc

10201 clearcc

10202 xstckcc

10203 zstckcc

10214 directcc

 

fprmtbl 2 4 #Finish cut parameters

10100 ncutscc

10101 depthcc

10102 xstckcc

10103 zstckcc

 

fprmtbl 3 5 #Groove cut parameters

10301 stepcc

10306 directcc

10312 dopeckcc

10316 depthcc

10320 clearcc

 

fprmtbl 104 4 #Thread cut parameters

10411 xmaj_thd

10413 zstrt_thd

10414 zend_thd

10419 face_thd

---

You need to look up the “old” numbers and replace with the “new” (X) values.

 

For example:

I see that the ‘10200’ should now be ‘13323’

and ‘10100’ (Finish cut parameters) is now ‘13341’

There are more differences than just these 2 examples! Be sure to check for new values for each Parameter Number your pre-X PST uses.