Yep I just got him to use what I know works.
from the tormach manual
7.5.2 Linear Motion at Feed Rate – G01 For linear motion at feed rate (for cutting or not), program: G01 X~ Y~ Z~ A~ F~
Word Definition
X~ X-axis coordinate
Y~ Y-axis coordinate
Z~ Z-axis coordinate
A~ A-axis coordinate
F~ Feed rate
This produces coordinated linear motion to the destination point at the current feed rate (or slower if the mill won’t go that fast). The axis words are optional, except that at least one must be used.
The G01 is optional if the current motion mode is G01.
If cutter radius compensation is active, the motion differs from the above; see Cutter Compensation later in this chapter.
If G53 is programmed on the same line, the motion also differs; see Absolute Coordinates later in this chapter.
It is an error if: •
All axis words are omitted
• G10, G28, G30 or G92 appear in the same block
• No F word is specified
Now the part that was failing and why
7.6.2.11 Feed Rate Mode – G93, G94 and G95
To set the active feed rate mode to inverse time, program: G93 Inverse time is used to program simultaneous coordinated linear and coordinated rotary motion.
In inverse time feed rate mode, an F word means the move should be completed in [one divided by the F number] minutes.
For example, if the F number is 2.0, the move should be completed in half a minute.
When the inverse time feed rate mode is active, an F word must appear on every line which has a G01, G02, or G03 motion, and an F word on a line that does not have G01, G02, or G03 is ignored.
Being in inverse time feed rate mode does not affect G00 (rapid traverse) motions.
To set the active feed rate mode to units per minute mode, program: G94 In units per minute feed rate mode, an F word is interpreted to mean the controlled point should move at a certain number of inches per minute, or millimeters per minute, depending upon what length units are being used.
To set the active feed rate mode to units per revolution mode, program: G95 In units per revolution mode, an F word is interpreted to mean the controlled point should move a certain number of inches per revolution of the spindle, depending on what length units are being used. G95 is not suitable for threading, for threading use G33 or G76.
It is an error if:
• Inverse time feed rate mode is active and a line with G01, G02, or G03 (explicitly or implicitly) does not have an F word
• A new feed rate is not specified after switching to G94 or G95 canned cycle return level – G98 and G99
So what you did to the post was a fix I will have a look at the direction change and fix that in the copy I have.
@Anonymous
To Get the machine to just goto a Z position When it's finished cutting just doing a G30 I am not 100% sure that it will do what you wont. I need you to test this.
you may be able to change it in pathpilot see below. unless @xander.luciano has some idea how to do it.
7.5.9 Return to Pre-defined Position – G30 and G30.1
G30 uses the values stored in parameters 5181 and 5183 as the X and Z final point to move to.
The parameter values are absolute mill coordinates in the native machine units of inches.
G30 makes a rapid traverse move from the current position to the absolute position of the values in parameters.
G30 X~ Z~ makes a rapid traverse move to the position specified by axes including any offsets, then makes a rapid traverse move to the absolute position of the values in parameters 5181 and/or 5183. Any axis not specified won’t move.
G30.1 stores the current absolute position into parameters 5181-5183.
It is an error if:
• Cutter Compensation is turned on