X4 drilling post errors - Verisurf

[mwc815]

Hi,

 

I'm running X4, and updated my post using the

method in the sticky post.I also installed

Verisurf Hole Axis for X4 build date 5-1-09. Now

every time I post out a drill cycle operation, I

get a window titled verisurf with a yes/no

option, that generatesan error log. The nc code

is good, it's just annoying. (I haven't had to

use the hole axis function yet.)

 

 

23 Jun 2009 08:15:14 AM - <0> - Report created.

23 Jun 2009 08:15:14 AM - <2> - Initialize posting log file

23 Jun 2009 08:15:14 AM - <2> - Using MP run version 13.00 and post components version 10.00

23 Jun 2009 08:15:14 AM - <2> - Initiate opening the post processor file(s).

23 Jun 2009 08:15:14 AM - <2> - Post processor file name: C:MCAMX4MILLPOSTSMPHAAS-VF-4.PST

23 Jun 2009 08:15:14 AM - <2> - The post processor file has been successfully opened.

23 Jun 2009 08:15:14 AM - <2> - Post version information (input):

23 Jun 2009 08:15:14 AM - <2> - UPDATEPOST Version 13. was used to modify this file.

23 Jun 2009 08:15:14 AM - <2> - The file was modified by this product on 09 Jun 09 12:40:52

23 Jun 2009 08:15:14 AM - <2> - The post was written to run with Mastercam Version 13.

23 Jun 2009 08:15:14 AM - <2> - The post product type is Mill.

23 Jun 2009 08:15:14 AM - <2> - Initialization of pre-defined post variables, strings, postblocks was successful.

23 Jun 2009 08:15:14 AM - <2> - Search for defined post variables, strings, postblocks was successful.

23 Jun 2009 08:15:14 AM - <2> - CONTROL DEFINITION - - Post variable 'met_ltol$' was re-initialized from 0.002 to 0.01

23 Jun 2009 08:15:14 AM - <2> - CONTROL DEFINITION - - Post variable 'atol$' was re-initialized from 0.5 to 0.01

23 Jun 2009 08:15:14 AM - <2> - CONTROL DEFINITION - - Post variable 'dec_seq_right$' was re-initialized from 3. to 0.

23 Jun 2009 08:15:14 AM - <2> - CONTROL DEFINITION - - Post variable 'fastmode$' was re-initialized from 0. to 1.

23 Jun 2009 08:15:14 AM - <2> - CONTROL DEFINITION - - Post variable 'arccheck$' was re-initialized from 1. to 111.

23 Jun 2009 08:15:14 AM - <2> - CONTROL DEFINITION - - Post variable 'larccheck$' was re-initialized from 1. to 111.

23 Jun 2009 08:15:14 AM - <2> - CONTROL DEFINITION - - Post variable 'rotfeed4$' was re-initialized from 2. to 1.

23 Jun 2009 08:15:14 AM - <2> - CONTROL DEFINITION - - Post variable 'rotfeed5$' was re-initialized from 3. to 1.

23 Jun 2009 08:15:14 AM - <2> - CONTROL DEFINITION - - Post variable 'lrotfeed4$' was re-initialized from 2. to 1.

23 Jun 2009 08:15:14 AM - <2> - CONTROL DEFINITION - - Post variable 'lrotfeed5$' was re-initialized from 0. to 1.

23 Jun 2009 08:15:14 AM - <2> - CONTROL DEFINITION - - Post variable 'sub_level$' was re-initialized from 0. to 0.

23 Jun 2009 08:15:14 AM - <2> - CONTROL DEFINITION - - Post variable 'peckacel$' was re-initialized from 0. to 1.

23 Jun 2009 08:15:14 AM - <2> - RUN TIME - PST(850), NCI(102) - The math calculation/formula has an error

23 Jun 2009 08:15:14 AM - <2> - RUN TIME - PST(850), NCI(104) - The math calculation/formula has an error

23 Jun 2009 08:15:14 AM - <2> - Successful completion of posting process!

 

 

any ideas?

 

Mike

[mwc815]

I uninstalled verisurf, and now the error dialog box says mastercam.

 

Mike

[Jim Evans from CNC Software]

According to the error log you have a problem with line 850 in the post.

 

code:

---

23 Jun 2009 08:15:14 AM - <2> - RUN TIME - PST(850), NCI(102) - The math calculation/formula has an error

23 Jun 2009 08:15:14 AM - <2> - RUN TIME - PST(850), NCI(104) - The math calculation/formula has an error

---

Updatepost would have encountered the same problem and documented the problem in the Updat LOG file as well as inside the post with some comments below the problem line. You can always copy the code (lines 840-860) from the post and post them here and maybe we can figure it out without the post. Please use the code tag (from the full reply form - don't forget to preview your post before submiting it - this makes the code more readable) when pasting in your post code

[mwc815]

Jim,

 

Here is the section with the error.

 

code:

---

pdrill0$ #Drill, motion test

gcode$ = zero

znci$ = initht$ * x_mult

 

pdrlcommonb #Canned Drill Cycle common call, before

if cstart$ = one, cflag = one

if drillcyc$ = 3, drlgsel = fsg1 (-ss1) + drillcyc$ * 2

else, drlgsel = fsg2 (dwell$) + drillcyc$ * 2

if initht$ <> refht$, drillref = 0

else, drillref = 1

z$ = depth$ * z_mult

if absinc$ = one, prv_zia = refht$ * z_mult

feed ?

#CNC<<ORIGINAL>> feed = pfr$

#CNC<<MSG-ERROR[856]>> The formula/boolean does not terminate properly, Label has not been defined[*38]

prv_dwell$ = zero

@dwell$

pcom_moveb

if drillcyc$ = 3 & use_rigid = 1, result = newfs(12, feed)

else, result = newfs(9, feed)

---

Thanks, Mike

[Jim Evans from CNC Software]

I'm betting the problem is that pfr$ is not valid. The $ indicates that this is a MP predefined variable but pfr$ is NOT a predefined variable. pfr was used as a user defined postblock name in our lathe posts, I don't remember it being in any of our Mill posts but it could have been.

 

Anyway, it looks like someone was trying to set the value of feed to what ever they thought was in pfr. If your code is correct, then just comment out the feed ? line like so.

 

code:

---

 #feed ? 

---

Our Mill post sets feed = to fr_pos$ which is the variable for positive feedrate so you could always do that as shown below. This should NOT cause a problem with your code either.

 

code:

---

      pcom_moveb

feed = fr_pos$

comment$

 

---

If you want to really figure out what someone was trying to do, search your post for pfr and see if it shows up anywhere else and you can always post the code here for some help.

[mwc815]

Jim,

I replaced #feed ? with #feed pffr$ and had the

same result. Replacing it with fr_pos$ worked.

 

Thanks again, Mike