Using mi3

[mayday]

is this possible, I havnt had to much luck yet. mostly my ignorance

 

in our standard controls this is the output for G00,G01.

 

# Motion G code selection

sg00 G00 #Rapid

sg01 G01 #Linear feed

sg02 G02 #Circular interpolation CW

sg03 G03 #Circular interpolation CCW

sg04 G04 #Dwell

sgcode #Target for string

 

fstrsel sg00 gcode sgcode

 

 

now in the high speed contorls I want to use mi3 as a toggle like this

 

Use High Speed Codes [0=No, 1=Yes] (mi3)? 0

 

if #1 is selected then this change should happen

sg00 G00G64

sg01 G01G64.1

 

I cant get the argument to work, I can hard code it but this is the only diferance between the 2 posts right now, and I would like to use just 1 post

 

any help?

Thanks

[Roger Martin from CNC Software]

MayDay,

 

Like this?

 

This is not hard-coded in the 'sgcode' string selection.

 

code:

---

 %                         

O0001

(PROGRAM NAME - SURF-ROUGH-CONTOUR-ENTRY-EXIT-ARC )

(DATE, Day-Month-Year - 10-02-04 TIME, Hr:Min - 13:59 )

N100 G20

N102 G0 G17 G40 G49 G80 G90

( 1/8 FLAT ENDMILL TOOL - 2 DIA. OFF. - 2 LEN. - 2 DIA. - .125 )

N104 T2 M6

N106 G0 G64 G90 G54 X9.75825 Y5.15887 S4278 M3

N108 G43 H2 Z3.06353

N110 G1 G64.1 Z2.71353 F6.16

N112 X6.44703

N114 G0 G64 Z2.96353

N116 Z3.06353

N118 X6.41202 Y5.25733

N120 G1 G64.1 Z2.71353

N122 X9.79326

N124 G0 G64 Z2.96353

N126 Z3.06353

N128 X9.79626 Y5.35579

N130 G1 G64.1 Z2.71353

N132 X6.40903

N134 G0 G64 Z2.96353

N136 Z3.06353

N138 Y5.45425

N140 G1 G64.1 Z2.71353

N142 X9.79626

N144 G0 G64 Z2.96353

N146 Z3.06353

N148 Y5.55272

N150 G1 G64.1 Z2.71353

N152 X8.6619

N154 X8.65585 Z2.71737

N156 X8.65525 Z2.71876

---

[mayday]

exactly Roger

 

uh, how?

[Guest CNC Apps Guy 1]

Here's how I do it,

 

code:

---

pcctrlon

if mi8 = 1, pbld, n, "G8P1", "(LOOK-AHEAD ON)", e

if mi8 = 2, pbld, n, "G5.1Q1", "(AICC ON)", e

if mi8 = 3, pbld, n, "G5P10000", "(HPCC ON)", e

prv_mi8 = mi8

!mi8

 

pcctrloff

if prv_mi8 =1, pbld, n, "G8P0", "(LOOK-AHEAD OFF)", e

if prv_mi8 =2, pbld, n, "G5.1Q0", "(AICC OFF)", e

if prv_mi8 =3, pbld, n, "G5P0", "(HPCC OFF)", e

!mi8

---

Then I have the calls in ptlchg_com (I think)program where I need the output to be. Also I initialized the post block in the general settings.

 

HTH

[mayday]

Thanks James, thats kinda where I started but then thought I could short cut it in the G code selection area, I think Ill go back to the ptlchg area with it

[Roger Martin from CNC Software]

Got to make you beg - just a little...

 

Check out the MP_EZ-HiSPeed.ZIP in the Posts folder on the forum FTP site.

[Roger Martin from CNC Software]

James may be slow at math, but he can type pretty fast.

 

MayDay,

 

How you approach this depends on when/where you need the codes to output. If you can just turn ON the mode at the toolchange and off at the end of the tool - you can go wih James' method.

BUT, If you need to turn the mode ON/OFF at each change in G0->G1 or G1->GO, that approach is not going to work for you.

[mayday]

James can be slow at math

Im prolly no faster,sure of that

and am really slow at this post stuff but what the hay, how else am I gonna learn.

 

I'll try and beg a little more Roger,THANKS

thats twice in one day you showed me a sample post to use.

 

Mayday teh get the hint

 

 

P.S.

the G84.2 works good

[Guest CNC Apps Guy 1]

I should have stipulated that the codes only need to be turned on at a tool change and off at the end of a cycle. If it needs to be on and off according to what G code is active, then Roger's method is the way to go.

[crazy^millman]

Roger I like that highspeed setup looks real good. I can see other applications for that.