quick question for the post guys

[cadmonster66]

I'm using MPA2100E post for my saber and arrow from Cincinnati yeah i knowwwwwww. Well he is sample of my output:

N70(DFS,"O1001")

N80 G91

N90 Y.265 F24.44

N100 G41 O1 Y-.265

N110 G3 X0. Y.53 I0. J.265

N120 G3 X0. Y0. I0. J-.53

N130 G3 X0. Y-.53 I0. J-.265

N140 G1 G40 Y.265

N150 Y-.265

N160 (ENS)

 

what I need is in Line 100 the O1 needs to be D1O1 .

Here are the parts of my post

______________________________________________-

# Toolchange / NC output Variable Formats

fmt O 4 tloffno #Diameter Offset Number

 

 

# Motion output components

 

pccdia #Cutter Compensation

if prv_cc_pos <> cc_pos & cc_pos & (gcode = two | gcode = three),

[

if omitseq = no,

scdc_error = scdc_error + strspace + strlp + strn + no2str(n) + strrp

result = mprint(scdc_error)

]

if prv_cc_pos <> cc_pos & cc_pos, prv_tloffno = c9k #Force Dxx#

sccomp

if cc_pos, tloffno

 

This cutter comp section has been modified from the original.I modified this section so it will give me an warning when I try to turn cutter comp on in a arc move.

The only reason why I need the post to output my Cutter Comp as D1O1(D2O2 D3O3 and so on for what ever tool number you are using) is because each machine handles the O1 offset differently and if you use D1O1 both machines will use the main offset page. The arrow you can use the main offset page to make comp changes . Mean while the saber if you go to the main offset page you can input all you want into the dia offset and it will never comp(you must go to totally different page when using O1 in the saber.

New operator scraped pretty expensive part today. Who when I asked him if he was sure in the different pages how to control the comp between the machines said helllllllll yeah ,so i left him not smart on my part

All boiled down to being my Arsh on the line today

And Johnny was not happy bout that today.

thx

John

OHHHHHHHH yeah still on V9 lololo

[Guest CNC Apps Guy 1]

Look in the fmt statements in your post...

 

code:

---

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

# Toolchange / NC output Variable Formats

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

fmt T 4 t #Tool number

fmt T 4 first_tool #First tool used

fmt T 4 next_tool #Next tool used

fmt D 4 tloffno$ #Diameter offset number

fmt H 4 tlngno #Length offset number

fmt G 4 g_wcs #WCS G address

fmt P 4 p_wcs #WCS P address

fmt S 4 speed #Spindle Speed

fmt M 4 gear #Gear range

---

Where you see tloffno change you "O" to a "D"

 

That shoudl get you where you want to be.

 

 

HTH

[cadmonster66]

Yes that will work, butttttttt say I'm using a re-sharp 3/4 endmill that's .005 undersized , the first number in the offset say "D1O1: D1 is the main tool offset which will work and say i want the O1 to be used on the outside of the part . Than I want to use same tool to do a pocket inside the part than I want the offset to be D1O2 I can change offset number when setting up the pocket with the tool info but how can i get the post to handle this

 

D1 in other words is tool offset 1 and the O1 is the offset to use on the outside and the D1O2 is use offset 2 in the pocket but still also read D1

thx

John

[3rdstring]

Does the D nuber always equal the tool number?

[cadmonster66]

Yes it does Chuck you have any ideas

John

[Guest]

If you NEED to use it that way and there is no way to change the machine so it doesn't require it, then I think you are going to have to set up a mi variable to set your cutting condition there. There is, I don't believe any way for Mastercam to determine that on it's own. So you are likely going to have to help it.

[Tim Johnson]

If you're doing this in two operations then you can manually change the offset number on the Toolpath parameters screen. As long as you don't reselect the tool the offset will stay. When I do this I will leave a note in the "Machine Group Properties" Group comment stating the operation number and that I manually made the offset change. That way six months later I don't accidently erase the offset by clicking on the tool.

[cadmonster66]

John,

I never really had to play with Mi Variables. Would you happen to know how i could go about starting to create the "D" variable

thx

John

[Guest]

I haven't tried or tested this but if I sat down to do it I'd probably start with something like this

 

in the variable definition area

code:

---

 fmt  O  2  cut_direct    #Capture cut direction from mi6$ 

---

in the tool change and null tool change sections

code:

---

sav_mi6 = mi6$

---

in your pccdia section it might look like this

code:

---

 pccdia          #Cutter Compensation

#Force Dxx#

if prv_cc_pos$ <> cc_pos$ & cc_pos$, prv_tloffno$ = c9k

sccomp

if sav_mi6 > 0,

[

cut_direct = mi6$

if cc_pos$, tloffno$, no_spc$, cut_direct

]

else,

[

if cc_pos$, tloffno$

]

---

I "think" that will work

 

Then in each section/op you would have control over "inside or outside" cutting as determined by your mi setting. I chose mi6$ as the example, you could substitute any MI or MR variable for it. Of course you would also need to define the field name definition through your control definition as well so on the MI section you have a name to see

[cadmonster66]

John,

I see you code is written for a version X post mine is for V9 will it make a big difference i how i input the code

John

[Guest]

Just drop the $ on any of the variables