NCPlot Forums

This macro doesn't appear to function the same as the built-in G90. With external G90 macro enabled, X motion is 1/2 what is specified. For example, run this program with the external G90 enabled:
G00 X1.0 Z0.0
G90 X0.5 Z1.0

Select the plot line produced by the G90 and it's location is:
Line at Feed
Tool 0
Start Z0.0 X0.25
End Z1.0 X0.25
Length 1.0
Delta Z 1.0
Delta X 0.0

It seems OK on v2.07b1, what version do you see this on?

Scott

Hi Scott,

I'm running v2.07b1 and have tried it both on my desktop and laptop machines with the same result. Here are the steps I used to reproduce the problem:
1) Set machine configuration to Lathe Diameter
2) Make G90 a G Code macro
3) Enter and run the following:
g00 x1.0 z00.0
g90 x0.95 z1.0

X for the G90 is 0.475

I've attached a screen capture that shows what I'm seeing.

David

David,

I finally figured out what's going on with this... The G-Code macro is getting the X as a radius value instead of diameter. If you are writing your own G-Code macro there is a system variable you can check to see what the active machine type is. Its variable #5100 and it contains one of three values:

0 - Mill
1 - Lathe / Radius
2 - Lathe / Diameter

You can use this variable to check the radius / diameter active type and adjust the incoming X value accordingly:
IF [[#24NE#0]AND[#5100EQ2]] THEN #24=#24*2

Scott