Sharnoa Tiger 3-4 Upgrade
An-107, Copyright © by Gil Hagiz
Last updated Mar-20-2007
Important
Numeryx is not affiliated with Sharnoa in any way.
NCPlus cannot run on R-741 computer. An upgrade requires a new control.
For service and tapes for Tiger 3 and 4 try these non-affiliated vendors:
http://www.cnc-machine-controls.com/Sharnoa/
http://www.atkinsontechnologies.com/
General
If you are familiar with the Sharnoa's Tiger 3-4 programming, here is a summary of the major changes.
Most G and M codes now follow the RS-274D standard.
There are many new G-codes and commands in English that are not described here.
For more info check the programming manual.
Format
- Mixed upper and lower case letters can be used.
- The % sign is not used at the beginning of a program.
- Incremental input is denoted by + instead of /. Use x+1 instead of x/1 (also g91 can be used).
- Block numbers are not checked for order and can be omitted.
- Block numbers are used for jumps and loops.
- Block number range is up to 9,999,999.
- Comments are preceded by backslash (\)
or
Open parenthesis at the beginning of a line (for that line only).
- Data format is not limited to 4.3 or 3.4. True floating point is used.
- F negative and F/ are not recognized.
- M-codes above M99 are not recognized.
- Axis-names for the 4th and 5th axes are selected in the INI file (instead of A and @).
G-code replacement
Note: Home is same as Fixture Offset. Local Coordinate is same as Floating Zero, which is added to current home.
- Old G8 is replaced by G14.
- Old G9 is replaced by G15.
- Old G92 X_Y_Z_ is replaced by G+52 X_Y_Z_(local coordinates, relative to current local coordinates).
- G52 X_Y_Z_sets the local coordinates relative to current Home.
- Old G92 alone is replaced by G52 X+ Y+ Z+ ... (set current position as zero).
- Old G99 alone is replaced by G52 alone (to cancel zero shift).
- Old G99 O_ is replaced by g54 to g59.3.
Data is not taken from the tool table but is set on the machine or entered into an offset table.
- Old G93 is replaced by G53, but it is the machine zero and not necessarily the reference.
- Old G98 is replaced by the word Scale.
- G92 works according to standard (setting current position to the programmed XYZ).
- Inch/metric is done by g70/g71 or the words mm – inch (instead of M170/M171).
- Drilling canned cycles follow the standard.
- Old M199 is replaced by G64, which is the default (canceled by G61).
Geometry/Motion
Arithmetic
- Arithmetic works according to the conventional rules, not from left to right.
#1=2+3*4 \the result is 14
#1=(2+3)*4 \the result is 20
All parameters are entered as #xx. Parameter number between parentheses is not recognized.
(2)1234 is replaced by #2=1234.
Math doesn't need G4 (in fact G4 is hardly needed at all). It can be mixed with NC data on the same line.
The highest parameter is #99 but that limit can be increased (up to a maximum of about 8000) by programming M101 in the beginning of a program.
Chain assignment is allowed: 123=9+5=8=7 is replaced by: #7=#8=5+(#9=123).
JMP is replaced by goto: #1==2JMP1000 is replaced by: if #1==2 then goto 1000 end
Number accuracy is 15 digit floating point.
Nesting for parenthesis and loops is about 30-level deep.
Colon is optional, space is used as a separator between 2 statements.
Loops can repeat trillions of times.
The function FRC(x) is replaced by Gil(x0,x1), which returns a number between x0 to x1 proportional to the number of repetition in the loop.
Gil(x0,x1) is same as x0+FRC(x1-x0)
Loops and jumps
|
TIGER |
NCPLUS |
Alternative |
G70 L1000 |
Goto 1000 |
G71 L1000
. . . .
N1000 <operation>
<operation>
G72 |
Gosub 1000
. . . .
n1000<operation>
<operation>
Return |
G71 L1000 E10
. . . .
N1000 <operation>
<operation>
G72
|
For #1=1 to 10
Gosub 1000
Next #1
. . . .
n1000 <operation>
<operation>
Return |
(version 6 and later)
Gosub 1000,10
. . . .
n1000 <operation>
<operation>
Return |
G51 E10
<operation>
G52 |
For #1=1 to 10
<operation>
Next #1 |
N10 . . . .
<operation>
G71 L10 E9 |
For #1=1 to 10
<operation>
Next #1 |
#1=0 repeat
<operation>
until (#1+=1)>9 |
Must change
Before anything else, here are a few changes that are required for all programs.
Remove % at the beginning.
Cancel M199.
Replace / by +
Replace C by P
Search for G5 and replace any g51 and g52 by the new FOR - NEXT commands.
Replace G92 by G52/G+52
Replace G99 by G52
Search for G12 and G13 and add P+ if there is no P (Full circle).
Search for G7 and replace any g70/g71/g72 with the new commands.
Search for G18/G19; if used change the direction of rotation.
Check other G and M codes that are listed above.
If tool radius comp is used, search for E; make changes according to chapter 3.