erhtetheht

1. ==========================================================
W i n C A M 2.23
==========================================================
N e w F u n c t i o n s i n W i n C A M 2.23
1.) NC Program Init
The Tool command in for init blocks can optionally be extended in
a way tha a second parameter specifies the first axis that will
move to the tool change position.
I.e InitBlock6 = Tool(2,Z). Moves first the Z and the X axis to the
tool change position and then changes the tool to tool number 2.
The command can also be applied to milling machines. Then the
specified axis is moved by the first nc block and the other 2 axis
will be moved by the next nc block to the tool change position.
N e w F u n c t i o n s i n W i n C A M 2.22
1.) NC Program Init
2.) Cut Off Cycle
3.) Sample lines for new wincam.ini sections
4.) S=0 problem NUM T Controls
5.) Program number is selectable for RS232 NC Program Export
3 new functions have been included within WinCAM 2.22. All of
them must be activated and parameterized in the wincam.ini file.
1.) NC Program Init
===================
In the [ProgramInit] section of wincam.ini several initialisation
tasks can be automated. If one of the function should be activated,
the Activate=1 key must be set.
The specified initialisation tasks are executed for each
new nc program i.e. on startup, with the Program-New menue or the
CAM NC Program-New Menue command.
1.1 Tool Holder Setup
----------------------
For each tool holder slot a tool number can be specified. This number
selects a tool from the tool library just as with the manual dialog.
The tool number must be a valid tool in the library.
Example:ToolHolderPosition3=12 selects tool 12 of the tool library
to slot 3 (T3) of the tool holder.
1.2 Init Blocks in the nc program.
----------------------------------
An arbitrary number of NC Blocks can be specified for initialisation.
First the number N of blocks must be specified with InitBlocks=N.
Each block can contain one command. The commands are not specified
by nc commands but by a generalized form, so that there is no dependency
of the used program format (Sinumerik, Fanuc..).
The format is "InitBlockN=Command" with N is the number of the inserted block.
Following commands can be used (Examples for ISO/DIN format):
SpindleRight .. Turn Spindle on left (M3)

2. SpindleLeft .. Turn Spindle on left (M4)
SpindleOff .. Turn Spindle on left (M5)
Speed(s) .. Sets the speed value an the matching G-code with the speed
s in [RPM]. (i.e. Speed(2000) gener. the nc line "G97 S2000")
Feed(f) .. Sets the feed value and matching G-code with feed f in
[mm/min] if metric mode is used or [inch/min] for Inch-Mode.
i.e. Feed(500) generates "G94 F500"
FeedRev(fr) *) .. Sets the feed per revolution value and matching G-Code with
feed fr in [mm/U] if metric mode is used or [inch/rev] for
Inch-Mode.
i.e. Feed(0.5) generates "G95 F0.5"
ConstCutSpeed(v).. Sets the speed value and the matching G-code for contant
*) cutting speed v in [m/min] metric or (feet/min] in Inch mode.
i.e. ConstCutSpeed(80) generates "G96 S80"
Tool(N) .. Selects tool number N. The toolholder slot N should be
occupied by a tool (see 1.1 Tool Holder Setup).
Befor the tool is changed the tool turret is moved to the
obigatory tool change position (see 1.3)
i.e. Tool(3) selects Tool number 3
MoveX(x) .. Moves to position x with G0. The X-Value is relative to the
CAM reference point as an absolute value, dor turning
machines
it is a diameter value.
i.e. MoveX(40) moves the X position to diameter 40 by
generating "G0 X40" for a turning machine or "G0 X40" for
a milling machine.
MoveOffsetX(x) .. Moves tool relative to the raw part diameter. The value
within
the brackets is interpreted as a RADIUS value!
i.e. MoveOffsetX(10.0) moves the X position of the
initial tool to the total diameter:raw part diameter plus 20.
MoveY(y) .. Moves to position y with G0. The Y-Value is relative to the
CAM reference point.
i.e. MoveY(20) moves y position to 20 by generating "G0 Y20"
MoveZ(z) .. Moves to position z with G0. The Z-Value is relative to the
CAM reference point.
i.e. MoveZ(20) moves z position to 20 by generating "G0 Y20".
*) For Sinumerik and ISO/DIN program format, you must take care of the order if
constant cutting speed is used:
First the feed command must be specified and then
the constant cutting speed command.
If you change the order so that the last command is a feed value i.e.
FeedRef(0.5) which produces the nc line "G95 F0.5" then G95 switches
off G96 (const cutting speed mode).
1.3 Tool Change Position
------------------------
If an init block contains Tool(N) then the tool moves to the tool change
position before the tool is changed. For a turning machine x is moved first,
then z, for a milling machine z is moved first, then x and y.
For turning machines x values are diameter values.
All target positions are concernd as position without tooloffsets so the
toolholder will always move to the same position for each selected tool.
Format:
ToolChangePositionX=x
ToolChangePositionY=y
ToolChangePositionZ=z
i.e (ToolChangePositionZ=150.0 moves to z150 before the tool is changed).
Values x,y, and z are used the same way as used in the MoveX/Y/Z()
Commands but without tooloffsets (see 1.2).

