MASSO Post Processor Help

[FabLab]

I have been working on a post for a Masso Ver5 G3 controller with a DHTC and air Scribe.
I have almost everything setup the way I would like it, Basically there are 2 things I would like to change and I cant figure out how to do it.

First:
The PP I started with has the following code:
--The cutter will slow down for corners and turn off THC below this radius
slowRadius = 10

--Minimum slow down speed.
--This is a scale factor. For instance 0.5 = 50% of the current feed rate
slowPercent = 0.4

I would like to remove that & just use SC rules but I am not sure how to do it, any help would be appreciated!!

Second:
The G-Code output for scribing looks good, I don't see any issues but the Plasma operation G-Code output has one annoyance that I cant figure out, Here is an example of the output:

N0960 T112 M06
N0970 G92.1
N0980 G200 F20 P0.12 D400 C0.08 V92 A0 O0 S0
N0990 G00 X1.5857 Y3.7500
N1000 X2.6887 Y2.5756
N1010 M03 (---45 amp .090 aluminum---)
N1020 G01 F100.0 <----- Why is it doing this?
N1030 F120.0 <----- Why is it doing this?
N1040 G03 Y2.6887 I-0.0566 J0.0566 F48.0
N1050 M667 F50.0 (---THC on---)
N1060 X2.0000 Y2.9740 I-0.6887 J-0.6887 F120.0
N1070 X1.0260 Y2.0000 I0.0000 J-0.9740
N1080 X2.0000 Y1.0260 I0.9740 J-0.0000
N1090 X2.9740 Y2.0000 I0.0000 J0.9740
N1100 X2.6887 Y2.6887 I-0.9740 J0.0000
N1110 M666 (---THC off---)

I understand it doesn't really hurt anything but it is annoying & I would like to understand why its doing that..
Again any help here would be appreciated!!

Thanks!

Jeff

[FabLab]

So, I figured out where the 2 different feed rates are coming from, but I cant figure out how to fix it.

N0960 T112 M06
N0970 G92.1
N0980 G200 F20 P0.12 D400 C0.08 V92 A0 O0 S0
N0990 G00 X1.5857 Y3.7500
N1000 X2.6887 Y2.5756
N1010 M03 (---45 amp .090 aluminum---)
N1020 G01 F100.0 <----- This is from the Plunge rate dialog within SheetCam
N1030 F120.0 <----- This is from the Feed rate dialog within SheetCam
N1040 G03 Y2.6887 I-0.0566 J0.0566 F48.0
N1050 M667 F50.0 (---THC on---)
N1060 X2.0000 Y2.9740 I-0.6887 J-0.6887 F120.0
N1070 X1.0260 Y2.0000 I0.0000 J-0.9740
N1080 X2.0000 Y1.0260 I0.9740 J-0.0000
N1090 X2.9740 Y2.0000 I0.0000 J0.9740
N1100 X2.6887 Y2.6887 I-0.9740 J0.0000
N1110 M666 (---THC off---)

Line N1020 should not be there (or at least I don't want it there ) the plunge rate should be set by the G200 F Value (line N0980) and the feed rate, well that should be the feedrate

I probably should have explained MASSO's G200 code in my first post:
This command defines the parameters for Plasma.

It can be placed at the start of the Gcode file and will populate the Plasma parameters shown on the Plasma Tab in the F2 screen

Syntax & Parameters

G200 uses the values to populate the Plasma parameters tab
F Value – Touch off feed rate
P Value – Piercing Height
D Value – Piercing delay This value is defined in Milliseconds
C Value –Cutting height
V Value - Cutting voltage , if set to “0” then the system goes into the “Auto Voltage” option where the system samples the voltage at cutting height and then maintains this voltage for the entire cut. To make use of this parameter the MASSO DTHC module is required.
A Value - Feed rate Anti Dive , (Please note that this parameter has not yet been implemented but will be added at a future date) This value is a percentage of the X & Y axis feed rate below which the Z-axis will lock when under THC control to prevent the torch from moving into the material. The axis will unlock and the THC resume operation once the feed rate increases above this value.
O Value - Ohmic ON/OFF. 0 is Ohmic OFF, 1 is Ohmic ON.
S Value - Stop after piercing and wait for Cycle start. 0 is do not stop, 1 is Stop and wait for Cycle Start.

More detail is here: MASSO G200

Any help here would be greatly appreciated!!

Thanks!
Jeff

[Les Newell]

In function OnMove() you have this code:

Code: Select all

function OnMove()
   local len = math.hypot(endX - currentX , endY - currentY)

Add a check for Z only moves (plunge from pierce height to cut height)

Code: Select all

function OnMove()
   local len = math.hypot(endX - currentX , endY - currentY)
   if(len < 0.001 and not (toolClass == "MarkerTool" and zScribe == 1)) then return end

It may be worth making the same change in OnRapid()

[FabLab]

Looks like that did the trick!

Thanks Les!
I really appreciate it!!!

Attached is my completed version of the Masso Ver5 G3 controller with a DHTC and Air Scribe (Multi-Head) PP.
I think its pretty clean & it does work for me, hopefully it can help someone else.

Jeff