Reply with QuoteIs this a mill or lathe? Tool length offsets in mill are called with G43 Hx.
Mach3 tool length offsets
When running programs using multiple tools I've discovered that the machine does not recognize / interpret length offsets from the program code. The length offset is whatever is shown active in the 'OFFSETS' screen. I am using T1 ... H1, Tx.....Hx etc. in the program. Changing the tool number showing in offsets results in appropriate Z values for the tool, turning offsets 'off' in the same screen results in the same Z position regardless of tool selected in the program (which is logical / makes sense).
Is there a toggle or command that causes the tool in the program to be recognized over the active in the 'offsets' screen?
Unable to post code to forum here at the moment, just hoping someone may have a quick 'check this' idea.
Similar Threads:
Is this a mill or lathe? Tool length offsets in mill are called with G43 Hx.
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Mill, using G43 on each tool change
Dstamp
Post some of you program, it may not be arranged correctly
Mactec54
not sure of the question here, it sounds like you want to enter your tool length offsets thru the program, correct?? using the G10 command?? correct ?? you need to know the format to do that, G10 G90 P or D or R or L I don't know your machine, but that's how you do it. I have never been a big fan of doing this
Wanting to enter tool number and have the program reference the correct tool length offset in the tool table, not tool length offsets from the program.
Tanks,
DLS
The active tool is what is shown in 'offsets' screen, not what is selected by G43 Tx Hx in program
The active tool length offset is only what is selected here
The machine is a refurb knee mill using Mach3. I have setup the Z so down is negative direction and up is positive direction.
well, forgive me if I keep it as basic as possible then, are you programming the following line???
T5 M6
G0X0Y0S5000M3
G43Z1.H5
??? G43 envokes the offset from whatever H value you enter.
if tool 5 has a value entered in the length offset column, that is the number that will be used
The semi colon in front of the line calling out the G43 causes Mach to ignore that particular line.
Dstump
By what the post processor has given you, this program is very badly formatted, I have said many times that Mach is very forgiving, to a lot of not the norm G-Code formats, But there is a limit of what it can run correctly, This would not run at all on a machining center, Can you save the program in MS word as text & post it here, If it is not to big I will clean it up for you so you can get your post processor fixed up to give you a good output
Mactec54
Please forgive me but I don`t understand what you mean by "enter the tool number", the tool number is called by the G code in Mach, there is no need to enter anything. If you want to manually call a tool then you need to do it in MDI mode, if you go to MDI and type in M6T4 for example then tool 4 will be shown in the "Tool Information" box showing the Diameter and Length as it is in the tool table, is this what you want to do ? ?Originally Posted by Dstamp
The "Tool Information" area on the main Mach3 screen is just for information, not for inputting tool numbers and offsets. All tool offsets should be either manually typed into the tool table or automatically done using the "probing/touch off" method.
As has been previously posted the line G43 H4 will call up the correct tooloffset from the tool table in Mach without you having to do anything at all, there are no tool offset lengths in the program, Mach doesn`t work like that it just uses the G43 H* line to get them from the tool table.
I think you need to change your Post Processor, I have never seen a Mach3 Post produce code like yours, FYI the best post I have found to modify for use with Mach3 is the Fanuc 0M, Mach is after all based on the Fanuc way of doing things and the code is good and "clean"
Regards
Rob
Correct,
Thanks, there are a couple of things yet to clean up, but removal of the semi colons worked. As the program is executed each Tx Hx command results in correct (desired / expected) tool showing up on the Tool Information portion of the screen.
Thanks,
I was hopeful it was something straightforward.
You can however enter the tool length into the tool table via Gcodethere are no tool offset lengths in the program, Mach doesn`t work like that it just uses the G43 H* line to get them from the tool table
Hood
And just to add to the above, if the offset you update is currently active and the same as the tool number then it will update the offset without calling a further G43H*
Hood
