debug switches

[hellrazor]

Would someone please explain exactly what

bug2, bug3, bug4, and whatno switches do.

The book just doesn't cut it for me.

Thanks,

Jerry

[Guest CNC Apps Guy 1]

Setting bug2 to a positive value (1-80) causes the post processor to display the name of the FIRST postblock (i.e. plin, etc...) used to generate each line of NC output. The postblock is displayed at the column that you specify in the value of bug2(ex. 30 will put the values at column 30{from the left press your space key 30 times and that is where the data from bug3 and/or bug4 will be displayed})

Setting bug3 to 1 tells you what line in the post generated that line of code.

Setting bug4 to 1 tells you what NCI line generated that line of code.

------------------

James Meyette

[hellrazor]

I have the switches in the post as such:

fastmode : 0

bug2 : 30

bug3 : 0

bug4 : 1

whatno : yes

an example of the output is:

%O1361 pheader 168

What is the number 168 all about?????!?

Thanks,

Jerry

 

[Guest CNC Apps Guy 1]

168 refers to what line in the NCI file generated/had influence for that output.

 

------------------

James Meyette

Fastmode set to 0 tells the post processor you are in the debugging mode.

bug2 tells the post to output information in column 30

bug4 tells the post what to output.

[This message has been edited by James Meyette (edited 04-10-2001).]

[hellrazor]

What about the Whatno. I am lost on this one.

What can you do with the nci file? Even if you know what line it is coming from what good is it?

Jerry

 

[Simtech]

When working on a post it oftens helps to know exactly what has been programmed in Mastercam and what is held in the Intermediate NC file (NCI).

From then on, it's just a matter of Post Processing the info for formatting purposes.

Said simply: is the post wrong or did I program it wrong in Mastercam!

[Guest CNC Apps Guy 1]

Very well put Simtech. Most people don't even need to venture there, only those that are into writing/de-bugging their own posts. Last year I modified about 150-200 or so posts and I don't use all the post debugging features available. For the most part I use the settings as as follows:

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

# Debugging & Factory Set Program Switches

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

fastmode : no

bug1 : 2

bug2 : 60

bug3 : 1

bug4 : 0

whatno : yes

This for the most part tells me all I have needed to know wwhen post debugging.

------------------

James Meyette

[Ken Potter]

You guys are great! I have been beating my brains out trying to figure that out till now! Yeeee Haaaa !

Kenneth Potter

[hellrazor]

How can you tell by looking at the NCI file if you have programmed something wrong in mastercam?

Jerry

 

[Guest CNC Apps Guy 1]

Hellrazor,

That's a pretty tall order to tell you all that in here. I'd suggest you give your local Mastercam Dealer a ring and speak with them about it. There's really too much detail to cover an issue like that in here.

------------------

James Meyette

[hellrazor]

I figured I was starting to go overboard.

thanks for all the help!

Jerry

 

[Guest CNC Apps Guy 1]

Jerry,

Those are great questions. This forum isn't really a good place for details about the software like that for a few reasons, the main reason being there are sooooooo many variables that the discussion would most likely go on for months.

Never be afraid to ask questions. You're digging into the software and that's great. You'll gain valuable knowledge that way.

Before I started dealing with posts, I got the Sept. 97 Post Processor User Guide. I read it cover to cover twice before I even looked at a post. Then I started changing how tool changes are dealt with, staging tools, and it took off from there. I'm not a guru but I really enjoy doing it now. I think if I had it to do over again, I'd probably print out MPFAN, read through it a few times then read through the Post Book but hey I still have a fair grasp of what is going on in the post.

 

Have fun,

------------------

James Meyette

[Mike Freimann]

Take a look in the C:Mcam8ChooksMP.HLP file. I just worked on a post that needed stock definition. I was able to get it from the job set up. Not a big thing when you know where to look. Just search you topic sometimes you get lucky. There is a lot of useful information in there. The latest NCI format is also in there.

Mike

 

[hellrazor]

How do you output the stock definitions?

I need to do this for a BLK FRM on a heidenhain post.

I took a look at the help file and it is still over my head.

thanks,

Jerry

 

[Allan Brown]

Mpheid_i.pst out of the V8.1 box uses the Heidenhain ISO BLK FRM equivalent - G30/G31.

For the Heidenhain Klartext Conversational mode, you'd be looking at something like this:

code:

---

fmt X 1 stck_x_min

fmt Y 1 stck_y_min

fmt Z 1 stck_z_min

fmt X 1 stck_x_max

fmt Y 1 stck_y_max

fmt Z 1 stck_z_max

 

pheader # File header

"0 BEGIN PGM ", *progname, *smetric

 

stck_x_min = stck_x - stck_ht/2

stck_x_max = stck_x + stck_ht/2

stck_y_min = stck_y - stck_wdth/2

stck_y_max = stck_y + stck_wdth/2

stck_z_min = stck_z - stck_thck

stck_z_max = stck_z

 

n, ";BLK FORM 0.1 Z", *stck_x_min, *stck_y_min, *stck_z_min

n, ";BLK FORM 0.2", *stck_x_max, *stck_y_max, *stck_z_max

---

[This message has been edited by Dave Thomson (edited 04-12-2001).]

[hellrazor]

I tried it and it said "format statement 1 has not been defined" how do I go about defining it?

Thank you!

Jerry

 

[Simtech]

You should have a section like this:

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

# Format Statements - i=incr, n=nonmodal, l=leave ldg, t=leave trlg, d=delta

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

fs 1 +1^4

fs 2 +1^4n

fs 3 3 0

fs 4 2 0n

fs 5 4 1t

fs 6 2 0ln

fs 7 3 0ln

fs 8 4 n

fs 9 1.4

fs 10 1.4ln

fs 11 +1.3ln

fs 12 4 ln

the number next to the "fs" is the format statement number.

[harmonson]

i am very new to this stuff, but i have a question that you can probably answer that is probably a very dumb question.

i was looking at the code that dave posted, and it is very similiar to the toolchange/nc output variable formats that i am not quite sure about. for example:

fmt X 2 xabs #X position output

fmt Y 2 yabs #Y position output

fmt Z 2 zabs #Z position output

fmt X 3 xinc #X position output

fmt Y 3 yinc #Y position output

fmt Z 3 zinc #Z position output

what do the 2's and 3's mean? my main problem is that i would like for the post to compensate for my tool lengths, so that i do not need to do the math for every tool every time i use them. does this make any sense? thanks.

 

[Guest CNC Apps Guy 1]

Below is a snip from MP_GEN.

fs2 is stating that it's decimals are absolute and are at 3 places out.

 

fs3 is stating that it's decimals are absolute and are at 3 places out and tha number is a delta.

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

# Format statements - n=nonmodal, l=leading, t=trailing, i=inc, d=delta

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

#Default english/metric position format statements

fs2 1 0.7 0.6 #Decimal, absolute, 7 place, default for initialize (

fs2 2 0.4 0.3 #Decimal, absolute, 4/3 place

fs2 3 0.4 0.3d #Decimal, delta, 4/3 place

 

------------------

James Meyette

[lovell110]

Since everybody is interested in the posts let me give you a tip on how you can really appreciate the software you use. When you set fastmode to no ste bug2 to a negative value (-30). Then you will see every little step M/C and the post do to generate your code. Its pretty cool if you ask me!

Have a great weekend!

 

[Guest CNC Apps Guy 1]

WHOOOOOOOOOEEEEEEEEEE

Now we're talking. You'll really see some stuff now.

------------------

James M.