First X Post Mod's

[CNCGUY]

O.K., I'm starting to jump in.

 

First - How do I turn on debug?

 

Second - How do I get rid of spaces in the posted code. I want the () next to the numbers. I did some searching, but nothing I did was able to fix it.

code:

---

 O1000 ( T5602R00 ) 

---

Third - I need to cancel cc before the wire can cut. Rather than cancel only before wire cut, it might be easier to cancel after every op. But then I need to make it active again before the next pass.

code:

---

G40 X2.1058   ----   THIS IS GOOD

G54 X1.69 Y0.

M43

S2 D2

G42 G01 X1.68 ---- THIS IS GOOD

---

code:

---

X-.05    ----   THIS NEEDS G40

M50

G54 X1.68 Y0.

M60

S3 D3

G01 X1.64 ---- THIS NEEDS G41/G42

---

Machine - Funuc Oi10C Wire EDM.

MCAM - X MR1

Post - MPWFANUC

 

Thanks for the help!!!!

[Rick Henrickson The Boeing Co.]

the debugg is in your control def under nc output

little box enable post file debugg

[Rick Henrickson The Boeing Co.]

in the control def there is something for spaces to. I am not sure if thats what you are looking for though

[Roger Martin from CNC Software]

1> In the Control Definition on the NC Output page (upper-right) is ‘Enable post file debug information’.

 

2> You can easily eliminate all the spaces, (it is a setting on the NC Output page in the Control Definition) but I’m assuming what you really want is to eliminate certain spaces.

 

In your PST you probably have something like this ->

 

"(", *progno$, ")", e$

 

 

Change this to (no_spc$ = No spaces “here”) ->

 

"(", no_spc$, *progno$, no_spc$, ")", e$

 

3> Where (version?) did your MPWFANUC.PST come from?

 

You are moving (without wire) from contour to another contour and your Comp doesn’t get can canceled?

 

What I get from MPWFANUC.PST ->

 

N220 X0.

N230 G40 Y0.

N240 M50

N250 G0 X-2.20388 Y1.31984

N260 M60

N270 G41 G1 Y1.16882

[4xxx4]

ptoolcomment and pheader$ are where you will find the spacing problem. You can choose a different header line than what you have now if there are different styles there and you can edit for the spacing you want. After you get the bug turned on it should be fairly simple for ya.

To turn the bug on go to the drop downs at the top. "Settings", "Machine definition manager", and pick the machine you are using. Choose to edit the machine and you will get a sheet with the machine defined. Got to the top left and find the "edit control definition" icon and click it to open the active control definition.

In one of the NC output sections it will have a checkbox for debugging output - check the box and save as you exit.

Now wasn't that simple? Good luck. I'll check out my post I have here and I might have a couple things you can sneak in to get what you need.

[CNCGUY]

Roger,

 

I have checked ‘Enable post file debug information’ but I still dont get the extra info???

 

I got the spacing thing worked out. Can be somewhat cumbersome when you have several things on one line (such as the date)!!!

 

quote:

---

3> Where (version?) did your MPWFANUC.PST come from?

---

Came from the istall disk

code:

---

 [post_VERSION] #DO NOT MOVE OR ALTER THIS LINE# V10.00 E1 P3 T1130447483 M10.00 I0 

# Post Name : MPWFANUC

# Product : Wire

# Machine Name : Generic

# Control Name : Fanuc

# Description : Generic 4 Axis Wire Post

# 4-axis : Yes

# Executable : MP 10.0

---

quote:

---

You are moving (without wire) from contour to another contour and your Comp doesn’t get can canceled?

---

Yes, that is correct!!

 

CC seems to work on the first pass - start of second pass - and end of third pass.

 

code:

---

G90

M31

G00 X-.15 Y-.975 (First Pass)

S1 D1

G41 G01 X-.04

(First pass code)

G40 X2.1058

M50

 

G54 X1.69 Y0. (Second Pass)

M60

S2 D2

G42 G01 X1.68

(Second pass Code)

X-.05

M50

 

G54 X1.68 Y0. (Third Pass)

M60

S3 D3

G01 X1.64

(Third pass Code)

G01 X0. Y-.427

G40 X-.05

---

[Guest]

CNCGUY, are you selecting thread point, geometry, and cut point when chaining.i don't understand your code.why do you have s2 d2 and s3 d3 if the wire is going to a new position?one other thing,the fanuc wire will not call up comp unless you approach perpindicular when cutting a straight line unless you change the direction of comp vector in the handy para. screen under wire compensation.that got me in trouble once.

[CNCGUY]

Del,

 

quote:

---

are you selecting thread point, geometry, and cut point when chaining

---

Not selecting thread cut!!! I assume its cutting because of the Wire Parameters Cuts Page 'suppress all cuts' is un-checked!!

 

quote:

---

why do you have s2 d2 and s3 d3 if the wire is going to a new position

---

We are cutting dovetail form tools. Only certain portions of them require skim passes.

[Roger Martin from CNC Software]

For post debug output...

 

In addition to the Control Definition switch, you need to make sure that bug2 in the PST is not '0'.

 

Try this ->

 

bug2$ : 40 #Append postline labels, non-zero is column position?

 

As for your Comp issue, I'd need to see your MCX file.

[CNCGUY]

Roger,

 

I got the debug issue worked out.

 

I would love to have you look at the file (to check for wierd things I've done too) but I cant get it on the FTP.

 

Troy

[Paul Decelles]

Do a zip2go and email it to me at [email protected]. I'll have a look and pass it on to Roger if I need to. Make sure the zip2go contains the .mcx, .pst, .control and .wmd files (I really don't need the other files).

[Roger Martin from CNC Software]

Troy,

 

You don't want to have 'Max. Lead Out:' set to 0.0. Doing this you're "short-circuiting" the cancel comp.

 

There are a few ways you can handle this...

1> Don't trim the lead-out (Uncheck the 'Max lead out' option).

2> Trim it, but with a non-zero value.

The comp (G40) will get occur on this "auto-calculated" lead out move.

3> If you really want the cut to end at a specific location. Define a CUT Point and add it to the end of the chain sequence and delete the little lead-out lines that you have in the original chain and uncheck the 'Auto position cut point option' (to do this you also need to uncheck the 'Tab Cuts (no dropout method)' option)

Now your path will end at that Cut Position location with comp turning off on the move from the end of the chain to the Cut Point.