3. 2.) Cut Off Cycle
=================
For a simple cut off a new cut off cycle can be used. The Cycle parameters must
be defined in the wincam.ini section [CutOff].
If the key Achtivate=1 is set to 1 a new cut off button is
visible in the CAM toolbar. With Activate=0 the button is not visible, which is
the default mode.
For the cut off cycle only the button must be pressed then the desired
z value must be applied (with mouse click or numeric input).
Then the cut off cycle is done by first moving to the tool change position,
then chaninging the to the desired cut off tool followed by the cut off at the
desired z-position.
The following Parameters must be set in the CutOff section of wincam.ini:
Tool=N .. Tool number with the Cut Off Tool. Usually the tool holder
should be set up with the tool holder setup function (1.1)
of the [ProgramInit] section.
ToolChangePositionX=x
ToolChangePositionZ=z
.. Position where the Cut Off tool is changed, description
(see 1.3).
CutDepth=d .. Absolute X depth for each cut step. After the cut step,
the tool is returned a defined value in [mm] or [inch].
(i.e Cutdepth=1.5 cut 1.5 mm for each step).
ReturnLength=l .. Absolute X value for return motion (+X) after a cut.
Delay=t .. Delay time at the lowest X position when the Cut Off cycle
is done.
Feed=Feed(f) .. Defines the cut cycle's feed value either in [mm/min],
[inch/min] or in
=FeedRev(fr)..[mm/rev], [inch/rev] (see 1.2).
Speed=Speed(f) .. Defines the cut cycle's speed value either in [U/min] or the
=ConstCutSpeed(v).. constant cutting speed in [m/min] or [feed/min]
see 1.2).
EndValueX=xe .. Specifies the X end position (diameter) for the cut off
cycle, usually a small negative x-value.
StartOffsetX=xs .. Specifies the start value relative to the raw part radius.
i.e StartOffsetX=2.0) moves x to diameter 34 if the raw part
diameter is 30mm.
3.) Sample lines for new wincam.ini sections
============================================
[ProgramInit]
Activate=1
ToolHolderPosition1=1
ToolHolderPosition2=3
ToolHolderPosition3=2
ToolHolderPosition4=4
ToolHolderPosition5=7
ToolChangePositionX=70
ToolChangePositionZ=15
InitBlocks=6
InitBlock1=SpindleLeft
InitBlock2=Speed(2000)
InitBlock3=Feed(300)
InitBlock4=Tool(2)
InitBlock5=MoveX(60)
InitBlock6=MoveZ(5)
[CutOff]
Activate=1
Tool=5

4. ToolChangePositionX=70
ToolChangePositionZ=20
CutDepth=2.0
ReturnLength=0.5
Delay=1.0
Feed=Feed(600)
Speed=Speed(2000)
StartOffsetX=2.0
EndValueX=-1.0
4.) S=0 problem NUM T Controls
==============================
For NUM T Controls it's not allowed to Program S0 with G96/G97
or F0 with G94/G95.
In the NC program a a low limit of F1/S1 is now applied for NUM T controls.
Further a init speed value can be specified in the [CAM] section
of wincam.ini to allow a default value for S in new NC programs.
i.e. InitSpeedNUMT = 1000.
If the key is not specified G97 S1 will be generated.
NUM1040 Turn:
If you add in the [CAM] Section the item 'NUM1040=1' nc code for the
NUM1040T will be generated. You can add this item by the help of 'WinConfig'
too.
(See INI-Button: Main menu/Common parameters)
5.) Program number is selectable for RS232 NC Program Export
============================================================
In the NC program export dialog now a program number can be
selected for the main program. So different wincam projects
can be hold on the original nc controls with different numbers.